|
|
| |
|
_BUTTON |
| |
Provides information on what button a user pushed in a dialog box. Useful in conjunction with the MULTIPRO command (see below)
0 if the OK button was pressed
1 if the Cancel button was pressed
[permalink]
|
| |
|
Average Rating: 10.0 (8 votes)
|
|
|
| |
|
_BUTTON |
| |
Hidden parameter _Button can be used to test whether the user chose OK or Cancel within a MULTIPRO box, but its usefulness probably does not extend to testing actions with other boxes. This is because there are cases where OK can return a 1, the same as cancel.
For example, suppose you want to prompt the end-user to pick some areas, so you write:
ASEL,R,P
*IF,_BUTTON,EQ,0,THEN
...
The problem with this technique is if the user is inclined to use the Apply button (or MMB), and then follow with OK to close the picking dialog, then _BUTTON will equal 1.
As a point of trivia, _BUTTON equals 2 after Apply is pressed, but this cannot be tested in an APDL macro, since the test will not be executed until the dialog is closed with OK, Cancel or Pick All. The Reset button does not appear to modify _BUTTON
[permalink]
|
| |
|
Average Rating: 10.0 (7 votes)
|
|
|
| |
|
_RETURN |
| |
Parameter returns number of geometry entity just created (5.3 does not support _return for the L command)
[STI: Please see Ch. 4.7 "Using the _STATUS and _RETURN Parameters in Macros" in the ANSYS APDL Guide for more information]
[permalink]
|
| |
|
Average Rating: 10.0 (12 votes)
|
|
|
| |
|
_STATUS |
| |
Executing an ANSYS command, whether in a macro or elsewhere, generates the parameter _STATUS. This parameter reflects the error status of that command:
0 for no error
1 for a note
2 for a warning
3 for an error
[STI: Please see Ch. 4.7 "Using the _STATUS and _RETURN Parameters in Macros" in the ANSYS APDL Guide for more information. A similar parameter _ERROR returns 0 for no error, 1 for warning, 2 for error after a command.]
[permalink]
|
| |
|
Average Rating: 3.3 (3 votes)
|
|
|
| |
|
*DEL |
| |
*del,array,,NOPR
Silently deletes an array using undocumented "NOPR" argument.
[permalink]
|
| |
|
Average Rating: 9.3 (35 votes)
|
|
|
| |
|
*DOWHILE |
| |
*DOWHILE,parm
*DOWHILE is similar to *DO and performs the commands bracketed by *ENDDO. *DOWHILE,Parm command loops repeatedly through the next *ENDDO command as long as Parm is true (greater than zero).
[STI: This is for 6.0]
[permalink]
|
| |
|
Average Rating: 6.2 (21 votes)
|
|
|
| |
|
*GET,,ACTIVE |
| |
*GET,Parm,ACTIVE,,SYNAME,,START,1
Gets the first 8 characters of the OS name (such as INTELNT). For more than 8 characters, use "9" for the START modifier. Note that some platforms may change between 5.4 through 5.6 (such as HPPA 8000).
A list of returned values for systems are shown below (for 8.0, although some systems listed below may no longer be supported):
RS6000 64
RS6000
HPPA 7000
HPPA 8000
HPPA 8000-64
HP IA64
SGI32
SGI64
SUN-USIII
FUJITSU
SOLARIS64
SOLARIS
DECAXP-OSF1
WINDOWS 64
INTEL NT
LINUX IA32
LINUX IA64
SUN4 SPARC
[permalink]
|
| |
|
Average Rating: 10.0 (7 votes)
|
|
|
| |
|
*GET,,ACTIVE |
| |
*GET,Parm,ACTIVE,0,SOLU,CNVG
You can also *GET the convergence indicator, where 0=not converged; 1=converged.
[permalink]
|
| |
|
Average Rating: 9.4 (17 votes)
|
|
|
| |
|
*GET,,ACTIVE |
| |
*GET,Parm,active,,date
Gets current system date (year, month, then day), for example, "20000704.0" for 07/04/2000.
Where year=nint(currdate/10000); month=nint((currdate-year*10000)/100); date=currdate-(year*10000+month*100)
[STI: I haven't found a way to grab the current time yet...]
[permalink]
|
| |
|
Average Rating: 10.0 (7 votes)
|
|
|
| |
|
*GET,,ACTIVE |
| |
*GET,Parm,active,,update
At 5.5, get the current ANSYS version or update number. For example, in 5.5.2, it returns 19990107.0. For 5.5.3, it returns 19990405.0
[permalink]
|
| |
|
Average Rating: 10.0 (2 votes)
|
|
|
| |
|
*GET,,ACTIVE |
| |
*GET,parm,ACTIVE,,SET,NSET
Retrieves the total number of results sets which are stored in the results file.
[permalink]
|
| |
|
Average Rating: 10.0 (14 votes)
|
|
|
| |
|
*GET,,ACTIVE |
| |
*GET,parm,ACTIVE,,AGREE
Gets agreement number
[STI: I found this one for a customer wanting to encrypt a macro for a specific company (agreement number). Kinda cool, IMHO.]
[permalink]
|
| |
|
Average Rating: 10.0 (4 votes)
|
|
|
| |
|
*GET,,CDSY |
| |
*GET,Parm,CDSY, ,NUM,MAX
Gets the max local coord. system number
You can also use the inquiry function
MAXCSYS = csyiqr(0,14)
[permalink]
|
| |
|
Average Rating: 9.4 (9 votes)
|
|
|
| |
|
*GET,,CE |
| |
*GET,Parm,CE,CeNum, TERM, num, [COEF | NODE | DOF]
Gets the node number, DOF, or coefficient in CE #CeNum, #num term.
The DOF key is as follows: 1=ux, 2=uy, 3=uz, 4=rotx, 5=roty, 6=rotz, 7=ax, 8=ay 9=az, 10=vx, 11=vy, 12=vz, 19=pres, 20=temp, 21=volt, 22=mag, 23=enke, 24=ends, 25=emf, 26=curr
[permalink]
|
| |
|
Average Rating: 10.0 (15 votes)
|
|
|
| |
|
*GET,,CE |
| |
*GET,Parm,CE,CeNum, [NTERM | CONST]
Gets the total number of terms or the constant for CE
[permalink]
|
| |
|
Average Rating: 10.0 (1 vote)
|
|
|
| |
|
*GET,,CE |
| |
*GET,Parm,CE,0,[MAX | NUM]
Gets the total #num number of CEs defined or the #max number of CEs.
[permalink]
|
| |
|
Average Rating: 10.0 (2 votes)
|
|
|
| |
|
*GET,,CINT |
| |
*GET,parm,CINT,cnum,CTIP,node,CONT,cnum,DTYPE,data
Gets the J-Integral or Stress Intensity Factor values. This is documented in 12.0 but maybe not as clearly as one may like. Upper-case letters are literal values used in this *GET.
cnum: CINT ID number (same ID as when contour was defined with CINT,NEW,cnum)
node: node number at crack tip
cnum: contour number (from 1 to max where max is from CINT,NCON,max)
data: jint is J-integral value. Use k1, k2, or k3 for stress intensity factors. iin1 through iin3 are the interaction integrals 1-3. Default (if left blank) is jint.
[permalink]
|
| |
|
Average Rating: 8.8 (4 votes)
|
|
|
| |
|
*GET,,COMMON |
| |
*GET,Parm,COMMON,,D3COM,,REAL,num
Uses #num double precision variable in the D3COM.INC include file (in the /ansys56/custom/include or /ansys56/customize/include directories, included in a "full" installation)
Example:
*GET,_z1,common,,stepcm,,int,16
Gets number of equilibrium iterations of the last substep of the last load step completed.
[permalink]
|
| |
|
Average Rating: 10.0 (1 vote)
|
|
|
| |
|
*GET,,COMMON |
| |
*GET,parm,common,,stepcm,,int,1
Newton-Raphson option key
[permalink]
|
| |
|
Average Rating: 10.0 (2 votes)
|
|
|
| |
|
*GET,,COMMON |
| |
*GET,parm,common,,stepcm,,int,69
Adaptive descent key
[permalink]
|
| |
|
Average Rating: 7.5 (4 votes)
|
|
|
| |
|
*GET,,COMMON |
| |
*GET,parm,common,,soptcm,,int,39
Equation solver values:
FRONT = 0, SPARSE=8, JCG=7, JCGOUT=2, ICCG=5, PCG=3, PCGOUT=3, ITER=0, etc.
[permalink]
|
| |
|
Average Rating: 10.0 (2 votes)
|
|
|
| |
|
*GET,,COMMON |
| |
*GET,parm,common,,soptcm,,int,66
Auto Solve Method
[permalink]
|
| |
|
Average Rating: 10.0 (1 vote)
|
|
|
| |
|
*GET,,COMMON |
| |
PCG common blocks:
*GET,parm,common,,stepcm,,int,138
PCG out-of-core key
*GET,parm,common,,stepcm,,int,105
PCG Single precision key
*GET,parm,common,,stepcm,,int,134
PCG Elem by Elem key
[permalink]
|
| |
|
Average Rating: 10.0 (1 vote)
|
|
|
| |
|
*GET,,COMMON |
| |
*get,parm,comm,,stepcm,,int,30
Number of nodal diameters:
[permalink]
|
| |
|
Average Rating: 7.1 (7 votes)
|
|
|
| |
|
*GET,,COMMON |
| |
Time & time step values
*get,TIME_END,common,,stepcm,,real,2
Get time at end of solve (TIME command)
*get,DT_INIT,common,,stepcm,,real,23
Get initial time step (DELTIM command)
*get,DT_MIN,common,,stepcm,,real,24
Get minimum time step (DELTIM command)
*get,DT_MAX,common,,stepcm,,real,25
Get maximum time step (DELTIM command)
[permalink]
|
| |
|
Average Rating: 10.0 (5 votes)
|
|
|
| |
|
*GET,,COMMON |
| |
Convergence values (CNVTOL):
*GET,param1,common,,stepcm,,real,28+i
Reference value of Lab
*GET,param2,common,,stepcm,,real,48+i
Tolerance about VALUE
*GET,param3,common,,stepcm,,int,34+i
Convergence norm
*GET,param4,common,,stepcm,,real,132+i
Minimum reference value
The parameter "i" to use is based on which criteria you are looking for:
I = 1 for F convergence
I = 2 for M convergence
I = 3 for U convergence
and there are more...
I tested some of these out on a model, and they work if you entered a value that is not the default. If you use the default value for any of these items, the *get returns a zero.
[permalink]
|
| |
|
Average Rating: 10.0 (1 vote)
|
|
|
| |
|
*GET,,COMMON |
| |
*GET,_cesha,common,,d3com,,real,178
This gets the current /ESHAPE setting
[STI: verified to work (at least) from 5.6 on up]
[permalink]
|
| |
|
Average Rating: 10.0 (2 votes)
|
|
|
| |
|
*GET,,COMMON |
| |
*get,parmname,common,,cfprp7,,real,13
Gets element edge length by ESIZE
*get,parmname,common,,cfprp7,,int,63
Gets number of element divisions specified by ESIZE
[permalink]
|
| |
|
| |
|
*GET,,COMMON |
| |
*GET,OMEGAX,common,,acelcm,,real,31
*GET,OMEGAY,common,,acelcm,,real,32
*GET,OMEGAZ,common,,acelcm,,real,33
*GET,DOMEGAX,common,,acelcm,,real,34
*GET,DOMEGAY,common,,acelcm,,real,35
*GET,DOMEGAZ,common,,acelcm,,real,36
Gets OMEGA and DOMEGA values for x, y, and z at the end of the load step.
[permalink]
|
| |
|
Average Rating: 10.0 (1 vote)
|
|
|
| |
|
*GET,,COMMON |
| |
*get,trf,common,,bfcom,,real,8
Get defined TREF value.
*get,tunf,common,,bfcom,,real,10
Get defined TUNIF value.
[permalink]
|
| |
|
Average Rating: 6.7 (6 votes)
|
|
|
| |
|
*GET,,COMMON |
| |
*get,parm,COMMON,,d3com2,,int,31
Gets the status of /UIS,MSGPOP. When writing macros you sometimes don't want those pesky warning messages to pop up all the time, so you use /uis,msgpop,3 to suppress them and put them back on with /uis,msgpop,0. The problem is if your macro is called by a macro that changed the msgpop status, then you kind of mess stuff up. The answer is to get the msgpop status before you change it then set it back.
Example usage:
*get,_oldMPS,COMMON,,d3com2,,int,31
/uis,msgpop,3
! Do my stuff
! ...
! ...
! ...
! Done with the stuff I want to suppress messages on
/uis,msgpop,_oldMPS
[permalink]
|
| |
|
Average Rating: 9.6 (27 votes)
|
|
|
| |
|
*GET,,COMMON |
| |
*get,parm,common,,stepcm,,real,10
Get the DMPRAT value for constant damping ratio.
[permalink]
|
| |
|
Average Rating: 10.0 (4 votes)
|
|
|
| |
|
*GET,,COMMON |
| |
*GET,XMIN,COMMON,,GRCOM,,REAL,44
/XRANGE min value
*GET,XMAX,COMMON,,GRCOM,,REAL,45
/XRANGE max value
*GET,YMIN,COMMON,,GRCOM,,REAL,6
/YRANGE min value
*GET,YMAX,COMMON,,GRCOM,,REAL,7
/YRANGE max value
[permalink]
|
| |
|
Average Rating: 10.0 (1 vote)
|
|
|
| |
|
*GET,,COMMON |
| |
*GET,PARM,common,,cmopt,,int,13232
Gets count of state variables in optimization (/OPT) run.
[permalink]
|
| |
|
Average Rating: 8.3 (6 votes)
|
|
|
| |
|
*GET,,COMMON |
| |
*GET,PARM,common,,cmopt,,int,13235
Gets count of design variables in optimization (/OPT) run.
[permalink]
|
| |
|
Average Rating: 10.0 (2 votes)
|
|
|
| |
|
*GET,,COMMON |
| |
To retrieve the node number at which the minimum or maximum results value occurs, first plot the nodal results of interest using the PLNSOL command, then execute one of the following:
*GET,Parm,COMMON,,CPOST1,,INT,107
to retrieve the node at which the minimum result value occurs, or
*GET,Parm,COMMON,,CPOST1,,INT,108
to retrieve the node at which the maximum result value occurs.
To determine whether the results are for the top, middle, or bottom of shells, use the following command:
*GET,Parm,COMMON,,CPOST1,,INT,5
Where PARM=1 for top, =2 for middle, =3 for bottom.
There are many other potential quantities of interest listed in the cpost1.inc file in the custom\include directory.
[permalink]
|
| |
|
Average Rating: 8.3 (12 votes)
|
|
|
| |
|
*GET,,COMMON |
| |
*GET,parm,COMMON,,BOLCMD,,REAL,16
Gets the current boolean tolerance value (value assigned to the BTOL command).
[permalink]
|
| |
|
Average Rating: 10.0 (2 votes)
|
|
|
| |
|
*GET,,CP |
| |
*GET,Parm,CP,CpNum,TERM,num,NODE
Gets the node number in CP #CpNum, #num term.
[permalink]
|
| |
|
Average Rating: 10.0 (1 vote)
|
|
|
| |
|
*GET,,CP |
| |
*GET,Parm,CP,CpNum,[DOF | NTERM]
Gets the DOF of the CP #CpNum or total number of terms. The DOF key is as follows: 1=ux, 2=uy, 3=uz, 4=rotx, 5=roty, 6=rotz, 7=ax, 8=ay 9=az, 10=vx, 11=vy, 12=vz, 19=pres, 20=temp, 21=volt, 22=mag, 23=enke, 24=ends, 25=emf, 26=curr
[permalink]
|
| |
|
Average Rating: 10.0 (1 vote)
|
|
|
| |
|
*GET,,CP |
| |
*GET,Parm,CP,0,[MAX | NUM]
Gets the total #num number of CPs defined or the #max number of CPs.
[permalink]
|
| |
|
Average Rating: 10.0 (4 votes)
|
|
|
| |
|
*GET,,ELEM |
| |
*GET,Parm,ELEM,elementNumber,EFOR,nodeNumber,item
where item is FX, FY, FZ, MX, etc.
Gets element nodal forces / moments associated with an element (without using selection and fsum).
[permalink]
|
| |
|
Average Rating: 10.0 (18 votes)
|
|
|
| |
|
*GET,,ETYP |
| |
*GET,Parm,ETYP, ,NUM,MAX
Gets the max element type number
You can also use the inquiry function
MAXETYP = etyiqr(0,14)
[permalink]
|
| |
|
Average Rating: 10.0 (3 votes)
|
|
|
| |
|
*GET,,NODE |
| |
*GET,par,NODE,n,NTEMP
Gets nodal structural temperatures applied on the model.
*VGET,parm(1),125,1,12,1,,,2
*VGETs nodal structural temperatures into an array.
[permalink]
|
| |
|
Average Rating: 8.4 (16 votes)
|
|
|
| |
|
*GET,,NODE |
| |
There is an undocumented *GET/*VGET for reaction forces as follows:
*GET,par,NODE,n,RF,Lab
where Lab can be UX,UY,UZ,ROTX,ROTY,ROTZ, or FX,FY,FZ,MX,MY,MZ
The *VGET is the same.
[STI: *GET for reaction force is documented at 5.6 but *VGET is not documented at 5.5 or 5.6]
[permalink]
|
| |
|
Average Rating: 7.1 (14 votes)
|
|
|
| |
|
*GET,,PARM |
| |
*GET,Parm,PARM,ARnn,ARTYPE
At 5.6.1, this returns the type of the ARxx parameter, not the type of the variable which ARnn is pointing to.
[permalink]
|
| |
|
Average Rating: -1.7 (3 votes)
|
|
|
| |
|
*GET,,PLAB |
| |
*GET,Parm,PLAB,mat,TEMP,Tvalue
Gets material value at given temperature.
For example:
*GET,EX1,EX,1,TEMP,70.0
Gets EX for material #1 at TEMP=70 and puts into parameter EX1.
[permalink]
|
| |
|
Average Rating: 10.0 (2 votes)
|
|
|
| |
|
*GET,,PLNSOL |
| |
*GET,parm,PLNSOL,,max
Works on both PLESOL and PLNSOL to obtain min/max values of last contour plot (use bmax/bmin to obtain bound value with Full Graphics on and ERNORM on). Note that the format is still "PLNSOL" as 3rd argument, although your plot may be of element solution (PLESOL).
[permalink]
|
| |
|
Average Rating: 10.0 (8 votes)
|
|
|
| |
|
*GET,,RCON |
| |
*GET,Parm,RCON, ,NUM,MAX
Gets the max REAL set number
You can also use the inquiry function
MAXREAL = rlinqr(0,14)
[permalink]
|
| |
|
Average Rating: 10.0 (2 votes)
|
|
|
| |
|
*GET,,TBLAB |
| |
*GET,parm,tblab,mat_number,NTEMP
Retrieves the number of temperature Tables defined for any TABLE (e.g., MISO)
*GET,parm,tblab,mat_number,TVAL,pos
Retrieves the temperature value at position "pos" of any TABLE defined as TBDATA (MISO for example)
It is useful for retrieving all strain/stress curves from database
[permalink]
|
| |
|
Average Rating: 10.0 (5 votes)
|
|
|
| |
|
*GET,,TBLAB |
| |
*GET,PARAM,tblab,matid,temp,0,ncon
Gets the number of constants (data values) for material tblab.
For example, to get the number of state variables defined for material ID #2, use:
*GET,param,STATE,2,TEMP,0,NCON
[permalink]
|
| |
|
Average Rating: 10.0 (3 votes)
|
|
|
| |
|
*GET/*VGET Sheet
|
| |
(PADT)
|
| |
This is a handy sheet with *GET and *VGET items. A user can print this out as a reference sheet when writing APDL macros.
[permalink]
|
| |
|
Average Rating: 6.3 (75 votes)
|
|
|
| |
|
*MOPER |
| |
*MOPER,ResVal(1,1),ResXYZ(1,1),MAP,InVal(1,1),InXYZ(1,1),kDim
kDim = 2, 2d (shell) 3, 3d (solid)
ANSYS 5.7 has a MAP option which will:
Given: A set of points InXYZ(nPt,3) and a value(s) InVal(nPt,nVal) at each point
A second Set of points ResXYZ(nOut,3), contained within the geometry of the first set of points.
Determine the value(s) ResVal(nOut,nVal) at each point in the second set.
*MOPER,ResVal(1,1),ResXYZ(1,1),MAP,InVal(1,1),InXYZ(1,1),kDim,Ratio,kOut
Ratio = MaxElSize/MaxGridDim of input data (auto default) (was 0.10 default)
kOut = 0, use closest point values 1, zero if ouside
"Here is the propose new description of the MAP option on *MOPER. The changes are:
Ratio will have an automatic default as recommended, based on the number of points. Field 8 is the Ration field (field 1 is the *MOPER command).
kOut is a proposed new option. The kOut setting points outside the field to zero should allow you to use the absolute value of the results as a mask vector. (0.0 will be false, non-zero (absolute value) will be true."
"For those of you who are using this command, I have found that the default value of 0.10 in field 8 is much too high for large problems. I suggest you supply a value in this field. A good value is:
Value = 1.0 / (sqrt(nIn)), where nin is the number of nodes in the input (known) set. (for kDim = 2)
Value = 1.0 / (cuberoot(nin)), where nin is the number of nodes in the input set (for kDim = 3)
[permalink]
|
| |
|
Average Rating: 9.5 (10 votes)
|
|
|
| |
|
*MOPER |
| |
*MOPER,Eloc(1,1),XYZ(1,1),INTP,Elem(1)
where:
*dim,XYZ,array,nPts,3
*dim,Elem,array,nPts
*dim,Eloc,array,nPts,3
This command finds the element containing the XYZ point, rather than the element with the closest centroid. The Eloc array is the element coordinates of the point.
Compare this, for example, with the *MOPER,,,ENEAR option.
[permalink]
|
| |
|
Average Rating: 7.1 (7 votes)
|
|
|
| |
|
*MOPER |
| |
*MOPER,sval(n),eloc(n,3),SGET,elem(n),label,comp
Finds stresses at certain points. This requires use of the *MOPER,,,INTP undocumented command prior to executing this command.
sval(n): output array containing stresses at the points of interest
eloc(n,3): input array containing relative locations inside the elements (output from INTP)
elem(n): input array containing element numbers related to the relative locations of "eloc" (output from INTP)
label,comp: stress component of interest (see PLNSOL,S for examples)
[permalink]
|
| |
|
Average Rating: 10.0 (6 votes)
|
|
|
| |
|
*OGDEN |
| |
*OGDEN,strain,stress,ltype,const,calc,sortsn,sortss,fname,ext
Ogden Hyperelastic Material
similar to *MOONEY for Ogden constitutive law for HYPER56, 58, & 74.
strain = name of array parameter vector containing experimental engineering strain values
stress = name of array parameter vector containing experimental engineering stress values
ltype = 1 simple tension,
2 equibiaxial tension or compression,
3 shear (using simple tension equations),
4 shear (using equibiaxial tension equations)
const = name of array containing ogden constants
calc = name of array containing calculated stress values
sortsn = sorted strain data to be used for *vplot command
sortss = sorted stress data to be used for *vplot command
fname = tb output filename (8 characters maximum).
ext = tb output file extension (8 characters maximum).
[STI: Ogden material is available for 18x family of elements at 5.7, so it is strongly recommended to use those elements instead.]
[permalink]
|
| |
|
Average Rating: 10.0 (4 votes)
|
|
|
| |
|
*RETURN |
| |
*RETURN,value
Break reading from an input file
Where value=0 returns to the top level, -n returns n levels, n returns to level n
Useful when breaking *DO loops or *IF conditional statements, for example.
[STI: Implemented at 5.7?]
[permalink]
|
| |
|
Average Rating: 10.0 (3 votes)
|
|
|
| |
|
*STATUS |
| |
*STATUS,_PRM
*STATUS,PRM_
Shows parameters which begin or end with an underscore.
[STI: Documented at 5.6]
[permalink]
|
| |
|
Average Rating: 7.1 (7 votes)
|
|
|
| |
|
*UILIST |
| |
*UILIST,filename,ext,dir
Lists the contents of a file to a 'pop-up' window when running interactively. It is similar to the *LIST command but this version runs from within a macro while *LIST does not.
[permalink]
|
| |
|
Average Rating: 10.0 (6 votes)
|
|
|
| |
|
*VFUN |
| |
*VFUN,array(1,1),DIRECT,array2(1,1)
Gets the direction cosines of a vector. For example:
*DIM,STRESS,array,nNodes,6
*vget sx,sy,sz, sxy,etc into STRESS(1,1), STRESS(1,2), etc
*DIM,DIR,array,nNodes,9
*VFUN,DIR(1,1),DIRECT,STRESS(1,1)
DIRECT will contain the 3 x 3 matrix of direction cosines
[STI: Works for 5.6.2]
[permalink]
|
| |
|
Average Rating: 5.8 (12 votes)
|
|
|
| |
|
*VFUN |
| |
*VFUN,uv(1,1),ACORD,xyz(1,1),areanum
Gets (u,v) 'natural' coordinates of a point lying on an area areanum when the global coordinates (x,y,z) are known.
uv is dimensioned (npoints,2)
xyz is dimensioned (npoints,3)
areanum is area number
*VFUN,xyz(1,1),GCORD,uv(1,1),areanum
The GCORD option is the inverse of the ACORD option.
[permalink]
|
| |
|
Average Rating: 4.0 (5 votes)
|
|
|
| |
|
*VGET,,ID1 |
| |
An undocumented *VGET for selecting Lines, Areas and Volumes by "hot spot"
*VGET,xyzarray,ID1,num,ID2,ID3,,,4
Xyzarray: 3 row array that the coordinates are stored in
ID1: Location in ANSYS memory of information - 40 = Line, 60 = Area, 80 = Volume
ID2: First offset in memory location - 8 = Lines, 6 = Areas and Volumes
ID3: Second offset in memory location - 3 = Lines, 2 = Areas and Volumes
for lines:
*dim,ls_cent,,3
*vget,ls_cent(1),40,num,8,3,,,4
lsel,s,loc,x,ls_cent(1)
lsel,r,loc,y,ls_cent(2)
lsel,r,loc,z,ls_cent(3)
for areas:
*dim,al_cent,,3
*vget,ls_cent(1),60,num,6,2,,,4
for volumes:
*dim,vl_cent,,3
*vget,vl_cent(1),80,num,6,2,,,4
[permalink]
|
| |
|
Average Rating: 9.3 (7 votes)
|
|
|
| |
|
*VOPER |
| |
*VOPER, ParR, Par1, Oper, Par2, CON1, CON2
For *VOPER, the Oper argument can take the form of and, or, or xor. This is for binary comparison of arrays. Hence, the values in the arrays Par1 and Par2 are taken such that negative numbers or zero is "0" and positive numbers are "1" for comparison.
For example, when Oper = and, both values in Par1(i) and Par2(i) need to match to return ParR(i)=1.
When Oper = or, if either value in Par1(i) and Par2(i) is "1", then ParR(i)=1.
When Oper = xor, both values in Par1(i) and Par2(i) need to be different to return ParR(i)=1.
Recall from above that when the comparisons are made, positive numbers are assumed to be "1" and negative (and zero) numbers are assumed to be "0". Hence, for XOR case, "3" and "4" will return "0" since "3->1" and "4->1", they are the same, so XOR returns "0" (false).
[permalink]
|
| |
|
Average Rating: 10.0 (1 vote)
|
|
|
| |
|
*VPUT |
| |
*VPUT, ParR, Entity, ENTNUM, Item1, IT1NUM, Item2, IT2NUM, KLOOP
To change selection status of entities, use a format similar to *VGET.
Use for Entity = node, elem, kp, line, area, or volu, ENTNUM = 1, and Item1 = nsel, esel, ksel, lsel, asel, or vsel. The array ParR would be similar to the *VGET array, where
-1 = unselected
0 = undefined
1 = selected
It is recommended to select all entities with nsel,all (or related command) prior to using *VPUT.
[permalink]
|
| |
|
Average Rating: 9.2 (6 votes)
|
|
|
| |
|
*VREAD |
| |
*VREAD,array(1,1),filename,ext,dir,ncol,row,column,plane,start_line
Undocumented fields are: row, column, plane to allow reading in matrix by row, column, or plane. start_line is the line of the file to start reading from.
[STI: documented from 5.7 onwards.]
[permalink]
|
| |
|
Average Rating: 9.2 (31 votes)
|
|
|
| |
|
*VSCFUN |
| |
*VSCFUN,LocPar,POS,myarray(1),compare,myvalue,tolerance
Determines position in array of value "myvalue" in array "myarray" and returns in LocPar. "compare" can be any comparison operator, such as GE, GT, LE, and LT. The first occurrence will be returned. "1" will be returned for no match. "tolerance" (default 1e-6) sets the tolerance for a match. [Note that EQ comparison is valid for 5.7 and 6.0 but was removed in 6.1 because it returns only first match.]Example:
*dim,a,,5
a(1)=1,2,3,4,5
*vscfun,b,POS,a(1),ge,3
Returns "3" for third index/position.
[permalink]
|
| |
|
Average Rating: 10.0 (9 votes)
|
|
|
| |
|
*VWRITE options/formats
|
| |
(Various sources)
|
| |
Tips on *VWRITE formats (Fortran style).
[permalink]
|
| |
|
Average Rating: 9.1 (39 votes)
|
|
|
| |
|
/AN3D |
| |
/AN3D for 3D annotation is documented at 5.6. It is undocumented but available at 5.5.
The following are the ANSYS 5.5 /AN3D commands.
/AN3D,POIN,x,y,z
/AN3D,LINE,x1,y1,z1,x2,y2,z2
/AN3D,AREA,npt,x1,y1,z1,x2,y2,z2,x3,y3,z3,x4,y4,z4
/AN3D,ARRO,symsiz,x1,y1,z1,x2,y2,z2
/AN3D,TEXT,x,y,z,text
/AN3D,SYMB,itype,x,y,z,size
[permalink]
|
| |
|
| |
|
/AUX02 |
| |
Binary file dump. Enter /AUX02 to find list of applicable commands.
Example usage from John Swanson:
/aux2 ! enter file dump utility
file,foo,rst ! specify file name
form,long ! dump the full record of information
dump,2 ! dump the second record (index record) xxx is the 11th integer
ptr,xxx ! dump the record at pointer xxx (this is an index of all the load sets.) The last non-zero integer is the last load set. The others are the load sets in order. This is the way to get the other load cases. Call this pointer yyy
ptr,yyy+103 ! this is the location of the double precision header for this load set (103 skips the integer header) omegay is the 13th value.
If you look at the file fdresu.inc (File Descriptor Result) on the distribution media you will see a full description of the structure of the .rst file, and you may be able to derive or modify the above sequence for accessing other information.
[permalink]
|
| |
|
Average Rating: 8.3 (3 votes)
|
|
|
| |
|
/AUX03 |
| |
Results file editor. Enter /AUX03 to find list of applicable commands.
[permalink]
|
| |
|
Average Rating: 10.0 (3 votes)
|
|
|
| |
|
/CLEAR |
| |
/CLEAR,SOLU
Clears the database of the current solution in memory while keeping the database intact. This nifty options allows you to dump the solution without exiting the program.
Note that in 5.7, you can choose to SAVE only the geometry & loads with a new argument to that command. Then, a user can (/CLEAR and) RESUME the database, leaving only geometry in memory.
A related command is LCZERO, although this does not dump the solution but zeroes it out instead.
[permalink]
|
| |
|
Average Rating: 8.8 (4 votes)
|
|
|
| |
|
/CONFIG |
| |
/CONFIG,PRXY,1
At 6.0, if Poisson's ratio is not input, a warning is presented to the user to let him/her know that a default value of 0.3 will be used. This configuration command changes the warning to a note, so there will not be a ton of warning messages issued during solve.
An alternative is to add in the config6x.ans file:
PRXY_DEF = 1
[permalink]
|
| |
|
Average Rating: 10.0 (2 votes)
|
|
|
| |
|
/CONFIG |
| |
/CONFIG,NODBB,1
Toggles whether or not the backup database file (jobname.dbb) will be written upon SAVE or /EXIT
[permalink]
|
| |
|
Average Rating: 10.0 (2 votes)
|
|
|
| |
|
/CONFIG |
| |
/CONFIG,NOCMDDB,1
or
NO_CMDDB=1 in config56.ans
Supresses addition of command history in database log file (LGWRITE).
[permalink]
|
| |
|
Average Rating: 10.0 (2 votes)
|
|
|
| |
|
/CONFIG |
| |
/CONFIG,NOELDBW,num
Controls writing of results info
1=do not write results to *.db but only *.rst
2=do not write results to *.rst, only *.db
3=do not write to either *.rst or *.db)
[STI: I use /CONFIG,NOELDB,1 to give max memory during solution rather than filling up database space -db with results. Please see CSI's Tip of the Week on memory management for more details. This was documented from 5.7 onwards, I believe.]
[permalink]
|
| |
|
Average Rating: 10.0 (3 votes)
|
|
|
| |
|
/CONFIG |
| |
/CONFIG,RESUPRES,0
or
RESUPREC=0 in config145.ans
In ANSYS 14.5, stresses, strains, and other element quantities are written in the result file (.rst) as single precision to save space (DOF solution and reaction forces are still written as double-precision). This command, when invoked before solving, will store all results in double-precision.
[permalink]
|
| |
|
Average Rating: 10.0 (3 votes)
|
|
|
| |
|
/DEBUG |
| |
The /DEBUG command generates debugging at various points in the output. You can specify one of three formats for /DEBUG: solution debug format, element debug format, and general debug format.
[STI: Please see this link for more details on /DEBUG]
[permalink]
|
| |
|
Average Rating: 10.0 (28 votes)
|
|
|
| |
|
/DEMO |
| |
/DEMO,num,1
Allows graphics benchmarks to be performed (getting a rough idea of graphics card performance). This command rotates the model "num" number of times and prints a summary of stats.
[permalink]
|
| |
|
Average Rating: 5.0 (1 vote)
|
|
|
| |
|
/DEV |
| |
/DEV,PSFN,NINC
Turn off incrementing of JPEG filenames (suppress the 'nnn' in jobnamennn.jpg).
/DEV,PSFN,NONINC
Resume incrementing of JPEG files.
[permalink]
|
| |
|
Average Rating: 10.0 (3 votes)
|
|
|
| |
|
/DFLAB |
| |
/DFLAB,dofnum,dlabel,flabel
Changes DOF #dofnum to "dlabel" (D) and Force to "flabel" (F). DOF numbers range from 1-32. For example, DOF number 1 is UX, 2 is UY, etc.
This should be the first command issued upon entering ANSYS.
/DFLAB,19,PRESSURE changes PRES label (#19) to PRESSURE
[permalink]
|
| |
|
| |
|
/DIRGET |
| |
/dirget,parm,filename,fileext
Gets the list of files with the file extension "filename" or "fileext"
For example:
/dirget,_str,all,tif
Gets all filenames with extension "TIF"
[STI: Note: This may only work on UNIX at 5.6.1, not on NT. I keep getting bombed out of ANSYS using this command on NT. Also, for 5.7 and above, look at the /INQUIRE command and strings for same functionality.]
[permalink]
|
| |
|
Average Rating: 10.0 (1 vote)
|
|
|
| |
|
/ENCRYPT |
| |
/ENCRYPT,Encryption_key,File_name,File_ext,Directory_Path/
The commands /ENCRYPT and /DECRYPT allow one to encrypt macros. See APDL Programmer's Guide for more details.
[permalink]
|
| |
|
Average Rating: 8.3 (6 votes)
|
|
|
| |
|
/FACET |
| |
/FACET,FINE,n
Changes tesselation where n is from 0 (coarsest, default) to 10 (finest). For XOX Shapes geometry only (IGES default importing or Connection Kit "Allow defeature" importing) Functionality replaced by GMFACE command (see below). [5.5 Beta]
[permalink]
|
| |
|
Average Rating: 10.0 (2 votes)
|
|
|
| |
|
/GST |
| |
/GST,Lab,Lab2
In batch mode, /GST,ON will write convergence data to file.gst using the ANSYS Graphics format (use Display utility to plot file).
On the other hand, /GST,ON,ON will write convergence data to file.gst using an XML format (use the Results Tracker utility from the ANSYS Product Launcher, Tools menu to plot file).
[permalink]
|
| |
|
Average Rating: 10.0 (4 votes)
|
|
|
| |
|
/HOLD |
| |
/HOLD,filename,timeint,timeout
Read a command from file "filename" if it exists. If it doesn't exist, wait "timeint" seconds, then keep trying again until "timeout" seconds.
[permalink]
|
| |
|
Average Rating: 8.6 (7 votes)
|
|
|
| |
|
/INQUIRE |
| |
/INQUIRE,strarray,DIRECTORY
This gets the working directory ANSYS was launched from.
[permalink]
|
| |
|
Average Rating: 10.0 (9 votes)
|
|
|
| |
|
/INQUIRE |
| |
/INQUIRE,strarray,JOBNAME
This gets the ANSYS jobname and puts it into a string array called "strarray".
[permalink]
|
| |
|
Average Rating: 10.0 (5 votes)
|
|
|
| |
|
/INQUIRE |
| |
/INQUIRE,strarray,TITLE,n
This gets the ANSYS title starting from character "n".
[permalink]
|
| |
|
Average Rating: 10.0 (5 votes)
|
|
|
| |
|
/MSTART |
| |
/MSTART,MTOOL,off
This turns off/on the Mechanical Toolbar. For ANSYS/Professional, if you want to start ANSYS without the Mechanical toolbar, add the following lines to your start56.ans file:
/MSTART,MTOOL,OFF
/MSTART,MAIN,ON
/MSTART,INPUT,ON
/MSTART,TOOL,ON
[permalink]
|
| |
|
Average Rating: 10.0 (1 vote)
|
|
|
| |
|
/NERR |
| |
/NERR,,,field
Ignores all error messages
If field is set to -1, ANSYS will keep running unless a fatal error occurs. All errors are written to jobname.out and jobname.err.
If field is set to -2, ANSYS will behave the same but errors are reported to jobname.err only, not jobname.out.
[permalink]
|
| |
|
Average Rating: 8.8 (33 votes)
|
|
|
| |
|
/PGRPH |
| |
/PGRPH,SAVE
Issue "SET" commands and "/PGRPH,SAVE" after each results set you want to save as PowerGraphics file format. A file called "jobname_LS_SS.pgr" will be generated for each results set based on LS (Load step) and SS (Substep).
[STI: This feature is available at 5.6 but officially released at 5.7. At 5.7, however, the procedure is very different. See POUTRES, PGWRITE, PGSAVE, PGRAPH, PGRSET commands at 5.7 for more details]
[permalink]
|
| |
|
Average Rating: 10.0 (1 vote)
|
|
|
| |
|
/PGRPH |
| |
/PGRPH,ON
This command will change ANSYS's behavior such that the PowerGraphics files ('jobname_LS_SS.pgr') will be used instead of the actual results set after subsequent "SET" commands. The PowerGraphics files provide faster plotting like PowerGraphics but still has some features/behavior present with Full graphics.
[STI: This feature is available at 5.6 but officially released at 5.7. At 5.7, however, the procedure is very different. See POUTRES, PGWRITE, PGSAVE, PGRAPH, PGRSET commands at 5.7 for more details]
[permalink]
|
| |
|
Average Rating: 10.0 (1 vote)
|
|
|
| |
|
/PNUM |
| |
/PNUM,DOMAIN,1
Shows domains generated for domain decomposition solver (DDS). Beta at 5.6, 5.7, but it is documented at 6.0.
[permalink]
|
| |
|
Average Rating: 10.0 (1 vote)
|
|
|
| |
|
/RMTMP |
| |
Removes/closes the file specified in /INPUT after it is read. /RMTMP should be the last command in the input file.
[permalink]
|
| |
|
| |
|
/TEE |
| |
/TEE,(new,append,end),filename,ext,dir
Echos the input automatically to another text file designated as the model is created.
[STI: This is an official command in 5.6]
[permalink]
|
| |
|
Average Rating: 10.0 (1 vote)
|
|
|
| |
|
/TRACK |
| |
/TRACK,MonLevel,PrintLevel,SumLevel
The /TRACK command issues a message when the program logic enters and leaves some of the higher level subroutines. Subroutines TrackBegin and TrackEnd (see Chapter 6 of UPF Guide) set up the /TRACK command.
MonLevel is the level for timing monitoring. PrintLevel is the level for enter/exit printout, and SumLevel is the level at which the timing sum is output. Each of these arguments can be any value between 0 and 9 (default is 0).
You can use the /TRACK command to identify which section of code is causing the program to abort. For example, to flag up to eight levels of subroutines to determine when the program logic enters and leaves them, you would issue the command /TRACK,,8.
Another very useful feature is to use /TRACK to get contact element statistics during solution in a batch run. Use /TRACK,,1,-1 and you will see contact & solution stats printed at the end of the run (batch only).
[permalink]
|
| |
|
Average Rating: 10.0 (9 votes)
|
|
|
| |
|
/TXTRE |
| |
/TXTRE,file,88
This option allows placement of an image on the screen (anywhere you want). A typical example of putting your own picture/logo in the bottom-right corner of the Graphics window is shown below:
/txtre,file,88,'MYLOGO','PNG',,2
/anum,1,13,1.5297,-0.98938
/lsym,1.556,-0.990,0,88,0.000,1
where "MYLOGO.PNG" is the name of your image file and "2" can be "0" for pixmap/bitmap, "1" or "jpeg" for JPEG, and "2" or "png" for PNG, as noted in the online-help for /TXTRE.
A similar command (this one is documented in /TXTRE) to replace the graphical ANSYS logo with your own is:
/txtre,file,51,'MYLOGO','PNG',,2
[permalink]
|
| |
|
Average Rating: 10.0 (11 votes)
|
|
|
| |
|
/UI |
| |
/UI, COPY, SAVE, JPEG
This undocumented option of the /UI command creates a JPEG file of the current graphics window. Also, see
/ui,copy,save,jpeg,graph,color,reverse,portrait or
/ui,copy,save,jpeg,grap,colo,norm,port,,100
[permalink]
|
| |
|
Average Rating: 10.0 (7 votes)
|
|
|
| |
|
/UI |
| |
/UI, WSIZE, xstart, ystart, xdist, ydist
This moves/modifies the graphics window size. Specify xstart as pixels from left side of screen, ystart as pixels from top of screen, and distance in pixels.
For example, issue "/ui,wsize,175,175,700,700/1.325" to see the window positioned 175 pixels from top left corner of screen with a width of 700 (preserving 1.325 aspect ratio).
[permalink]
|
| |
|
Average Rating: -2.0 (5 votes)
|
|
|
| |
|
/UI |
| |
/UI,RAISE
Raises the Graphics Window to the forefront. Useful with /UI,copy,save,jpeg to make sure no other toolbars, widgets, etc. obscure view.
[permalink]
|
| |
|
Average Rating: 10.0 (3 votes)
|
|
|
| |
|
/UI |
| |
/ui,copy,save,png,graph,color,reverse,portrait,yes
Generates a PNG file of the active contents of the ANSYS Graphics window [verified at 6.0].
[permalink]
|
| |
|
Average Rating: 10.0 (4 votes)
|
|
|
| |
|
/UIS |
| |
/UIS,MSGPOP,4
Suppresses error message pop-up dialog box. (Error messages will still be recorded in the jobname.err file and output window/file.)
[permalink]
|
| |
|
Average Rating: 7.5 (8 votes)
|
|
|
| |
|
/UNDO |
| |
/UNDO,on
Turns on UNDO feature which is active for most commands (prior to session editor at 5.6). Saves a file to "jobname.undo". Valid options are "on, off, prompt, status".
UNDO
After /UNDO feature is activated above, this command actually undos the last command.
[permalink]
|
| |
|
Average Rating: -2.5 (2 votes)
|
|
|
| |
|
/XML |
| |
/XML,filename,ext,directory
This ANSYS command allows to write current load step results in XML format for use in Workbench Simulation.
Similar to other ANSYS commands, the 2nd through 4th arguments allow specification of the filename to save to. "Filename" defaults to the jobname, "Ext" defaults to "xml", and "Directory" defaults to the current working directory. Use of this command will write out geometry and results, as specified by the XMLOPT undocumented command.
[permalink]
|
| |
|
Average Rating: 8.9 (18 votes)
|
|
|
| |
|
~EUI |
| |
~eui,wm iconify .dlgAnsysGUI
Minimize ANSYS window
~eui,wm deiconify .dlgAnsysGUI
Maximize ANSYS window
[STI: Works for 6.1 and above]
[permalink]
|
| |
|
Average Rating: 8.6 (7 votes)
|
|
|
| |
|
~EUI |
| |
~eui, 'puts [clock format [clock seconds] -format "%c"]'
This writes the current date and time to the Output Window/File.
[permalink]
|
| |
|
Average Rating: 10.0 (5 votes)
|
|
|
| |
|
12 Predefined Views
|
| |
Matthew Pausley (Nuvotronics, Inc.)
|
| |
This is an XML file that can be used in Workbench Mechanical to provide 12 common views aligned with the coordinate axes. The naming convention is “Up-Axis + Axis of viewing”, i.e. “Z+X” means “Z axis is up, looking in the direction of positive X”.
To import this XML file into Workbench Mechanical, go to "View menu > Windows > Manage Views", then click on the "Import..." icon in the Manage Views panel to import this XML file.
[permalink]
|
| |
|
Average Rating: 8.3 (3 votes)
|
|
|
| |
|
180 Series Elements: Why Should One Use Them in Linear Analysis
|
| |
(ANSYS, Inc.)
|
| |
Presentation on 18x elements (continuum, beam, shell) and its features related to both linear and nonlinear analyses.
[permalink]
|
| |
|
Average Rating: 9.2 (82 votes)
|
|
|
| |
|
22x Coupled-Field Elements [PDF]
|
| |
Sheldon Imaoka (ANSYS, Inc.)
|
| |
"The 22x direct coupled-field elements (PLANE223, SOLID226-227) provide a wide
array of material behavior for multiphysics applications - these include piezoelectricity, piezoresistivity, thermoelasticity, and thermoelectricity. This memo hopes to introduce
some of the pertinent features of these elements."
(Week 34, week of 06/11/06.)
[permalink]
|
| |
|
Average Rating: 8.9 (37 votes)
|
|
|
| |
|
3-Dimensional Thermal Analysis and Active Cooling of Short-Length High-Power Fiber Lasers
|
| |
L. Li, H. Li, T. Qiu, V. L. Temyanko, M. M. Morrell, and A. Schülzgen
|
| |
"A fully 3-dimensional finite element model has been developed
that simulates the internal temperature distribution of short-length highpower
fiber lasers. We have validated the numerical model by building a
short, cladding-pumped, Er-Yb-codoped fiber laser and measuring the core
temperature during laser operation. A dual-end-pumped, actively cooled,
fiber laser has generated >11 W CW output power at 1535 nm from only
11.9 cm of active fiber. Simulations indicate power-scaling possibilities
with improved fiber and cooling designs."
[ANSYS Thermal, version 6.1]
[permalink]
|
| |
|
Average Rating: 9.0 (10 votes)
|
|
|
| |
|
3D Graphics |
| |
By setting the environment variable ANSXXX to 1 and using OpenGL graphics (-d 3d), one can resize the window to any aspect ratio (not limited to max ratio of 1:1.67). Note that this doesn't work under Windows; it works for UNIX with OpenGL only (on HP-UX, you need to run the OpenGL version of ANSYS).
[permalink]
|
| |
|
Average Rating: 10.0 (2 votes)
|
|
|
| |
|
A 3D Dynamical Biomechanical Tongue Model to Study Speech Motor Control
|
| |
Jean-Michel Gérard, Reiner Wilhelms-Tricarico, Pascal Perrier & Yohan Payan
|
| |
"A 3D biomechanical dynamical model of human tongue is presented, that is elaborated in
the aim to test hypotheses about speech motor control. Tissue elastic properties are accounted
for in Finite Element Modeling (FEM). The FEM mesh was designed in order to facilitate the
implementation of muscle arrangement within the tongue. Therefore, its structure was
determined on the basis of accurate anatomical data about the tongue. Mechanically, the
hypothesis of hyperelasticity was adopted with the Mooney-Rivlin formulation of the strain
energy function. Muscles are modeled as general force generators that act on anatomically
specified sets of nodes of the FEM structure. The 8 muscles that are known to be largely
involved in the production of basic speech movements are modeled. The model and the
solving of the Lagrangian equations of movement are implemented using the ANSYS™
software. Simulations of the influence of muscle activations onto the tongue shape are
presented and analyzed."
[ANSYS Nonlinear, version unspecified]
[permalink]
|
| |
|
Average Rating: 5.0 (6 votes)
|
|
|
| |
|
A 64-Pixel Linear Thermopile Array Chip Designed for Vacuum Environment
|
| |
U. Dillner, E. Kessler, V. Baier, A. Berger, T. Eick, D. Behrendt, H. Urban
|
| |
"We report on the development of a 64-pixel high performance linear thermopile array chip designed for
vacuum environment based on a silicon nitride membrane as substrate, Bi0.87Sb0.13/Sb as thermoelectric
materials combination and an Ag-black broadband absorber layer. The array chip was mounted on a
ceramic substrate and placed on the socket of a commercial hybrid package with 64 pins.
Measurements of the linear array chip in vacuum environment and in absence of an entrance filter
delivered a responsivity of 245 V/W, a sensitivity of 166 µVm²/W, a specific detectivity of
1.6x109 cmHz1/2/W at an electrical resistance of 9 k and a thermal time constant of 150 ms. The pixelto-
pixel cross-talk was reduced to less than 0.4 % due to slits in the membrane between adjacent pixels
made by dry etching."
[ANSYS Thermal, version unknown]
[permalink]
|
| |
|
Average Rating: 10.0 (3 votes)
|
|
|
| |
|
A brief overview of the condition number
|
| |
Aaron Acton (ANSYS, Inc.)
|
| |
"This article presents an overview of the condition number for a matrix and the potential effect of ill conditioning on the solution of a system of linear equations. The information is intended to be general, although specifi c information relevant to finite-element analysis is also included. Vector and matrix norms are introduced before de fining the condition number, and the choice of matrix norm in the calculation of the condition number is discussed. A method of estimating the condition number is also provided, including a sample implementation in the ANSYS Parametric Design Language (APDL)."
[permalink]
|
| |
|
Average Rating: 9.6 (12 votes)
|
|
|
| |
|
A Compilation of Anand Parameters for Selected SnPb and Pb-free Solder Alloys
|
| |
Zane Johnson (University of Minnesota)
|
| |
"Finite-element (FE) simulation is widely used in
electronic packaging. It is particularly useful in the design of
solder joint attachments. To ensure fidelity, FE simulation must
capture the highly nonlinear behavior of solder. One useful
material model for solder is Anand’s viscoplastic model. A
compilation of Anand parameters reported in the literature for
a variety of solder alloys is provided."
[permalink]
|
| |
|
Average Rating: 10.0 (7 votes)
|
|
|
| |
|
A DOS-Enhanced Numerical Simulation of Heat Transfer and Fluid Flow Through an Array of Offset Fins with Conjugate Heating in the Bounding Solid
|
| |
E.M. Sparrow, J.P. Abraham, P.W. Chevalier
|
| |
"The method of Design of Simulation (DOS) was used to guide and enhance a numerical
simulation of fluid flow and heat transfer through offset-fin arrays which form the interior
geometry of a cold plate. The basic problem involved 11 independent parameters. This
prohibitive parametric burden was lessened by the creative use of nondimensionalization
that was brought to fruition by a special transformation of the boundary conditions.
Subsequent to the reduction of the number of parameters, the DOS method was employed
to limit the number of simulation runs while maintaining an accurate representation of the
parameter space. The DOS method also provided excellent correlations of both the dimensionless
heat transfer and pressure drop results. The results were evaluated with
respect to the Colburn Analogy for heat and momentum transfer. It was found that the
offseting of the fins created a larger increase in the friction factor than that which was
realized for the dimensionless heat transfer coefficient."
Similar paper can be found here.
[ANSYS Flotran, version unknown]
[permalink]
|
| |
|
Average Rating: 10.0 (5 votes)
|
|
|
| |
|
A Finite Element Model For Pre- And Post-Test Calculations of the FOREVER-Experiments
|
| |
H. G. Willschuetz, E. Altstadt, F. P. Weiss, B. R. Sehgal
|
| |
"An axis-symmetric Finite Element (FE) model is developed based on the multi-purpose code ANSYS/Multiphysics. Using the Computational Fluid Dynamics (CFD) module the temperature field within the melt pool and within the vessel wall is evaluated. The transient structural mechanical calculations are then performed applying a creep model which takes into account large temperature, stress and strain variations." (Document 2)
[permalink]
|
| |
|
Average Rating: 9.8 (54 votes)
|
|
|
| |
|
A High-Performance Tunneling Accelerometer
|
| |
Edward Boyden, Osamah El Rifai, Brian Hubert, Maurice Karpman, Dave Roberts
|
| |
Design of a MEMS tunneling accelerometer. Uses ANSYS for part of the design verification. In Acrobat, search for occurences of "ANSYS" in the PDF file.
[permalink]
|
| |
|
Average Rating: 9.0 (48 votes)
|
|
|
| |
|
A Highly-Sensitive Fiber Bragg Grating Transverse Strain Sensor Using Micro-Structure Fibers
|
| |
Charles Jewart
|
| |
"In this thesis, we developed fiber Bragg grating sensors in specialty micro-structural fibers that can not only detect structural stress along the fiber, but also can detect stress along the transverse directions with high sensitivity. Finite element analysis (ANSYS) was used to design and study both longitudinal and transverse strain induced in microstructural fibers by external loads."
[ANSYS Structural, version 10.0]
[permalink]
|
| |
|
Average Rating: 10.0 (2 votes)
|
|
|
| |
|
A Linearly-Polarized Compact UHF PIFA with Foam Support
|
| |
Shashank D. Kulkarni, Robert M. Boisse, and Sergey N. Makarov
|
| |
"Preliminary work on the design of a low-cost linearly-polarized broadband PIFA operating in the
UHF band (440 MHz) is presented. Extensive simulations using Ansoft HFSS are performed in order to model
and optimize the antenna performance. High-density polystyrene foam is employed as a dielectric
substrate/support for all antenna prototypes. The metal sheets are made of copper foil. To minimize the antenna
dimensions, a tapered patch with slots and capacitive loading is used. The fabricated antennas have the
measured bandwidth of about 60MHz (14%) and are centered at 440 MHz. Change in antenna performance
close to the human body is briefly discussed."
Ansoft HFSS v10
[permalink]
|
| |
|
| |
|
A Mathematical Model for Fiber Reinforced Hyperelastic Material and Results with Finite Element Method
|
| |
Mustafa Resit Usal, Melek Usal, Ahmet Kabul
|
| |
"In this research, constitutive equation has been obtained that characterizes nonlinear mechanical behavior of fiber reinforced hyperelastic material, whose matrix material is isotropic."
ANSYS 5.5
[permalink]
|
| |
|
Average Rating: 9.4 (8 votes)
|
|
|
| |
|
A Microchip-Based PCR Device Using Flexible Printed Circuit Technology
|
| |
Keyue Shen, Xiaofang Chen, Min Guo, Jing Cheng,
|
| |
"Rapid heat transfer is crucial for an efficient polymerase chain reaction (PCR), and this makes temperature control one of the most
essential features in a micro-PCR system, which always includes a heater and a sensor composing a closed-loop. Yet, the fabrication of the
heater and the sensor often prevented micro-PCR systems from achieving both cost-effectiveness and fabrication-easiness. For most of the
early researches micromachining techniques were used to allow sensors and heaters be integrated on a silicon or glass chip. However, the
cost prevented them from wide applications. The work described in this paper is part of our effort to solve the cost/fabrication dilemma. An
innovative digital temperature control system was developed by introducing a heater/sensor switching procedure. Only one temperature
controlling element fabricated by flexible printed circuit technology was utilized in the constructed PCR device with minimum fabrication
steps. The glass chip-based device was made from low cost materials and assembled with adhesive bonding. Through seemingly simple
steps, we obtained both disposability and portability at the same time. Temperature stability within ±0.3 ?C and a transitional rate of 8 ?C/s
during heating/cooling was achieved. A 244 bp DNA fragment of hepatitis C virus was successfully amplified in our device by a three-stage
thermal cycling process. Further improvement was assisted by finite element analysis, and demonstrated by experiment."
[ANSYS Thermal, version 7.0]
[permalink]
|
| |
|
Average Rating: 10.0 (6 votes)
|
|
|
| |
|
A New High Resolution Thermal Detector Array
|
| |
U. Dillner, R. Riesenberg
|
| |
"The performance of the new thermal detector array arrangement is calculated using thermal finite element analysis. The influence of the thermal intra- and inter-subarray cross-talk on the resolution in dependence on some geometrical dimensions of the array is presented."
[ANSYS Thermal, version 5.7]
[permalink]
|
| |
|
Average Rating: 10.0 (3 votes)
|
|
|
| |
|
A New Type of High Bandwidth RF MEMS Switch - Toggle Switch
|
| |
Bernd Schauwecker, Karl M. Strohm, Winfried Simon, Jan Mehner, and Johann-Friedrich Luy
|
| |
"A new type of RF MEMS switch for low
voltage actuation, high broadband application and
high power capability is presented. Mechanical and
electromagnetic simulations of this new RF MEMS
switch type are shown and the fabrication process
and measurement results are given. The switching
element consists of a cantilever which is fixed by a
suspension spring to the ground of the coplanar line.
The closing voltage is 16V. The switches exhibit low
insertion loss (<0.85dB@30GHz) with good isolation
(>22dB@30GHz).
I."
[permalink]
|
| |
|
Average Rating: 10.0 (1 vote)
|
|
|
| |
|
A Non-Linear Domain Decomposition Method
|
| |
Iakov Mordukhovich Klebanov, Andrei Nikolaevich Davydov
|
| |
"A new domain decomposition technique for parallelization of physically non-linear problems in solid mechanics is developed. It is extended for any stress-strain diagrams. The approach is based on the approximating generalized models of subdomains that leads to a considerably fewer number of iterations requiring updating of substructure parameters. The analytical proof of the convergence of the theoretical iterative procedure and the demonstration of convergence of its numerical implementation with the help of ANSYS are presented."
[permalink]
|
| |
|
Average Rating: 9.4 (54 votes)
|
|
|
| |
|
A Novel Micromachined 2x128-Element Linear Themoelectric Infrared Radiation Sensor Array
|
| |
Jurgen Muller, Volker Baier, Ulrich Dillner, Rudolf Guttich, Ernst Kessler
|
| |
"As a component for infrared spectrometric analytical instruments a 2x128-element thin-film thermopile linear array sensor with a staggered pixel arrangement was constructed. Contrary to most of the known 1-dimensional and 2-dimensional thermoelectric infrared sensor arrays working all on the base of doped polysilicon, we use the material group Bi-Sb-Te to obtain highest values of thermoelectric efficiency and specific detectivity to realize an optimum of spectral wavelength resolution."
[ANSYS Thermal, version unknown]
[permalink]
|
| |
|
| |
|
A Parametric Study of Flip Chip Reliability Based on Solder Fatigue Modelling
|
| |
Scott Popelar
|
| |
"The solder fatigue model has been utilized to investigate the reliability of flip chip joints subjected to thermal cycling. In particular, a parametric study had been performed which shows how various flip chip design parameters will affect solder joint fatigue. Finite element models have been developed to analyze the effect of die size, die thickness, solder joint height, cap diameter and underfill properties on solder fatigue." (This is Part I of the study. Part II of this paper is available here.)
[permalink]
|
| |
|
Average Rating: 9.4 (27 votes)
|
|
|
| |
|
A SMA Actuated Artificial Earthworm
|
| |
A. Menciassi, S. Gorini, G. Pernorio, P. Dario
|
| |
"This paper presents the design and development of a
microrobot which aims to replicate the locomotion principle of
earthworms. The undulatory locomotion of living earthworms
has been investigated deeply from the biological point of view,
but attempts of replication of earthworm models in real size are
limited. The authors designed an artificial earthworm with four
modules which can be driven independently according to defined
undulatory patterns with a typical frequency of 0.5 Hz. Each
module is actuated by one or more SMA springs whose
configuration has been designed in order to limit the wiring
problems and optimizing working frequency. The robot is
covered by a shaped silicone material which can be used as a
platform to insert tiny legs for obtaining differential friction
conditions. Preliminary tests demonstrate that the earthworm
prototypes can move with a speed of 0.22 mm/s, thus
approximating the behavior of biological earthworms.
earthworms. Hopefully, the artificial moving earthworm will
constitute a platform for improving the knowledge of
mechanisms regulating motion and perception abilities of
these creatures."
Model in paper does not use TB,SMA constitutive model.
[permalink]
|
| |
|
Average Rating: -3.3 (3 votes)
|
|
|
| |
|
A Software Package Linking PE2D and ANSYS for SSC Magnet Design
|
| |
Nick Kallas, Chris Haddock, Jay Jayakumar, David Orrell, Greg Snitchler, Giancarlo Spigo, Jon Turner
|
| |
"The design of the Cold Mass(CM) of superconducting
magnets at the Magnet Systems Division(MSD) of the
Superconducting Super Collider Laboratory(SSCL) involves
among others the optimization of field quality and structural
performance as related to the quench behavior of the magnets.
It is desirable to be able to study the changes in field quality
due to dimensional changes of the cold mass components under
stress as the magnet is cooled and energized. This document
describes a software package of functions which enable the
computer aided study of this aspect of cold mass design."
[ANSYS Structural, version 4.4a]
[permalink]
|
| |
|
Average Rating: 5.0 (4 votes)
|
|
|
| |
|
A Stress-Induced Thermal Actuator for Optical Purpose
|
| |
Gang Liu, Sebaek Oh
|
| |
"We present a micromachined, stress-induced, thermal bimorph actuator for optical purpose. Piston motions of more than 3um are demonstrated by FEM simulation. Upon the release from the substrate, the actuators lift off the substrate due to a large built-in bending moment arising from the compressive residual stress in the poly-silicon layer and tensile residual stress in the metal layer. Large displacement and low operating voltage (<2V) are obtained simultaneously."
[permalink]
|
| |
|
Average Rating: 8.8 (17 votes)
|
|
|
| |
|
A System Level Cooling Solution for Cellular Phone Applications
|
| |
Hassan Hashemi, Abdolreza Langari
|
| |
Paper on using ANSYS for thermal analysis of MCMs.
"To characterize package thermal performance at a component level, the authors used ANSYS 5.5. A sub modeling analysis technique was employed for this analysis."
[permalink]
|
| |
|
Average Rating: 9.5 (10 votes)
|
|
|
| |
|
A Three-Dimensional Finite Element Analysis of Stress Distribution in a Coronary Atherosclerotic Plaque: In-Vivo Prediction of Plaque Rupture Location
|
| |
Jacques Ohayon, Gérard Finet, François Treyve, Gilles Rioufol and Olivier Dubreuil
|
| |
"This paper aims at predicting the plaque rupture
location of one patient with stable angina and
scheduled to undergo percutaneous coronary
intervention. The peak circumferential stress (PCS) is considered as the
determining biomechanical factor in the mechanisms leading to rupture of the
atherosclerotic plaque and is often used as a predictor of atherosclerotic plaque
rupture location. Up to now, to define the site of PCS concentrations, twodimensional
(2D) finite element (FE) analyses were performed on the smallest
luminal cross-sectional area of the coronary plaque. In-vivo three-dimensional
(3D) FE modeling of atherosclerotic coronaries may be very valuable and more
accurate than the 2D FE analysis in helping cardiologists evaluate the risk of
spontaneous plaque rupture in a patient. In this work, the performances of the
2D and 3D FE approaches have been compared and the limits of the 2D
structural analysis has been pointed out."
[ANSYS Structural, version 8.0]
[permalink]
|
| |
|
Average Rating: 10.0 (5 votes)
|
|
|
| |
|
A Vision-Based Technique for Objective Assessment of Burn Scars
|
| |
Leonid V. Tsap, Dmitry B. Goldgof, Sudeep Sarkar, and Pauline S. Powers
|
| |
"In this paper a method for the objective assessment of burn scars is proposed. The quantitative measures developed in this research provide an objective way to calculate elastic properties of burn scars relative to the surrounding areas. The approach combines range data and the mechanics and motion dynamics of human tissues. Active contours are employed to locate regions of interest and to find displacements of feature points using automatically established correspondences. Changes in strain distribution over time are evaluated. Given images at two time instances and their corresponding features, the finite element method is used to synthesize strain distributions of the underlying tissues."
[ANSYS Structural, version 5.3]
[permalink]
|
| |
|
Average Rating: 8.3 (9 votes)
|
|
|
| |
|
A_FILMAX
|
| |
Ernst Hustedt (Air New Zealand Engineering)
|
| |
Calculate maximum possible fillet radius for lines 1 and 2 and store in variable FILMAX.
[permalink]
|
| |
|
Average Rating: 9.7 (20 votes)
|
|
|
| |
|
A_HYDRO1
|
| |
Ernst Hustedt (AMES Ltd.)
|
| |
"I wrote a macro years ago to calculate distributed loads. The idea behind it is to define a profile using 3-noded shells above the surface to be loaded and calculate the height of the profile above each node of the surface. The nodal force is the height calculated for each node. In a second macro the point loads are scaled proportionally to the area associated with each node.
"I guess ANSYS has some better functionality now to do this sort of thing. I add the code for what it's worth. It did the job for me at the time."
For A_HYDRO1 (part 1 of 2), this is a macro to calculate hydrostatic loads under an arbitrary profile. The procedure involves calculating the vertical distance from each point to be loaded to a ceiling of arbitrary shape, where the ceiling is defined by triangular patches.
[permalink]
|
| |
|
Average Rating: 9.1 (51 votes)
|
|
|
| |
|
A_HYDRO2
|
| |
Ernst Hustedt (AMES Ltd.)
|
| |
"I wrote a macro years ago to calculate distributed loads. The idea behind it is to define a profile using 3-noded shells above the surface to be loaded and calculate the height of the profile above each node of the surface. The nodal force is the height calculated for each node. In a second macro the point loads are scaled proportionally to the area associated with each node.
"I guess ANSYS has some better functionality now to do this sort of thing. I add the code for what it's worth. It did the job for me at the time."
For A_HYDRO2, this is a macro to modify nodal forces calculated in A_HYDRO1.MAC proportionally to their areas.
[permalink]
|
| |
|
Average Rating: 9.4 (9 votes)
|
|
|
| |
|
A_NUM
|
| |
Mitch Voehl (CEC Corp)
|
| |
Macro to get area number by keypoint number.
[permalink]
|
| |
|
Average Rating: 7.7 (11 votes)
|
|
|
| |
|
A2COMET
|
| |
Fern Thomassy (Southwest Research Institute)
|
| |
Creates a COMET/Acoustics model from an ANSYS model.
[permalink]
|
| |
|
Average Rating: 9.5 (41 votes)
|
|
|
| |
|
A2GLUE
|
| |
Eric Miller (PADT)
|
| |
Work around for standard AGLUE that avoids the "ungluing" that can occur
[permalink]
|
| |
|
Average Rating: 8.9 (9 votes)
|
|
|
| |
|
Abstracts from papers presented at the 1998 ANSYS Conference
|
| |
(ANSYS, Inc.)
|
| |
Abstracts only.
[permalink]
|
| |
|
Average Rating: 9.0 (25 votes)
|
|
|
| |
|
ABTOANS |
| |
From 8.0 onwards, an undocumented macro ABTOANS allows user to convert an ABAQUS input file to ANSYS.
[permalink]
|
| |
|
Average Rating: 8.0 (23 votes)
|
|
|
| |
|
AC_ANGLE
|
| |
Mike Yaksh (NAC Int'l)
|
| |
Combines the real and imaginary components for a given load set to obtain the field at a specified electrical angle. This will only combine the nodal data and the SMISC element table items. For the NMISC element table items, use ac_anget.mac
[permalink]
|
| |
|
Average Rating: 7.7 (28 votes)
|
|
|
| |
|
ACAL
|
| |
(Tech Inno)
|
| |
This macro calculates the sum of areas for all selected elements.
Macro amended by S. Kukula (Dyson Ltd) with *VMASK to account for non-consecutive area numbering.
[permalink]
|
| |
|
Average Rating: 5.5 (20 votes)
|
|
|
| |
|
Accumulated Creep Strain and Energy Density Based Thermal Fatigue Life Prediction Models for SnAgCu Solder Joints
|
| |
Ahmer Syed
|
| |
"This paper describes in detail the life prediction models for
SnAgCu solder joints. The models are based on published
constitutive equations for this alloy and thermal cycle fatigue
data on actual components. The approach uses advance finite
element modeling and analysis techniques and is based on
mechanics of deformation. Both accumulated creep strain and
creep strain energy density based models are developed. The
model has been correlated with a number of data points and
predicts life within 25% in most cases. The framework of
modeling and prediction methodology described here is fully
compatible with the framework used for SnPb solder
previously."
[permalink]
|
| |
|
Average Rating: 10.0 (12 votes)
|
|
|
| |
|
ACCURATE
|
| |
Vladimir Tkach (NPO Energomash)
|
| |
"This macro evaluate Mesh Discretization Error and Criteria for Accuracy of Finite Element Solutions based on Chandresh Shah’s article (2002).
"
[permalink]
|
| |
|
Average Rating: 9.4 (8 votes)
|
|
|
| |
|
ACMN
|
| |
Eric Miller (PADT)
|
| |
Looks for and then plots and lists any areas shared by two volumes
[permalink]
|
| |
|
Average Rating: 10.0 (1 vote)
|
|
|
| |
|
ACOMPLOT
|
| |
Eric Miller (PADT)
|
| |
Finds any areas that are shared by the selected set of volumes and plots them. Useful to check VGLUEs
[permalink]
|
| |
|
Average Rating: 10.0 (9 votes)
|
|
|
| |
|
Acoustic Elements [ZIP]
|
| |
Sheldon Imaoka (ANSYS, Inc.)
|
| |
"For many years, ANSYS has 2D and 3D acoustic elements, including those used to model an
“infinite” boundary. These elements can be used in modal, harmonic, and transient analyses, and
fluid-structural interaction can also be accounted for in these simulations.
This memo hopes to review the following topics related to harmonic acoustic analyses: basic
comparison of structural and acoustic elements, modeling complex impedance boundary conditions,
and defining complex pressure loading. A set of input files, which analyze the case of a simple
radiating sphere, is included with this memo."
(Week 28, week of 01/02/05.)
[permalink]
|
| |
|
Average Rating: 9.5 (39 votes)
|
|
|
| |
|
Acoustic Postprocessing [ZIP]
|
| |
Sheldon Imaoka (ANSYS, Inc.)
|
| |
"Acoustic analyses in ANSYS provides insight to the propagation of sound, and both
visual and aural postprocessing can aid in this objective. This memo hopes to cover
postprocessing methods for acoustic problems other than standard contour and XY plots."
(Week 42, week of 11/18/07)
[permalink]
|
| |
|
Average Rating: 10.0 (9 votes)
|
|
|
| |
|
Advanced Analysis Of Structural Reliability Using Commercial FE-Codes
|
| |
Christian Bucher, Dagmar Hintze, and Dirk Roos
|
| |
"The paper focuses on two main issues, i.e. (a) The application of existing code for probabilistic analysis together with existing Finite Element Code for advanced Monte Carlo analysis (b) Presentation of a local-global approximation strategy for the response surface method. This so-called "weighted radii" approximation appears to provide the flexibility and accuracy needed for the reliability analysis of complex structures." (Probabilistics)
[permalink]
|
| |
|
Average Rating: 10.0 (6 votes)
|
|
|
| |
|
Advanced Mask Modeling Accuracy and Stability Study-University of Wisconsin Mask Modeling
|
| |
R. Scott Mackay
|
| |
"As lithography error budgets on pattern placement become more stringent for sub-130 nm technology, it is imperative that all mask-related distortions be quantified, controlled, and minimized. It will be essential to identify the influence of thin film stress on pattern placement errors. In this research, the effect of mask material properties, manufacturing, and usage on image placement will be evaluated. Finite element (FE) models have been developed to simulate this pattern transfer process, using equivalent modeling techniques. Analytical, experimental, and FE procedures have been combined to accurately determine these effects on final pattern distortions."
[permalink]
|
| |
|
Average Rating: 10.0 (3 votes)
|
|
|
| |
|
Advanced Tools for Design and Analyses of High Temperature Cyclic Loaded Turbine Components
|
| |
U. Gampe, I. Martynov, J. Keyser
|
| |
"The paper presents a new concept to predict viscoplastic deformations in components under thermal mechanical loading. This approach is based both on material data from uniaxial creep tests and additional laboratory component tests to consider the influence of multiaxiality. This concept was used for analysis of feature tests of flat tensile specimens with central hole. The maximum test temperature was 600 °C and the surface of the hole was attacked by cyclic thermal shocks." (This paper refers to use of ANSYS User-Defined Materials. A related paper is Laboratory Component Testing for Investigation of Material Degradation from Creep-Fatigue Interaction.)
[permalink]
|
| |
|
Average Rating: 9.1 (28 votes)
|
|
|
| |
|
Advancing Analysis Capabilities In ANSYS Through Solver Technology
|
| |
Gene Poole, Yong-Cheng Liu, and Jan Mandel
|
| |
"This paper will describe implementation considerations for the addition of new solver technology to a large legacy code, compare resource requirements for the various solver choices and present some comparative results from several customer generated problems. The AMG solver benefits, both in improved robustness and parallel processing efficiency will be described. The paper will also discuss some of the implementation challenges that have been overcome to add new solver technology to a large existing code. The role of solver technology in meeting current and future demands of large scale commercial analysis codes will be discussed."
[permalink]
|
| |
|
Average Rating: 10.0 (8 votes)
|
|
|
| |
|
Advancing Front Surface Mesh Generation in Parametric Space Using a Riemannian Surface Definition
|
| |
Joseph Tristano, Steven Owen, and Scott Canann
|
| |
[Click here for PDF file]
This is the new Riemann triangular mesher added in ANSYS 5.5
"A method is presented for meshing 3D CAD surfaces in parametric space using an advancing front approach and a metric map to govern the size and shape of the triangles in the parametric space."
[permalink]
|
| |
|
Average Rating: 8.5 (24 votes)
|
|
|
| |
|
AEXT
|
| |
Juha Tyllinen (KONE Corporation)
|
| |
This macro creates an area by 'extruding' line - Similar to ANSYS command VEXT.
[permalink]
|
| |
|
Average Rating: 10.0 (7 votes)
|
|
|
| |
|
AFACE
|
| |
John Crawford (Honeywell)
|
| |
Used to generate areas from selected shell elements. Useful to create volume from imported FE mesh.
[permalink]
|
| |
|
Average Rating: 10.0 (21 votes)
|
|
|
| |
|
Algebraic Multigrid By Smoothed Aggregation For Second And Fourth Order Elliptic Problems
|
| |
Petr Van Ek, Jan Mandel, and Marian Brezina
|
| |
"An algebraic multigrid algorithm for symmetric, positive definite linear systems is developed based on the concept of prolongation by smoothed aggregation. Coarse levels are generated automatically. We present a set of requirements motivated heuristically by a convergence theory. The algorithm then attempts to satisfy the requirements. Input to the method are the coefficient matrix and zero energy modes, which are determined from nodal coordinates and knowledge of the differential equation. Efficiency of the resulting algorithm is demonstrated by computational results on real world problems from solid elasticity, plate bending, and shells."
[permalink]
|
| |
|
Average Rating: 8.3 (3 votes)
|
|
|
| |
|
ALLP |
| |
ALLP,num_loop
Creates areas with holes in them. It supports up to 4 internal loops and one external loop. Listing of lines can be random within each loop, but each loop must be grouped together. "allp,3,1,3,4,7,11,14,6,8,9" where 3=number of total loops (one external, two internal, and the other numbers are line numbers in random order. This means that loop one would be lines 1,3,4, loop two would be 4,7,11, and loop 3 would be 14,16,8,9.
[permalink]
|
| |
|
Average Rating: 10.0 (2 votes)
|
|
|
| |
|
ALOOP
|
| |
Stefano Lucarelli (Mannesmann VDO AG)
|
| |
This input file asks for selection of one or more areas and loops until all areas directly or indirectly connected to the original ones are selected then plots them
[permalink]
|
| |
|
Average Rating: 10.0 (7 votes)
|
|
|
| |
|
ALSM
|
| |
John Crawford (Honeywell)
|
| |
I ended up writing a macro that selects/reselects/unselects meshed areas, and then copied it and modified it for doing the same with volumes.
[permalink]
|
| |
|
Average Rating: 10.0 (6 votes)
|
|
|
| |
|
AMER |
| |
AMER,area1,area2,etc.
"Glues" areas together. Same command as AGLUE. See AGLUE for details on the usage of this command.
[permalink]
|
| |
|
| |
|
An Approach to Combined Laplacian and Optimization-Based Smoothing for Triangular, Quadrilateral, and Quad-Dominant Meshes [PDF]
|
| |
Scott A. Canann, Joseph R. Tristano, Matthew L. Staten
|
| |
"In this paper, an overall mesh smoothing scheme is presented for meshes consisting of triangular, quadrilateral, or mixed triangular and quadrilateral elements. This paper describes an efficient and robust combination of constrained Laplacian smoothing together with an optimization-based smoothing algorithm."
[permalink]
|
| |
|
Average Rating: 10.0 (16 votes)
|
|
|
| |
|
An Architecture for Fluid/Structure Analysis of Turbomachinery Blading
|
| |
David A. Johnston, Charles J. Cross, J. Mitch Wolff
|
| |
"Aeroelastic stability and response analyses used in the design of turbomachinery
blading are typically uncoupled: the unsteady aerodynamics and structural dynamics are
treated in separate models, with boundary conditions sequentially updated after stationary
periodic convergence is met. Higher fidelity simulations are achieved by coupling the
fluid and structure domains such that boundary conditions are updated once or several
times per physical time step of the simulation."
"As a starting point, the turbomachinery CFD research code
TURBO (Chen and Briley, 2001) and the commercial structural solver ANSYS® has been
chosen for coupling, although FSI is designed with modularity for future inclusion of
other fluid and structural solvers."
[ANSYS Dynamics, version unspecified]
[permalink]
|
| |
|
Average Rating: 10.0 (3 votes)
|
|
|
| |
|
An Efficient FETI Implementation on Distributed Shared Memory Machines with Independent Numbers of Subdomains and Processors
|
| |
Michel Lesoinne and Kendall Pierson
|
| |
"Until now, many implementations of the FETI method have been designed either as sequential codes on a single CPU, or as parallel implementations with a One Subdomain per Processor approach. This approach has been particularly typical of implementations on distributed memory architectures such as the IBM SP2. In the last couple of years, several computer manufacturers have introduced new machines with a Distributed Shared Memory (DSM) programming model {e.g. SGI Origin 2000, or HP Exemplar. In such architectures, the physical memory is distributed among the processors or CPU boards but any memory location can be accessed logically by any CPU independently of where the particular memory page being accessed has physically been allocated. As more and more machines of this type are available with a relatively small number of processors, the interest in implementing FETI with an independent number of subdomains and processor has increased. We report on such an implementation of FETI and highlight the benefits of this feature. We have found that medium size to large problems can be solved even on a sequential machine with time and memory requirements that are one to two order of magnitude better than a direct solver."
[permalink]
|
| |
|
Average Rating: 10.0 (2 votes)
|
|
|
| |
|
An Interpretation of the Physics of Fluid-Structure Interaction in the Frequency Domain
|
| |
Jan Christian Anker
|
| |
"This paper constitutes an attempt to interpret the physics of FSI where the structure is vibrating. The structure considered is a very simple physical device, namely a flat cantilever plate. Many presumably important details are only briefly mentioned, other are left completely out of the discussion. The intention with the paper is to emphasize that there are cases where Fluid - Structure Interaction can be successfully simulated without having to utilize a Navier-Stokes Solver coupled with a (non-linear) Structural Analysis Program, a concept that requires vast amounts of computer time for linear vibrations (but is highly relevant for other applications)."
[ANSYS Dynamics, version unspecified]
[permalink]
|
| |
|
Average Rating: 10.0 (3 votes)
|
|
|
| |
|
An Introduction to the Conjugate Gradient Method Without the Agonizing Pain
|
| |
Jonathan R. Shewchuk
|
| |
This paper presents a very well-written explanation of conjugate gradient methods. It is helpful in understanding better the idea behind CG solvers in ANSYS (PCG, JCG, ICCG, AMG, etc.).
[permalink]
|
| |
|
Average Rating: 10.0 (5 votes)
|
|
|
| |
|
An Investigation into Vibration in Switched Reluctance Motors
|
| |
Pragasen Pillay and William (Wei) Cai
|
| |
"Two disadvantages of the switched reluctance motor
(SRM) are its torque ripple and acoustic noise. Previous work on
vibration modes and resonant frequencies of the laminations of
an 8-6 SRM is extended here to include the effects of the frame.
Both a smooth frame and a ribbed frame are examined, and the
presence of numerous additional vibratory modes in the ribbed
frame demonstrated. Accelerometer tests behind a pole verify
some of the theoretical predictions."
[ANSYS Dynamics, version unspecified]
[permalink]
|
| |
|
Average Rating: 10.0 (1 vote)
|
|
|
| |
|
An Object Oriented Approach to Geometry Defeaturing for Finite Element Meshing [PDF]
|
| |
Anton V. Mobley, Michael P. Carroll, and Scott A. Canann
|
| |
"In this paper, an object-oriented approach to automatic geometry defeaturing is presented. The geometric and finite element data abstractions are given, along with the basic algorithms used."
[permalink]
|
| |
|
Average Rating: 10.0 (6 votes)
|
|
|
| |
|
Analysis and Modeling of Fiber-Wrapped Columns and Concrete-Filled Tubes
|
| |
Mohsen Shahawy, Tom Beitelman, and Amir Mirmiran
|
| |
"Carbon-wrapping of concrete column adds to its strength and ductility. The behavior of carbon-wrapped concrete is in general very similar to that of glass-wrapped concrete. The bilinear confinement that was developed- for glass-wrapped concrete can be applied to carbon-wrapped concrete. However, a better fit can be obtained by re-calibrating the model for an entire database that consists of both carbon-wrapped and glass-wrapped concrete. Such database needs to be accompanied by a set of accurate coupon tests on the properties of the jacket. The finite element modeling is also useful in predicting the response of carbon-wrapped concrete. A more accurate estimate of jacket properties make the analysis fit the test results better."
[permalink]
|
| |
|
Average Rating: 7.7 (37 votes)
|
|
|
| |
|
Analysis and Simulation of the Ultrasonic/Sonic Driller/Corer(USDC)
|
| |
X. Bao, Z. Chang, S. Sherrit, B.P. Dolgin, Y. Bar-Cohen, D.S. Pal, S. Du, T. Peterson
|
| |
"An ultrasonic/sonic driller/corer (USDC) was developed to address the challenges to the NASA objective of planetary in-situ
rock sampling and analysis. The USDC uses a novel drive mechanism, transferring ultrasonic vibration into impacts on a
drill stem at sonic frequency using a free-flying mass block (free-mass). The main parts of the device and the interactions
between them were analyzed and numerically modeled to understand the drive mechanism and allow design of effective
drilling mechanism. A computer program was developed to simulate the operation of the USDC and successfully predicted
the characteristic behavior of the new device. This paper covers the theory, the analytical models and the algorithms that were
developed and the predicted results."
[ANSYS Piezoelectric, version 5.4]
[permalink]
|
| |
|
Average Rating: 10.0 (4 votes)
|
|
|
| |
|
Analysis and Testing of Graphite/Epoxy Concrete Bridge Girders Under Static Loading
|
| |
B. M. Kavlicoglu, F. Gordaninejad, M. Saiidi, Y. Jiang
|
| |
"An innovative graphite/epoxy-concrete (G/E-C) cross-section was developed and tested under two-point
static loading. Finite element analysis and theoretical modeling of the cross-section was performed. The
cross-section was a box girder with an outer G/E U-beam and inner G/E box beam with concrete webs
and flange in between. Shear connection between G/E box beam and concrete slab was provided by a
two-part structural epoxy resin. Additional shear connection was provided by steel stirrups located at
254 mm (10 in.) spacing along longitudinal axis of the test specimen. It was observed that, steel stirrups
contributed the load carrying capacity after initiation of slippage between G/E beams and concrete.
Moreover, a series of bond strength tests were performed to examine the behavior of structural epoxy
resin for connection between G/E and concrete. Six G/E strips were subjected to tensile tests to evaluate
the longitudinal and transverse elastic moduli of the laminate. Using the proper material properties and
assumptions, it was possible to demonstrate the behavior of the section under static loads theoretically
and in finite element analysis."
[ANSYS Structural, version 5.5]
[permalink]
|
| |
|
Average Rating: 8.1 (16 votes)
|
|
|
| |
|
Analysis Of Gasketed Flanges With Ordinary Elements Using APDL Control
|
| |
Yasumasa Shoji, Satoshi Nagata
|
| |
"The analysis of gasketted flanges is now becoming an essential technique to design pressure vessels or piping, because the design code is being modified. On the other hand, the gasket has an extreme nonlinearity which causes the analysis to be very difficult, especially using linear material properties. A finite element analysis program other than ANSYS has the element library for gasket element, but ANSYS does not have it yet.""The authors developed a method to model this nonlinear gasket by using the elements available in ANSYS Rel. 5.5 for 2-dimensional axisymmetric analysis and those in Rel. 5.6 for 3-dimensional analysis. In this paper, the concept and the procedure of the modeling is introduced. The data input is possible using a template, without using any other ANSYS commands. The whole analysis execution is controlled by APDL."[STI: Gasket elements are available from version 6.1 onwards, after this paper was written]
[permalink]
|
| |
|
Average Rating: 7.9 (29 votes)
|
|
|
| |
|
Analysis Of Reinforced Concrete Structures Using ANSYS Nonlinear Concrete Model
|
| |
Antonio F. Barbosa and Gabriel O. Ribeiro
|
| |
"This paper considers the practical application of nonlinear models in the analysis of reinforced concrete structures. The results of some analyses performed using the reinforced concrete model of the general purpose finite element code ANSYS are presented and discussed."
[permalink]
|
| |
|
Average Rating: 9.1 (179 votes)
|
|
|
| |
|
Analysis Of The FOREVER-Experiments Using A Finite Element Model
|
| |
Eberhard Altstadt, Thomas Moessner, Baj Ral Sehgal, Hans-Georg Willschütz
|
| |
"An axis-symmetric Finite Element (FE) model is developed based on the multi-purpose code ANSYS/Multiphysics. Using the Computational Fluid Dynamics (CFD) module the temperature field within the melt pool and within the vessel wall is evaluated. The transient structural mechanical calculations are then performed applying a creep model which takes into account large temperature, stress and strain variations." (Document 1)
[permalink]
|
| |
|
Average Rating: 7.5 (10 votes)
|
|
|
| |
|
Analytical Modeling Of Glued Laminated Girder Bridges Using ANSYS
|
| |
Anil Kurian
|
| |
"This paper aims at developing a finite element model of glued laminated girder bridges that can predict accurately the analytical behavior of the bridges. Two models have been developed to study the characteristics of this type of bridge. Two case studies have been considered to validate the accuracy of the models. The first case study is a long span single-lane bridge, the Tuscaloosa Bridge, in Alabama. The second case study is a medium span two-lane bridge, the Cow Gu lch Bridge, in Montana. The models show good correlation with the experimental data and hence, the models can be used to find the maximum deflections in the bridge."
Use of ANSYS 5.0 (1992 version)
[permalink]
|
| |
|
Average Rating: 8.8 (25 votes)
|
|
|
| |
|
Analytical Simulation of a 1D Single Crystal Silicon Electrostatic Micromirror [PDF]
|
| |
H. Camon, F. Larnaudie, F. Rivoirard, B. Jammes
|
| |
A torsional micromirror. Use of ANSYS to extract lumped parameters for use in SABER model. (MEMS)
[permalink]
|
| |
|
Average Rating: 8.6 (11 votes)
|
|
|
| |
|
Analyzing Hyperelastic Materials w/ Some Practical Considerations
|
| |
Paris Altidis and Vince Adams
|
| |
Presentation from the Midwest ANSYS User Group
[ANSYS Nonlinear, version unspecified]
[permalink]
|
| |
|
Average Rating: 10.0 (8 votes)
|
|
|
| |
|
Analyzing Microminiature Devices [PDF]
|
| |
Steve Groothuis
|
| |
(from ANSYS Solutions magazine, volume 1, #1) (MEMS)
[permalink]
|
| |
|
Average Rating: 10.0 (7 votes)
|
|
|
| |
|
ANF File Format
|
| |
The ANF File format is used by CADfix and the Connection Kit products to define ANSYS geometry, especially in the context of translating CAD geometries into ANSYS. This document covers the commands used in the ANF files.
[permalink]
|
| |
|
Average Rating: 7.5 (2 votes)
|
|
|
| |
|
ANFOUT
|
| |
John Swanson (SAS, Inc./ANSYS, Inc.)
|
| |
Macro that traverses the solid model and writes an anf file.
Posted by Eric Miller (PADT)
[permalink]
|
| |
|
Average Rating: 8.9 (14 votes)
|
|
|
| |
|
ANFOUT2
|
| |
John Swanson (SAS, Inc./ANSYS, Inc.), slightly modified by John Crawford (Honeywell)
|
| |
Macro that traverses the solid model and writes an anf file. Modified by John Crawford to include not just highest level component (i.e., write both volumes and 'free' areas which are selected).
[permalink]
|
| |
|
Average Rating: 10.0 (4 votes)
|
|
|
| |
|
ANGLEMOD
|
| |
John Crawford (Honeywell)
|
| |
From ANSYS Solutions article "Big Insights from Small Macros", Vol. 2 No. 1 pg. 27. Generates a cantilever beam to determine required elements per fillet for modeling studies
[permalink]
|
| |
|
Average Rating: 10.0 (11 votes)
|
|
|
| |
|
ANHARM
|
| |
Bill Bulat (CSI)
|
| |
Animates pressure results of harmonic analysis in /POST1 by contouring the real part of the solution while varying the phase angle. (While 5.6 has the feature, I like the way Bill has implemented this -- take a look: it's a bit more efficient than the 5.6 macro - STI)
[permalink]
|
| |
|
Average Rating: 9.8 (32 votes)
|
|
|
| |
|
Anisotropic Plasticity and Failure Prediction in Wood Composites
|
| |
David M. Moses, Helmut G.L. Prion
|
| |
"Two case studies are summarized using anisotropic plasticity and the Weibull weakest link failure model to predict the behavior of wood and wood composites. The linear elastic orthotropic model normally used for wood is shown to be insufficient for the prediction of ultimate strength in wood. Non-linear, non-recoverable behavior in compression in each of the orthogonal material directions is of particular interest in cases where localized crushing governs the load-displacement behavior of wood.""The anisotropic plasticity option in ANSYS was used to predict yielding and post-yield behavior for the wood composite used in this study because yield stresses in orthogonal directions were found to be in the ratio of 1:1.2:5. A user-programmable Fortran subroutine was developed for ANSYS to carry out the failure analysis (and to calculate the volume integration of the stresses) at each load-step in post-processing. The model was verified using two cases: I) the ASTM D143 shear block test, and II) bolted connections."
[permalink]
|
| |
|
Average Rating: 9.2 (33 votes)
|
|
|
| |
|
ANOL
|
| |
Bram Weisman (SBM-IMODCO)
|
| |
"I wrote some macros to simplify common annotation tasks. They let me place annotation on the screen n lines above the title. This eliminates picking and placement guesswork. Below is the one that places annotation on the
left side. Initially, I only had one argument for the actual text (arg3). Then I realized that the /tlab command allows up to 60 characters, but
currently only 32 get passed through as arguments to macros. So I added a second one (arg4).
"Generally for ANOL, I won't use the second argument (the character offset). If you use a
zero for ARG1, your text will precisely overlay the /title and I believe this is independent of screen resolution, but might be dependent on certain other text settings.
"To get a feel for this, try issuing the following:
ANOL,4,,'This is four lines above title',''
ANOL,3,,'This is three lines above title',''
ANOL,2,,'This is two lines above title',''
ANOL,1,,'This is one lines above title',''
"Also try the following:
/title,This is the title
ANOL,0,,'This is the title',''
The two are perfectly overlaid on my system."
[permalink]
|
| |
|
Average Rating: 10.0 (13 votes)
|
|
|
| |
|
ANS2ABA
|
| |
Dave Lindeman (3M)
|
| |
This macro (actually, an input file of an ABAQUS verification problem) provides an example of using ANSYS to preprocess and write out an ABAQUS input deck. From the author: "Note that this is an APDL script that illustrates a translation procedure and NOT an independent macro (i.e., this is just a starting place for others -- customization IS required)."
[permalink]
|
| |
|
Average Rating: 9.8 (112 votes)
|
|
|
| |
|
ANS2PAT
|
| |
Gordon May (Rolls Royce Compressor Key System)
|
| |
ANSYS to Patran 2 Neutral File translator: this macro translates element and nodal data FOR THE CURRENTLY SELECTED SET OF ELEMENTS into Patran 2 Neutral File (PNF) format.
[permalink]
|
| |
|
Average Rating: 9.8 (21 votes)
|
|
|
| |
|
ANS2UNV
|
| |
Rogelio Perez (Schneider Electric Industries SAS)
|
| |
This macro creates an I-deas universal file (.unv) from ANSYS for SOLID45, SOLID92, and SOLID95. Based on ANS2PAT macro.
[permalink]
|
| |
|
Average Rating: 10.0 (4 votes)
|
|
|
| |
|
AnsBGA Utilities
|
| |
(AnsBGA)
|
| |
AnsBGA Utilities include the following:
- AnsKBD - Hot Keys
AnsKBD allows you to assign any key combinations, such as <F7>, <Control-n>, <Alt-F1>, <Control-Shift-t> etc. to your macros.
- Realtime macEdit + Tail Utility.
Yes it works on windows and all other platforms
Just press <Alt-t> when the Ansys GUI is active to launch tail + real time macro editor.
- AnsBGA enhanced ASK (1 Liner Multipro)
This is a neat replacements for multipro and *ask commands. You can build multi prompts having 1 to 20+ inputs in just one line of code. This one command effectively replaces *ask and multipro commands. For example this one liner creates a prompt for three inputs.
~eui,'_ask "Your message here" "parm1=2, parm2=string, parm3" '
where parm1, parm2, parm3 are three parameters having 2, 'string' and nothing as the default values.
- GUI Configuration
Just press the "Config Utility" button below for more information.
Press <Control-Alt-S> to bring up this window.
Alternative download here.
[permalink]
|
| |
|
Average Rating: 6.6 (22 votes)
|
|
|
| |
|
AnsKeys HotKeys
|
| |
Carlos Shultz (PADT)
|
| |
"AnsKeys HotKeys is a Visual Basic program which will provide HotKeys for commonly issued commands and hide/unhide the ANSYS Process Status dialog box."
This is very useful to map Function keys (and Shift-Function or Ctrl-Function) for commonly-used commands. Hiding the Process Status is also available.
Although it is recommended to download the latest version from PADT's website above, there is an alternative download here.
To use this, after installation, launch AnsKeys. You can minimize the window, but the application must be running for your F1-F12 keys to work. Also, it will pop up the old-style Input Window if you are using the new (default) GUI.
[permalink]
|
| |
|
| |
|
ANSYS 25th Anniversary
|
| |
(ANSYS, Inc.)
|
| |
25th anniversary publication of ANSYS, Inc.
[permalink]
|
| |
|
| |
|
ANSYS Advantage 2007 Issue 1
|
| |
(ANSYS, Inc.)
|
| |
ANSYS Advantage, Issue 1 of 2007.
Spotlight Supplement on Sports and Leisure Industry.
[permalink]
|
| |
|
| |
|
ANSYS Advantage 2007 Issue 2 |
| |
(ANSYS, Inc.)
|
| |
ANSYS Advantage, Issue 2 of 2007.
Spotlight Supplement on Biomedical Industry.
[permalink]
|
| |
|
| |
|
ANSYS Advantage 2007 Issue 3
|
| |
(ANSYS, Inc.)
|
| |
ANSYS Advantage, Issue 3 of 2007.
Spotlight Supplement on Environmental Design.
[permalink]
|
| |
|
| |
|
ANSYS Advantage 2007 Issue 4
|
| |
(ANSYS, Inc.)
|
| |
ANSYS Advantage, Issue 4 of 2007.
Spotlight Supplement on Materials Industry.
[permalink]
|
| |
|
| |
|
ANSYS Advantage 2008 Issue 1
|
| |
(ANSYS, Inc.)
|
| |
ANSYS Advantage, Issue 1 of 2008.
Spotlight Supplement on Engineering Simulation for Rotating Machinery
[permalink]
|
| |
|
| |
|
ANSYS Advantage 2008 Issue 2
|
| |
(ANSYS, Inc.)
|
| |
ANSYS Advantage, Issue 2 of 2008.
Spotlight Supplement on Products and Technology.
[permalink]
|
| |
|
| |
|
ANSYS Advantage 2008 Issue 3
|
| |
(ANSYS, Inc.)
|
| |
ANSYS Advantage, Issue 3 of 2008.
Spotlight Supplement on Engineering Simulation for the Energy Industries.
[permalink]
|
| |
|
Average Rating: 10.0 (1 vote)
|
|
|
| |
|
ANSYS Advantage 2008 Issue 4
|
| |
(ANSYS, Inc.)
|
| |
ANSYS Advantage, Issue 4 of 2008.
Spotlight Supplement on Ansoft.
[permalink]
|
| |
|
| |
|
ANSYS Advantage 2009 Issue 1
|
| |
(ANSYS, Inc.)
|
| |
ANSYS Advantage, Issue 1 of 2009.
Spotlight Supplement on ANSYS 12.0.
[permalink]
|
| |
|
| |
|
ANSYS and Tcl/Tk customization
|
| |
John Swanson
|
| |
Information on using Tcl/Tk with ANSYS to create customized GUI. Tcl/Tk is used in ANSYS, such as the Contact Wizard, Solution Control Wizard, or Materials GUI at 5.7/6.0.
[permalink]
|
| |
|
Average Rating: 10.0 (27 votes)
|
|
|
| |
|
ANSYS and UIDL customization
|
| |
John Swanson
|
| |
UIDL is the ANSYS language used to define the dialog boxes and Main Menu. This information is related to learning more about UIDL to create custom dialog boxes. An alternative is to use Tcl/Tk.
[permalink]
|
| |
|
Average Rating: 9.5 (11 votes)
|
|
|
| |
|
ANSYS Cast Iron Material Model Matches Experimental Data
|
| |
(ANSYS, Inc.)
|
| |
"[The purpose of this paper is to] verify the accuracy of the ANSYS cast iron material model. Results from ANSYS are compared with experimental data for a biaxially loaded cruciform geometry."
[permalink]
|
| |
|
Average Rating: 9.5 (11 votes)
|
|
|
| |
|
ANSYS Distributed Solver Setup Tutorial
|
| |
(ANSYS, Inc.)
|
| |
This is a document for ANSYS 8.1 distributed solvers and how to set them up, specifically for Windows and Linux.
[permalink]
|
| |
|
Average Rating: 8.8 (58 votes)
|
|
|
| |
|
ANSYS Equation Solvers: Usage and Guidelines
|
| |
Gene Poole (ANSYS, Inc.)
|
| |
Discussion of ANSYS solvers, focusing on the sparse direct solver and PCG iterative solver.
Originally presented at the 2002 Conference.
[permalink]
|
| |
|
Average Rating: 10.0 (7 votes)
|
|
|
| |
|
ANSYS File Unit Numbers
|
| |
(ANSYS, Inc.)
|
| |
In some cases, ANSYS error messages may reference a file unit number when a file cannot be read/written. Knowing what file unit numbers correspond to which files can be helpful in determining the problem.
[permalink]
|
| |
|
Average Rating: 9.4 (9 votes)
|
|
|
| |
|
ANSYS Function Boundary Conditions
|
| |
Achuth Rao (ANSYS, Inc.)
|
| |
When using the ANSYS Function Editor and Function Loader to define Function Boundary Conditions, a special type of table is used.
This document outlines the syntax of the function loading table.
[permalink]
|
| |
|
Average Rating: 9.8 (23 votes)
|
|
|
| |
|
ANSYS Material Modeling: Hyperelastic Material Characterization
|
| |
(ANSYS, Inc.)
|
| |
Overview of the hyperelastic curve-fitting capabilities introduced in ANSYS 7.0.
[permalink]
|
| |
|
Average Rating: 10.0 (9 votes)
|
|
|
| |
|
ANSYS Mechanical - A Powerful Nonlinear Simulation Tool
|
| |
Grama Bhashyam (ANSYS, Inc.)
|
| |
A whitepaper describing various ANSYS features in the area of nonlinear mechanics, including element formulation, constitutive models, and contact technology.
[permalink]
|
| |
|
Average Rating: 9.6 (14 votes)
|
|
|
| |
|
ANSYS Multiphysics Capabilities for MEMS Modeling and Simulation - Part 1 of 3
|
| |
Jan Mehner, Juergen Wibbeler
|
| |
Part 1 of 3: Analyzing electrostatic-structural interactions in Micro Electro Mechanical Systems
ANSYS Solutions Vol. 3, Number 2
[permalink]
|
| |
|
Average Rating: 10.0 (5 votes)
|
|
|
| |
|
ANSYS Multiphysics Capabilities for MEMS Modeling and Simulation - Part 2 of 3
|
| |
Jan Mehner, Juergen Wibbeler
|
| |
Part 2 of 3: Analyzing fluid-structural interactions
ANSYS Solutions Vol. 3, Number 3
[permalink]
|
| |
|
Average Rating: 10.0 (4 votes)
|
|
|
| |
|
ANSYS Multiphysics Capabilities for MEMS Modeling and Simulation - Part 3 of 3
|
| |
Jan Mehner, Juergen Wibbeler, Fouad Bennini
|
| |
Part 3 of 3: Exporting macromodels for circuit and
system simulation tools.
ANSYS Solutions Vol. 3, Number 4
[permalink]
|
| |
|
Average Rating: 10.0 (3 votes)
|
|
|
| |
|
ANSYS News 1995 Issue 3
|
| |
(ANSYS, Inc.)
|
| |
ANSYS News publication (1995). This was the precursor to "Analysis Solutions" and, later, "ANSYS Solutions" magazines.
[permalink]
|
| |
|
| |
|
ANSYS News 1995 Issue 4
|
| |
(ANSYS, Inc.)
|
| |
ANSYS News publication (1995). This was the precursor to "Analysis Solutions" and, later, "ANSYS Solutions" magazines.
[permalink]
|
| |
|
| |
|
ANSYS News 1996 Issue 1
|
| |
(ANSYS, Inc.)
|
| |
ANSYS News publication (1996). This was the precursor to "Analysis Solutions" and, later, "ANSYS Solutions" magazines.
[permalink]
|
| |
|
| |
|
ANSYS News 1996 Issue 2
|
| |
(ANSYS, Inc.)
|
| |
ANSYS News publication (1996). This was the precursor to "Analysis Solutions" and, later, "ANSYS Solutions" magazines.
[permalink]
|
| |
|
| |
|
ANSYS News 1996 Issue 3
|
| |
(ANSYS, Inc.)
|
| |
ANSYS News publication (1996). This was the precursor to "Analysis Solutions" and, later, "ANSYS Solutions" magazines.
[permalink]
|
| |
|
| |
|
ANSYS PDS article in Machine Design [PDF]
|
| |
Stefan Reh
|
| |
While this may not be a conventional technical paper, it presents information on ANSYS PDS (Probabilistic Design System), a beta feature in 5.6 and officially released in 5.7. Instead of a deterministic approach, a stochastic method provides better product reliability measures.
[permalink]
|
| |
|
Average Rating: 3.3 (6 votes)
|
|
|
| |
|
ANSYS PDS overview [PDF]
|
| |
Stefan Reh
|
| |
A three-page overview/summary sent on the XANSYS Mailing list on PDS, beta in ANSYS 5.6, officially released at 5.7.
[permalink]
|
| |
|
Average Rating: 7.5 (4 votes)
|
|
|
| |
|
ANSYS Seems to Freeze on Windows
|
| |
Sheldon Imaoka (ANSYS, Inc.)
|
| |
Description of a possible reason of why your ANSYS session may seem to 'hang' on Windows and how to avoid it.
[permalink]
|
| |
|
Average Rating: 10.0 (2 votes)
|
|
|
| |
|
ANSYS Short Course
|
| |
Tim Langlais (University of Minnesota)
|
| |
A short course on ANSYS, using ANSYS 5.4.
[permalink]
|
| |
|
Average Rating: 10.0 (2 votes)
|
|
|
| |
|
ANSYS Solutions 2002 Winter
|
| |
(ANSYS, Inc.)
|
| |
ANSYS Solutions 2002 Issue 1. Industry Spotlight: Aerospace Industry Nonlinear Analysis
[permalink]
|
| |
|
Average Rating: -10.0 (1 vote)
|
|
|
| |
|
ANSYS Solutions 2003 Fall
|
| |
(ANSYS, Inc.)
|
| |
ANSYS Solutions 2003 Issue 2. Industry Spotlight: Industrial Equipment
[permalink]
|
| |
|
| |
|
ANSYS Solutions 2003 Spring
|
| |
(ANSYS, Inc.)
|
| |
ANSYS Solutions 2003 Issue 1. Industry Spotlight: Biomedical
[permalink]
|
| |
|
| |
|
ANSYS Solutions 2003 Summer
|
| |
(ANSYS, Inc.)
|
| |
ANSYS Solutions 2003 Issue 3. Industry Spotlight: Government and Defense
[permalink]
|
| |
|
| |
|
ANSYS Solutions 2004 Fall
|
| |
(ANSYS, Inc.)
|
| |
ANSYS Solutions 2004 Issue 3. Industry Spotlight: Power Generation
[permalink]
|
| |
|
| |
|
ANSYS Solutions 2004 Spring
|
| |
(ANSYS, Inc.)
|
| |
ANSYS Solutions 2004 Issue 1. Industry Spotlight: Consumer Products
[permalink]
|
| |
|
| |
|
ANSYS Solutions 2004 Summer
|
| |
(ANSYS, Inc.)
|
| |
ANSYS Solutions 2004 Issue 2. Industry Spotlight: Chemical and Processing
[permalink]
|
| |
|
| |
|
ANSYS Solutions 2005 Fall
|
| |
(ANSYS, Inc.)
|
| |
ANSYS Solutions 2005 Issue 4. Industry Spotlight: Automotive
[permalink]
|
| |
|
| |
|
ANSYS Solutions 2005 Spring
|
| |
(ANSYS, Inc.)
|
| |
ANSYS Solutions 2005 Issue 2. Industry Spotlight: Biomedical Technology
[permalink]
|
| |
|
Average Rating: 10.0 (1 vote)
|
|
|
| |
|
ANSYS Solutions 2005 Summer
|
| |
(ANSYS, Inc.)
|
| |
ANSYS Solutions 2005 Issue 3. Industry Spotlight: Microsystems and Nanotechnology
[permalink]
|
| |
|
| |
|
ANSYS Solutions 2005 Winter
|
| |
(ANSYS, Inc.)
|
| |
ANSYS Solutions 2005 Issue 1. Industry Spotlight: Global Product Development
You can also download John Crawford's RUNCONTACT macro, referenced in his article on page 33.
[permalink]
|
| |
|
| |
|
ANSYS Solutions 2006 Issue 1
|
| |
(ANSYS, Inc.)
|
| |
ANSYS Solutions 2006 Issue 1. Industry Spotlight: Semiconductor Technology
[permalink]
|
| |
|
| |
|
ANSYS Solutions 2006 Issue 2
|
| |
(ANSYS, Inc.)
|
| |
ANSYS Solutions 2006 Issue 2. Industry Spotlight: Aerospace Systems
[permalink]
|
| |
|
| |
|
ANSYS Solutions 2006 Issue 3
|
| |
(ANSYS, Inc.)
|
| |
ANSYS Solutions 2006 Issue 3. Industry Spotlight: Military and Defense Systems
[permalink]
|
| |
|
| |
|
ANSYS Solutions 2006 Issue 4
|
| |
(ANSYS, Inc.)
|
| |
ANSYS Solutions 2006 Issue 4. Industry Spotlight: Factory and Plant Equipment
[permalink]
|
| |
|
| |
|
ANSYS Solutions 2006 Issue 5
|
| |
(ANSYS, Inc.)
|
| |
ANSYS Solutions 2006 Issue 5. Industry Spotlight: Oil and Gas
[permalink]
|
| |
|
Average Rating: 10.0 (1 vote)
|
|
|
| |
|
ANSYS-Structural Design of Micromachined Fabry-Pérot Filters for WDM Applications
|
| |
K. Mutamba, J. Pfeiffer, J. Peerlings, R. Riemenschneider and N. Dragojevic
|
| |
"Due to the recent progress in the fabrication of micro-optical devices and the maturity reached in the integration of electromechanical functions on various semiconductor micro-devices, new concepts for optical microelectromechanical systems (OMEMS) have emerged... Analyses have been carried out with the ANSYS FEM (Finite Elements Method) Program for two types of electrostatically actuated Fabry-Pérot filters."
[permalink]
|
| |
|
Average Rating: 10.0 (4 votes)
|
|
|
| |
|
ANSYS2STL
|
| |
Iker Gómez Vázquez (ITP)
|
| |
This is a macro to convert an ANSYS structural mesh into an ASCI STL (stereolithography) file.
Since the STL format is based on a triangular surface mesh, this macro selects all external nodes, generates SURF154 elements, then exports these to the STL file.
Macro updated on 03/17/2009.
[permalink]
|
| |
|
Average Rating: 1.4 (7 votes)
|
|
|
| |
|
ANSYSSTANDARD.TLB |
| |
You can swap the command line to the bottom by making a small change to the GUI resource file:
In your ANSYS 6.1 directory, go to docu/english/toolbars. Edit ANSYSSTANDARD.TLB and change the line that says:
*ANS_STD.location: n
to
*ANS_STD.location: s
[where "n" is for north and "s" is for south]
Likewise, to change the location of the "Main Menu" from left to right, edit:
*ANS_MAIN.location: w
to
*ANS_MAIN.location: e
[where "w" is for west and "e" is for east]
[permalink]
|
| |
|
Average Rating: 10.0 (3 votes)
|
|
|
| |
|
ANVECT
|
| |
Bill Bulat (CSI)
|
| |
Animates velocity vectors from Flotran transient results
[permalink]
|
| |
|
Average Rating: 10.0 (12 votes)
|
|
|
| |
|
ANVOLT
|
| |
Bill Bulat (CSI)
|
| |
Animates voltage results of harmonic analysis in /POST1 by contouring the real part of the solution while varying the phase angle.
[permalink]
|
| |
|
Average Rating: 10.0 (2 votes)
|
|
|
| |
|
APDL and Vector Operations [ZIP]
|
| |
Sheldon Imaoka (ANSYS, Inc.)
|
| |
"Vector and matrix operations in APDL are an invaluable method of manipulating array data, as they provide very fast, computationally efficient means of helping the user perform pre- or post-processing operations on the model.
There are many ways of storing data, ranging from arrays to tables to strings. Moreover,
manipulation of numerical data can be in the form of vectors or matrices via the *Vxxx and *Mxxx commands, respectively. The user is referred to the APDL Programmer’s Guide in the ANSYS online help for a thorough discussion of the capabilities of APDL, but, in this memo, a basic introduction to vector operations will be covered."
(Week 24, week of 03/21/04.)
[permalink]
|
| |
|
Average Rating: 10.0 (9 votes)
|
|
|
| |
|
APDL Coding Standards [PDF]
|
| |
Sheldon Imaoka (ANSYS, Inc.)
|
| |
"Because of the flexibility and automation APDL (ANSYS Parametric Design Language) provides,
many users tend to write input files and macros in addition to using the GUI.
There are currently no recognized ‘standards’ of writing APDL macros or input files, although
there may exist standards within companies on APDL coding. The lack of APDL coding standards
may make inheriting someone else’s input files or macros more difficult. Also, parameter or
component conflicts may also arise when using multiple macros.
This memo hopes to provide some ideas for groups or individuals wishing to develop APDL
standards in writing macros or input files."
(Week 17, week of 02/18/02.)
[permalink]
|
| |
|
Average Rating: 10.0 (24 votes)
|
|
|
| |
|
APDL Implementation of a 3D FEM Capacitance Simulator for Arbitrarily Shaped Interconnects [PDF]
|
| |
Andreas Hieke
|
| |
Alternative download link here
An alternate CMATRIX macro created by A. Hieke called CAMACO.
[permalink]
|
| |
|
Average Rating: 7.5 (4 votes)
|
|
|
| |
|
Application of the Finite Element Method In Cold Forging Processes
|
| |
Cristina Maria Oliveira Lima Roque, Sérgio Tonini Button
|
| |
"In this study, the application of a commercial general finite element software - ANSYS - has been applied to model a forming operation. Models have been developed to simulate the ring compression test and to simulate a basic forming operation (upsetting) that is applied in most of the cold forging parts sequences." (Plasticity, contact, finite strain)
[permalink]
|
| |
|
Average Rating: 10.0 (16 votes)
|
|
|
| |
|
Applying Anand Model to Represent the Viscoplastic Deformation Behavior of Solder Alloys
|
| |
G. Z. Wang, Z. N. Cheng, K. Becker, J. Wilde
|
| |
"A unified viscoplastic constitutive law, the Anand model, was applied to represent the
inelastic deformation behavior for solders used in electronic packaging. The material
parameters of the constitutive relations for 62Sn36Pb2Ag, 60Sn40Pb, 96.5Sn3.5Ag, and
97.5Pb2.5Sn solders were determined from separated constitutive relations and experimental
results. The achieved unified Anand model for solders were tested for constant
strain rate testing, steady-state plastic flow and stress/strain responses under cyclic loading.
It is concluded that the Anand model can be applied for representing the inelastic
deformation behavior of solders at high homologous temperature and can be recommended
for finite element simulation of the stress/strain responses of solder joints in
service."
[ANSYS Nonlinear, version unknown]
[permalink]
|
| |
|
Average Rating: 10.0 (3 votes)
|
|
|
| |
|
ARCH_BUCK
|
| |
Sheldon Imaoka (CSI)
|
| |
Buckling of arch (example of use of pressure load stiffness matrix)
For many eigenvalue (and nonlinear) buckling problems, inclusion of the pressure load stiffness matrix (BEAM188/189, SHELL181, SURF154) significantly affects results. For nonlinear buckling problems, this may also affect convergence rate.
* Theoretical: 771.12
* SHELL93 only (1st eig 840.73)
* SHELL181 only (1st eig 771.72)
* SHELL93 & SURF154 (1st eig 771.07)
* SHELL93 & SURF154, face 4 (1st eig 840.78)
Change "COMPTYPE" parameter to run above 4 cases.
[permalink]
|
| |
|
Average Rating: 9.1 (439 votes)
|
|
|
| |
|
AREACAL
|
| |
Carl Ostervig (Tech Inno)
|
| |
This macro calculates the number and area for all selected elements.
[permalink]
|
| |
|
Average Rating: 10.0 (2 votes)
|
|
|
| |
|
AREATEST
|
| |
(ANSYS, Inc.)
|
| |
Tests areas for consistent normals (not needed at 5.6 since /PSYM,ADIR,1 allows plotting of normals). Also, you may need to rename this macro "ATEST" or "NORMALS" since "AREAS" is a status topic command.
[permalink]
|
| |
|
Average Rating: 10.0 (2 votes)
|
|
|
| |
|
ARPLOT
|
| |
(Unknown source)
|
| |
Annotates each area with its size (/AN3D)
[permalink]
|
| |
|
Average Rating: 10.0 (2 votes)
|
|
|
| |
|
Arrays |
| |
Passing arrays as arguments to macros
Example from John Swanson:
/batch,list
*create,macro,mac
a = arg1(1)
b = arg1(2)
c = arg1(3)
*stat
*end
*dim,xx1,,3
xx1(1) = 10
xx1(2) = 20
xx1(3) = 30
macro,'xx1'
/exit,nosave
[permalink]
|
| |
|
Average Rating: 8.3 (6 votes)
|
|
|
| |
|
ARVL |
| |
ARVL
Selects all areas associated with currently active volumes.
[permalink]
|
| |
|
Average Rating: 10.0 (1 vote)
|
|
|
| |
|
ASBL |
| |
ASBL,NA,NL,SEPO,KEEPA,KEEPL
The SEPO undocumented argument is similar to ASBA command. For ASBL, the divided areas will share lines by default but will have separate lines if SEPO is the value in the 3rd field.
The reason why this argument is undocumented is that, in some cases, separate, coincident keypoints may not be generated.
[permalink]
|
| |
|
Average Rating: 10.0 (2 votes)
|
|
|
| |
|
ASBW |
| |
ASBW,area,,,,,,,MESH
This divides a meshed area. (Warning - this may cause a corrupt database - use at your own risk! - STI)
[permalink]
|
| |
|
Average Rating: 10.0 (4 votes)
|
|
|
| |
|
ASK
|
| |
Navtej Singh (Intel)
|
| |
"You will be prompted with variable name and value in a single dialouge box.
Enter the variable name upto 32 chars long.
Enter the variable value upto 128 chars long. Value can be numeric or string. No need to enter quotes for string.
On clicking enter this script will set the variable name with the value in ANSYS properly either as a nummeric or string."
[permalink]
|
| |
|
Average Rating: 8.6 (14 votes)
|
|
|
| |
|
ASLE |
| |
ASLE,s,1
Selects areas based on elements. Second argument is selection method (s, r, u). Third argument is to select areas if any of its elements are selected (0) or only if all of its areas are selected (1). This command behaves similar to other "select based on" commands like NSLL.
[STI: Works with 5.7 and above]
[permalink]
|
| |
|
Average Rating: 10.0 (6 votes)
|
|
|
| |
|
ASLM_BW
|
| |
Bram Weisman (SBM-IMODCO)
|
| |
Based on ALSM macro, created by John Crawford to select/reselect/unselect meshed areas. Written to take advantage of vectors to execute faster.
[permalink]
|
| |
|
Average Rating: 10.0 (1 vote)
|
|
|
| |
|
ASLN |
| |
ASLN,s,1
Selects areas based on nodes. See ASLE undocumented command (or NSLL documented command) for usage.
[permalink]
|
| |
|
Average Rating: 8.3 (3 votes)
|
|
|
| |
|
ASME Code and Ratcheting in Piping Components
|
| |
Tasnim Hassan and Vernon C. Matzen
|
| |
"The main objective of this research is to develop an analysis program which can accurately
simulate ratcheting in piping components subjected to seismic or other cyclic loads. Ratcheting is
defined as the accumulation of deformation in structures and materials with cycles. This
phenomenon has been demonstrated to cause failure to piping components (known as ratchetingfatigue
failure) and is yet to be understood clearly. The design and analysis methods in the ASME
Boiler and Pressure Vessel Code for ratcheting of piping components are not well accepted by the
practicing engineering community."
[permalink]
|
| |
|
Average Rating: 8.3 (3 votes)
|
|
|
| |
|
ASSOPTION |
| |
ASSOPTION,,FRONTAL
Resets element assembly option to frontal assembly rather than symbolic assembly for the sparse solver at 6.0.
ASSOPTION,,,,0.0
Do not drop non-zero terms from global matrix.
ASSOPTION,,,,,sing
For DANSYS, uses single core to assemble.
ASSOPTION,,pcg
Use symbolic assembly (default behavior from 6.0).
[permalink]
|
| |
|
Average Rating: 10.0 (4 votes)
|
|
|
| |
|
ASWP
|
| |
Bram Weisman (SBM-IMODCO)
|
| |
Divides a picked area with the working plane, retaining the area attributes for the newly-created areas.
[permalink]
|
| |
|
Average Rating: 10.0 (2 votes)
|
|
|
| |
|
ATLAS TRT Barrel Electronics Cooling: Duke mockup measurements and FEA calculations
|
| |
W. Ebenstein, J. Fowler, S. Oh, V. Vassilakopoulos, and C. Wang
|
| |
"This report summarizes measurements and calculations using the most recently proposed cooling scheme. Heat generated by the ASDBLR and DTMROC stamp boards is conducted to an aluminum plate sandwiched between the upper and lower stamp boards (hereafter referred to as the 'middle cooling plate'). The heat is then carried up through a vertical aluminum post, and finally to a large aluminum plate above all of the upper stamp boards (the 'upper cooling plate'), to which cooling tubes are attached."
[permalink]
|
| |
|
Average Rating: 10.0 (1 vote)
|
|
|
| |
|
attrib_2_Load
|
| |
(ANSYS, Inc.)
|
| |
"This script will apply a force load (magnitude 1000) on each entity that is flagged with an attribute beginning with DSA in the first assembly. There are two mechanisms by which this is done; one via the part manager the other via the DS tree."
[permalink]
|
| |
|
Average Rating: 8.6 (25 votes)
|
|
|
| |
|
attrib_2_Load_FEA
|
| |
(ANSYS, Inc.)
|
| |
"This script will apply load and boundary conditions based on attributes that exist on the model. They are filtered by an attribute prefix and divided by parts by a seperator."
[permalink]
|
| |
|
Average Rating: 10.0 (5 votes)
|
|
|
| |
|
attrib_2_MeshSizing
|
| |
(ANSYS, Inc.)
|
| |
"attributePrefix is intended to be the prefix of the attribute used in the CAD to represent mesh-sizing."
[permalink]
|
| |
|
Average Rating: 10.0 (6 votes)
|
|
|
| |
|
AVE_TMP
|
| |
Ted Harris (PADT)
|
| |
Computes the average temperature (from a thermal analysis) of the selected set of nodes. Example of the use of *VMASK.
[permalink]
|
| |
|
Average Rating: 9.5 (22 votes)
|
|
|
| |
|
AVGTEMP
|
| |
David Power (Mallett Technology Inc.)
|
| |
"Get average element temperature for each element from nodal body loads.
Unfortunately it's pretty slow for large models, and I haven't had any time to restructure it to make it run faster, although I'm sure I could make better use of the array operations."
[permalink]
|
| |
|
Average Rating: 4.4 (8 votes)
|
|
|
| |
|
AVPRIN |
| |
AVPRIN,,effnu
AVPRIN also works in /POST26 (it is documented only to work with /POST1). Issue AVPRIN,,effnu with effnu prior to any PRVAR or PLVAR commands (this is where the actual calculations are performed).
[STI: This works at 5.6.2; I don't know about earlier releases. The whole equivalent strain thing may be resolved in a cleaner fashion by 5.7.1, at the earliest]
[permalink]
|
| |
|
| |
|
AVSUCD
|
| |
Ian Sigal (University of Toronto)
|
| |
"The macro writes an AVS UCD file that can be read by Amira. This allows quick display and post-processing. I use the macro to export a model formed of Solid92 tetrahedrals, but only the results in the four corners are written to the file. The macro also writes the element solutions, although these are not read by Amira, but are accepted in the AVS UCD standard."
[permalink]
|
| |
|
Average Rating: 10.0 (4 votes)
|
|
|
| |
|
AXIGET
|
| |
Rod Scholl (PADT)
|
| |
Selects axi-symmetric elements based upon their keyopts. (PLANE42/82 Only)
[permalink]
|
| |
|
Average Rating: 10.0 (2 votes)
|
|
|
| |
|
B188TO89
|
| |
René Fiege (Jos. L. Meyer GmbH)
|
| |
"I attached a little macro to define new BEAM189s on the nodes and properties of the existing 188 elements."
[permalink]
|
| |
|
Average Rating: 10.0 (1 vote)
|
|
|
| |
|
BALLSHEAR
|
| |
Steve Groothuis (Micron Technology, Inc.)
|
| |
"I have uploaded a nice mechanical contact problem using solder and a shearing ram (original work is found in Huang, et al. ECTC paper). That paper spells out the material properties necessary to perform a rate-dependent mechanical load using ANSYS. Compare the paper's Figure 3 with the /POST26 plvar plot (excellent correlation with minimal data)."
[permalink]
|
| |
|
Average Rating: 9.5 (179 votes)
|
|
|
| |
|
BAR
|
| |
Timothy Berger (UCLA)
|
| |
"I have included a rather long input file that I used for my Ph.D. dissertation on an SGI Origin 2000 supercomputer. I believe it is the low density mesh version but if you run into problems, go to lines 157-167 starting from /BATCH and lower the numbers as you see fit for my mesh parameters. I removed all of the constraint equations from the file below as it will slow ANSYS down considerably if they are included."
For additional notes by author, see contents of macro for more details.
[permalink]
|
| |
|
Average Rating: 9.1 (23 votes)
|
|
|
| |
|
Basics of ANSYS Macros [PDF]
|
| |
David Haberman (CSI)
|
| |
Basics of creating and using macros (APDL) in ANSYS.
[permalink]
|
| |
|
Average Rating: 8.0 (20 votes)
|
|
|
| |
|
Basics of Element Tables in ANSYS [PDF]
|
| |
Sheldon Imaoka (CSI)
|
| |
Short description on the usage and features of element tables in ANSYS.
[permalink]
|
| |
|
Average Rating: 9.6 (49 votes)
|
|
|
| |
|
Basics on Structural Damping (Addendum) [ZIP]
|
| |
Sheldon Imaoka (ANSYS, Inc.)
|
| |
"Since ANSYS 5.6, there have been numerous enhancements as well as facets
of the software program that have changed, including treatment of damping.
This article is meant to serve as an addendum to Section 6 of the author’s
"Structural Damping" memo, which was written in October, 2000."
(Week 46, week of 04/27/08)
[permalink]
|
| |
|
Average Rating: 10.0 (4 votes)
|
|
|
| |
|
Basics on Structural Damping [ZIP]
|
| |
Sheldon Imaoka (ANSYS, Inc.)
|
| |
This is an old document I wrote a while ago on damping which I sometimes use. Although written back at version 5.6, it is still applicable at version 7.0.
"Damping is required in many dynamic applications, yet because there are many ways to include it, there is often confusion regarding the implementation of damping in ANSYS. This memo hopes to provide a general summary of the representation of damping available in ANSYS."
(Week 21, week of 11/25/02.)
See also Addendum to "Basics on Structural Damping" memo.
[permalink]
|
| |
|
Average Rating: 9.2 (52 votes)
|
|
|
| |
|
BATCH
|
| |
Sheldon Imaoka (ANSYS, Inc.)
|
| |
This is an example of how to drag-and-drop a .db file onto a DOS batch file to initiate an analysis.
- Unzip the file and rename "Run Nonlinear.txt" to "Run Nonlinear.bat". Place it on your desktop.
- Place "solve_batch.inp" in your D: drive or edit "Run Nonlinear.bat" to change the location of this APDL input file.
- Drag and drop any .db file containing a ready-to-solve nonlinear analysis onto "Run Nonlinear.bat". You will find that the solution will initiate in the same working directory, and you can also track the nonlinear solution graphically as the solution is solving in batch.
[permalink]
|
| |
|
Average Rating: 6.7 (6 votes)
|
|
|
| |
|
BATTLE
|
| |
Dave Lindeman (3M)
|
| |
A macro used to play "Battleship" on ANSYS. (It's a very cool macro. I modified the macro very slightly since the answer was being revealed at 5.5 and 5.6, so /num,0 and /num,1 were added to prevent this from occurring. -- STI)
From the author:
By the way, please note that this is mugware - if you enjoy the game, or are mildly amused by the thought of a game written in APDL, please send one of your company mugs to the address below.Enjoy!Dave Lindeman
CAE Specialist
3M Company
3M Center 235-1F-36
St. Paul, MN 55144
[permalink]
|
| |
|
Average Rating: 9.1 (80 votes)
|
|
|
| |
|
BBLDIV
|
| |
Bill Bulat (OMM)
|
| |
From the author:
"I whipped up the following simple macro (I call it bbldiv.mac) to help assign divisions to predefined lines when you don't know their direction, but you do know their end keypoints. Useful for bottom-up modeling with input scripts."
[permalink]
|
| |
|
Average Rating: 6.0 (5 votes)
|
|
|
| |
|
BCSOPTION |
| |
BCSOPTION,ropt,mopt,msiz,io_opt,dump_opt,dbg
Controls sparse solver options.
ROPT can be changed to mmd, metis, sgi, or wave (equation reordering method)
MOPT can be changed to forc or limit and MSIZ is size in MB (up to 2 GB) to force or limit sparse solver memory to a certain amount. (At 7.0, MOPT can also be set to default, incore, optimal, or minimum with MSIZ left blank to use default, in-core, optimal out-of-core, or minimum out-of-core solutions)
IO_OPT can be set to -1 to override default I/O saves. This keeps the solver memory in-core to avoid backing up the workspace (LN22). It prevents the solver from releasing/reallocating memory by keeping the solver memory permanently allocated during solution.
DUMP_OPT can be changed to asc or bin to dump input matrices to disk in ASCII or Binary format
DBG can be set to -5 which prints performance stats. (At 7.0 and above, this is same as setting to performance value)
[STI: Works only for 5.7 and above. See EQSLV,sparse,,-5 for 5.6 and prior. Documented at 7.0 and above]
[permalink]
|
| |
|
Average Rating: 10.0 (10 votes)
|
|
|
| |
|
BEAFORCE
|
| |
Juha Tyllinen (KONE Corporation)
|
| |
Macro applies pressure distribution for approximation of bearing force. See contents of macro for details.
[permalink]
|
| |
|
Average Rating: 9.7 (17 votes)
|
|
|
| |
|
BEAM176CROSS
|
| |
Sheldon Imaoka (ANSYS, Inc.)
|
| |
Simple example of new beam-to-beam contact capability in ANSYS 10.0 using CONTA176. (Note that version 10.0 or higher must be used.) Sample image of results.
[permalink]
|
| |
|
Average Rating: 9.2 (42 votes)
|
|
|
| |
|
BEAMNET
|
| |
Artem Kulachenko (Mid Sweden University)
|
| |
Adds beam elements on outer edges of shell elements. From the author:
Attached please find a macro that creates a net of beam/link elements on 4/3 node shells.An example of its use:
/prep7
et,1,41
rect,0,1,0,1
amesh,1
et,2,4
beamnet,41,2
[permalink]
|
| |
|
Average Rating: 10.0 (4 votes)
|
|
|
| |
|
BEAMPRES
|
| |
Bram Weisman (Alan C. McClure Associates, Inc.)
|
| |
Applies linearly varying pressure on beams.
[permalink]
|
| |
|
Average Rating: 9.8 (22 votes)
|
|
|
| |
|
BEARING
|
| |
Mark Kessler (BAE Systems)
|
| |
"Applies a bearing load using discreet forces. Written primarily to apply a bearing load to a model that has been tet meshed where using a pressure gradient would require rebuilding the model."
[permalink]
|
| |
|
Average Rating: 8.7 (27 votes)
|
|
|
| |
|
Behavioural modeling for heterogeneous systems based on FEM descriptions
|
| |
Joachim Haase, Sven Reitz, Peter Schwarz
|
| |
"To simulate more complex systems using Spice-compatible circuit and system simulation programs, behavioural models of the components are required. The focus of the paper is to discuss two possibilities to derive such models from FEM descriptions."
[permalink]
|
| |
|
Average Rating: 10.0 (4 votes)
|
|
|
| |
|
Bellcore Response Spectrum Analysis using ANSYS and Pro/ENGINEER
|
| |
Andy Bax and Chris Andersen
|
| |
Bellcore test (see other related DRD presentation).
[permalink]
|
| |
|
Average Rating: 10.0 (10 votes)
|
|
|
| |
|
Benchmark Tests on ANSYS Parallel Processing Technology
|
| |
Kentaro Suzuki
|
| |
"ANSYS Inc. has released parallel processing solvers, DDS (Distributed Domain Solver) and AMG (Algebraic Multigrid Solver) in ANSYS version 5.7 in order to meet the requirements from the market.""In this paper, simple tests are first carried out to confirm the features and capabilities of DDS and AMG for different types of analyses. Furthermore, real-life problems such as thermal stress of an engine block (7.3 million DOF) and elastic-plastic-creep behavior of an IC packaging (about 84,000 DOF) are analyzed. The effectiveness of ANSYS parallel processing solvers is also studied."
[permalink]
|
| |
|
Average Rating: 5.0 (6 votes)
|
|
|
| |
|
Beta Electrical Contact Features at 6.0 [ZIP]
|
| |
Sheldon Imaoka (ANSYS, Inc.)
|
| |
"This issue describes a beta feature at 6.0, which is electrical contact capability of 17x surface-to-surface contact elements. This new capability allows contact in thermal-electric and structural-thermal-electric problems."
(Week 13, week of 01/07/02.)
[permalink]
|
| |
|
Average Rating: 7.9 (29 votes)
|
|
|
| |
|
BILINEAR
|
| |
John Swanson (SAS, Inc./ANSYS, Inc.)
|
| |
Used when specifying a material which has different tensile and compressive moduli. A test input file is also available.
[permalink]
|
| |
|
Average Rating: 10.0 (11 votes)
|
|
|
| |
|
Biomechanical Interaction Between Cap Thickness, Lipid Core Composition and Blood Pressure in Vulnerable Coronary Plaque: Impact on Stability or Insta
|
| |
Gerard Finet, Jacques Ohayon and Gilles Rioufol
|
| |
"A ‘thin’ fibrous cap atheroma is the typical
morphological characteristic of vulnerable plaque. Yet
the very pathological studies that have provided these
descriptions have also shown the actual prediction of
plaque rupture to be rather less exact. Other relevant
characteristics must be involved in the mechanisms of
plaque rupture—blood pressure loading (P) and the
material properties of the soft atheromatous core—as
predictors of the distribution of the peak circumferential
stress (PCS) locations."
[ANSYS Structural, version 5.7]
[permalink]
|
| |
|
Average Rating: 10.0 (2 votes)
|
|
|
| |
|
BLOCK_RAD
|
| |
Kal Torak
|
| |
Simple input file showing radiation between two blocks using /AUX12 radiation matrix method.
[permalink]
|
| |
|
Average Rating: 9.4 (71 votes)
|
|
|
| |
|
BMSweep: Locating Interior Nodes During Sweeping [PDF]
|
| |
Matthew L. Staten, Scott A. Canann, and Steve J. Owen
|
| |
"BMSweep is a new algorithm to determine the location of interior nodes while volume sweeping."
[permalink]
|
| |
|
Average Rating: 10.0 (3 votes)
|
|
|
| |
|
BODE01
|
| |
Bill Bulat (CSI)
|
| |
Macro produces a bode plot using 2 predefined variables in /post26.
[permalink]
|
| |
|
Average Rating: 10.0 (6 votes)
|
|
|
| |
|
BOOT
|
| |
Sheldon Imaoka (ANSYS, Inc.)
|
| |
Old model originally created back in ANSYS 6.0. Recently tested and seems to solve fine as-is in ANSYS 12.1, so I expect all versions in-between should run fine, too. Hyperelasticity, self-contact, rigid-deformable contact are present. Animation of same model (with finer mesh) is on the gallery page.
[permalink]
|
| |
|
Average Rating: 8.3 (3 votes)
|
|
|
| |
|
BOW
|
| |
Mark Troscinski (ANSYS, Inc.)
|
| |
Example of bowshock on cylinder.
[permalink]
|
| |
|
Average Rating: 9.5 (96 votes)
|
|
|
| |
|
BSPLINE |
| |
BSPLINE,ALL,First,[Next],[OPEN | CLOSED],,sx1,sy1,sz1,sx2,sy2,sz2
Use more keypoints for BSPLINE to have an open or closed loop.
[STI: At 5.6.2, CLOSED option didn't seem to work for arbitrary sets of keypoints...]
[permalink]
|
| |
|
Average Rating: 8.3 (6 votes)
|
|
|
| |
|
Buckling in Workbench Simulation [PDF]
|
| |
Sheldon Imaoka (ANSYS, Inc.)
|
| |
"Buckling may be a concern for some situations, where a user may need to modify the
design to prevent buckling within a given load range. Conversely, failure analysis may
need to be performed when a structure has collapsed.
ANSYS and Workbench Simulation have many tools to aid users in solving
geometric instability problems, ranging from linear (eigenvalue) buckling to nonlinear,
post-buckling analyses."
(Week 41, week of 10/14/07)
[permalink]
|
| |
|
Average Rating: 8.9 (65 votes)
|
|
|
| |
|
Building Parametric Models [PDF]
|
| |
David Haberman (CSI)
|
| |
This memo provides an overview of APDL, defining parameters, and creating parametric models.
[permalink]
|
| |
|
Average Rating: 10.0 (8 votes)
|
|
|
| |
|
Calculating effective Coefficient of Thermal Expansion [PDF]
|
| |
Bill Bulat (CSI)
|
| |
Tips on how to define coefficient of thermal expansion and converting that material data to format that ANSYS can use.
[permalink]
|
| |
|
Average Rating: 9.8 (44 votes)
|
|
|
| |
|
Calculations on Micromachined Electro-Thermal Sensor Devices
|
| |
Bernd Folkmer, Martin Hirt, Michael Vosseler, Hartmut Glosch, Frank Hedrich, Sophie Billat, Walter L
|
| |
"In this contribution the experiences gained using ANSYS/Multiphysics software for analysis of micro machined electro-thermal sensor devices are described."
[permalink]
|
| |
|
Average Rating: 10.0 (5 votes)
|
|
|
| |
|
Cannot View ANSYS Online Help on Windows
|
| |
Sheldon Imaoka (ANSYS, Inc.)
|
| |
After installing a Windows Hotfix, if ANSYS is installed on a file server, the ANSYS Online Help cannot be viewed. This tip describes how to fix this problem.
[permalink]
|
| |
|
| |
|
Cast Iron Plasticity
|
| |
(ANSYS, Inc.)
|
| |
Presentation on Cast Iron plasticity model introduced in ANSYS 6.1 (part of the "Advanced Analysis with ANSYS" seminar during the 2002 User's Conference).
[permalink]
|
| |
|
Average Rating: 9.4 (8 votes)
|
|
|
| |
|
Cavity mechanics and vibrations under Lorentz forces excitation
|
| |
Danilo Barni
|
| |
(Harmonic, modal analyses)
[permalink]
|
| |
|
Average Rating: 6.7 (6 votes)
|
|
|
| |
|
CBC_RAMP
|
| |
Bill Bulat (CSI)
|
| |
Macro for defining a cubic ramp for use w/ ANSYS/LS-Dyna for performing quasi-static explicit analyses.
[permalink]
|
| |
|
Average Rating: 8.8 (17 votes)
|
|
|
| |
|
CBDOF, BFINT |
| |
CBDOF/BFINT,,,,,,,,,,TOLOUT,MOVETOL
Vary distance for projecting results.
The TOLOUT parameter is the fraction of the size of the nearest element by which a point can be outside the element. (Default is 0.5)
The MOVETOL parameter is the max motion of a node outside the body to reach the surface of the body (value > 1). This allows nodes to be moved to the surface by a specified amount prior to interpolation/extrapolation.
[permalink]
|
| |
|
Average Rating: 10.0 (1 vote)
|
|
|
| |
|
CECHECK |
| |
CECHECK,Item,Tolerance,Flag
Checks constriant equations for non-zero rigid reactions.
Item is "All (default), CE, or CP"
Flag is "RIGID (default) | ALL | Dof" where DOF can be individual UX, UY, TEMP (THERM?), etc.
[permalink]
|
| |
|
Average Rating: 10.0 (3 votes)
|
|
|
| |
|
CELIST |
| |
CELIST,,,,option
For the 17x contact elements which support MPC formulation, one can list the internally-generated MPC equations (CE)
CELIST,,,,ALL: list all constraint equations
CELIST,,,,INTE: list only internally-generated constraint equations associated with MPC-based contact
CELIS,,,,CONV: convert internal CEs to real CEs
All of the above options must be done in /SOLU after a SOLVE.
[STI: undocumented at 8.0]
[permalink]
|
| |
|
Average Rating: 8.5 (10 votes)
|
|
|
| |
|
CERIG vs RBE3, RIGID184 [ZIP]
|
| |
Sheldon Imaoka (ANSYS, Inc.)
|
| |
"Constraint equations provide many useful features in ANSYS, such as tying together dissimilar meshes, representing parts of the system not explicitly modeled, or distributing loads. Two automated methods of generating constraint equations are the CERIG and RBE3 commands. Because there is often confusion over their use, this memo hopes to provide some information on differences between the two methods.
"Constraint equations in ANSYS are linear, so they are not valid for large-rotation analyses. RIGID184 is a beta element in version 6.1 which provides rigid link/beam capabilities, valid for large-rotation problems. The latter part of this memo will cover some details of this undocumented feature, available in 6.1."
(Week 19, week of 07/08/02.)
[permalink]
|
| |
|
Average Rating: 9.9 (72 votes)
|
|
|
| |
|
CESGEN |
| |
CESGEN,2,_ntot,all
Generates/copies constraint equations (CEs).
[permalink]
|
| |
|
Average Rating: -2.5 (2 votes)
|
|
|
| |
|
CEWRITE |
| |
write out constraint equations (jobname.ce)
[permalink]
|
| |
|
Average Rating: 10.0 (10 votes)
|
|
|
| |
|
Chaboche Nonlinear Kinematic Hardening Model [PDF]
|
| |
Sheldon Imaoka (ANSYS, Inc.)
|
| |
"The Chaboche nonlinear kinematic hardening model was added in ANSYS
5.6 to complement the existing isotropic and kinematic hardening rules that
users relied on. Despite its availability for nearly ten years as of the time
of this writing, the Chaboche model has enjoyed limited popularity, in part
because of the perceived complexity of calibrating the material parameters.
This memo hopes to introduce the basics related to the Chaboche nonlinear
kinematic model."
(Week 47, week of 05/04/08)
[permalink]
|
| |
|
Average Rating: 9.7 (16 votes)
|
|
|
| |
|
Characterization and Analysis on the Solder Ball Shear Testing Conditions
|
| |
Xingjia Huang, S.W. Ricky Lee, Chien Chun Yan, and Sam Hui
|
| |
"This paper presents both experimental investigation and computational analysis on the solder ball shear testing conditions for ball grid array (BGA) packages." (Creep, contact)
[permalink]
|
| |
|
Average Rating: 4.4 (9 votes)
|
|
|
| |
|
CHECKIGES
|
| |
Julián Díaz (ITR México)
|
| |
"This is a very simple macro, but I've found it very useful when I have an iges file with common errors of duplicate geometry and small lines. All it does is look for lines smaller that .1 inches and plots them along with the attached areas, this can be useful to have a glipse of where could the problems be."
[permalink]
|
| |
|
Average Rating: 10.0 (2 votes)
|
|
|
| |
|
CIRCLE
|
| |
John Crawford (Honeywell)
|
| |
A UIDL function (granule file) to create circles by picking. To change the menu put the following in a menu granule:
:!
:N Men_CIRC
:S 0, 0, 0
:T Menu
:A Circles
:D Circles
Fnc_CIRCLEWP
Fnc_CIRCLEKP
:E END
:!
[permalink]
|
| |
|
Average Rating: 10.0 (1 vote)
|
|
|
| |
|
CIRCU125 |
| |
Undocumented DIODE element (5.5, 5.6).
[STI: Documented & released at 5.7]
[permalink]
|
| |
|
Average Rating: 10.0 (13 votes)
|
|
|
| |
|
CLEAN
|
| |
Tom Glade (PACCAR Technical Center)
|
| |
"Here's a macro I use to clean up TYPEs, REALs, and MPs."
[permalink]
|
| |
|
Average Rating: 9.4 (8 votes)
|
|
|
| |
|
CLEAN_MODEL
|
| |
René Fiege (Meyer Werft GmbH)
|
| |
"The macro deletes not used attributes (real, mat, type, section), similar to the clean macro from Tom Glade, but with vector operations. It can easily be enlarged to document the used attributes (see macro).
"Do not use the macro with referencing attributes, like tapered beams. All attributes, which are not an attribute of an element will be deleted."
[permalink]
|
| |
|
Average Rating: 0.0 (1 vote)
|
|
|
| |
|
CLIST |
| |
CLIST,csys,Nstart,Nend,Ninc
Displays coordinates for nodes in given "csys" coordinate system without using DSYS. Use of DSYS is cumbersome since it affects displays as well as listings, so this is a better alternative.
[permalink]
|
| |
|
Average Rating: 9.4 (9 votes)
|
|
|
| |
|
CLOSED_TANK
|
| |
Sheldon Imaoka (ANSYS, Inc.)
|
| |
Comparison of FLUID30 (acoustic fluid element) and FLUID80 (contained fluid element) for sloshing in a tank.
[permalink]
|
| |
|
Average Rating: 9.2 (25 votes)
|
|
|
| |
|
CLOSELINE
|
| |
Ernst Hustedt (Air New Zealand Engineering)
|
| |
The macro selects those lines that surround a picked point, or those lines that are exterior, depending on the case. Try the attached igs file and pick completely outside, inside but close to an outer line, inside outer loop but close to an inner line etc. and see what happens.""Extending it to 3-D should be possible by starting with the WP aligned with the screen csys or so."
[permalink]
|
| |
|
Average Rating: 0.0 (2 votes)
|
|
|
| |
|
Closing the Gaps on Data Interoperability [PDF]
|
| |
Don Hemmelgarn
|
| |
PowerPoint presentation
[permalink]
|
| |
|
Average Rating: 10.0 (4 votes)
|
|
|
| |
|
Clustering Results Around Peaks for Full-Harmonic Analyses in ANSYS
|
| |
Aaron Acton (ANSYS, Inc.)
|
| |
"This article presents a method for obtaining full harmonic solutions clustered around potential peak responses.
Full harmonic analyses provide exact solutions, typically calculated at equally spaced intervals over
the desired frequency range. Mode-superposition analyses, however, provide approximate solutions, but can be
clustered around potential resonant peaks. The hybrid method discussed in this article uses a modal solution to
determine natural frequencies, which are then used to calculate clusters of points surrounding those frequencies.
Full harmonic solutions can then be performed at these clustered points. Examples and input les are provided
in order to utilize this method."
[permalink]
|
| |
|
Average Rating: 10.0 (3 votes)
|
|
|
| |
|
CMAP_ANSYS_VIRIDIS
|
| |
Cristóbal Tapia (University Stuttgart)
|
| |
This is a colormap for Viridis, which is the new colormap designed by Nathaniel Smith and Stéfan van der Walt for matplotlib.
[permalink]
|
| |
|
Average Rating: 6.0 (5 votes)
|
|
|
| |
|
CMDIF
|
| |
Eric Miller (PADT)
|
| |
"ANSYS has a *get,,common command that lets you grab things from memory.
The only problem with this is that you can't just give the *get the name
of the block, you need to tell it its position (count) in the block. As
an example, the 3rd value listed in a common block is at position 3 (or
index 3).
The way you use a common block is you look in the ansys/custom/include
directory for the value you want to know.
In this case I did a search for a file that contained "/cplane" and
found it in d3com.inc.
Looking in the file I found that the value kycpln is what I was looking
for and the common block was /d3com/
Sometimes you can just count to find out what the index is, but this
block is huge and has arrays in it. So instead, I used the macro below.
I did:
/cplane,0
cmndif,0,'d3com',0
/cplane,1
cmndif,1,'d3com',0
And the macro wrote:
Found: 91 0 1.
So I would then do: *GET,_cpstat,COMMON,,D3COM,,int,91
to retrieve the value.
Another example would be if I wanted to know what the global minimum and
max number of divisions
per line was (DESIZE):
desize,10,11
cmndif,0,'cfprp7',0
desize,20,21
cmndif,1,'cfprp7',0
Yields:
Found: 99 10 20.
Found: 100 11 21.
For this I would use:
*get,_mnlnsz,common,,cfprp7,,int,99
*get,_mxlnsz,common,,cfprp7,,int,100"
[permalink]
|
| |
|
Average Rating: 9.3 (7 votes)
|
|
|
| |
|
CMF
|
| |
Ernst Hustedt (Air New Zealand Engineering)
|
| |
Make a compound fillet at two straight lines.
[permalink]
|
| |
|
Average Rating: 10.0 (1 vote)
|
|
|
| |
|
CMGET
|
| |
John Crawford (Honeywell)
|
| |
"A macro that retrieves the components saved using cmput.mac."
[permalink]
|
| |
|
Average Rating: 10.0 (1 vote)
|
|
|
| |
|
CMPUT
|
| |
John Crawford (Honeywell)
|
| |
"A macro that saves all the currently selected entities in components"
[permalink]
|
| |
|
Average Rating: 10.0 (3 votes)
|
|
|
| |
|
CMRESU
|
| |
Juha Tyllinen (KONE Corporation)
|
| |
"Here is a fully vectorized version where you can select the entity type you are saving. The saved component (well, select status) is stored as file with 'cmp' extension and includes two header lines: entity type and number of selected entities. CMSave saves the status and CMResu resumes it from the file."
[permalink]
|
| |
|
Average Rating: 10.0 (1 vote)
|
|
|
| |
|
CMREVIEW
|
| |
Tom Glade (PACCAR Technical Center)
|
| |
Reviews defined components of a specific type (node, element, keypoint, line, area, or volume components).
[permalink]
|
| |
|
Average Rating: 10.0 (1 vote)
|
|
|
| |
|
CMSAVE
|
| |
Juha Tyllinen (KONE Corporation)
|
| |
"Here is a fully vectorized version where you can select the entity type you are saving. The saved component (well, select status) is stored as file with 'cmp' extension and includes two header lines: entity type and number of selected entities. CMSave saves the status and CMResu resumes it from the file."
[permalink]
|
| |
|
| |
|
CMWRITE |
| |
CMWRITE,Fname,Fext,Fdir,ipos,[_ | BLOCK | UNBLOCK]
Write component information to file, where ipos = 0,write at beginning of file, 1, write at end of file
For 7.0 and later.
[permalink]
|
| |
|
Average Rating: 8.3 (12 votes)
|
|
|
| |
|
CNF_FREQRESP
|
| |
Rick Morgans (Adelaide University)
|
| |
Outputs velocities for a single frequency analysis in COMET/Acoustics from an ANSYS harmonic analysis.
[permalink]
|
| |
|
Average Rating: 10.0 (5 votes)
|
|
|
| |
|
CNHTXFR2
|
| |
Brad Lamirand (Cooper Turbocompressor, Inc.)
|
| |
Steady state conjugate heat transfer in a pipe.
[permalink]
|
| |
|
Average Rating: 9.0 (26 votes)
|
|
|
| |
|
CNTR |
| |
CNTR,PRINT,nlevel
CNTR,print,0 (default) - only print the troubleshooting when solution diverges in the end
CNTR,print,1 - above + print the troubleshooting when bi-section occurs
CNTR,print,2 - above + print the message for each load step
CNTR,print,3 - above + print the message for each sub-step
CNTR,print,4 - above + print the message for each iteration and much more
[permalink]
|
| |
|
Average Rating: 10.0 (3 votes)
|
|
|
| |
|
CNVG_TIME
|
| |
Mitch Voehl (CEC Corp)
|
| |
Macro to get last converged substep.
[permalink]
|
| |
|
Average Rating: 10.0 (1 vote)
|
|
|
| |
|
COAX
|
| |
Johann Riedler (EPCOS)
|
| |
"I created an input-file that simulates the skin-effect of a two-dimensional sector of a coax. During postprocessing you can clearly see the effect of the penetrating magnetic field into the metal. One may extend this model to 3D (perhaps coarser)."
[permalink]
|
| |
|
Average Rating: 10.0 (19 votes)
|
|
|
| |
|
COIL_EMF
|
| |
Bill Bulat (CSI)
|
| |
Used to report per-turn EMF induced in predefined closed loop paths.
[permalink]
|
| |
|
Average Rating: 7.5 (12 votes)
|
|
|
| |
|
Collaborative Virtual Prototyping: A Product Development Imperative [PDF]
|
| |
Marc Halpern
|
| |
PowerPoint presentation
[permalink]
|
| |
|
Average Rating: 8.8 (4 votes)
|
|
|
| |
|
Comparison of FLUID29 and FLUID79 Elements
|
| |
Carl Howard (University of Adelaide)
|
| |
"Analyses were conducted to verify that similar results could be obtained by using the displacement formulated fluid elements FLUID79 or the pressure formulated fluid elements FLUID29."
[permalink]
|
| |
|
Average Rating: 10.0 (7 votes)
|
|
|
| |
|
Comparison of Linear and Non-linear Soft Tissue Models with Post-operative CT Scan in Maxillofacial Surgery
|
| |
Matthieu Chabanas, Yohan Payan, Christophe Marecaux, Pascal Swider, and Franck Boutault
|
| |
"A Finite Element model of the face soft tissue is proposed
to simulate the morphological outcomes of maxillofacial surgery. Three
modelling options are implemented: a linear elastic model with small
and large deformation hypothesis, and an hyperelastic Mooney-Rivlin
model. An evaluation procedure based on a qualitative and quantitative
comparison of the simulations with a post-operative CT scan is detailed.
It is then applied to one clinical case to evaluate the differences between
the three models, and with the actual patient morphology. First results
shows in particular that for a “simple” clinical procedure where stress is
less than 20%, a linear model seams sufficient for a correct modelling."
[ANSYS Nonlinear, version unspecified]
[permalink]
|
| |
|
| |
|
Comparison of Rectangular and Spherical Models
|
| |
Carl Howard (University of Adelaide)
|
| |
"The purpose of this investigation was to compare the two modelling techniques for an infinite boundary. The first technique involves setting the elements on the edges of the model to have an absorptive property by changing the material properties so that mu=1. The second technique involves the use of infinite elements (infinite129) that must be placed on a constant radius curvature."
[permalink]
|
| |
|
Average Rating: 10.0 (11 votes)
|
|
|
| |
|
COMPFILLET
|
| |
Joe Metrisin (Florida Turbine Technologies, Inc.)
|
| |
"One way I've used to create a compound fillet or spline shape during an optimization run is by use of an elliptical coordinate system. You can get a very well behaved ellipse suitable for optimization with only 3-4 parameters. The procedure is to create two keypoints, and a local cylindrical coordinate system with the par1 option. Then, a line created between these two keypoints will have an elliptical shape.
[permalink]
|
| |
|
Average Rating: 10.0 (19 votes)
|
|
|
| |
|
Compiling UPFs and Creating Customized ANSYS Executables [PDF]
|
| |
Sheldon Imaoka (ANSYS, Inc.)
|
| |
"ANSYS User Programmable Features (UPFs) are quite powerful means of
customizing ANSYS beyond the scripting capabilities of the ANSYS Parametric
Design Language (APDL). Writing one’s own constitutive models
or complex loading functions or even creating a user-defined element are
possible with UPFs.
Because some users may find it challenging to get started using UPFs,
this memo hopes to discuss general issues related to compiling and linking
a customized version of ANSYS for Windows and Linux environments."
(Week 51, week of 02/08/09)
[permalink]
|
| |
|
Average Rating: 10.0 (19 votes)
|
|
|
| |
|
COMPMENU
|
| |
Jim Patterson (Hendrickson Trailer Suspension Systems)
|
| |
"I have a set of macros to generate toolbars based on the defined components in the db. You can then call these toolbars from the main toolbar to aid in the selecting of the components. This includes "select", "also select", and "unselect". You can also "remake" the components from the toolbar. As someone who works with assemblies of shell models almost
constantly, this has been a huge time saver for me."
Tested on 5.7 through 6.1. Unzip the file and read the supplied Word document for instructions.
[permalink]
|
| |
|
Average Rating: 10.0 (6 votes)
|
|
|
| |
|
Comprehensive Solder Fatigue And Thermal Characterization Of A Silicon Based Multi-Chip Module Package Utilizing Finite Element Analysis Methodologies
|
| |
Bret A. Zahn
|
| |
"Viscoplastic finite-element simulation methodologies were utilized to predict ball and bump solder joint reliability for a silicon based five-chip multi-chip module package under accelerated temperature cycling conditions." (Nonlinear, Anand)
[permalink]
|
| |
|
Average Rating: 10.0 (9 votes)
|
|
|
| |
|
Compressive Strength of Solid Clay Brick Masonry under Eccentric Loading
|
| |
A. Brencich, C. Corradi, L. Gambarotta, G. Mantegazza, E. Sterpi
|
| |
"Arches, vaults and pillars generally experience eccentric normal force. As a consequence, the classical theories of masonry collapse, developed for concentrically compressed brickwork, are not directly applicable. In this paper experimental data on solid clay brick and lime-mortar masonry prisms, eccentrically loaded, are presented. Comparing the results to the response of a FEM model, some hints on the collapse mechanism of masonry show that the edge effects greatly affect the load carrying capacity of the brickwork. Besides, the plane section assumption is found to be acceptable up to the ultimate compressive strength, allowing relatively simple models to be used for arch-type structures." (Concrete SOLID65)
[permalink]
|
| |
|
Average Rating: 9.8 (26 votes)
|
|
|
| |
|
COMPTEN
|
| |
Carl Ostervig (Tech Inno)
|
| |
This macro analysis iteratively structures with different material properties (Youngs modulus) in tension and compression. [STI: Please note that this macro looks at SX and SY. See BILINEAR macro for a more general compression/tension macro based on principal stresses.]
[permalink]
|
| |
|
Average Rating: 4.2 (6 votes)
|
|
|
| |
|
Conceptual Design for the SRRC Elliptically Polarizing Undulator EPU5.6. Part II: Magnetic Loading and Structure Deformation
|
| |
Ch. Wang, M.C. Lin, C.H. Chang, L.H. Chang, H.H. Chen, T.C. Fan, K.T. Hsu, J.Y. Hsu, C.S. Hwang, K.T
|
| |
"In part II of the conference paper, we address our efforts on the determination of the maximal magnetic loading on the individual magnetic arrays, and on the estimation of the resulting structure deformation by using the 3D finite element code ANSYS."
[permalink]
|
| |
|
Average Rating: 10.0 (3 votes)
|
|
|
| |
|
Connection Kits and ANF files |
| |
Sheldon Imaoka (ANSYS, Inc.)
|
| |
The ANSYS Connection Kits for Parasolid, SAT (ACIS), Unigraphics, Pro/ENGINEER, and CATIA all generate ANF files in the working directory.
One can save this jobname.anf file instead of reimporting the model, in case one has a parametric input file defining loads, materials, etc. or if the geometry needs to be archived.
If the CAD model does change, however, reimporting of the model is required, as this ANF file is a static 'snapshot' of the CAD assembly/part when it was imported.
[permalink]
|
| |
|
Average Rating: 10.0 (2 votes)
|
|
|
| |
|
Constellation Pathfinder: A University Nanosatellite
|
| |
C.D. Rayburn, H.E. Spence, H.E. Petschek, M. Bellino, J. Vickers, M. Murphy
|
| |
"This paper updates the progress of the Constellation Pathfinder Mission (CPM) design. Specifically, preliminary results in areas including satellite design, orbital mechanics, thermal design, structural design, and attitude determination and control are discussed."
[permalink]
|
| |
|
Average Rating: 8.8 (4 votes)
|
|
|
| |
|
Constitutive Relationship Development, Modeling and Measurement of Heat Stressing of Micro-SMD Assembly with Sn3.9Ag0.6Cu SAC Alloy
|
| |
Qiang Xiao, William Armstrong, James Pitarresi, Satish Chaparala, Brian Rogeman, Bahgat Sammakia, Lu
|
| |
"The thermal-mechanical response of electronic packages was simulated using the commercial finite element code ANSYS coupled with the Garofalo model to represent the solder constitutive creep response. The measured properties for bulk and thin-cast Sn3.9Ag0.6Cu SAC alloy were used in the FE modeling."
[permalink]
|
| |
|
Average Rating: 0.0 (2 votes)
|
|
|
| |
|
Construction Machinery Cab Vibro-Acoustic Analysis and Optimisation
|
| |
L. Bregant, G. Miccoli, M. Seppi
|
| |
"A 3D cavity representing the earth-moving machine cab has been modelled by means of a FE structural mesh (Ansys), reproducing the characteristics of the real structure. Starting from the cab vibration load experimental acquisition, a BEM coupled analysis (Sysnoise) has been carried out to evaluate the cab inner vibro-acoustic field as a function of the physical properties of each structural element. A multi-objective design optimisation code (modeFrontier) drives the analysis process flow taking into account the cab parameter structural modifications and carrying out the vibro-acoustic field optimisation."
[ANSYS Dynamics, version unspecified]
[permalink]
|
| |
|
Average Rating: 10.0 (4 votes)
|
|
|
| |
|
CONTA17x |
| |
Pure thermal contact:
Use KEYOPT(1)=2 for pure thermal option (TEMP DOF only) for 5.7.
This pure thermal contact feature is documented at 6.0.
[permalink]
|
| |
|
Average Rating: 10.0 (9 votes)
|
|
|
| |
|
CONTA17x |
| |
Support of "debonding" for bonded or no-separation contact. Use real constants 27 (max tensile stress) and 28 (max shear stress) to specify limits at which point the bonded or no-separation contact becomes like standard contact.
[STI: beta at 9.0]
[permalink]
|
| |
|
Average Rating: 8.7 (19 votes)
|
|
|
| |
|
CONTAC26
|
| |
CONTAC26 "2-D Point-to-Ground Contact" was undocumented at ANSYS 8.1. It should be replaced by CONTA175.
[permalink]
|
| |
|
Average Rating: 10.0 (1 vote)
|
|
|
| |
|
CONTAC48
|
| |
CONTAC48 "2-D Point-to-Surface Contact" was undocumented at ANSYS 8.1. It should be replaced by either node-to-surface CONTA175 or surface-to-surface CONTA171-172.
[permalink]
|
| |
|
Average Rating: 0.0 (3 votes)
|
|
|
| |
|
CONTAC49
|
| |
CONTAC49 "2-D Point-to-Surface Contact" was undocumented at ANSYS 8.1. It should be replaced by either node-to-surface CONTA175 or surface-to-surface CONTA173-174.
[permalink]
|
| |
|
| |
|
Contact Analysis of Workpiece-Fixture System Under Time-Varying Machining Loads Using Finite Element Method
|
| |
N. Kaya, F. Öztürk
|
| |
"Proper fixture design is crucial to product quality in terms of precision, accuracy and finish of the machined part. Fixturing systems must be capable of positioning, holding and supporting the workpiece throughout the machining process. In this paper, modular fixture design verification analysis is carried out for time-varying machining forces using nonlinear finite element analysis. Chip removal effect is taken into account using element death technique and the frictional contact between workpiece and fixture elements is also considered. This paper also adresses applying optimal clamping forces in order to minimize the deformation. A case study is presented to demonstrate the suggested methodology."
[permalink]
|
| |
|
Average Rating: 10.0 (10 votes)
|
|
|
| |
|
Contact Analysis Tips [PDF]
|
| |
Sheldon Imaoka (ANSYS, Inc.)
|
| |
"Generally speaking, nonlinear analyses involving contact can be quite challenging
to solve when the contacting area changes during the load history.
However, ANSYS Workbench Simulation has very robust contact technology,
along with diagnostic tools that can help the user obtain converged,
accurate solutions. This memo hopes to discuss some tips related to contact
analyses in hopes of aiding the user who encounters difficulties when solving
contact analyses."
(Week 52, week of 02/22/09)
[permalink]
|
| |
|
Average Rating: 9.7 (30 votes)
|
|
|
| |
|
Contact Wizard Enhancements at 6.0 [PDF]
|
| |
Sheldon Imaoka (ANSYS, Inc.)
|
| |
Describes some of the enhancements made to the Contact Wizard at ANSYS 6.0, including support of 17x contact elements' thermal features and ability to edit contact pair options through same interface.
(Week 5, week of 10/22/01.)
[permalink]
|
| |
|
Average Rating: 9.3 (23 votes)
|
|
|
| |
|
CONTACT_SHELL
|
| |
Sheldon Imaoka (CSI)
|
| |
Shows rigid-flexible contact w/ shell offset.
[permalink]
|
| |
|
Average Rating: 9.2 (130 votes)
|
|
|
| |
|
ContactName_NrTypeAdd
|
| |
Przemyslaw Siedlaczek (MESco)
|
| |
Workbench macro sets contact name by adding number and type ID.
[permalink]
|
| |
|
Average Rating: 10.0 (2 votes)
|
|
|
| |
|
ContFrictVsTemp
|
| |
Przemyslaw Siedlaczek (MESco)
|
| |
Workbench macro adds APDL code to the contact branches to define temperature-dependent coefficient of friction.
[permalink]
|
| |
|
Average Rating: 10.0 (2 votes)
|
|
|
| |
|
CONTPRES
|
| |
Sheldon Imaoka (ANSYS, Inc.)
|
| |
Simple 2D example comparing SY (y-component of stress) at contact surface with CONTPRES (contact pressure). With surface-projection-based contact, results match very well, showing benefits of using surface-project-based contact (KEYOPT(4)=3 for 17x contact elements).
[permalink]
|
| |
|
Average Rating: 10.0 (6 votes)
|
|
|
| |
|
CONTROL
|
| |
Dave Lindeman (3M)
|
| |
"Listed below are an ANSYS input file, and a UITFIN subroutine that demonstrate the implementation of a PID control system using a simple spring-mass system."
UITFIN.F subroutine
[permalink]
|
| |
|
Average Rating: 10.0 (12 votes)
|
|
|
| |
|
Control Data to be Saved |
| |
Sheldon Imaoka (ANSYS, Inc.)
|
| |
Starting from ANSYS 5.7, the SAVE command has an additional argument to control what data will be saved to the jobname.db database file. The Slab argument allows a user to specify ALL, MODEL, or SOLU to be saved, analogous to the /EXIT command. Use SAVE,,,,MODEL or /EXIT,MODEL to save model information only in the DB file to conserve disk space - recall that all of the results are already contained in the results files (RST, RTH, RMG, etc.), so one doesn't need to save results data to the DB file as well.
[permalink]
|
| |
|
Average Rating: 10.0 (1 vote)
|
|
|
| |
|
CONTS2S
|
| |
G. N. S. Prakash
|
| |
"'conts2s.mac' macro creates surface to surface contact elements between nodal components with the default options. Only nodal components(target & contact), material number and coefficient of friction can be given as arguments. Use Contact wizard or your custom code to modify other properties. This macro is helpful when number of components in Ansys models are large or sometimes when the Contact wizard becomes slow with large db files and if we need to create a lot of contact pairs."
[permalink]
|
| |
|
Average Rating: 7.0 (5 votes)
|
|
|
| |
|
CONV_FINS
|
| |
Sheldon Imaoka (CSI)
|
| |
Simple natural convection problem of heated fins, 2D tri.
[permalink]
|
| |
|
Average Rating: 9.4 (25 votes)
|
|
|
| |
|
CONVECT
|
| |
Steve Groothuis (Micron Technology, Inc.)
|
| |
Example of using MP data to apply temp-dependent film coefficient. Please note that this macro does not have geometry and will not run by itself. It is meant to serve as an example in applying film coefficients.
[permalink]
|
| |
|
Average Rating: 9.1 (60 votes)
|
|
|
| |
|
Converting piezoelectric data [PDF]
|
| |
Sheldon Imaoka (CSI)
|
| |
Conversion of material properties of piezoelectric ceramics (such as PZT) has caused many users confusion because of the difference between manufacturer-supplied data and the format required by ANSYS. This memo hopes to clarify this point and to provide users with information on conversion routines.
Accompanying Spreadsheet.
[permalink]
|
| |
|
Average Rating: 9.1 (41 votes)
|
|
|
| |
|
Converting pressures to nodal forces [PDF]
|
| |
Sheldon Imaoka (CSI)
|
| |
Tip on converting element pressures to nodal forces. This can be useful for mode superposition methods where LVSCALE may not be suitable.
SI_P2F Macro and test input file.
[permalink]
|
| |
|
Average Rating: 8.1 (32 votes)
|
|
|
| |
|
Converting Prony Series to Frequency Domain
|
| |
Sheldon Imaoka (ANSYS, Inc.)
|
| |
Simple example showing how to convert Prony series for viscoelasticity from time domain to frequency domain. This is to convert TB,PRONY to TB,ELASTIC/SDAMP for use in harmonic response analyses.
[permalink]
|
| |
|
Average Rating: 10.0 (7 votes)
|
|
|
| |
|
Cooling the APS Storage Ring Radio-Frequency Accelerating Cavities: Thermal/Stress/Fatigue Analysis and Cavity Cooling Configuration
|
| |
K. Primdahl, R. Kustom
|
| |
"Heat transfer studies, including finite-element analysis and
test results, of the Advanced Photon Source (APS) storage ring
352-MHz radio-frequency (rf) accelerating cavities are
described. Stress and fatigue life of the copper are discussed.
Configuration of water cooling is presented."
[permalink]
|
| |
|
| |
|
COPLOT |
| |
COPLOT,secnum
Plots a beam cross section secnum as MESH200 elements on the screen. Useful to see graphically where the 'section nodes' are if you run this in a blank database.
Sample input below:
finish
/clear
/prep7
sect,1,beam,I
secd,1,1.5,1,0.1,0.1,0.1
/pnum,node,1
/efacet,2
coplot,1
See CUPLOT for related command
[permalink]
|
| |
|
Average Rating: 10.0 (3 votes)
|
|
|
| |
|
COUETTE
|
| |
Sheldon Imaoka (CSI)
|
| |
Example of couette flow, viscous heating option for incompressible flow at Flotran 5.6.
[permalink]
|
| |
|
Average Rating: 9.8 (28 votes)
|
|
|
| |
|
COUPCOIN
|
| |
Alex Komissarov (GEAE)
|
| |
A macro used to couple DOF of nodes in a given cylindrical coordinate system within a specified tolerance.
[permalink]
|
| |
|
Average Rating: 6.9 (8 votes)
|
|
|
| |
|
COUPLE_DOF
|
| |
Jyotis Sardar (IIT MADRAS)
|
| |
"Here's a macro I created, that will generate couples in the required DOF's, merely by prompting the user to pick the source and target lines."
[permalink]
|
| |
|
Average Rating: 8.0 (10 votes)
|
|
|
| |
|
Coupled Structural-Acoustic Analysis Using ANSYS [PDF]
|
| |
Carl Howard (University of Adelaide)
|
| |
Paper on using SHELL63 and SOLID45 with FLUID30 in acoustic analyses.
[permalink]
|
| |
|
Average Rating: 9.8 (27 votes)
|
|
|
| |
|
COUPLED-SEQ
|
| |
Sheldon Imaoka (ANSYS, Inc.)
|
| |
Simple example demonstrating a sequential structural-thermoelectric analysis with plasticity and contact. The thermoelectric side uses UPGEOM to update displacements from the structural analysis.
[permalink]
|
| |
|
Average Rating: 7.1 (7 votes)
|
|
|
| |
|
Coupling low-order elements to high-order elements in ANSYS
|
| |
Aaron Acton
|
| |
"This article presents several methods for obtaining coupling at the interface between low- and high-order elements in ANSYS. This situation can be encountered when modelling the fluid-structure interaction between a solid domain, modelled with quadratic elements, and an acoustic fluid domain, modelled with linear elements.
The two methods determined to be most suitable for achieving this coupling are by using either constraint equations or contact elements, both of which are likely more-robust methods than by simply attaching coincident nodes on matching meshes. Examples are provided for each case described herein, and the results from each are compared to the ANSYS 11.0 verification problem VM177."
[permalink]
|
| |
|
Average Rating: 9.0 (10 votes)
|
|
|
| |
|
CPJOINS
|
| |
Mark Kessler (BAE Systems)
|
| |
"A macro to create couples at coincident locations."
[permalink]
|
| |
|
Average Rating: 10.0 (3 votes)
|
|
|
| |
|
CPMERGE |
| |
CPMERGE,lab
Merges different couple sets with duplicate degrees of freedom into one couple set.
"Lab" can be any valid DOF label (e.g., 'UX')
Similar to NUMMRG,CP
[permalink]
|
| |
|
Average Rating: 10.0 (5 votes)
|
|
|
| |
|
CPQUERY
|
| |
Sheldon Imaoka (ANSYS, Inc.)
|
| |
This macro counts the number of coupled sets associated with the current selected set of nodes.If the first argument is 1, then the macro will count the total number of coupled sets if any of its nodes are selected. Otherwise, the coupled set will only be counted if all of its nodes are selected.
[permalink]
|
| |
|
Average Rating: 9.4 (9 votes)
|
|
|
| |
|
CPSGEN |
| |
CPSGEN,2,_ntot,all
Generates/copies coupled sets (CPs).
[permalink]
|
| |
|
Average Rating: 10.0 (2 votes)
|
|
|
| |
|
CPWRITE |
| |
write out coupled sets (jobname.cp)
[permalink]
|
| |
|
Average Rating: 10.0 (10 votes)
|
|
|
| |
|
Creating a Helical Path
|
| |
Paul McGarry (Galway-Mayo Institute of Technology)
|
| |
"A step by step GUI method for creating a left or right-handed helix, in any axis, for any pitch or diameter."
[permalink]
|
| |
|
Average Rating: 7.1 (7 votes)
|
|
|
| |
|
Creating APDL Macros [PDF]
|
| |
Mike Rife (CSI)
|
| |
The use of the Ansys Parametric Design Language, APDL, to create simple but reusable macros can be a significant time saver. This Tip of the Week will show two examples of macros written for current Ansys users. These macros may be extended or used as templates for future macros.
Helical fin macro and Strain energy plotting macro.
[permalink]
|
| |
|
Average Rating: 9.7 (15 votes)
|
|
|
| |
|
Creating Custom Animations [ZIP]
|
| |
Sheldon Imaoka (ANSYS, Inc.)
|
| |
"Animations are quite useful, both in presenting results of an analysis to others as well as obtaining better insight into the complex response of a system. While ANSYS has many built-in animation capabilities, sometimes, it may be necessary to create a macro for a customized animation. This memo covers one method of generating such animations."
(Week 1, week of 09/24/01.)
[permalink]
|
| |
|
Average Rating: 9.4 (31 votes)
|
|
|
| |
|
Creep and Plasticity
|
| |
Guoyu Lin (ANSYS, Inc.)
|
| |
Discussion on creep (implicit and explicit time integration), along with using it with plasticity models. (From XANSYS posting)
[permalink]
|
| |
|
Average Rating: 9.9 (37 votes)
|
|
|
| |
|
Creep Resistance and Creep Bending Resistance of Light Metal Matrix Composites for Research in Airframe Structural Effiency
|
| |
E. Neubauer and H.Peter Degischer
|
| |
"Main aim of the research in the frame of the AMTT programme was the testing of a fiber reinforced Al-alloy. For investigation of the creep behaviour of this material, creep tests under bending were performed. The tested material was Al99.85+0.1%Mg reinforced with Al2O3 fibers (Altex/Sumitomo), which was prepared by means of gas pressure infiltration. Main benefit of such a material for application would be the lowering of the weight of the material without a loss of properties." (see Appendix A for ANSYS use in this document)
[permalink]
|
| |
|
Average Rating: 9.5 (10 votes)
|
|
|
| |
|
CTPIPE3
|
| |
Mark Kessler (BAE Systems)
|
| |
"A macro to create a series of elements from one picked node to all other selected nodes."
[permalink]
|
| |
|
| |
|
CUBIC
|
| |
Bob Weathers (Trane)
|
| |
Performs monotonic cubic interpolation in a table.
[permalink]
|
| |
|
Average Rating: 5.0 (3 votes)
|
|
|
| |
|
CUPLOT |
| |
CUPLOT,filename
Plots a user-defined beam cross section stored in filename as MESH200 elements on the screen. Useful to see graphically where the 'section nodes' are if you run this in a blank database.
See COPLOT for related command
[permalink]
|
| |
|
Average Rating: 10.0 (1 vote)
|
|
|
| |
|
CURING
|
| |
Steve Groothuis (Micron Technology, Inc.)
|
| |
"Try this sample input file demonstrating VE cure simulation. The data originated from a Ph.D. dissertation ("Viscoelastic stress analysis and fatigue life prediction of a flip-chip-on-board electronic package.", PAUL B. KOENEMAN, Thesis (Ph.D.). University of Texas at Austin, Austin, TX 78712, USA, 1999. 113pp.)."
[permalink]
|
| |
|
Average Rating: 9.5 (62 votes)
|
|
|
| |
|
Customizing GUI Behavior [PDF]
|
| |
Sheldon Imaoka (ANSYS, Inc.)
|
| |
"The /UIS and /MSTART commands provide the user with control over much of the GUI behavior. At 5.7 and 6.0, this has been extended to include control over the multilegend feature, background color, and mouse button assignment for dynamic rotations. Used in conjunction with the startxx.ans file, this allows the user to change GUI behavior in each ANSYS session."
(Week 6, week of 10/29/01.)
[permalink]
|
| |
|
Average Rating: 8.5 (10 votes)
|
|
|
| |
|
CUTCONTROL |
| |
CUTCONTROL,NOSHAPE,1
Tells ANSYS to not do any element shape-checking during the course of a nonlinear analysis.
[permalink]
|
| |
|
Average Rating: 10.0 (7 votes)
|
|
|
| |
|
CUTCONTROL |
| |
CUTCONTROL,PIVSTOP,psvalue
When a negative pivot is encountered, ANSYS usually continues with the analysis.
Setting psvalue to 1 will cause ANSYS to bisect as soon as a negative pivot is encountered.
Setting psvalue to 2 will cause ANSYS to stop the solution as soon as a negative pivot is encountered.
This can be useful, for example, in a nonlinear buckling analysis as a means of determining when a limit load may be reached.
[permalink]
|
| |
|
Average Rating: 9.0 (21 votes)
|
|
|
| |
|
CUTCONTROL |
| |
CUTCONTROL,CUTBACKFACTOR,cutvalue
For automatic time-stepping, this controls the bisection factor. By default, cutvalue is 0.5 (hence the term "bisection"), so ANSYS cuts the timestep in half and resolves if convergence is not achived in that timestep. This can control the cutback factor. (see related undocumented OPNCONTROL,OPENUPFACTOR command.)
[STI: now documented in latest ANSYS releases.]
[permalink]
|
| |
|
Average Rating: 10.0 (3 votes)
|
|
|
| |
|
CVCTRL
|
| |
Chris Kennedy (Think PEAK, Inc.)
|
| |
Prompts for yield stress of material and uses it to set up /CVAL command so that post-processing plots will show elements that exceed the YIELD stress value as red, and elements which have a compressive stress lower than -YIELD as blue. If the minimum stress is not less than -YIELD than the actual minimum is used instead of -YIELD.
[permalink]
|
| |
|
Average Rating: 7.8 (9 votes)
|
|
|
| |
|
CWZDELE |
| |
CWZDELE,real_no,type_flag
Deletes a 17x contact pair, based on the real constant real_no. If type_flag is set to "1", this command not only deletes the contact elements, but it removes the real constant and element types associated with that contact pair.
For example, CWZDELE,3,1 deletes the 17x contact elements associated with real constant 3 (EDELE) and removes the real constant and element types (RDELE, ETDELE).
[permalink]
|
| |
|
Average Rating: 10.0 (7 votes)
|
|
|
| |
|
CYC_PRINC
|
| |
Christian Semler (Mechanical Dynamics Ltd.)
|
| |
"Here is an input file which computes principal stresses for a particular sector from a cyclic symmetry analysis, on all corner nodes, without using the /CYCEXPAND command. This enables the use of the *VGET command, so further manipulations are possible."
[permalink]
|
| |
|
Average Rating: 9.3 (120 votes)
|
|
|
| |
|
CYCGEN
|
| |
(ANSYS, Inc.)
|
| |
Class3 Error 1999-24, SCOPUS #6957
Corrects problem if internal CE exist for modal cyclic symmetry models
[permalink]
|
| |
|
Average Rating: 9.9 (50 votes)
|
|
|
| |
|
Cyclic Symmetry Analysis
|
| |
(ANSYS, Inc.)
|
| |
Presentation on cyclic symmetry enhancements at ANSYS 6.1 (part of the "Advanced Analysis with ANSYS" seminar during the 2002 User's Conference).
[permalink]
|
| |
|
Average Rating: 9.6 (13 votes)
|
|
|
| |
|
CYCSOL
|
| |
(ANSYS, Inc.)
|
| |
Class3 Error 1999-24, SCOPUS #6957
Corrects problem if internal CE exist for modal cyclic symmetry models
[permalink]
|
| |
|
Average Rating: 8.8 (4 votes)
|
|
|
| |
|
CYLINFLO
|
| |
Sheldon Imaoka (CSI)
|
| |
Simple example of natural convection of horizontal cylinder.
[permalink]
|
| |
|
Average Rating: 8.6 (14 votes)
|
|
|
| |
|
DADD |
| |
dadd,labr,lab1,lab2,fact1,fact2,const
LABR = (FACT1 X LAB1) + (FACT2 X LAB2) + CONST
Where:
labr = DOF result (usually same as lab1)
lab1 = DOF used for calcs
lab2 = DOF used for cals
fact1 = Scale factor applied to lab1
fact2 = Scale factor applied to lab2
const = Constant value
This command subtracts out rigid body displacements so you can view deformed shapes better.
Note: when power graphics is on, the updated displacement may not be displayed after the command is entered and a "pldisp" is performed. You can either do an "ALLSEL$/REPLOT" or turn off power graphics "/GRAPH,FULL$/REPLOT".
[Verified in 6.1]
[permalink]
|
| |
|
Average Rating: 10.0 (8 votes)
|
|
|
| |
|
DADD
|
| |
Keith DiRienz (FEA Technologies)
|
| |
Sample input file to demonstrate the use of the undocumented DADD command.
[permalink]
|
| |
|
Average Rating: 4.3 (7 votes)
|
|
|
| |
|
DAKOTA
|
| |
Dave Lindeman (3M)
|
| |
"I recently experimented with coupling ANSYS and DAKOTA, and thought the list might be interested in the results. DAKOTA, if you're not familiar with it, is a public-domain optimization code available from Sandia National Laboratories (see http://endo.sandia.gov/DAKOTA/). It has several advanced optimization algorithms (e.g., genetic algorithms), supports discrete variables, and has several other features that make it a nice complement to the optimization and probabilistic design modules within ANSYS. And it's FREE.
"Anyways, the procedure for using DAKOTA with ANSYS consists of creating a DAKOTA input file (DAKOTA in the attachments) that identifies the design variables, state variables, optimization method, etc. Also, within this file you identify the command to be issued to execute the code you are using to generate the response variables (analysis_driver = 'ansys.prl', in the attached example). To execute ANSYS I use an intermediate Perl script (ansys.prl) that translates the design variable file generated by DAKOTA (parameters_file = 'dakota.dv') into something ANSYS can understand (written out to ansys.dv). The Perl script then executes ANSYS. Note that the Perl script is general purpose -- it should work for any application. The only thing you should need to change is filenames, in particular the name of your ANSYS script (in my example, 'ANSYS'). The ANSYS script reads in the design variable file using /INPUT, performs the analysis, then outputs the result variables to a file (results_file = 'dakota.rv') using *CFOPEN and *VWRITE.
"To execute the analysis you use (for example) the command line: dakota -i DAKOTA > dakota.log &
"That's pretty much it. Pretty straightforward once you figure out the DAKOTA input file syntax. The attached example is the simple beam optimization problem used in the ANSYS documentation."
[permalink]
|
| |
|
Average Rating: 9.0 (29 votes)
|
|
|
| |
|
DCONTOUR
|
| |
Doug Woolridge (Mercury Marine)
|
| |
Creates a second contour using 2D annotation under the original color contour. The values on the new contour are scaled by 'scale_factor'.A modified macro DCONTOU2 by Vincent Raillard changes this to have 2 - 9 uniform contours.
[permalink]
|
| |
|
Average Rating: 10.0 (1 vote)
|
|
|
| |
|
DDS |
| |
For info on the Distributed Domain Solver, which is beta at 5.6 (released at 5.7), contact your ASD.
[STI: DDS needs to be compiled by the user at 5.6 beta; it is not a trivial task, so it may be better to use 5.7 production release of PDS]
[permalink]
|
| |
|
Average Rating: 10.0 (2 votes)
|
|
|
| |
|
DEBUG |
| |
When creating macros or input files, it is often useful to execute them one line at a time to determine where your programming logic breaks down. Placing this command as the first line in the file allows you to do this.
Type in "debug" to see command syntax.
[permalink]
|
| |
|
Average Rating: 9.6 (14 votes)
|
|
|
| |
|
Delamination in Patterned Films
|
| |
X.H. Liu, M.W. Lane, T.M. Shaw, E. Simonyi
|
| |
"When the dielectric constant of an insulator in an interconnect is reduced, mechanical
properties are often compromised, giving rise to significant challenges in
interconnect integration and reliability. Due to low adhesion of the dielectric an interfacial
crack may occur during fabrication and testing. To understand the effect of
interconnect structure, an interfacial fracture mechanics model has been analyzed
for patterned films undergoing a typical thermal excursion during the integration
process. It is found that the underlayer pattern generates a driving force for delamination
and changes the mode mixity of the delamination. The implications of our
findings to interconnect processes and reliability testing have been discussed."
[ANSYS Structural, version unknown]
[permalink]
|
| |
|
| |
|
DEMOTLBR
|
| |
(PADT)
|
| |
"To use this demonstration of the ANSYS toolbar capabilities extract these files to your working directory. You must then copy the tlbrlist61.ans file from the ANSYS installation docu/english/tlbrlist61.ans to your working directory. Add DEMO.TLB to the bottom of the file. Run ANSYS and then move the split bar at the bottom up to show the bottom pane where the demo toolbar is embedded."
Example showing how to customize the ANSYS 6.1 Toolbar.
[permalink]
|
| |
|
Average Rating: 10.0 (3 votes)
|
|
|
| |
|
Design and Analysis of Ultrasonic Actuator in Consideration of Length-Reduction for a USDC (Ultrasonic/Sonic Driller/Corer)
|
| |
Z. Chang, S. Sherrit, M. Badescu, X. Bao, and Y. Bar-Cohen
|
| |
"The USDC uses a novel driving mechanism, transferring
ultrasonic vibration to sonic frequency impacts with the aid of a free-flying mass block (free-mass). The free mass then
drives the drill bit. The actuator consists of a stack of piezoelectric disks with a horn that amplifies the induced vibration
amplitudes. The standard USDC is a slender device, and some times its length is too long for specific NASA missions.
It is of current interest to have novel designs that reduce the length of the device. For this purpose, two novel horn
designs were examined analytically. One is the flipped horn, the other is the planar folded horn. The new designs of the
horn were analyzed using finite element modeling and the results allow for the determination of the control parameters
that can optimize the performance of the ultrasonic horn in terms of the tip displacement and velocity. The results of the
modeling are described and discussed in this paper."
[ANSYS Piezoelectric, version 5.4]
[permalink]
|
| |
|
Average Rating: 10.0 (5 votes)
|
|
|
| |
|
Design and Characterization of Thin Film Microcoolers
|
| |
Chris LaBounty, Ali Shakouri, John E. Bowers
|
| |
"Thin film coolers can provide large cooling power densities compared to bulk thermoelectrics due
to the close spacing of hot and cold junctions. Important parameters in the design of such coolers
are investigated theoretically and experimentally. A three-dimensional finite element simulator
(ANSYS) is used to model self-consistently thermal and electrical properties of a complete device
structure."
[ANSYS Thermal, version 5.5.3]
[permalink]
|
| |
|
| |
|
Design and Implementation of a Flow Microsensor by using Silicon Microelectronics Technology
|
| |
Roberto Rodrigues and Rogerio Furlan
|
| |
"This work presents the design of a gas flow microsensor that was implemented by using silicon microelectronics technology. Its main features are a low power consumption (tens of mW) and the possibility of integration in flow microactuators. It was adopted a calorimetric device with free-standing microfilaments and thermoresistive sensor elements. Analytical and numerical modeling were developed for device analyses and design. The free-standing microfilaments were fabricated using surface micromachining. Characteristic curves, of output voltage vs. flow, were obtained by using a commercial flow sensor for calibration. A good agreement was obtained comparing the flow microsensor experimental characteristic curves with numerical simulation results."
[permalink]
|
| |
|
Average Rating: 10.0 (7 votes)
|
|
|
| |
|
Design And Manufacturing Of Micro Via-In-Pad Substrates For Solder Bumped Flip Chip Applications
|
| |
John Lau, Chris Chang, Ricky Lee, Tsung-Yuan Chen, David Cheng, Tzyy Jang Tseng, Dyna Lin
|
| |
"A novel and low-cost micro via-in-pad (VIP) substrate for supporting a solder bumped flip chip is presented in this study. Non-linear finite element analyses are used to determine the stress and strain in the copper VIP and the solder joint. Time-dependent non-linear analysis is used to predict the thermal-fatigue life of the VIP solder joint." (Nonlinear, Anand)
[permalink]
|
| |
|
Average Rating: 7.5 (2 votes)
|
|
|
| |
|
Design of Antennas for Mobile and Vehicle Applications
|
| |
Jaehoon Choi
|
| |
Presentation on ultra wide band and planar inverted F antennas.
[permalink]
|
| |
|
Average Rating: 10.0 (2 votes)
|
|
|
| |
|
Design Optimization of an Automotive Universal Joint Considering Manufacturing Cost
|
| |
Nick Cristello and Il Yong Kim
|
| |
"This paper presents the shape optimization of an
automotive universal joint, by simultaneously considering
manufacturing cost, maximum drivable joint angle and
part volume. Comprised of three main components - two
yokes and a cross trunnion - a universal joint is a linkage
used to transmit rotational motion from one shaft to
another when the axes are coplanar, but not coinciding. In
this research, universal joint designs are analyzed and
compared using a weighted sum of three objective
functions: minimization of machining cost, maximization
of adjoining shaft joint angle, and minimization of total
part volume. Part modeling and analysis is conducted
using the Finite Element Analysis package ANSYS and
optimization is implemented using MATLAB. The
results show Pareto frontiers for both the flange and weld
yoke, constructed using the Adaptive Weighted Sum
technique. These frontiers clearly illustrate the trade-off
between machining cost and joint angle; that is, to
increase the joint angle, a corresponding increase in the
cost of the part is required. It has been shown that
maximization of driveable joint angle requires a
simultaneous increase in machining cost of 4.4% and
2.7% for the flange and weld yoke, respectively."
[ANSYS Structural, version 9.0]
[permalink]
|
| |
|
Average Rating: 10.0 (5 votes)
|
|
|
| |
|
Design, Fabrication, and Testing of Fixed-Valve Micro-Pumps [PDF]
|
| |
F. Forster, R. Bardell, M. Afromowitz, N. Sharma, and A. Blanchard
|
| |
Use of Flotran for micropump analysis. (MEMS)
[permalink]
|
| |
|
Average Rating: 6.7 (3 votes)
|
|
|
| |
|
Designing the Liquid-Nitrogen Injection Rakes for the European Transonic Windtunnel Project
|
| |
Ian Glendinning
|
| |
Article from Heat Engineering magazine, back in 1993. Static and transient stress and thermal analysis performed in ANSYS 4.4a.
[permalink]
|
| |
|
Average Rating: 10.0 (3 votes)
|
|
|
| |
|
DesignSpace Tutorial 1
|
| |
Sheldon Imaoka (ANSYS, Inc.)
|
| |
Simple tutorial on analyzing parts using DesignSpace with focus on compatibility with SolidWorks.
[permalink]
|
| |
|
Average Rating: 9.4 (69 votes)
|
|
|
| |
|
DesignSpace Tutorial 2
|
| |
Sheldon Imaoka (ANSYS, Inc.)
|
| |
Simple tutorial on analyzing assemblies using DesignSpace with focus on compatibility with SolidWorks.
[permalink]
|
| |
|
Average Rating: 8.5 (23 votes)
|
|
|
| |
|
Developing The Basis For Target Injection And Tracking In Inertial Fusion Energy Power Plants
|
| |
D.T. Goodin, C.R. Gibson, R.W. Petzoldt, N.P. Siegel, L. Thompson, A. Nobile, G.E. Besenbruch, K.R.
|
| |
The use of ANSYS's thermal and CFD capabilities to analyze the target injection and tracking of an Inertial Fusion Energy power plant
[permalink]
|
| |
|
Average Rating: 10.0 (4 votes)
|
|
|
| |
|
Development of CAD Model for MEMS Micropumps [PDF]
|
| |
M. Arik, S. M. Zurn, A. Bar-Cohen, Y. Nam, D. Markus, and D. Polla
|
| |
Use of ANSYS in modal and harmonic analysis of micropumps (PZT cantilever beams). (MEMS)
[permalink]
|
| |
|
Average Rating: 4.2 (6 votes)
|
|
|
| |
|
Development of Convective Reflow-Projection Moiré Warpage Measurement System and Prediction of Solder Bump Reliability on Board Assemblies Affected by
|
| |
Wei Tan (Georgia Institute of Technology)
|
| |
"The effect of PWB warpage on the low cycle fatigue of the solder bumps on
board assemblies was investigated using FEM and experimental study. The three-
dimensional (3-D) models of PWBAs with varying board warpage were used to estimate
the solder bump fatigue life for different types of plastic ball grid array (PBGA) packages
mounted on PWBs. In order to improve the accuracy of FE results, the projection moiré
technique was used to measure the initial warpage of PWBs, and this warpage was used
as a geometric input to the FEM. Both Sn-Pb and lead-free solder materials were used in
this study. The simulation results were validated and correlated with the experimental
results obtained using the projection moiré system and accelerated thermal cycling tests.
Design of experiments and an advanced prediction model were generated to predict board
level solder bump fatigue life based on the initial PWB warpage, package dimensions and
locations, and solder bump materials."
[permalink]
|
| |
|
| |
|
DGEN |
| |
DGEN, 2,_ntot,1,_ntot
Generates/copies DOF constraints.
[permalink]
|
| |
|
Average Rating: 10.0 (3 votes)
|
|
|
| |
|
DGNR8
|
| |
Eric Miller (PADT)
|
| |
"Finds degenerate 2D and 3D elements (i.e., when nodes 3 and 4 are identical), selects them, and then plots them. This works for many cases, such as SOLID45 or PLANE82, etc. Does not work for lower- or higher-order pyramids, but macro can easily be modified for these cases."
[permalink]
|
| |
|
Average Rating: 10.0 (2 votes)
|
|
|
| |
|
Difference between Large rotation, Finite Strain, Stress-Stiffening
|
| |
Sheldon Imaoka (CSI)
|
| |
Discussion on the differences between large rotation (large deflection), finite strain (large strain), and stress-stiffening effects in nonlinear analyses. (From XANSYS posting)
[permalink]
|
| |
|
Average Rating: 9.6 (13 votes)
|
|
|
| |
|
Difference between PSTRES and SSTIF
|
| |
Sheldon Imaoka (CSI)
|
| |
Discussion on the differences between PSTRES and SSTIF commands. (From XANSYS posting)
[permalink]
|
| |
|
Average Rating: 10.0 (10 votes)
|
|
|
| |
|
Differences Between Implicit and Explicit Dynamics
|
| |
Sheldon Imaoka (ANSYS, Inc.)
|
| |
Discussion of the differences between implicit and explicit dynamics. (Differences between regular ANSYS and ANSYS/LS-DYNA)
[permalink]
|
| |
|
Average Rating: 8.1 (40 votes)
|
|
|
| |
|
Different Methods of Connecting Parts Together [PDF]
|
| |
Sean Harvey (CSI)
|
| |
Connecting Parts - A study of Continuous Mesh versus Bonded Contact versus Constraint Equations.
[permalink]
|
| |
|
Average Rating: 9.4 (62 votes)
|
|
|
| |
|
DIFFUSION
|
| |
Steve Groothuis (Micron Technology, Inc.)
|
| |
"As a starting point, if you can accept the following analogy between thermal and moisture diffusion, I think you will be pleased in solving the time-dependent diffusion using this technique. As far as the temperature-dependent moisture diffusion, alternating between moisture mechanics and thermal mechanics can probably be done by updating material properties."
| Properties | Moisture | Thermal | | Field variable | Wetness (C/Csat) | Temperature | | Density | 1 | Density | | Conductivity | D*Csat | Conductivity | | Specific Gravity | Csat | Specific gravity |
where Csat is saturated moisture concentration and D is diffusion coefficient."We use this analogy to simulate moisture absorption in multi-material semiconductor packages under various temperature and RH conditions. It works quite well. Ee Hua Wong (Institute of Microelectronics, Singapore) has developed the technique using ANSYS/Thermal simulations. Mr. Wong has produced several papers outlining the technique."
[permalink]
|
| |
|
Average Rating: 9.7 (60 votes)
|
|
|
| |
|
DIRECT |
| |
DIRECT,on
Use of direct assembly of equations. This is automatically done for PLANE2, PLANE42, SOLID45, SOLID92, SOLID95, and thermal analyses.
[STI: Direct assembly of equations is available in ANSYS 5.7 for structural static, transient, modal, and full harmonic; thermal static and transient; electrostatics.]
[permalink]
|
| |
|
Average Rating: 5.7 (7 votes)
|
|
|
| |
|
Disabling the lock feature of 6.0 |
| |
Sheldon Imaoka (ANSYS, Inc.)
|
| |
Starting from 6.0, the jobname.lock lock file is generated to prevent multiple runs with the same jobname from being executed from the same working directory.
To disable this feature, set the environment variable "ANSYS_LOCK" to "OFF".
For details, please refer to the documentation, either: "Installation and Configuration Guide for UNIX", Ch. 4.2.7 Setting Other Environment Variables, or "Installation and Configuration Guide for Windows", Ch. 4.1.5 Setting Other Environment Variables.
[permalink]
|
| |
|
Average Rating: -10.0 (2 votes)
|
|
|
| |
|
Disruption Load Calculations Using ANSYS Transient Electromagnetic Simulations for the ALCATOR C-MOD Antennas
|
| |
Peter H. Titus
|
| |
"ANSYS has been used to compute eddy current loads in C-Mod antenna components due to a disruption. The antennas are on the outbuard mid-plane, away from the direct involvement with halo currents, which characterize loading in the inner divertor and wall. Only inductively driven currents are computed. A rather complex but manageable electromagnetic model is used. Three of the antennas used in C-Mod were analyzed, Lower Hybrid, ICRH, and MHD antennas. The goal of these simulations was principally to quantify upper bound disruption loads."
[permalink]
|
| |
|
Average Rating: 9.6 (12 votes)
|
|
|
| |
|
DISTCALC
|
| |
Carl Ostervig (Tech Inno)
|
| |
This macro calculates the distance between two nodes, selected by picking. Normally this facility is available in the preprocessor only. This macro works in all processors.
[permalink]
|
| |
|
Average Rating: 9.0 (5 votes)
|
|
|
| |
|
DISTKP2L
|
| |
Wangming Lu (Impact Technologies, LLC)
|
| |
"I have developed the following macro: Given a key point level component,and a line number, it will evaluate the distance from each key point in this component to the input line. The result is returned in an array called distk (you can
change into your name, of course). While using this, pls. be careful, it is not fully
tested yet."
[permalink]
|
| |
|
Average Rating: 10.0 (1 vote)
|
|
|
| |
|
DISTLOAD
|
| |
Nick Veikos (CAEAI), modified by Jim Kosloski (CAEAI)
|
| |
Attached is a macro for applying surface loads. You have to create a file with your own equation defining the load distribution as a function of x,y,z coordinates. You can use any equation possible with ADPL commands.
[permalink]
|
| |
|
Average Rating: 9.7 (17 votes)
|
|
|
| |
|
DistributedLoad
|
| |
Paris Altidis (Borg Warner)
|
| |
Zip file containing two example macros of applying distributed pressures.
[permalink]
|
| |
|
Average Rating: 9.7 (18 votes)
|
|
|
| |
|
DNSOL_VIEW
|
| |
Adam Shinbrot (Spine-Tech Inc.)
|
| |
"GLOBAL INFO: This macro is basically just a couple of routines that use dnsol to align two nodes (arg1 and arg2) on the theoretically fixed body, and adjusts the rest of the nodal results accordingly.
I needed to do this with a multi-body model where I wanted to look at the motion of one body relative to another with the motion of the first body subtracted from the global result."
Example input file can be downloaded here.
[permalink]
|
| |
|
Average Rating: 10.0 (3 votes)
|
|
|
| |
|
Drucker-Prager Models [PDF]
|
| |
Sheldon Imaoka (ANSYS, Inc.)
|
| |
"The Drucker-Prager material model is used for pressure-dependent inelastic behavior
of materials such as soils, rock, concrete, and powder. Because ANSYS offers three
different Drucker-Prager constitutive models, this memo hopes to provide a comparison
of the available options."
(Week 44, week of 03/16/08)
[permalink]
|
| |
|
Average Rating: 9.8 (24 votes)
|
|
|
| |
|
DYDXI
|
| |
Bob Weathers (Trane)
|
| |
Calculates first derivative at the ith entry in a table.
[permalink]
|
| |
|
Average Rating: 10.0 (2 votes)
|
|
|
| |
|
Dynamic FEA and Simulation for A Series of Blast-Resist-door
|
| |
Lu Xinzheng and Jiang Jianjing
|
| |
"A series of blast-resist-door were used widely. In order to know the behavior of the doors under blast load and verify the
safety of the doors, dynamic finite element analysis and simulation are carried out with advanced FEA software, ANSYS/LS-DYNA
and SAP. Contact surfaces are introduced to simulate the relation between the door leaf and doorframe, as well as the relation
between the door hinges and bearings. Altogether 24 different load cases are analyzed to simulate various load conditions."
[ANSYS LS-DYNA, version unspecified]
[permalink]
|
| |
|
Average Rating: 9.2 (6 votes)
|
|
|
| |
|
Dynamic Mouse Controls |
| |
Sheldon Imaoka (ANSYS, Inc.)
|
| |
Another one for new users: Instead of selecting the "Dynamic Mode" option of the Pan-Zoom-Rotate widget to dynamically rotate, zoom, and pan the model, use the Ctrl-key modifier. Simply hold down the ctrl-key while using your left-, middle-, and right-mouse buttons to pan, zoom, and rotate your model (you don't need the Pan-Zoom-Rotate dialog box open to do this). Also, there is sometimes confusion as to how the middle mouse button's 'dynamic zoom' feature works: moving the mouse up and down will zoom, whereas moving the mouse left and right will rotate the model about the screen axis.
[permalink]
|
| |
|
Average Rating: 10.0 (2 votes)
|
|
|
| |
|
Dynamic Pile Testing and Finite Element Calculations for the Bearing Capacity of a Quay Wall Foundation
|
| |
F. Kirsch, B. Plaßmann, T. Huch, W. Rodatz
|
| |
"In April 1999 the construction of a new quay wall in the port of Hamburg started. In a first
stage two new berths with an overall length of 1400 m will be built. In order to proof the bearing capacity of
the foundation dynamic pile testing is performed to a great extent. To date more than thirty different piles
were tested by the Institute for Foundation Engineering and Soil Mechanics of the Technical University of
Braunschweig. In order to check for possible set-up effects redriven tests were performed. For comparison
reasons static load tests were also carried out, one of which was done with an instrumented pile to allow skin
friction and end bearing to be evaluated separately. The CAPWAP results proofed to be very helpful especially
in those cases where the testing situation differed from the later service condition. Special questions
called for detailed finite element analysis of the load-settlement behaviour of single piles in certain construction
stages."
Although ANSYS is not explicitly mentioned, F. Kirsch also used ANSYS in two related papers, Stability of the vault developing over Soilcrete bodies and Ground Improvement and Its Numerical Analysis.
[permalink]
|
| |
|
Average Rating: 9.3 (7 votes)
|
|
|
| |
|
Dynamic Prompt Timeout |
| |
The dynamic prompt appears for 2 seconds by default in 6.0. To lengthen the time before the dynamic prompt disappears, do the following:
1) Make a backup of the file 'C:\Program Files\Ansys Inc\ANSYS61\LIB\Euidl1.0\scripts\anscmdprompt.itk'
2) Edit 'anscmdprompt.itk' at line 468, which contains the string " set _helpWinAfter [after
2000 \", and change the value to the time in miliseconds you wish to have the help visible.
[At 7.0, this is controlled by line 69 ' variable _helpWinTimer 20000' instead, and default is 20 seconds]
[permalink]
|
| |
|
Average Rating: 10.0 (1 vote)
|
|
|
| |
|
Dynamic Shock Simulation Of A Computer Hard Drive Using an ANSYS/LS-DYNA Implicit-Explicit Sequential Solution
|
| |
Chris Andersen, John Stricklin
|
| |
"This paper describes a nonlinear transient dynamic analysis of a computer hard drive using ANSYS in combination with ANSYS/LS-DYNA. The model includes the enclosure, platters, spindle, read/write heads, and other key components. The objective of the analysis was to determine the interaction between the parts in this assembly, such as lift off and impact between the read/write heads and platters, when the hard drive is subjected to a 250 G half sinusoid shock load. This load simulates a shock test, which the manufacturer does to qualify hard drives." From 2000 Conference
[permalink]
|
| |
|
Average Rating: 9.2 (40 votes)
|
|
|
| |
|
dynprompt57.ans |
| |
At 5.7, the dynamic input file prompting was introduced, where the command format was displayed as you typed a command.
Modify "dynprompt57.ans" to add your own macro argument format, so when you type your own macros, the proper arguments are also displayed.
[STI: at 6.0, this file is called "dynprompt60.ans", where the last two numbers indicate the version number.]
[permalink]
|
| |
|
Average Rating: 10.0 (4 votes)
|
|
|
| |
|
E72TO142
|
| |
Tim Lansberry
|
| |
This is an ANSYS macro that converts solid72 elements to fluid142 elements. It defines a new element type for the fluid elements. Useful for creating models for FLOTRAN converted from other CAD packages which use a solid element type.
[permalink]
|
| |
|
Average Rating: 10.0 (5 votes)
|
|
|
| |
|
E72TO45
|
| |
Tim Lansberry
|
| |
This is an ANSYS macro that converts solid72 elements to solid45 elements. It defines a new element type for the solid45 elements.
[permalink]
|
| |
|
Average Rating: 6.7 (6 votes)
|
|
|
| |
|
E92TO142
|
| |
Tim Lansberry
|
| |
This is an ANSYS macro that converts solid92 elements to fluid142 elements. It defines a new element type for the fluid elements. Useful for creating models for FLOTRAN converted from other CAD packages which use a solid element type.
[permalink]
|
| |
|
Average Rating: 10.0 (8 votes)
|
|
|
| |
|
Easing the Strain
|
| |
Glen Hartung
|
| |
Analysis of the Spiderman Theme Park Ride
[permalink]
|
| |
|
Average Rating: 10.0 (2 votes)
|
|
|
| |
|
Economic Method for the Collection of Complex Materials Data for the Design of Microsystems [PDF]
|
| |
Jürgen Wilde, Markus Thoben, Klaus Becker
|
| |
Use of Anand model.
[permalink]
|
| |
|
Average Rating: 10.0 (2 votes)
|
|
|
| |
|
EFATIGUE
|
| |
Hursha Narayan (Robert Bosch Corporation)
|
| |
"I wrote this macro to make fatigue life prediction in Ansys more interactive and also to plot damage accumulation in a structure. The macro works under Unix environment or with Unix utilities in Windows. The user has to make appropriate changes (very minimal) to the macro for it to work. I'm also including a sample file that the macro uses to direct the user how to input material properties."
[permalink]
|
| |
|
Average Rating: 9.2 (42 votes)
|
|
|
| |
|
Effect of Package Design and Layout on BGA Solder Joint Reliability of an Organic C4 Package
|
| |
Biju Chandran, Deepak Goyal, and Jeffrey Thomas
|
| |
"Ball Grid Array (BGA) is currently the interconnect of choice for attaching microprocessors on a printed circuit board (PCB). The reliability of solder joints is one of the critical issues in BGA surface mount technology (SMT). During reliability testing, BGA fatigue failures were observed on test vehicles (TV). Finite element analysis and physical failure analysis were used to determine the risk to the product in the field. As part of this effort, parametric finite element analysis was carried out to determine the effect of design features like the package size, and BGA pattern on the propensity of fatigue failure. The results of the finite element analysis and physical failure analysis showed that the risk to fatigue failure was much greater on a peripheral / partial grid array package than in a full grid array package."
[permalink]
|
| |
|
Average Rating: 10.0 (3 votes)
|
|
|
| |
|
Effect of Simulation Methodology on Solder Joint Crack Growth Correlation
|
| |
Robert Darveaux
|
| |
"A generalized solder joint fatigue life model for surface
mount packages was previously published in Refs [1,2]. The
model is based on correlation to measured crack growth data
on BGA joints during thermal cycling. It was subsequently
discovered by Anderson et.al. that the ANSYS TM 5.2 finite
element code used in the model had an error in its method for
calculating plastic work [3]. It was shown that significant
error in life prediction could result by using a recent version
of the code where the bug has been fixed. The error comes
about since the original crack growth constants were derived
based on plastic work calculations that had the bug.
In this paper, crack initiation and growth constants are re-calculated
using ANSYS 5.6. In addition, several other
model related issues are explored with respect to the crack
growth correlations. For example, 3D slice models were
compared to quarter symmetry models. Anand’s constitutive
model was compared with Darveaux’s constitutive model. It
was shown that the crack growth rate dependence on strain
energy density always had an exponent of 1.10 +/- 0.15. This
is in the range of the original correlation, so the accuracy of
relative predictions should still be within +/- 25%. However,
the accuracy of absolute predictions could be off by a factor
of 7 in the worst case, if the analyst uses a modeling
procedure that is not consistent with that used for the crack
growth correlation. The key to good accuracy is to maintain
consistency in the modeling procedure."
[permalink]
|
| |
|
Average Rating: 10.0 (6 votes)
|
|
|
| |
|
Effects of Nonlinear Geometric and Material Properties on the Seismic Response of Fluid/Tank Systems
|
| |
He Liu, Daniel H. Schubert
|
| |
"To explore the effects large deformation and nonlinear material properties have on the seismic response of fluid/tank systems, the computer program ANSYS was selected to develop a Finite Element Analysis (FEA) model of a ground level, cylindrical steel shell and roof tank structure with contained fluid under seismic load. The ANSYS program was selected for its ability to include shell and structural steel elements, contained fluid elements, fluid-structure interactions, material and geometric nonlinearities, and contact type elements. For purposes of this study, analysis results from a linear elastic, small deformation fixed base model are compared with an elasto-plastic material property model with large deformation assumptions. Results show the significant difference in results based on the assumptions used and indicate that current design code based values may not be conservative in resultant loading calculations."
[permalink]
|
| |
|
Average Rating: 10.0 (34 votes)
|
|
|
| |
|
elastdata_Unix.zip
|
| |
Hursha Narayan (Robert Bosch Corporation)
|
| |
Macro for a fully automated procedure for calculating M-R coefficients from Test Data
"I have developed a macro that fully automates the importing of elastomer test data into ANSYS and calculate the Mooney-Rivlin coefficients. The macro uses Lagrange interpolation technique to calculate the stress data at equal intervals of strain. This can then be read into an array in ANSYS to evaluate the M-R coeffs. I'm sending you Windows and Unix version of the macro. The difference between the two versions are in the awk and script files that I use to manipulate data. The user needs to go through all the files just to change the directories where the files will be located and accessed. The files reformat(Unix) and reformat.csh(windows) should have rwx permissions. The reformat.csh used in windows can be converted to a batch file. Awk utility should be available under windows. The procedure expects Simple Tension, Planar Tension and Biaxial Extension data to be available."
Windows version can be downloaded here.
[permalink]
|
| |
|
Average Rating: 6.2 (8 votes)
|
|
|
| |
|
Elastic Foundation Stiffness
|
| |
Sheldon Imaoka (ANSYS, Inc.)
|
| |
Short explanation of what elastic foundation stiffness (SURF154) is and how to calculate the resulting stiffness for non-planar cases. In Workbench Mechanical, this feature is referred to as an "Elastic Support".
[permalink]
|
| |
|
Average Rating: 9.3 (7 votes)
|
|
|
| |
|
ELBOW290
|
| |
Sheldon Imaoka (ANSYS, Inc.)
|
| |
Attached is a simple, made-up example demonstrating use of ELBOW290 elbow element. There are 3 layers defining the pipe (plasticity and hyperelasticity). The pipe is rotated until local buckling occurs. An image of the file shape (showing the pipe in 3D) is here.
[permalink]
|
| |
|
Average Rating: 8.3 (12 votes)
|
|
|
| |
|
Electromagnetic, Thermal, and Structural Analysis of RF Cavities Using ANSYS
|
| |
N. Hartman, R. A. Rimmer
|
| |
"We report on techniques developed for producing electromagnetic, thermal, and structural solutions to RF cavity design problems in ANSYS, using one model. Methods for preparing imported geometry from solid modeling programs are discussed, and meshing techniques are suggested. A study of mesh density is presented, comparing mesh size with heat flux and Q factor convergence. The general analysis protocol is presented in a stepwise fashion, describing the macros that are used for conducting RF calculations. Finally, these techniques are applied to a proposed RF cavity for the NLC damping rings, which is shown as an example."
[permalink]
|
| |
|
Average Rating: 10.0 (13 votes)
|
|
|
| |
|
Electromechanical analysis of micromechanical SOI-fabricated RF resonators
|
| |
T. Lamminmaki, K. Ruokonen, I. Tittonen, T. Mattila, O. Jaakkola, A. Oja, H. Seppa, P. Seppala, and
|
| |
"In this paper, finite element method (FEM) simulations are used to model mechanical properties of MEMS resonators. Using a static displacement analysis the effective spring constant and mass are calculated. Nonlinearity of the mechanical restoring force is simulated to analyze large amplitude behavior of the resonator."
[permalink]
|
| |
|
Average Rating: 10.0 (5 votes)
|
|
|
| |
|
Electromechanical Transducer Element for MEMS Analysis in ANSYS [PDF]
|
| |
Miklos Gyimesi, Dale Ostergaard
|
| |
Presented at MSM 1999. (MEMS)
[permalink]
|
| |
|
Average Rating: 10.0 (2 votes)
|
|
|
| |
|
ELEM2PT
|
| |
S. Evans (University of New South Wales)
|
| |
"I made a quick n' dirty macro a while ago for finding the element centroid nearest to a point...it doesn't QUITE solve the problem, since adjacent elements differing greatly in size can screw things up. But here it is anyway...it's a brute-force job (I used it for a couple of thousand elements)."
[permalink]
|
| |
|
Average Rating: 8.8 (4 votes)
|
|
|
| |
|
Element for Modelling of Interaction Between Foundations and Bedrock in ANSYS Software
|
| |
Radim Cajka, Ondrej Víta
|
| |
"Ansys provides standard solutions to contact
tasks. It is a high-performing computing tool that
offers several modifications, making it possible to
create a new element and adjust the calculation to
individual requirements. When dealing with
specific problems relating to the contact between
the foundation and the foundation soil, it is
possible to create an element that will take into
account the behaviour of a soil layer under the
foundation exposed to shear. The shearing load
can be caused by undermining, concrete creep, or
concrete shrinkage."
Example of user-defined element (older USER100-105)
[ANSYS Nonlinear, version 5.7.1]
[permalink]
|
| |
|
Average Rating: 10.0 (4 votes)
|
|
|
| |
|
ELGROUP
|
| |
John Crawford (Honeywell)
|
| |
"A macro which creates a file of esel commands for the currently selected elements. The macro will prompt the user for the name of the file which will be created. The default name is 'elgroup'."
[permalink]
|
| |
|
| |
|
ELLIPSE
|
| |
Janet Wolf (ANSYS, Inc.)
|
| |
Macro to make creating ellipses easier.
[permalink]
|
| |
|
Average Rating: 9.6 (23 votes)
|
|
|
| |
|
ELSIZE |
| |
ELSIZE, Size, Ndiv, Kshape, Kstr
Provides same functionality of two 'newer' commands: ESIZE, Size, Ndiv and ESHAPE, Kshape, Kstr
[permalink]
|
| |
|
Average Rating: 10.0 (2 votes)
|
|
|
| |
|
Email Notification after Batch Run
|
| |
Darren Hodson (AstraZeneca)
|
| |
Information on automatic email notification after batch run is completed.
[permalink]
|
| |
|
Average Rating: 8.5 (13 votes)
|
|
|
| |
|
EMF1
|
| |
Mike Yaksh (NAC Int'l)
|
| |
"Example of computing the emf in a coil for a 2D planar model. The last thing on the screen will be a plot of the EMF. This macro cycles
thought difference positions. Some more details on the CEs can be found in the EMAG training guides. One of the problems in the training uses the CEs for a sliding type application. Hope this helps."
Please see updated EMF2 macro.
[permalink]
|
| |
|
Average Rating: 8.8 (21 votes)
|
|
|
| |
|
EMF2
|
| |
Bjoern Possner (VEM motors GmbH)
|
| |
Updated Mike Yaksh's EMF1 macro.
"The older version of the EMF1 macro doesn´t account for the speed or frequency with which the magnet is being mooved under the coil.
In addition, this macro has a correction with the 3600rpm value."
[permalink]
|
| |
|
Average Rating: 7.5 (12 votes)
|
|
|
| |
|
EMID |
| |
EMID,STRAIGHTEN
Straightens elements with midside nodes to force midnode to lie exactly in-between corner nodes.
[permalink]
|
| |
|
Average Rating: 10.0 (5 votes)
|
|
|
| |
|
EMTGEN
|
| |
Vladimir Zhulin (ANSYS, Inc.)
|
| |
TRANS126 elements may be used for simulating fully coupled electrostatic structural coupling between a MEMS device and ground provided the gap distance between the device and the ground is small compared to the overall surface area dimensions of the device. This assumption allows for a point-wise closed-form solution of capacitance between the surface nodes and ground -- ie CAP = EPS*AREA/GAP where EPS is the free-space permittivity, AREA is the area associated with the node, and GAP is the gap between the node and ground. The area for each node is computed using the ARNODE function in ANSYS.
This macro is used to attach TRANS126 elements from a set of surface nodes of a device to ground. The macro generates one TRANS126 element for every surface node. Nodes are created at a specfied offset representing the ground location.
See IN-3D input file for an example.
[permalink]
|
| |
|
Average Rating: 8.9 (22 votes)
|
|
|
| |
|
EngineeringChecker
|
| |
(ANSYS, Inc.)
|
| |
"This file determines if the displacement for a total deformation result is greater than 1/10 of the diagonal of the geometry's bounding box. If it is greater, a comment is added to the "solution" node of the tree. The comment will tell how much greater than the diagonal of the bounding box the displacement is."
One of the sample DesignSpace 6 macros provided, which can be found in the installation directory. Use "Tools > Run Macro" to run this macro.
[permalink]
|
| |
|
Average Rating: 10.0 (8 votes)
|
|
|
| |
|
ENODE |
| |
ENODE,var
Selects all elements attached to (var=0) any currently active nodes or (var=1) all currently active nodes.
[permalink]
|
| |
|
Average Rating: 10.0 (2 votes)
|
|
|
| |
|
ENSIGHT
|
| |
Renato N. Elias (Federal University of Rio de Janeiro)
|
| |
This macro can be used to export tetrahedral meshes to EnSight or ParaView. This macro writes out the mesh information to a file called "jobname.geo".
For use with EnSight, also download accompanying sample EnSight case file.
[permalink]
|
| |
|
Average Rating: 10.0 (4 votes)
|
|
|
| |
|
EORIENT |
| |
EROIENT to reorient SOLID46 is documented at 5.6 but is undocumented at 5.5.
[STI: I haven't had much success with it at 5.5, though.]
[permalink]
|
| |
|
Average Rating: 10.0 (7 votes)
|
|
|
| |
|
EPGEN |
| |
EPGEN ,inum,numincr,estart,eend,eincr,face
Generates/copies pressures.
inum is number of times to perform (>1)
numincr is element number increment
estart,eend,eincr is range of element numbers starting from estart to eend incremented by eincr (can use "all" for estart)
face is element face number
[permalink]
|
| |
|
| |
|
EQSLV |
| |
EQSLV,AMG,toler
Algebraic MultiGrid Solver
Beta at 5.6, released at 5.7.
[STI: Uses CG methods but better scalability for SMP parallel processing]
[permalink]
|
| |
|
Average Rating: 10.0 (1 vote)
|
|
|
| |
|
EQSLV |
| |
EQSLV,DOMAIN,toler
Distributed Domain solver
Beta at 5.6, released at 5.7. At 5.7, this is renamed EQSLV,DDS
[permalink]
|
| |
|
Average Rating: 10.0 (1 vote)
|
|
|
| |
|
EQSLV |
| |
EQSLV,JCGX,toler
Special JCG solver which uses the previous solution as a starting vector for the new solution. Creates a *.full file. Used with THOPT fast thermal solution method.
[permalink]
|
| |
|
| |
|
EQSLV |
| |
EQSLV,SPARSE,,-5
Provides much more detailed information (performance stats, debug info) related to the sparse solver at 5.5 & 5.6. In versions 5.7 and above, this has been changed to the BCSOPTION command
EQSLV,SPARSE,pvttol,-1
The PVTTOL value is the pivot tolerance value. Diagonal terms of the stiffness matrix are compared to the largest value (MAX) such that if the term is < MAX * PVTTOL, pivoting for that row is delayed. PVTTOL defaults to 0.0 and should be less than 0.1.
MKL_NPROCS environment variable
The MKL_NPROCS environment variable can be set to the number of processors for parallelization of the sparse solver at 5.6.2 and 5.7 on Windows NT only. (Other platforms do not need this environment variable)
[STI: This is NOT needed at 5.7.1 and above on Windows. Standard use of /config,nproc or the config57.ans file should be used, and this environment variable should be removed.]
[permalink]
|
| |
|
Average Rating: 10.0 (1 vote)
|
|
|
| |
|
ERF
|
| |
Sheldon Imaoka (CSI)
|
| |
This macro creates a table called ERF with error function values.
[permalink]
|
| |
|
Average Rating: 10.0 (2 votes)
|
|
|
| |
|
ESEL |
| |
ESEL,,LAYER,MAT,matno
Selection by presence of non-zero thickness layer with material m. Use "ESEL,,LAYER,,layerno" to select elements with non-zero thickness of layer "layerno".
[permalink]
|
| |
|
Average Rating: 10.0 (3 votes)
|
|
|
| |
|
ESPLIT |
| |
ESPLIT,iel1,iel2,incr
ESPLIT,ALL
Splits all selected (or specified via iel1 and iel2) quad elements to tris.
In previous versions of ANSYS the newly created tri's are not recognized by graphical picking, but you can list them. In order for the database to be correct you have to either (a) issue NMODIF,ALL or (b)CDWRITE and CDREAD the model into a new database. This undocumented command may not be the best solution for every situation but definitely one to know about.
In later versions of ANSYS (5.5 or later), MOPT,SPLIT can be used instead prior to meshing.
[permalink]
|
| |
|
Average Rating: 10.0 (4 votes)
|
|
|
| |
|
ETWRITE |
| |
Write out element types (jobname.etyp)
[permalink]
|
| |
|
Average Rating: 10.0 (2 votes)
|
|
|
| |
|
Evaluation of Acoustic Propagation Paths into the Human Head
|
| |
William D. O’Brien, Jr. and Yuhui Liu
|
| |
"The overall goal has been to develop an acoustic wave propagation model using well-understood and
documented computational techniques that track and quantify an air-borne incident acoustic wave
propagated around, into and in the human head. This model serves as a computational tool to elucidate the
acoustic wave propagation around, into and in the human head. Specifically, the model determines two
features: (1) alternate acoustic propagation paths to the cochlear shell that exist besides the normal air-borne
acoustic propagation path (eardrum-ossical path) through the auditory canal and (2) sound pressure
amplitude in the cochlear shell (relative to the air-borne sound pressure amplitude) via the alternate
propagation paths. A 3D finite-element solid mesh was constructed using a digital image database of an
adult male head. Coupled acoustic-mechanical finite-element analysis (FEA) was used to model the wave
propagation through the fluid-solid-fluid media."
[ANSYS Acoustics, version 6.1]
[permalink]
|
| |
|
Average Rating: 6.7 (3 votes)
|
|
|
| |
|
Example Applications
|
| |
(Pacific Northwest National Laboratory)
|
| |
Examples of use of ANSYS in engineering analysis
[permalink]
|
| |
|
Average Rating: 9.3 (7 votes)
|
|
|
| |
|
Example harmonic analysis using the large mass method [PDF]
|
| |
David Haberman (CSI)
|
| |
Step-by-step instructions on performing an example harmonic analysis using the large mass method.
[permalink]
|
| |
|
Average Rating: 8.4 (22 votes)
|
|
|
| |
|
Examples of using ANSYS in Ship Design
|
| |
(Delta Marine)
|
| |
Examples of using FEA for structural and CFD analyses of ships.
[permalink]
|
| |
|
Average Rating: 9.8 (25 votes)
|
|
|
| |
|
EXPANSION
|
| |
Sheldon Imaoka (ANSYS, Inc.)
|
| |
This is a description of an ANSYS Workbench 13.0 project and the use of the HSFLD242 (hydrostatic fluid) element. It is a fictitious model of the expansion of a tire and subsequent displacement-loading to a rigid surface (e.g., ground). The Workbench archived project is here.
[permalink]
|
| |
|
Average Rating: 9.8 (25 votes)
|
|
|
| |
|
ExportBranchAsShortcut
|
| |
(ANSYS, Inc.)
|
| |
"When run from DesignSpace, this script writes out a JScript shortcut file that can recreate the active branch contents on demand."
One of the sample DesignSpace 6 macros provided, which can be found in the installation directory. Use "Tools > Run Macro" to run this macro.
[permalink]
|
| |
|
Average Rating: 8.8 (4 votes)
|
|
|
| |
|
EXPROFILE |
| |
EXPROFILE,ldtype,load,value,pname,fname,fext
Exports ANSYS data as CFX-Pre profile data.
To export ANSYS data to CFX-Pre, perform the following steps:
- Flag surface or volumetric data to export by an "interface number" with the VAL2 argument of SF,,FSIN,,val2 or BFE,,FVIN,,val2 commands
- Use EXUNIT command to specify units for export.
- Use EXPROFILE command to generate the CFX profile file.
For EXPROFILE, the following are the arguments:
ldtype: SURF or VOLU
load: for ldtype=SURF, DISP, TEMP, or HFLU; for ldtype=VOLU, DISP, FORC, or HGEN
value: surface or volume interface number specified with VAL2 argument of SF,,FSIN or BFE,,FVIN
pname: field name in CFX profile file
fname, fext: filename and extension for CFX profile file
[STI: beta in 9.0, fully documented in 10.0]
[permalink]
|
| |
|
Average Rating: 10.0 (6 votes)
|
|
|
| |
|
EXUNIT |
| |
EXUNIT,ldtype,load,untype,name
Specifies units for export of ANSYS data as CFX-Pre profile data.
To export ANSYS data to CFX-Pre, perform the following steps:
- Flag surface or volumetric data to export by an "interface number" with the VAL2 argument of SF,,FSIN,,val2 or BFE,,FVIN,,val2 commands
- Use EXUNIT command to specify units for export.
- Use EXPROFILE command to generate the CFX profile file.
For EXUNIT, the following are the arguments:
ldtype: SURF or VOLU
load: for ldtype=SURF, DISP, TEMP, or HFLU; for ldtype=VOLU, DISP, FORC, or HGEN
untype: units are either COMM or USER
name: unit name is SI or FT for untype=COMM
[STI: beta in 9.0, fully documented in 10.0]
[permalink]
|
| |
|
Average Rating: 9.4 (8 votes)
|
|
|
| |
|
EZ_RFOR
|
| |
Mitch Voehl (CEC Corporation)
|
| |
This is an ANSYS macro that stores and sums reaction forces for specified/selected nodes into POST26 variables. It will store the x, y, and z translational reaction forces for all selected nodes and then sum them up. Be sure that you have previously set NUMVAR to a sufficiently large value to store all of the reaction forces.
[permalink]
|
| |
|
Average Rating: 10.0 (14 votes)
|
|
|
| |
|
F3D
|
| |
Marcelo A Toledo (Multibrás S.A. Eletrodomésticos)
|
| |
"This is the macro i was writing about (named f3d.mac). For example ,if you want to aplly a pressure force of 450N at 45 degrees just type
"f3d,450,1,1,0". The first argument is the magnitude and the last three are vector components in the same direction of the force . The macro will ask you to pick a area to aplly the force."
[permalink]
|
| |
|
Average Rating: 10.0 (8 votes)
|
|
|
| |
|
FANBOX2
|
| |
(ANSYS, Inc.)
|
| |
Example of use of fan model and forced convection.
[permalink]
|
| |
|
Average Rating: 8.8 (21 votes)
|
|
|
| |
|
Fast Nonlinear Transient Thermal Solver [PDF]
|
| |
(ANSYS, Inc.)
|
| |
Information on the fast nonlinear thermal solution method (THOPT), beta in 5.6 and documented in 5.7
[permalink]
|
| |
|
Average Rating: 10.0 (6 votes)
|
|
|
| |
|
Fatigue Code Benchmark
|
| |
Riccardo Testi (Piaggio & C. spa)
|
| |
A comparison of fatigue codes — LMS Virtual.Lab (Durability), FEMFAT, and MSC.Fatigue — for use with ANSYS
Web version here
[permalink]
|
| |
|
Average Rating: 6.2 (8 votes)
|
|
|
| |
|
FCENT |
| |
FCENT,OFF
For harmonic response analyses using OMEGA or CMOMEGA with CORIOLIS command, one would want Coriolis effects without the load vector. FCENT,OFF turns off the centrifugal forces associated with OMEGA or CMOMEGA. This will be the actual behavior at ANSYS 12.0, so it will not be needed beyond ANSYS 11.0.
[permalink]
|
| |
|
Average Rating: 10.0 (2 votes)
|
|
|
| |
|
FCENTRIF |
| |
FCENTRIF,OFF
Turns off centrifugal force effects. In a stationary frame of reference, centrifugal force is not in the equations of motion; however, it may be included in harmonic analysis at 11.0, so this command will turn that effect off.
[permalink]
|
| |
|
Average Rating: 10.0 (1 vote)
|
|
|
| |
|
FCLEAR
|
| |
Chris Kennedy (Think PEAK, Inc.)
|
| |
Fast /CLEAR of ANSYS database.
[permalink]
|
| |
|
Average Rating: 10.0 (5 votes)
|
|
|
| |
|
FE Analysis of ATLAS: End Cap Support Structure - PSD Spectrum Analysis
|
| |
C.J.Nelson
|
| |
"This report investigates the effect of a PSD (Power Spectral Density) random input load on an
early FE model of the ATLAS EndCap Support Structure. Statistical predictions of the
maximum displacement are presented."
[ANSYS Structural, version 5.3]
[permalink]
|
| |
|
Average Rating: 8.8 (4 votes)
|
|
|
| |
|
FFTDFT
|
| |
Juan Carlos Lancha (OHL, S.A.)
|
| |
From the author:
"These small APDL macros perform Fourier transforms (FFT and DFT) of discrete signals. This procedure
decomposes a time domain signal into a sum of harmonic (frequency domain) signals. It’s a useful
APDL tool when dealing with dynamic and harmonic problems in ANSYS."
[permalink]
|
| |
|
Average Rating: 10.0 (14 votes)
|
|
|
| |
|
FGEN |
| |
FGEN, 2,_ntot,1,_ntot
Generates/copies nodal forces.
[permalink]
|
| |
|
Average Rating: 10.0 (1 vote)
|
|
|
| |
|
FILDEL
|
| |
John Crawford (Honeywell)
|
| |
A macro to remove a fillet radius and connect the neighboring two lines with a sharp corner.
[permalink]
|
| |
|
Average Rating: 10.0 (1 vote)
|
|
|
| |
|
File Compression
|
| |
Sheldon Imaoka (ANSYS, Inc.)
|
| |
Tip on compressing ANSYS files and different compression algorithms and software, such as gzip, zip, bzip2, lzop, and 7-zip.
[permalink]
|
| |
|
Average Rating: 10.0 (2 votes)
|
|
|
| |
|
FindContactsAttachedToParts
|
| |
(ANSYS, Inc.)
|
| |
"This file determines which contacts are associated with each part in a selected model. A comment is added to the "model" node of each active branch in the tree which lists the parts and the contacts associated with it. This macro will only work if the model has more than one part in it."
One of the sample DesignSpace 6 macros provided, which can be found in the installation directory. Use "Tools > Run Macro" to run this macro.
[permalink]
|
| |
|
Average Rating: 8.6 (7 votes)
|
|
|
| |
|
FindFreeStandingPartsInTree
|
| |
(ANSYS, Inc.)
|
| |
"This file determines which parts in a selected model have no contacts associated with it. If the part has no contacts associated with it, that part will be selected in the tree. This macro will only work if the model has more than one part in it.
This macro should be used at the model level or below. It is not intended for use at the project level or for multiple levels."
One of the sample DesignSpace 6 macros provided, which can be found in the installation directory. Use "Tools > Run Macro" to run this macro.
[permalink]
|
| |
|
Average Rating: 10.0 (5 votes)
|
|
|
| |
|
FindPartsWithNoContacts
|
| |
(ANSYS, Inc.)
|
| |
"This file determines which parts in a selected model have no contacts associated with it. If the part has no contacts associated with it, a check is also done to see if any supports are associated with that part. A comment is added to the "model" node of each selected branch in the tree. The comment will contain the names of the parts with no contacts and it will also show an error if those parts have no supports. This macro will only work if the model has more than one part in it."
One of the sample DesignSpace 6 macros provided, which can be found in the installation directory. Use "Tools > Run Macro" to run this macro.
[permalink]
|
| |
|
Average Rating: 10.0 (2 votes)
|
|
|
| |
|
Finite Deformations Of An Earthworm Segment
|
| |
H. Kunz
|
| |
Use of Mooney-Rivlin model.
[permalink]
|
| |
|
| |
|
Finite Element Analysis at Mannesmann VDO Fuel Systems [PDF]
|
| |
Zlatko Penzar
|
| |
PowerPoint presentation
[permalink]
|
| |
|
Average Rating: 8.3 (12 votes)
|
|
|
| |
|
Finite Element Analysis for Solder Ball Connect (SBC) Structural Design Optimization
|
| |
J.S. Corbin
|
| |
"Solder Ball Connect (SBC) is a second-level
surface mount electronics packaging
technology in which ceramic modules
containing one or more chips are joined to a
circuit card (FR-4) by means of an array of
nonhomogeneous solder columns. These
columns consist of a high-temperature-melting
90%Pb/lO%Sn solder sphere attached to the
module and card with eutectic solder fillets.
The solder structures accommodate the bulk
of the strain (which is due to the thermal-
expansion mismatch between FR-4 and the
9211 ceramic of the modules) generated during
power cycling. If the solder structures are not
properly designed, the thermal strain can be a
source of premature fatigue failure. In this
work, finite element analysis is used to
characterize the plastic strains that develop
in the SBC interconnection during thermal
cycling. Since plastic strain is a dominant
parameter that influences low-cycle fatigue, it
is used as a basis of comparison for various
structural alternatives. Designed experiment
techniques are used to systematically evaluate
the thermal strain sensitivity to structural
variables. Results are used to identify an
optimally reliable structure that is robust in
terms of assembly-process variables."
[permalink]
|
| |
|
Average Rating: 10.0 (4 votes)
|
|
|
| |
|
Finite Element Analysis of an AC Solenoid Including the Effects of Harmonic Loading and Magnetic Saturation
|
| |
A. Bax, C. Andersen, M. Yaksh, D. Ostergaard
|
| |
From 1994 Conference
[permalink]
|
| |
|
Average Rating: 9.7 (15 votes)
|
|
|
| |
|
Finite Element Analysis Of Crowning Sealing Caps
|
| |
Henri Champliaud, L Van Ngan
|
| |
"Metal closures, with an integrated gasket, are widely used in the food industry to ensure the sealing of the glass bottles by setting. The success of this bottle-capping is due to the relevant choice of the variables in the manufacturing process. Actually, the effects of the various variables of the process are not precisely understood.""In this paper, the leakage pressure of an assembly, with given parameters of a standard setting operation is predicted. The study is concentrated firstly on the simulation of setting the cap on the bottle, and secondly, on the global distribution of the efforts of contact on the gasket according to the internal pressure. Finally, the leakage pressure of the assembly is determined using practical tests that relate the leakage pressure with the global force exerted on the gasket."
[permalink]
|
| |
|
Average Rating: 7.1 (7 votes)
|
|
|
| |
|
Finite Element Analysis Of Plasticity-Induced Crack Closure For Inclined Cracks
|
| |
L. W. Wei and M. N. James
|
| |
"The contact occurring in inclined cracks is a general contact problem, and thus a general contact analysis must be implemented in which a combined load and displacement control procedure is used. The commercial FE code ANSYS 5.4 used in this work provides the utilities to deal with general contact problems."
[permalink]
|
| |
|
Average Rating: 10.0 (11 votes)
|
|
|
| |
|
Finite Element Analysis To Investigate The Significance Of Functional Gradients In Dental Restorations [PDF]
|
| |
Tan Kok Wai, Alex and Anand Asundi
|
| |
Use of SOLID46 element.
[permalink]
|
| |
|
Average Rating: 10.0 (4 votes)
|
|
|
| |
|
Finite Element Based Reduced Order Modeling of MEMS [PDF]
|
| |
Dale Ostergaard, Miklos Gyimesi
|
| |
Presented at MSM 2000. (MEMS)
[permalink]
|
| |
|
Average Rating: 10.0 (1 vote)
|
|
|
| |
|
Finite Element Based Solder Joint Fatigue Life Predictions for a Same Die Stacked Chip Scale Ball Grid Array Package
|
| |
Bret Zahn
|
| |
"Viscoplastic finite-element simulation methodologies were utilized to predict solder joint reliability for a same die size, stacked, chip scale, ball grid array package under accelerated temperature cycling conditions (-40C to +125C, 15min ramps/15min dwells). The effects of multiple die attach material configurations were investigated along with the thickness of the mold cap and spacer die. The solder structures accommodate the bulk of the plastic strain that is generated during accelerated temperature cycling due to the thermal expansion mismatch between the various materials that encompass the stacked die package. Since plastic strain is a dominant parameter that influences low-cycle fatigue, it was used as a basis for evaluation of solder joint structural integrity. The paper discusses the analysis methodologies as implemented in the ANSYS finite element simulation software tool and the corresponding results for the solder joint fatigue life. Some ANSYS parametric design language commands are included for the benefit of those readers who are familiar with the tool."
[permalink]
|
| |
|
Average Rating: 9.7 (15 votes)
|
|
|
| |
|
Finite Element Limit Load Analysis of Thin-Walled Structures by ANSYS (Implicit), LS-DYNA (Explicit) and in Combination
|
| |
Wilhelm Rust
|
| |
"After discussing general properties of implicit Finite Element analysis using ANSYS and explicit analysis
using LS-DYNA it is shown when and how quasi-static limit load analyses can be performed by a transient
analysis using explicit time integration. Then we focus on the remaining benefits of implicit analysis
and how a proper combination of ANSYS and LS-DYNA can be used to prepare the transient analysis by
common preprocessing and static analysis steps. Aspects of discretization, solution control, consideration
of imperfections and methods of checking the results are outlined."
[ANSYS LS-DYNA, Nonlinear, version unspecified]
[permalink]
|
| |
|
Average Rating: 6.2 (4 votes)
|
|
|
| |
|
Finite Element Method Analysis Of Non-Linear Behaviour Of Implants And Stents [PDF]
|
| |
J. Awrejcewicz, M. Ciach, K. Wlodarczyk
|
| |
Example of using ANSYS for stent application (Mooney-Rivlin and kinematic hardening plasticity).
[permalink]
|
| |
|
Average Rating: 10.0 (6 votes)
|
|
|
| |
|
Finite Element Modeling of Capacitor Micromachined Ultrasonic Transducers
|
| |
Yongrae Roh and Butrus T. Khuri-Yakub
|
| |
"A finite element model of cMUTs is constructed using the commercial code ANSYS. The complex load impedance seen by individual cells is compared with the plane wave real impedance seen by a parallel combination of the cells to make a transducer. The result shows the origin and level of crosstalk between array elements, with evidence of coupling through Stoneley and Lamb waves." (acoustics)
[permalink]
|
| |
|
Average Rating: 8.8 (8 votes)
|
|
|
| |
|
Finite Element Modeling Of Damage Accumulation In Bolted Composite Joints Under Incremental Tensile Loading
|
| |
Th. Kermanidis, G. Labeas, K.I. Tserpes and Sp. Pantelakis
|
| |
"A three-dimensional progressive damage model was developed in order to simulate the damage accumulation of bolted single-lap composite joints under in-plane tensile loading. The parametric study includes stress analysis, failure analysis and material property degradation. Stress analysis of the three-dimensional geometry was performed using the ANSYS FE code. Failure analysis and degradation of material properties were implemented using a progressive damage model, which is incorporated in an ANSYS macro-routine."
[permalink]
|
| |
|
Average Rating: 8.3 (21 votes)
|
|
|
| |
|
Finite Element Modeling of Elastic Modulus in Ductile Irons: Effect of Graphite Morphology
|
| |
S.H. Pundale, R.J. Rogers, G.R. Nadkarni
|
| |
"This investigation is the first to deal with the modeling and prediction of effective elastic modulus of ductile irons using finite elements. Both plane stress and axisymmetric formulations were used to predict elastic moduli. With finite elements, it is possible to include microstructural parameters that are extremely difficult or impossible to model analytically. Assuming that the graphite nodules act as voids, the effective elastic modulus was modeled by considering the effect of small strains for nodule variables of volume fraction, shape, size and distribution. (No matrix variables have been considered.)"
[permalink]
|
| |
|
Average Rating: 6.2 (4 votes)
|
|
|
| |
|
Finite Element Modeling of Human Artery Tissue with a Nonlinear Multi-Mechanism Inelastic Material
|
| |
Sergey Sidorov
|
| |
"In this dissertation, a nonlinear multi-mechanism inelastic material model is formulated for modeling vascular tissue, collagen recruitment and elastin degradation. The model is implemented into the commercial finite element software package ANSYS with user programmable features."
ANSYS 10.0, USERMAT
[permalink]
|
| |
|
| |
|
Finite Element Predictions of Plasticity-Induced Fatigue Crack Closure in Three-Dimensional Cracked Geometries
|
| |
Jeffrey Skinner, Jr.
|
| |
"Elastic-plastic finite element analyses were performed to predict the crack opening level profiles in semi-elliptical surface cracks."
[permalink]
|
| |
|
Average Rating: 8.6 (21 votes)
|
|
|
| |
|
Finite Elements for Thermoelectric Device Analysis in ANSYS
|
| |
Elena Antonova and David Looman
|
| |
"A new set of ANSYS coupled-field elements enables users to accurately and efficiently analyze thermoelectric devices. This paper reviews the finite element formulation, which, in addition to Joule heating, includes Seebeck, Peltier, and Thomson effects. Examples of steady-state and transient simulations of a thermoelectric generator and a single-stage Peltier cooler are presented for thermoelectric analysis verification. An analysis of a multistage thermoelectric cooler is performed to demonstrate ANSYS parametric analysis capability."
[permalink]
|
| |
|
Average Rating: 9.2 (6 votes)
|
|
|
| |
|
FINS
|
| |
Mike Rife (CSI)
|
| |
This macro is used to create a long cylinder with a radial, helical fin
[permalink]
|
| |
|
Average Rating: 8.8 (4 votes)
|
|
|
| |
|
First Micromachined Silicon Load Cell for Loads up to 1000 kg
|
| |
Henk Wensink, Meint J. de Boer, Remco J. Wiegerink, Robert A.F. Zwijze, Miko C. Elwenspoek
|
| |
"In this paper, a bulk micromachined silicon load cell is presented, designed for loads up to 1000 kg. ANSYS simulations were used to determine the load cell dimensions and strain gauge positions."
See related paper.
[permalink]
|
| |
|
Average Rating: 10.0 (1 vote)
|
|
|
| |
|
FIX
|
| |
Kannan Sundararajan (General Electric-Power Systems)
|
| |
This macro uses the %_FIX% parameter to fix a particular nodal component after a load step.
For details on %_FIX%, see the Commands online help for the "D" command.
[permalink]
|
| |
|
Average Rating: 2.5 (6 votes)
|
|
|
| |
|
FIXDIVS
|
| |
James Kosloski (CAEAI)
|
| |
"I have attached a macro that changes the 'next' divisions for all the meshed lines to the same as the current mesh divisions. So you can run this macro then choose /psym,ldiv,0"
[permalink]
|
| |
|
Average Rating: 10.0 (1 vote)
|
|
|
| |
|
FIXIT
|
| |
Bill Bulat (ANSYS, Inc.)
|
| |
"I noticed that the only nodes that get moved back to the halfway point were those on the "source" area meshed with 200s. All the other nodes along the crack front wound up at the quarter point, as intended. If VEXT is not an
option, try the I'm attached "fixit" macro that allows node relocation as follows:
- MODM,NOCH
- relocate nodes on the meshed area back to the quarter point
- MODM,CHEC
To see how it works:
- Enter prep7
- Run the macro. You'll be prompted to pick the crack node, then one (only one) of the corner nodes around the crack node, then the midside node
between them. The macro relocates the midside node. Repeat until all midside nodes are relocated to the quarter point.
[permalink]
|
| |
|
Average Rating: 3.3 (9 votes)
|
|
|
| |
|
FLDATA |
| |
FLDA,C2TA,MOME,0.0
FLDA,C2TA,PRES,0.0
Zero out damping term in momentum and pressure equations for a Flotran run.
[STI: I think C2TA is referring to the perturbation term in Eqn 7.2-10 in the Theory Manual -- the command minimizes diffusive term in transport equation (?)]
[permalink]
|
| |
|
Average Rating: 8.6 (7 votes)
|
|
|
| |
|
FLDSURF (new)
|
| |
Jeroen Valensa (Modine Mfg. Co.)
|
| |
From the author:
"The reason for not using the afsurf macro is that it takes so long to generate the elements - on very large thermal models I have seen that
method take 12 hours, where my macro will do the same thing in about 15 minutes. The way to do the coupling is to create the surf152 elements
first, using esurf. Select the solid elements over which the 152's will be overlaid, and select the nodes on the surfaces of the solid elements
where you want the 152's to be created. Set the type, mat, and real. Change keyopt 5 to 0 (no extra node) - this will be changed back to 1 by
the macro. Then just issue the esurf command, with nothing after it (no extra node assignment). Now you are almost ready to run the macro!
Just select the NODES of the fluid116 elements and the surf152 ELEMENTS. An easy way to do this in your model would be:
esel,s,type,,9
nsle
esel,s,type,,8
Now run the macro, it will automatically map the closes fluid node to
each surf152 element to be the extra node for that element. It may take
a while if you have a large number of 116s and 152s, so just be patient.
You won't get any feedback while it is running."
[permalink]
|
| |
|
Average Rating: 10.0 (1 vote)
|
|
|
| |
|
FLDSURF (old)
|
| |
Simon Shang (Aerojet Propulsion), slightly modified by Jeroen Valensa (Modine Mfg. Co.)
|
| |
Another way of defining SURF152 elements with FLUID116 instead of using AFSURF. Use component names for surface area and line as input arguments to this macro.
Original XANSYS posting
[permalink]
|
| |
|
Average Rating: 10.0 (3 votes)
|
|
|
| |
|
Flip Chip Reliability Modeling Based on Solder Fatigue as Applied to Flip Chip on Laminate Assemblies
|
| |
Scott Popelar, Michael Roesch
|
| |
"A 63Sn/Pb solder fatigue model has been previously developed based on a correlation of flip chip solder fatigue data combined with nonlinear finite element analysis. This model has been successfully applied in the prediction of PBGA and CSP fatigue lives as well as a parametric study investigating the reliability of flip chip assemblies and the influence of specific design parameters. In this investigation, flip chip reliability predictions are generated based on solder fatigue modeling and compared to actual thermal cycling reliability data. The influence of both solder fatigue and underfill delamination are considered in interpretation of the experimental data."
[permalink]
|
| |
|
Average Rating: 9.3 (7 votes)
|
|
|
| |
|
Floating Metal Plane on Thermal and Electrical Performance of an Enhanced Plastic Ball Grid Array Package
|
| |
Humayun Kabir, Richard Groover, David Tovar and Joe Joroski
|
| |
"Three-dimensional finite element models of a cavity down thin and thermally enhanced BGA (T2BGA) package have been developed using ANSYS. This model has been used for thermal characterization of the above package under different cooling (airflow) conditions and to investigate the effects of heat spreader thickness on package junction to ambient thermal resistances for no airflow condition."
[permalink]
|
| |
|
Average Rating: 10.0 (5 votes)
|
|
|
| |
|
FLOHGEN
|
| |
(ANSYS, Inc.)
|
| |
Transfers joule heating loads from a harmonic analysis to Flotran analysis.
[permalink]
|
| |
|
Average Rating: 10.0 (6 votes)
|
|
|
| |
|
FLOTRAN Chills Out Hot Aerospace Electronics
|
| |
Mark Troscinski, Jiang Guangnan, Zhang Minyi
|
| |
Examples of use of Flotran for electronics applications.
From ANSYS Solutions, Vol. 4 Number 2.
[permalink]
|
| |
|
Average Rating: 9.4 (8 votes)
|
|
|
| |
|
Flotran conjugate heat transfer tips
|
| |
Sheldon Imaoka (CSI)
|
| |
Tips on settings to use in Flotran for conjugate heat transfer problems. (From XANSYS posting)
[permalink]
|
| |
|
Average Rating: 9.3 (23 votes)
|
|
|
| |
|
Flotran Enhancements at 6.0 [PDF]
|
| |
Sheldon Imaoka (ANSYS, Inc.)
|
| |
"There have been several enhancements to Flotran at 6.0. These changes include more robust default settings, an additional advection scheme, a new coupling algorithm, and improvements to the ALE mesh morpher."
(Week 10, week of 12/10/01.)
[permalink]
|
| |
|
Average Rating: 10.0 (8 votes)
|
|
|
| |
|
Flotran natural convection tips
|
| |
Mark Troscinski (ANSYS, Inc.)
|
| |
Tips on settings to use in Flotran for natural convection problems. (From XANSYS posting)
[permalink]
|
| |
|
Average Rating: 10.0 (12 votes)
|
|
|
| |
|
FLOTRAN_THERM
|
| |
Brad Lamirand (Cooper Turbocompressor)
|
| |
Here is a quick example of sequential fluid [Flotran] to thermal coupled field analysis.
[permalink]
|
| |
|
Average Rating: 8.8 (73 votes)
|
|
|
| |
|
FLUID_PRES
|
| |
Sheldon Imaoka (CSI)
|
| |
Example showing 'fluid pressure' contact, beta at 5.6.
[permalink]
|
| |
|
Average Rating: 9.3 (34 votes)
|
|
|
| |
|
FLUID116 Example
|
| |
Sheldon Imaoka (ANSYS, Inc.)
|
| |
A very simple example showing how to generate FLUID116 and connect it to a thermal solid (SOLID70 in this case) via SURF152 using the AFSURF command.
[permalink]
|
| |
|
Average Rating: 10.0 (7 votes)
|
|
|
| |
|
FLUID66
|
| |
FLUID66 "Thermal-Fluid Pipe" was undocumented around 5.6. It should be replaced with FLUID116.
[permalink]
|
| |
|
| |
|
FORCED_CONV
|
| |
Sheldon Imaoka (CSI)
|
| |
Simple forced convection problem of heated fins, 2D tri. Just modified CONV_FINS example.
[permalink]
|
| |
|
Average Rating: 6.2 (4 votes)
|
|
|
| |
|
Formatting output text of results (PRxxxx family of commands) [PDF]
|
| |
Sheldon Imaoka (CSI)
|
| |
This memo outlines some of the options available in ANSYS to produce and to format output listings: (1) the use of the /FORMAT statement with the PRxxxx series of commands and (2) the application of *VWRITE to create custom output.
[permalink]
|
| |
|
Average Rating: 9.8 (22 votes)
|
|
|
| |
|
FOUNDATION
|
| |
Sheldon Imaoka (ANSYS, Inc.)
|
| |
A very simple example comparing use of SURF154 elastic foundation stiffness (EFS real constant) with force-distributed constraints (using MPC-based 17x contact elements) tied to a COMBIN14 spring element.
[permalink]
|
| |
|
Average Rating: 10.0 (11 votes)
|
|
|
| |
|
FRICTION_TEST2
|
| |
Brent Bristol (SpeedFam-IPEC)
|
| |
From the author: "The following macro demonstrates a method for obtaining friction forces directly from a contact interface [and restart capability]."
[permalink]
|
| |
|
Average Rating: 9.2 (38 votes)
|
|
|
| |
|
FSUM |
| |
FSUM,,CONT
Sums contact forces only for CONTA171-174 (at 5.6.1)
[permalink]
|
| |
|
Average Rating: 9.1 (16 votes)
|
|
|
| |
|
FTST |
| |
FTST,SEQV
Uses equivalent stress in fatigue calculations. Issue prior to FTCALC command. [5.4]
[permalink]
|
| |
|
Average Rating: 6.6 (16 votes)
|
|
|
| |
|
FTST |
| |
FTST,SINT
Uses stress intensity in fatigue calculations. Issue prior to FTCALC command. [5.4]
[permalink]
|
| |
|
Average Rating: 10.0 (9 votes)
|
|
|
| |
|
Full Graphics vs. PowerGraphics Comparison
|
| |
(CAEAI)
|
| |
A comprehensive comparison of Full Graphics vs. PowerGraphics and the effect of setting different options.
PDF file can also be downloaded here
[permalink]
|
| |
|
Average Rating: 10.0 (13 votes)
|
|
|
| |
|
Fully Automatic Adaptive Mesh Refinement Integrated into the Solution Process
|
| |
Joseph R. Tristano, Zhijan Chen, D. Alfred Hancq, Wa Kwok
|
| |
"Finite element analysts and designers need to feel confident in the results of their analyses before sending a product to prototype or production. Mesh discretization can greatly influence the desired results. In this paper we present framework for adaptive mesh refinement to obtain FEA results with a desired accuracy. The process involves adaptively refining the mesh based on solution error norms until the result desired converges to certain accuracy. The adaptive refinement/meshing process must be fully automatic and very robust. We present an exhaustive method to create a fully automatic and integrated process that takes advantage of many of the mesh refinement and mesh optimization algorithms found in literature. The results of the process provide the user with the desired accuracy in the smallest number of iterations possible."
[Workbench Simulation, version 7.1]
[permalink]
|
| |
|
Average Rating: 7.5 (2 votes)
|
|
|
| |
|
FXFRM08
|
| |
Bill Bulat (CSI)
|
| |
Produces fourier transform of time domain response.
[permalink]
|
| |
|
Average Rating: 10.0 (5 votes)
|
|
|
| |
|
G_MUR
|
| |
Mike Yaksh (NAC Int'l)
|
| |
Loads the murx from the results for the active elements into material sets matching the element number +100 generates the macro chg_mat.mac
[permalink]
|
| |
|
| |
|
GASKET
|
| |
Sheldon Imaoka (ANSYS, Inc.)
|
| |
Very simple example showing how to use element birth & death to include a non-uniform initial gap. Usually, initial gap for gasket material (TB,GASKET,,,,PARA) is assumed to be a uniform input. By using element birth and death while perturbing the nodes, one can include a non-uniform initial gap.
[permalink]
|
| |
|
Average Rating: 8.3 (3 votes)
|
|
|
| |
|
Gasket Materials
|
| |
(ANSYS, Inc.)
|
| |
Presentation on the gasket materials and companion interface elements, introduced at ANSYS 6.1 (part of the "Advanced Analysis with ANSYS" seminar during the 2002 User's Conference).
[permalink]
|
| |
|
Average Rating: 10.0 (2 votes)
|
|
|
| |
|
GCGEN |
| |
GCGEN, Ccomp, Tcomp, NUMC, RADC, Tlab, Shape
Ccomp
Name of the component containing nodes on the contact surface [CM]. Assemblies are not permitted.
Tcomp
Name of the component containing nodes on the target surface. Assemblies are not permitted.
NUMC
Generate NUMC contact elements whose contact node is closest to the centroid of each target element face. If Shape = TRI, the program will generate 2*NUMC CONTAC49 elements for each quadrilateral target element face. (That is, each triangular contact element base will be connected to NUMC contact nodes.) Defaults to an unlimited number of contact elements generated per target face.
RADC
Generate contact elements whose contact node is within a radius of RADC measured from the centroid of each target element face. Defaults to no limit on the radius.
Tlab
Label to identify the target surface of line or shell elements. The top surface will be used unless Tlab = BOT. Tlab is ignored if the target elements are solids.
Shape
Label that controls the shape of CONTAC49 element bases. Using the TRI feature can sometimes improve contact performance if the target elements have warped quadrilateral faces:
(blank) --
The contact element bases will have the same shape (triangular or quadrilateral) as the corresponding target element faces (default).
TRI --
The contact element bases will always be triangular.
Notes:
Generates 2-D contact (CONTAC48) or 3-D contact (CONTAC49) elements. Each contact element connects nodes on a target element face to a contact node. The "target" end of a contact element is called the contact element base. A target element face is defined as a face on a selected element whose nodes belong to the target component. If the selected element is a solid then the target face must also be external to the model, while for a line or shell element all nodes of the element will belong to the target face. The active element type attribute (TYPE) must be a contact element (CONTAC48 or CONTAC49) and must match the dimensionality of the target element. The other active attributes (MAT, TYPE, REAL, ESYS) will be used for the generated elements. The target elements must be defined before using this command. Midside nodes on target element faces are ignored.
It is highly recommended to use newer CONTA171-175 elements instead of CONTAC48-49.
[permalink]
|
| |
|
Average Rating: 10.0 (1 vote)
|
|
|
| |
|
General ANSYS Tips (5.5)
|
| |
Carl Howard (University of Adelaide)
|
| |
- Where to get help
- Insufficient disk space
- Bulk compression mode
- Choice of solver
- Element Normals
- Boolean operations on solid models
- Meshing
- Loading an array from a file
- Using ETABLE and extracting the results to an array
- Output when using the GUI
- Generating editable WMF figures
[permalink]
|
| |
|
Average Rating: 9.2 (18 votes)
|
|
|
| |
|
Geometrical Aspects of a Hollow-Cathode Magnetron (HCM)
|
| |
Zhehui Wang and Samuel A. Cohen
|
| |
"A hollow-cathode magnetron (HCM), built by surrounding a planar sputtering-magnetron cathode with a hollow-cathode structure (HCS), is operable at substantially lower pressures than its planar-magnetron counterpart... Detailed magnetic field distribution was calculated using the ANSYS code, and confirmed by Hall probe measurements."
[permalink]
|
| |
|
| |
|
GETA4L
|
| |
Mark Fahey (Lingk & Sturzebecher)
|
| |
"Here is a macro that I made for myself to get all areas that have four lines. From these areas I decide what to map mesh."
[permalink]
|
| |
|
Average Rating: 10.0 (7 votes)
|
|
|
| |
|
GETAL
|
| |
John Crawford (Honeywell)
|
| |
Loops through repeated ASLL, LSLA commands
[permalink]
|
| |
|
| |
|
GETDIR
|
| |
Bob Weathers (Trane)
|
| |
Returns string with current working directory
[permalink]
|
| |
|
Average Rating: 5.0 (1 vote)
|
|
|
| |
|
GETEN
|
| |
John Crawford (Honeywell)
|
| |
A macro to loop through the esln and nsle commands to select related nodes/elements
[permalink]
|
| |
|
Average Rating: 10.0 (1 vote)
|
|
|
| |
|
GETFACE
|
| |
Sheldon Imaoka (ANSYS, Inc.)
|
| |
This is a simple macro to group tetrahedral elements into element components based on the face number (1-4) that is exposed in selected surface(s). When using this macro, be sure that only a single face for a given element is exposed on selected surfaces.
This is useful for the EDLOAD command using ANSYS LS-DYNA when applying pressures since element faces must be used. Can also be used for general elements with the SFE command.
Feel free to customize/modify the macro for other element shapes (pyramid, wedge, hex) by increasing the number of faces checked.
[permalink]
|
| |
|
| |
|
GETFILE
|
| |
Matthew Sutton (PADT)
|
| |
Tcl script which opens a dialog box for a user to select an input file to read from (/INPUT).
Use ~eui,'source getfile.tcl' to run the Tcl script, after saving it to your working directory.
[permalink]
|
| |
|
Average Rating: 9.7 (15 votes)
|
|
|
| |
|
GETLK
|
| |
John Crawford (Honeywell)
|
| |
Loops through repeated LSLK, KSLL commands
[permalink]
|
| |
|
| |
|
GETMASS
|
| |
Sheldon Imaoka (CSI)
|
| |
This is a macro which *GET density and volume of selected elements and provides total volume and total mass of selected elements.
May be useful for 2D axisymmetric elements, too.
See Tips section for CSI's Tip of the Week on mass property calculation.
[permalink]
|
| |
|
Average Rating: 10.0 (8 votes)
|
|
|
| |
|
GETPATHNAME
|
| |
James Kosloski (CAEAI)
|
| |
There exists a *GET to get pathname based on path number. However, this macro gets the current pathname in case you don't know what the path number is.
[permalink]
|
| |
|
Average Rating: 10.0 (2 votes)
|
|
|
| |
|
GETREAL
|
| |
Bob Weathers (Trane)
|
| |
An example of how to parse through real constants which have been previously defined.
[permalink]
|
| |
|
Average Rating: 10.0 (2 votes)
|
|
|
| |
|
GETSELTOL
|
| |
James Kosloski (CAEAI) and Bram Weisman (SBM Atlantia)
|
| |
"This macro gets the current value of SELTOL and stores it in the parameter SELTCUR"
[permalink]
|
| |
|
| |
|
GETTRIS
|
| |
Sheldon Imaoka (ANSYS, Inc.)
|
| |
This macro searches for triangular elements in the selected element set. It then puts the number of triangular elements in a scalar parameter and selects those triangular elements (if any).
[permalink]
|
| |
|
Average Rating: 6.0 (5 votes)
|
|
|
| |
|
GETVA
|
| |
John Crawford (Honeywell)
|
| |
Loops through repeated VSLA, ASLV commands
[permalink]
|
| |
|
Average Rating: 10.0 (1 vote)
|
|
|
| |
|
GMFACE |
| |
GMFACE,FINE,n
Same function as /FACET,FINE,n above, controls tesselation of area where n is from 0 (coarsest, default) to 10 (finest). For XOX Shapes geometry only (IGES default importing or Connection Kit "Allow defeature" importing) [5.5, documented in 5.6 in Errata]
The GMFACE command can be issued before the default IGES import, or after import in TOPO REPAIR. In TOPO REPAIR, you can issue the command repeatedly (with APLOTs in between) until the desired level of refinement has been achieved. Once you end TOPO REPAIR (by pressing FINISH or issuing GAPFINISH), the GMFACE command has no effect.
[permalink]
|
| |
|
Average Rating: 10.0 (2 votes)
|
|
|
| |
|
GPLT
|
| |
Eric Miller (PADT)
|
| |
Simplified interface for GPLOT command
[permalink]
|
| |
|
| |
|
Graphics Startup |
| |
GRPHENTR=1 in config56.ans
Allows startup of GUI mode without requiring the "-g" option when using command "ansys56".
[permalink]
|
| |
|
| |
|
Grayscale colormap
|
| |
Juha Tyllinen (KONE Corporation)
|
| |
Color map (contours) which uses grayscale. Use /cmap,jkt,cmap to read in file.
[permalink]
|
| |
|
Average Rating: 9.1 (63 votes)
|
|
|
| |
|
Greyscale colormap
|
| |
John Thompson (ANSYS, Inc.)
|
| |
Color map file to produce grayscale contours. Use /cmap,greyscl.cmap to read this file in.
[permalink]
|
| |
|
Average Rating: 8.0 (38 votes)
|
|
|
| |
|
GRPH2SVG
|
| |
Sheldon Imaoka (ANSYS, Inc.)
|
| |
This is a quick hack I did to generate SVG files from within ANSYS. There are 3 macros contained in the zip file: GRPH2SVG.MAC is the main one, and the other two are called by GRPH2SVG.The macro redirects the plot to an ANSYS Graphics file "stiplot.grph". Then, the macro parses through the GRPH file and generates an SVG file called "stiplot.svg". You can change the font, font size, etc. as you see fit from within the macro. (For details on the contents of the GRPH file, refer to the ANSYS Programmer's Guide for details.)Because this parses the GRPH file from within ANSYS, it is slow for complex plots, so I recommend using it only for XY plots — this is only meant to serve as an example of what can be done with APDL and reading the GRPH file contents. Also, I did not bother including support for raster graphics - this macro only supports vector graphics. (If you want raster graphics, use of PNG is better. SVG is really a vector graphics implementation.)
If you're running Firefox, or if you use Internet Explorer and have the Adobe SVG Viewer Plug-in, you can see a sample contour plot and sample XY plot generated from this macro.Because this was created by hand, there may be mistakes - you can let me know if you encounter any. Otherwise, instead of using this macro, you can create an EPS file and use your favorite illustration software to convert it to an SVG file.
[permalink]
|
| |
|
Average Rating: 10.0 (3 votes)
|
|
|
| |
|
GSCONTOURS
|
| |
Darrel Hill (University of Saskatchewan)
|
| |
Macro (not CMAP file) to create grayscale contours.
"I coded this version only for the win32C (X11c) Graphics device. **Will not work at all with the default win32 (X11)**. Contours in contour plots should have 100 shades of grey with the default input. Parameters can be changed in the code to darken, lighten and/or make more/less shades of grey."
[permalink]
|
| |
|
Average Rating: 10.0 (6 votes)
|
|
|
| |
|
GUIRESET
|
| |
(ANSYS, Inc.)
|
| |
Sometimes, it is reported that the Picker does not respond at 7.1. This macro forces a reset of the picker such that it will work again. Also, it provides diagnostic information to send to ANSYS, Inc.
Use the attached macro as follows:
- In ANSYS GUI, issue "guireset" and execute the macro.
- Then when the picker box gets stuck issue "Ctrl-Shift-Delete".This should free up the picker.
- Ask user to send us the diagnostic information from the ANSYS output window such as below along with details of what he/she was doing when this problem occured:
#### PLEASE REPORT THIS INFORMATION ####
trace for EventType?
{w {::namespace inscope ::euidl::graphicPicking resolveEventType}}
IgnoreCancel value is 1
PARAMETER _BUTTON = 0.000000
TURN OFF WORKING PLANE DISPLAY
#### THANK YOU, AND SORRY FOR THE INCONVENIENCE ####
[permalink]
|
| |
|
Average Rating: 7.7 (49 votes)
|
|
|
| |
|
HARM_FULL_EX
|
| |
David Haberman (CSI)
|
| |
Direct displacement method (full harmonic with applied displacment).
Modal analysis then frequency sweep.
Results are scaled to get acceleration, displacement, and g's vs frequency.
[permalink]
|
| |
|
Average Rating: 9.8 (45 votes)
|
|
|
| |
|
HARM_LMM
|
| |
David Haberman (CSI)
|
| |
Harmonic linear Sweep Example. Modal super position with the large mass method was the solution technique.
[permalink]
|
| |
|
Average Rating: 10.0 (15 votes)
|
|
|
| |
|
HARM_LMM_CLUST
|
| |
David Haberman (CSI)
|
| |
Harmonic linear Sweep Example. Modal super position with the large mass method was the solution technique. The cluster option was used to allow for enough resolution around the natural freq.
[permalink]
|
| |
|
Average Rating: 10.0 (11 votes)
|
|
|
| |
|
HARM_LMM_SPEC
|
| |
David Haberman (CSI)
|
| |
Harmonic Log Sweep Example. Allows a user to input varibles that are consistent with design spec. Modal super position with the large mass method was the solution technique.
[permalink]
|
| |
|
Average Rating: 10.0 (15 votes)
|
|
|
| |
|
HARMC_EMM
|
| |
Mohammad Gharaibeh (State University of New York at Binghamton)
|
| |
Example of a harmonic response analysis (linear sweep) of a plate using mode-superposition method with enforced motion.
[permalink]
|
| |
|
Average Rating: 10.0 (3 votes)
|
|
|
| |
|
HARMONIC_AND_RANDOM
|
| |
Sheldon Imaoka (ANSYS, Inc.)
|
| |
This zip file contains a simple example - single input PSD table for base excitation of a fictitious structure - run as both random vibration and harmonic response analyses.
The user can review the contents of the two input files and see how one can relate harmonic analyses (the transfer function) to the response PSD in random vibration analyses. (Actually, one can also look it up in any dynamics textbook, but this just shows how one can do it in ANSYS.)
(See also TFUN undocumented command to get the transfer function after a random vibration analysis.)
[permalink]
|
| |
|
Average Rating: 8.0 (10 votes)
|
|
|
| |
|
HARMONIC_CMS
|
| |
Sheldon Imaoka (ANSYS, Inc.)
|
| |
Simple beam example showing procedure for using CMS (component mode synthesis). Same results for the full model (no CMS) and the CMS model.
[permalink]
|
| |
|
Average Rating: 10.0 (2 votes)
|
|
|
| |
|
HDPUG's Design for Lead-Free Solder Joint Reliability of High-Density Packages
|
| |
J. Lau, W. Dauksher, J. Smetana, R. Horsley, D. Shangguan, T. Castello, I. Menis, D. Love, B. Sulliv
|
| |
"The lead-free solder-joint reliability of the high-density packages, 256-pin PBGA (plastic ball grid array), 388-pin
PBGA, and 1657-pin CCGA (ceramic column grid array), on PCB (printed circuit board) subjected to temperature
cycling is investigated. Emphasis is placed on the determination of the creep responses (e.g., stress, strain, and strain
energy density) of the lead-free solder joints of these packages. The lead-free solder is assumed to obey the
Garofalo-Arrhenius creep constitutive law. The results presented herein should be useful for a better understanding
of the thermal-mechanical behaviors of the lead-free solder joints in these high-density package assemblies."
[permalink]
|
| |
|
Average Rating: 8.3 (3 votes)
|
|
|
| |
|
HELIX
|
| |
Don Shaffer (Siemens Westinghouse Power Corp)
|
| |
"Here is a helix macro worked up from some xansys discussions several years ago. Several others on the list contributed parts of this."
[permalink]
|
| |
|
Average Rating: 5.4 (12 votes)
|
|
|
| |
|
HELIX2
|
| |
Raziel Vallejo (GE)
|
| |
A modified version of D. Shaffer's HELIX macro.
[permalink]
|
| |
|
Average Rating: 10.0 (4 votes)
|
|
|
| |
|
HFTH
|
| |
Mark Troscinski (ANSYS, Inc.)
|
| |
"Please take a look at this input file. It's a sample problem I've run for someone who was using microwave radiation to heat paper-type products. The model is pretty simple, but it should illustrate the basic steps in running the coupled HF-electromagnetics/thermal problem."
[permalink]
|
| |
|
Average Rating: 10.0 (23 votes)
|
|
|
| |
|
HGEN
|
| |
Sheldon Imaoka (ANSYS, Inc.)
|
| |
When using spatially-varying tabular loads for heat generation rate, a common mistake is to specify the table name only for VAL1 in the BFE command. If this is done, subsequent values will use the same value as VAL1, giving constant heat generation rate per element.
Instead, each node should be given its own value with the BFE command by specifying the table name in all values. This is a simple example demonstrating this.
(This issue does not exist if using spatially-varying tables with the BF command since the BF command is directly specifying heat generation rate per node.)
[permalink]
|
| |
|
Average Rating: 10.0 (8 votes)
|
|
|
| |
|
High End Workbench Tip
|
| |
(PADT)
|
| |
Taken from PADT's SWAU group meeting on performing high-end analyses with Workbench Simulation.
[permalink]
|
| |
|
Average Rating: 9.6 (23 votes)
|
|
|
| |
|
Hill's Potential [ZIP]
|
| |
Sheldon Imaoka (ANSYS, Inc.)
|
| |
"Anisotropic plasticity using Hill’s yield criterion was introduced in ANSYS 5.7,
and the extensions to anisotropic creep and viscoplasticity were added in ANSYS
6.0. While Hill’s stress potential is most commonly used for rolled sheets, it can
be used for other situations where three orthogonal planes of symmetry are
preserved. This memo will introduce details of the usage of Hill’s potential in
ANSYS."
(Week 50, week of 08/31/08)
[permalink]
|
| |
|
Average Rating: 10.0 (4 votes)
|
|
|
| |
|
History of ANSYS University Support Program
|
| |
D.E. Dietrich (Curtiss-Wright Electro-Mechanical Corporation)
|
| |
This document describes the history of the ANSYS University Support Program as well as history of ANSYS/ED software.
[permalink]
|
| |
|
Average Rating: 7.5 (4 votes)
|
|
|
| |
|
History of XANSYS Mailing List
|
| |
Dan Bohlen (GE Aircraft Engines)
|
| |
History of the XANSYS mailing list.
[permalink]
|
| |
|
| |
|
HOLE
|
| |
Zane Ullman (Dana Corp)
|
| |
This macro is from the ANSYS Solutions, Vol 4 No 1 article, "Repairing FEA Geometry with ANSYS Macros." This macro finds missing holes after the user provides the line number from a failed VA error message. This facilitates finding and fixing holes in imported geometry.
[permalink]
|
| |
|
Average Rating: 10.0 (3 votes)
|
|
|
| |
|
HORZ
|
| |
Rod Scholl (PADT)
|
| |
Generates a big long horizontal line at specified location
[permalink]
|
| |
|
Average Rating: 10.0 (1 vote)
|
|
|
| |
|
How to automatically release a license on Windows NT, usually due to an aborted job
|
| |
Bram Weisman (Alan C. McClure Associates, Inc.)
|
| |
Information on how to release a license on Windows NT if an ANSYS job has aborted. This is based on Elan licensing (ANSYS 5.4-5.6). (From XANSYS posting)
[permalink]
|
| |
|
Average Rating: 10.0 (4 votes)
|
|
|
| |
|
How to miminize the Progress bar/window on Windows NT
|
| |
(various)
|
| |
Tip on how to minimize the progress bar during solution on Windows NT.
[permalink]
|
| |
|
Average Rating: 10.0 (3 votes)
|
|
|
| |
|
How to rename multiple image files (jobname000.tif, jobname001.tif, etc.) on Windows NT
|
| |
Sheldon Imaoka (CSI)
|
| |
How to rename the ANSYS-generated TIF (or JPEG, etc.) files under Windows NT via a DOS batch script. (From XANSYS posting)
[permalink]
|
| |
|
| |
|
How to run an ANSYS job in batch at a scheduled time, with or without low priority on Windows NT
|
| |
Sheldon Imaoka (CSI)
|
| |
How to run batch jobs under Windows NT using the 'at' (a.k.a. scheduling) utility, with or without low priority to allow single-processor machines to be used for other purposes during solution. (From XANSYS posting)
[permalink]
|
| |
|
Average Rating: 8.0 (5 votes)
|
|
|
| |
|
How to suspend ANSYS on Windows NT if it is writing too many warnings
|
| |
Bram Weisman (Alan C. McClure Associates, Inc.)
|
| |
Discussion on suspending the ANSYS process on Windows if the output window is getting written to too much (warning messages). (From XANSYS posting)
[permalink]
|
| |
|
Average Rating: 10.0 (2 votes)
|
|
|
| |
|
HPKP
|
| |
John Crawford (Honeywell)
|
| |
A macro which creates a hardpoint on an area using existing keypoints.
[permalink]
|
| |
|
Average Rating: 10.0 (2 votes)
|
|
|
| |
|
HRCPLX
|
| |
(ANSYS, Inc.)
|
| |
Class3 Error 1999-26, SCOPUS #7034
Reverses sign for phase angle
[permalink]
|
| |
|
Average Rating: 9.6 (12 votes)
|
|
|
| |
|
HROPT |
| |
HROPT, Method, MAXMODE, MINMODE, MCout
The MCout argument is undocumented, where it can take the values of "yes" or "no" (default). It writes out modal coordinates in an external text file called "jobname.mcf" for mode-superposition method.
[STI: from release 7.0 and above]
[permalink]
|
| |
|
Average Rating: 10.0 (6 votes)
|
|
|
| |
|
HSAREA
|
| |
Sheldon Imaoka (ANSYS, Inc.)
|
| |
Macro to get 'hotspot' of selected areas. Puts (x,y,z) and area numbers in an array, which can be used for selection, etc. of areas via APDL.Note that while the 'hotspot' of areas should be the centroid, the actual hotspot slightly differs from this. Consequently, no ASUM/GSUM is required, and that is why an undocumented *VGET is used for obtaining hotspot locations.
[permalink]
|
| |
|
Average Rating: 9.0 (5 votes)
|
|
|
| |
|
HSVOLU
|
| |
Sheldon Imaoka (ANSYS, Inc.)
|
| |
Macro to get 'hotspot' of selected volumes. Puts (x,y,z) and volume numbers in an array, which can be used for selection, etc. of volumes via APDL.Note that while the 'hotspot' of volumes should be the centroid, the actual hotspot slightly differs from this. Consequently, no VSUM/GSUM is required, and that is why an undocumented *VGET is used for obtaining hotspot locations.
[permalink]
|
| |
|
Average Rating: 10.0 (6 votes)
|
|
|
| |
|
Human Heart Valves. Hyperelastic Material Modeling
|
| |
Mihai Stuparu
|
| |
"Performing a finite element analysis (FEA) on a hyperelastic material is difficult due to
nonlinearity, large deformation, and material instability. This paper provides a brief review of the
hyperelastic theory and discusses several important issues that should be addressed when using
ANSYS. Analysis on a fatigue specimen is used as an example of one of our product development
challenges upon which these issues were illuminated. We believe that a stable material model in
combination with a good understanding of structural instability for traditional materials is the key
to success in simulating hyperelastic materials using ANSYS."
[ANSYS Nonlinear, version 5.6]
[permalink]
|
| |
|
Average Rating: 10.0 (1 vote)
|
|
|
| |
|
Hybrid Finite Element - Trefftz Method for Open Boundary Analysis [PDF]
|
| |
Miklos Gyimesi, Igor Tsukerman and Doug Lavers
|
| |
Presented at MSM 2000. (MEMS)
[permalink]
|
| |
|
Average Rating: 10.0 (2 votes)
|
|
|
| |
|
Hybrid P-Element and Trefftz Method for Capacitance Computation [PDF]
|
| |
Miklos Gyimesi, Jian-She Wang, Dale Ostergaard
|
| |
Presented at MSM 2000. (MEMS)
[permalink]
|
| |
|
| |
|
Hyper-Elastic Contact Analysis of a Push-Button Diaphragm Seal
|
| |
Jeffrey R. Annis
|
| |
"Presented is the non-linear finite element analysis of a rubber diaphragm seal utilizied in a pushbutton design. Analysis considerations encompassed, nonlinear hyper-elastic material behavior of the rubber, large deflection analysis of seal complex motion, and contact analysis with mating parts. Design parameters of primary interest were, seal deflection patterns and seal actuation force as a function of travel."
[permalink]
|
| |
|
Average Rating: 10.0 (14 votes)
|
|
|
| |
|
HYPER158
|
| |
HYPER158 "3-D 10-Node Tetrahedral Mixed u-P Hyperelastic Solid" was undocumented at ANSYS 10.0. SOLID187 should be used instead - it supports more than Mooney-Rivlin with TB,HYPER, and toggles Mixed u-P via KEYOPT(6) (note that Mixed u-P formulations in HYPERxx and 18x elements are slightly different).
[permalink]
|
| |
|
Average Rating: 10.0 (1 vote)
|
|
|
| |
|
HYPER56
|
| |
HYPER56 "2-D 4-Node Mixed u-P Hyperelastic Solid" was undocumented at ANSYS 10.0. PLANE182 should be used instead - it supports more than Mooney-Rivlin with TB,HYPER, and toggles Mixed u-P via KEYOPT(6) (note that Mixed u-P formulations in HYPERxx and 18x elements are slightly different).
[permalink]
|
| |
|
Average Rating: 10.0 (1 vote)
|
|
|
| |
|
HYPER58
|
| |
HYPER58 "3-D 8-Node Mixed u-P Hyperelastic Solid" was undocumented at ANSYS 10.0. SOLID185 should be used instead - it supports more than Mooney-Rivlin with TB,HYPER, and toggles Mixed u-P via KEYOPT(6) (note that Mixed u-P formulations in HYPERxx and 18x elements are slightly different).
[permalink]
|
| |
|
Average Rating: 8.3 (3 votes)
|
|
|
| |
|
HYPER74
|
| |
HYPER74 "2-D 8-Node Mixed u-P Hyperelastic Solid" was undocumented at ANSYS 10.0. PLANE183 should be used instead - it supports more than Mooney-Rivlin with TB,HYPER, and toggles Mixed u-P via KEYOPT(6) (note that Mixed u-P formulations in HYPERxx and 18x elements are slightly different).
[permalink]
|
| |
|
| |
|
HYPER84
|
| |
HYPER84 "2-D Hyperelastic Solid" was undocumented at ANSYS 10.0. PLANE182/183 should be used instead - it supports more than Mooney-Rivlin or Blatz-Ko with TB,HYPER.
[permalink]
|
| |
|
| |
|
HYPER86
|
| |
HYPER86 "3-D Hyperelastic Solid" was undocumented at ANSYS 10.0. SOLID185 should be used instead - it supports more than Mooney-Rivlin or Blatz-Ko with TB,HYPER.
[permalink]
|
| |
|
| |
|
Hyperelasticity
|
| |
(ANSYS, Inc.)
|
| |
Presentation on the various hyperelastic strain energy functions available in ANSYS (part of the "Advanced Analysis with ANSYS" seminar during the 2002 User's Conference).
[permalink]
|
| |
|
Average Rating: 9.0 (5 votes)
|
|
|
| |
|
IBEAM_181
|
| |
Sheldon Imaoka (CSI)
|
| |
Lateral torsional buckling (example of use of WARP DOF for BEAM188/189)
For an I-beam, considering WARP DOF (in 5.6) is important (i.e., unrestrained or restrained warping). Consider the I-beam modeled with BEAM188 elements or with SHELL181:
* BEAM188 (Unrestrained warping) -- 387.3
* BEAM188 (Restrained warping) -- 569.6
* SHELL181 (concentrated load) -- 560.8
* SHELL181 (distributed load) -- 564.1 (similar to beam case)
This input file uses SHELL181.
[permalink]
|
| |
|
Average Rating: 9.3 (98 votes)
|
|
|
| |
|
IBEAM_188
|
| |
Sheldon Imaoka (CSI)
|
| |
Lateral torsional buckling (example of use of WARP DOF for BEAM188/189)
For an I-beam, considering WARP DOF (in 5.6) is important (i.e., unrestrained or restrained warping). Consider the I-beam modeled with BEAM188 elements or with SHELL181:
* BEAM188 (Unrestrained warping) -- 387.3
* BEAM188 (Restrained warping) -- 569.6
* SHELL181 (concentrated load) -- 560.8
* SHELL181 (distributed load) -- 564.1 (similar to beam case)
This input file uses BEAM188.
[permalink]
|
| |
|
Average Rating: 9.0 (125 votes)
|
|
|
| |
|
ICPKG
|
| |
Steve Groothuis (Micron Technology, Inc.)
|
| |
"An example of IC package assembly using element birth and death - a simple 5-step die attach, injection molding, and cool-down processes during IC packaging. (compliments to Bill Bulat on concept)"
Unzip the file and read in "icpkg.inp".
[permalink]
|
| |
|
Average Rating: 10.0 (23 votes)
|
|
|
| |
|
Identification Methodology of Electrical Equivalent Circuit of the Piezoelectric Transformers by FEM
|
| |
Pigache François, Nadal Clément
|
| |
Methodology using Ansys analyses for the identification of Electrical Equivalent Circuit of piezoelectric transformer. The demonstration is done with typical multilayered Rosen transformer but the method is relevant for any kind of transformer structures.
[permalink]
|
| |
|
Average Rating: 10.0 (4 votes)
|
|
|
| |
|
IGESOUT
|
| |
Gabriel Arias (IDAC)
|
| |
"Macro for generating solid bodies in IGES file format directly from finite element meshes (nodes and elements) in ANSYS"
Alternative link here
[permalink]
|
| |
|
Average Rating: 10.0 (9 votes)
|
|
|
| |
|
IM1
|
| |
Steve Varnam (IDAC)
|
| |
IM1.MAC is used in POST1 of ANSYS 5.3 to read in as element table (ETABLE) items the post data required for element PIPE20.
[permalink]
|
| |
|
Average Rating: 10.0 (4 votes)
|
|
|
| |
|
IM10
|
| |
Steve Varnam (IDAC)
|
| |
IM10.MAC is used in POST1 of ANSYS 5.3 to read in as element table (ETABLE) items the post data required for element COMBIN14.
[permalink]
|
| |
|
Average Rating: 9.0 (5 votes)
|
|
|
| |
|
IM12
|
| |
Steve Varnam (IDAC)
|
| |
IM12.MAC is used in POST1 of ANSYS 5.3 to read in as element table (ETABLE) items the post data required for element BEAM44.
[permalink]
|
| |
|
Average Rating: 8.8 (4 votes)
|
|
|
| |
|
IM21
|
| |
(IDAC)
|
| |
IM21 is a general utility that is used to obtain maximum numbers of all entities, with the option to merge and/or compress entity numbers before. This is useful when creating entity generation macros that work on an existing model.
[permalink]
|
| |
|
Average Rating: 5.0 (2 votes)
|
|
|
| |
|
IM26
|
| |
Steve Varnam (IDAC)
|
| |
IM26.MAC is used in POST1 of ANSYS 5.4 to read in as element table (ETABLE) items the post data required for element CONTAC48.
[permalink]
|
| |
|
Average Rating: 2.5 (2 votes)
|
|
|
| |
|
IM27
|
| |
Steve Varnam (IDAC)
|
| |
IM27.MAC is used in POST1 of ANSYS 5.4 to read in as element table (ETABLE) items the post data required for element COMBIN40.
[permalink]
|
| |
|
Average Rating: 8.3 (3 votes)
|
|
|
| |
|
IM28
|
| |
Steve Varnam (IDAC)
|
| |
IM28.MAC is used in POST1 of ANSYS 5.4 to read in as element table (ETABLE) items the post data required for element LINK1.
[permalink]
|
| |
|
Average Rating: 10.0 (1 vote)
|
|
|
| |
|
IM29
|
| |
Steve Varnam (IDAC)
|
| |
IM29.MAC is used in POST1 of ANSYS 5.4 to read in as element table (ETABLE) items the post data required for element LINK10.
[permalink]
|
| |
|
Average Rating: 10.0 (2 votes)
|
|
|
| |
|
IM5
|
| |
Steve Varnam (IDAC)
|
| |
IM5.MAC is used in POST1 of ANSYS 5.3 to read in as element table (ETABLE) items the post data required for element BEAM4.
[permalink]
|
| |
|
Average Rating: 10.0 (1 vote)
|
|
|
| |
|
IM6
|
| |
Steve Varnam (IDAC)
|
| |
IM6.MAC is used in POST1 of ANSYS 5.3 to read in as element table (ETABLE) items the post data required for element CONTAC12.
[permalink]
|
| |
|
Average Rating: 10.0 (1 vote)
|
|
|
| |
|
IM60
|
| |
Steven Varnam (IDAC)
|
| |
IM60 modifies the currently selected line set to have an orientation keypoint, which is required for meshing the lines with either BEAM44 or BEAM188/189. The orientation keypoints are automatically generated and all the line attributes are kept.
[permalink]
|
| |
|
Average Rating: 5.8 (6 votes)
|
|
|
| |
|
IM63
|
| |
Steve Varnam (IDAC)
|
| |
Creates a spider between master and slave nodes.
[permalink]
|
| |
|
Average Rating: 10.0 (3 votes)
|
|
|
| |
|
IM7
|
| |
Steve Varnam (IDAC)
|
| |
IM7.MAC is used in POST1 of ANSYS 5.3 to read in as element table (ETABLE) items the post data required for element COMBIN39.
[permalink]
|
| |
|
Average Rating: 9.2 (6 votes)
|
|
|
| |
|
IM82
|
| |
(IDAC)
|
| |
"A macro that avoids the need for repetitive work when creating areas from many closed loops of Line geometry in ANSYS. This is particularly useful when the analyst has been supplied Line geometry containing many closed loops via CAD or has created closed loops that need to be converted to Areas for element meshing purposes."
[permalink]
|
| |
|
Average Rating: 10.0 (2 votes)
|
|
|
| |
|
IM9
|
| |
Steve Varnam (IDAC)
|
| |
IM9.MAC is used in POST1 of ANSYS 5.3 to read in as element table (ETABLE) items the post data required for element BEAM3.
[permalink]
|
| |
|
Average Rating: 10.0 (4 votes)
|
|
|
| |
|
IM94
|
| |
Tim Atchison (IDAC)
|
| |
"A macro that makes it simple for users to apply a free moment to an area (or group of areas). It avoids the need to create "spider-webs" of stiff beams and only asks the user to enter the areas or component required and the magnitude of the moment. By providing simple access to the RBE3 command it doesn't stiffen the surface in the same way that stiff beams will and at the same time does all the setting up and implementing of RBE3 for you."
[permalink]
|
| |
|
Average Rating: 10.0 (14 votes)
|
|
|
| |
|
Impact Of Ball Via Configurations On Solder Joint Reliability In Tape Based Chip-Scale Packages [PDF]
|
| |
Bret Zahn
|
| |
"Three-dimensional finite element analysis has been applied to determine the time-dependent solder joint fatigue response of a tape based chip-scale package under accelerated temperature cycling." (Nonlinear, Anand)
[permalink]
|
| |
|
Average Rating: 8.8 (4 votes)
|
|
|
| |
|
IMPEDANCE
|
| |
Sheldon Imaoka (ANSYS, Inc.)
|
| |
Example of the use of complex impedance at a surface, which is a new feature in version 13.0 (for 3D FLUID30, FLUID220, FLUID221 acoustic elements). This is a radiating monopole source. Comparison with infinite FLUID130 shows same results with appropriate value of SF,,IMPD defined.
[permalink]
|
| |
|
Average Rating: 10.0 (18 votes)
|
|
|
| |
|
Implicit Creep
|
| |
(ANSYS, Inc.)
|
| |
Presentation on implicit creep (part of the "Advanced Analysis with ANSYS" seminar during the 2002 User's Conference).
[permalink]
|
| |
|
Average Rating: 10.0 (11 votes)
|
|
|
| |
|
importJPEG1
|
| |
Mark Tate (Hamilton Sundstrand)
|
| |
"Here is a Word Macro that I hacked together a while back that copies a group of graphic files into Word, two per page, with figure numbers. You can change the extension from jpg to png. It looks for files with a root name and add numbers to form the full name, i.e. root001.jpg, root002.jpg, etc."
[permalink]
|
| |
|
Average Rating: 9.4 (8 votes)
|
|
|
| |
|
importJPEG2
|
| |
Gary Betts (Metso Minerals Ltd)
|
| |
"Here is a macro for MS Word that will count and import all the jpegs in a defined folder into Word."
[permalink]
|
| |
|
Average Rating: 8.3 (3 votes)
|
|
|
| |
|
IMPORTPARA
|
| |
Sheldon Imaoka (ANSYS, Inc.)
|
| |
Example of use of Tcl/Tk to bring up custom dialog box to import parasolid files.
This could be used in an input file to automatically prompt the user to import a particular parasolid file through a dialog box.
It can be easily extended to include any Connection Kit product (ACIS/SAT, Pro/E, UG, CATIA, etc.).
[permalink]
|
| |
|
Average Rating: 8.6 (18 votes)
|
|
|
| |
|
importPPT
|
| |
Mark Tate (Hamilton Sundstrand)
|
| |
A visual basic PowerPoint macro to import JPEG files into PowerPoint, one image per slide. Edit the file in a text editor to change variables or directory locations, etc.
[permalink]
|
| |
|
Average Rating: 8.8 (8 votes)
|
|
|
| |
|
Improvements to Time-History Postprocessing at 6.0 [PDF]
|
| |
Sheldon Imaoka (ANSYS, Inc.)
|
| |
"This tips and tricks focuses on improvements at 6.0 on the Time-History postprocessor. (After I did this, I realized that a lot of this was already covered in the 6.0 Update seminar, but, oh well...)"
(Week 8, week of 11/12/01.)
[permalink]
|
| |
|
Average Rating: 8.5 (10 votes)
|
|
|
| |
|
IMPULSE
|
| |
Brad Lamirand (Cooper Turbocompressor, Inc.)
|
| |
Example of Flotran model which solves a sinusoidally varying flow from pi/4 to 7*pi/4.
[permalink]
|
| |
|
Average Rating: 10.0 (14 votes)
|
|
|
| |
|
IN-3D
|
| |
Vladimir Zhulin (ANSYS, Inc.)
|
| |
3D beam under electrostatic load. Coupled-field problem using TRANS126 elements. Requires EMTGEN macro.
[permalink]
|
| |
|
Average Rating: 4.7 (19 votes)
|
|
|
| |
|
INDCTNC0
|
| |
Bill Bulat (ANSYS, Inc.)
|
| |
"You may be able to modify the following macro to suit your needs. I use it
to calculate the inductance of excited MVP massive conductors. The volt DOF
in ANSYS is not physical voltage, it's the time integral of voltage."
[permalink]
|
| |
|
Average Rating: 10.0 (11 votes)
|
|
|
| |
|
INISTATE
|
| |
Sheldon Imaoka (ANSYS, Inc.)
|
| |
This is a very simple example using Workbench Mechanical 12.0.1 to demonstrate use of the INISTATE command in defining initial stress.
Open Workbench 12.0.1 (or 12.1) and use "File > Restore Archive ..." and select the zip file to open the model. Solving should take less than a minute.
The model is a simple bar.
The first analysis branch has 10e3 psi initial stress only in the x-direction.
Notice that the block is free to expand - it only has symmetry boundary conditions.
The final results show basically zero stress and displacement of -8.1455e-4 inches.
Since initial stress is 10e3 and elastic modulus is 29e6 with a length of 2.3622 inches:
10e3 / 29e6 * 2.3622 = 8.1455e-4
which is the same answer as given by ANSYS.
The second analysis branch also has 10e3 psi initial stress only in x-direction.
However, there is a Frictionless Support preventing the block from expanding.
Final results show displacement basically of zero, and stress of 10e3 psi.
This is because the initial stress cannot relax due to the boundary conditions, so the final stress = initial stress in this particular case.
[permalink]
|
| |
|
Average Rating: 8.9 (31 votes)
|
|
|
| |
|
INITROT
|
| |
Sean Harvey (CSI)
|
| |
This macro takes in parameters to pass to the EDIVELO command for rotational input, this macro prompt the user for two points instead of 3 angles. Two point input is often times easier to enter than 3 direction angles
[permalink]
|
| |
|
Average Rating: 10.0 (1 vote)
|
|
|
| |
|
Inquiry Function Matrix
|
| |
Jeroen Valensa (Modine Mfg. Co.)
|
| |
This is a handy reference sheet listing the different inquiry functions and options available.
[permalink]
|
| |
|
Average Rating: 8.0 (27 votes)
|
|
|
| |
|
INS_SEC
|
| |
Bill Bulat (CSI)
|
| |
Macro to convert instantaneous thermal coefficients of expansion to secant values, with example input file. (This is a zipped file)
[permalink]
|
| |
|
Average Rating: 0.0 (2 votes)
|
|
|
| |
|
INT_AREAS
|
| |
Mitch Voehl (CEC Corp)
|
| |
From the author: "I've attached a macro which can find interior areas (holes) in some circumstances. Prior to running the macro, first create all of your areas and then perform and area overlap or area partition to divide them up. Then run the macro. The macro will save the interior areas as the component 'int_a'."
[permalink]
|
| |
|
Average Rating: 0.0 (2 votes)
|
|
|
| |
|
Integrating ANSYS with Modern Numerical Optimization Technologies
|
| |
Shen-Yeh Chen
|
| |
"Design automation with finite element analysis as a simulation and evaluation tool is becoming more and more desired. The ability to do automatic design iteration has constantly been a popular research and engineering topic. In this article, we will show how Honeywell Engines & Systems took advantage of the flexible environment of ANSYS to achieve this goal." (Optimization, APDL)
[permalink]
|
| |
|
Average Rating: 8.7 (15 votes)
|
|
|
| |
|
INTERP
|
| |
Vladimir Tkach (NPO Energomash)
|
| |
"This example interpolates stress-strain curve by polynomial function -
Strain=A1+A2*StressA3*Stress^2, in temperature area between Proportional, Yield and
Ultimate stresses and reads it into ANSYS db-file."
[permalink]
|
| |
|
Average Rating: 10.0 (10 votes)
|
|
|
| |
|
Introduction to Hidden Parameters
|
| |
John Crawford
|
| |
An introduction to hidden parameters, those which begin or end with an underscore. Use of parameters with a trailing underscore can be used to 'hide' macro parameters if they are to be shared by several users.
[permalink]
|
| |
|
Average Rating: 10.0 (5 votes)
|
|
|
| |
|
Introduction to Inquiry Functions
|
| |
John Crawford
|
| |
Inquiry functions are similar to *GET functions, used to retreive information about the current database. These can be used in macros to automate procedures and obtain information in a simple manner.
[permalink]
|
| |
|
Average Rating: 8.7 (26 votes)
|
|
|
| |
|
Introduction to the Residual Vector Method [ZIP]
|
| |
Sheldon Imaoka (ANSYS, Inc.)
|
| |
"The residual vector method can improve the accuracy of mode-superposition
harmonic response or transient analyses, especially when the high-frequency
content of the structure is excited. This memo provides details on how users
can take advantage of this analysis technique introduced in ANSYS 11.0."
(Week 45, week of 04/20/08)
[permalink]
|
| |
|
Average Rating: 10.0 (3 votes)
|
|
|
| |
|
Inventor
|
| |
Robert SeCaur (ANSYS, Inc.)
|
| |
In Workbench Design Simulation 8.0, Named Selections can be imported from certain CAD systems. For Inventor, this .vbs file will aid in exporting a group as a Named Selection.
"Here is the macro code for Inventor. It will create an attribute set on each selected entity (the name for this is immaterial) and an attribute in that set (the name for this is what will be looked at for creating a WB side attribute). More than anything this was a proof of concept script and does not have some of the "niceties" one might like (e.g. just adding to an already existing attribute set instead of creating a new one, or modifying an existing value if an attribute already exists of a given name in the given set). However, this script would allow you (with multiple invocations) to create multiple attributes on a given entity. That is something that an entity naming scheme does not allow conveniently. This is particularly significant for named selections, since an entity may need to be included in several named selections (perhaps one for load, one for mesh sizing, etc.)."
[permalink]
|
| |
|
Average Rating: 9.5 (11 votes)
|
|
|
| |
|
INVTCHG
|
| |
Peter Frei (Rockwell Automation AG)
|
| |
Converts 10-node SOLID87 tetrahedra to 20-node degenerate SOLID117 tetrahedra (need to specify element type for SOLID117 beforehand and enter that ID as the parameter "etMag").
[permalink]
|
| |
|
Average Rating: 3.3 (3 votes)
|
|
|
| |
|
IOPTN |
| |
IOPTN,FILTER,value
Filters IGES entities, including construction, infinite, blank, and lower-order entities (entities not used for BREP construction).
IOPTN,FILTER,ALL (ON) - Default behavior to filter all undesirables
IOPTN,FILTER,NONE - Turn off filtering and get everything
IOPTN,FILTER,BLANK - Filter only the blank entities (not to be displayed)
IOPTN,FILTER,LOWER - Filter the lower order entities and keep everything else
[permalink]
|
| |
|
Average Rating: 10.0 (2 votes)
|
|
|
| |
|
Iterative Determination of Save Working Loads (SWL) for Crawler Cranes
|
| |
G. Kolarov, K.-H.Reckziegel, T.Göllnitz
|
| |
"A program for the calculation of Save Working Loads (SWL) is introduced. It uses ANSYS and its parametric design language. The models are based on large displacements, small strains and linear-elastic material. The limit state method with partial safety coefficients is applied. For a crawler crane many configurations exist and they have to be calculated for different positions and load cases. Special attention is paid to the overall structural stability of the crane and to the effectiveness of the calculations."
[permalink]
|
| |
|
Average Rating: 8.8 (4 votes)
|
|
|
| |
|
JB_FORC
|
| |
John Swanson (SAS, Inc./ANSYS, Inc.)
|
| |
A macro to apply JxB forces on a Flotran model. "FYI, here is a macro which I wrote for a Japan User Meeting. It calculates nodal forces from J X B and applies them as forces to the model. It is only for 8 node bricks, and it has NOT been tested."
[permalink]
|
| |
|
Average Rating: -10.0 (4 votes)
|
|
|
| |
|
JOBNAME
|
| |
Sheldon Imaoka (CSI)
|
| |
Gets jobname, title, subtitle and puts in arrays
[permalink]
|
| |
|
Average Rating: 10.0 (3 votes)
|
|
|
| |
|
jobname.solc |
| |
Regarding the undocumented jobname.solc feature:
- Open up a text editor and place and /solu commands you want (not /SOLU itself). Main use I've seen of jobname.solc is really to change CNVTOL or NSUBST, although I think other options are available.
- Save file as jobname.solc in working directory.
If I recall correctly, jobname.solc will be deleted when it is read from, similar to jobname.abt. Also, I think it works on the next substep.
[permalink]
|
| |
|
Average Rating: 10.0 (14 votes)
|
|
|
| |
|
JS_CURVEWRITE
|
| |
Jeff Strain (PADT)
|
| |
"A macro to write output PSD data at selected nodes with the number of selected nodes varying with each run. I did the "write a macro from a macro" thing and took advantage of two fairly recently added capabilities: C formatting in *VWRITE and string arrays, mainly for the 128 character capability.
"My macro creates a character array called p (I needed to conserve characters). The top row of the array starting at the second column contains selected node numbers. The second row starting at the second column contains GRMS values at each node. Starting in the third row, the first column is filled with frequency breakpoints; the second column over contains output PSD data for each of the selected nodes."
This can be used as an example of writing output to a file.
[permalink]
|
| |
|
Average Rating: 10.0 (7 votes)
|
|
|
| |
|
JUSTMESHIT
|
| |
Prasad S. (QuEST Pvt. Ltd.)
|
| |
"The macro meshes all the areas after getting the specifications from the user.
You can change the element type in the macro as per your requirement. At present shell63 is being used for the area mesh.
In this macro a muliplication factor has been considered for the bent curves, so that when compared to the straight curves, bent curves will have element edge length smaller based on the input factor.
If the factor is >1, the bent curves contain finer divisions,
If the factor is <1, the bent curves contain coarser divisions."
[permalink]
|
| |
|
Average Rating: 9.2 (12 votes)
|
|
|
| |
|
JWASEL
|
| |
Joe Woodward (PADT)
|
| |
This macro allows you to select the 'inside' surface of a volume, in case your volume has a 'void' inside of it.
[permalink]
|
| |
|
Average Rating: 10.0 (4 votes)
|
|
|
| |
|
KBFOCUS
|
| |
Eric Miller (PADT)
|
| |
"Below you will find a little macro that can be run to fix the more common issues with focus on the command line not behaving as expected at 6.1. It is a partial hack that needs to be run after the GUI is up, so you can't put it in your start61.ans file (sorry). It also does not fix focus loss with the picker (which is intentional) or the pan-zoom-rotate dialog (not so intentional). Those will require more than a simple Tcl/Tk script."
[permalink]
|
| |
|
Average Rating: 5.0 (7 votes)
|
|
|
| |
|
KCOR
|
| |
Don Shaffer (Siemens Westinghouse Power Corp)
|
| |
Lists selected keypoints in CSYS 0 and 1.
[permalink]
|
| |
|
Average Rating: 10.0 (1 vote)
|
|
|
| |
|
KEYMOD |
| |
KEYMOD,itype,knum,value
Allows changing element keyoptions during solution. Use it instead of KEYOPT in /SOLU to change keyoptions between load steps, such as for contact elements.
[permalink]
|
| |
|
Average Rating: 10.0 (7 votes)
|
|
|
| |
|
KEYW |
| |
KEYW,BETA,1
Turns on GUI filtering of Beta features in releases of ANSYS. Add to "start5x.ans" file prior to launching ANSYS.
[permalink]
|
| |
|
| |
|
KEYW |
| |
KEYW,ALPHA,1
Turns on GUI filtering of Alpha features? I find this pretty useless since the features are not as good/robust as beta (above), but it is cool to see upcoming features of ANSYS.
[permalink]
|
| |
|
Average Rating: 0.0 (2 votes)
|
|
|
| |
|
KEYW |
| |
KEYW,QALOGKEY,1
Shows detailed information from the granule (GRN) files in the jobname.log file. This is handy to find out what the granule function name is (Fnc_xxx) for a given dialog box/menu.
When plotting experimental and calculated curves for *MOONEY/*EVAL, this isn't recorded in the log file. Using this keyword will show the commands necessary to plot the curves together (or you can manually use /NOERASE like I do).
[permalink]
|
| |
|
Average Rating: 10.0 (3 votes)
|
|
|
| |
|
KEYW |
| |
KEYW,PR_SGUI,1
Supresses "Solution is done" message [5.5.3 and above]
Setting this keyword will not have an adverse effect on the menus, but to be safe, use the above setting for the SOLVE command only, then reset PR_SGUI to zero after SOLVE.
[permalink]
|
| |
|
Average Rating: 10.0 (7 votes)
|
|
|
| |
|
KEYW |
| |
KEYW,SIMPLOFF,1
At 5.6, the "Abridged Menu" with the Solution Control Wizard is the default. I find that since the abridged menu or Solution Control wizard doesn't support all nonlinear or dynamics options, this confuses customers. If you put this in your start56.ans file, this will always show the unabridged menu (similar to 5.5 and prior versions). (STI)
[permalink]
|
| |
|
Average Rating: 2.5 (2 votes)
|
|
|
| |
|
KEYW |
| |
keyw,cuwidget
Resets menus in case they may be grey and inaccessible.
[permalink]
|
| |
|
Average Rating: 10.0 (1 vote)
|
|
|
| |
|
KEYW |
| |
KEYW,PR_SGVOF,1
When redefining arrays in an interactive session, the user is prompted if they really want to redefine an existing array. The above command disables this prompt in ANSYS 15.0 and above, so if an existing array is redefined with the *DIM command, it will do so silently.
See also *DEL,,NOPR.
[permalink]
|
| |
|
Average Rating: 10.0 (3 votes)
|
|
|
| |
|
KLIST |
| |
KLIST,all,,,xyz
Shows more significant digits for keypoint listings.
[permalink]
|
| |
|
Average Rating: 10.0 (5 votes)
|
|
|
| |
|
KLL
|
| |
G. N. S. Prakash
|
| |
" The macro kll.mac adds the broken lines of the selected volumes. Normally some of the complex curves from the CAD software become segmented after importing into Ansys and also due to Boolean operations and require considerable effort in joining these segments into single curves. Typing 'kll' just after import would recognize and add all these segments. It works on the principle that the keypoints on edges have only 2 lines attached to them and keypoints at corners have 3 or mores lines attached to them. Hence, if it finds any keypoint on a edge, it would be removed by joining the adjoining lines.
" Please note, it works on lines attached to volumes only and not for independent areas or lines."
[permalink]
|
| |
|
Average Rating: 6.2 (4 votes)
|
|
|
| |
|
KPMV
|
| |
Don Shaffer (Siemens Westinghouse Power Corp)
|
| |
"Macro moves keypoint arg1 to the location of keypoint arg2 and if arg3 equals 1 merges them."
[permalink]
|
| |
|
Average Rating: 10.0 (2 votes)
|
|
|
| |
|
KROT |
| |
Similar to NROTA but rotates keypoints. Can be viewed with /PSYM,NDIR,1 and is supported by CDREAD and CDWRITE
[permalink]
|
| |
|
Average Rating: 10.0 (1 vote)
|
|
|
| |
|
KSLE |
| |
KSLE,s,1
Selects keypoints based on selected elements. See ASLE undocumented command (or NSLL documented command) for usage.
[permalink]
|
| |
|
Average Rating: 10.0 (2 votes)
|
|
|
| |
|
L_NLIST
|
| |
Chris Bridge (2H Offshore Engineering Ltd)
|
| |
A macro to list selected nodes but in a specified format without repeated header information.
[permalink]
|
| |
|
Average Rating: 10.0 (5 votes)
|
|
|
| |
|
Lab Tests Improve Accuracy of FEA
|
| |
(ANSYS, Inc.)
|
| |
"Test results steer fine-tuning of ANSYS/LS-DYNA simulation in Motorola cell phone study" (from ANSYS Solutions Magazine, Vol. 2 No. 2)
[permalink]
|
| |
|
Average Rating: 10.0 (7 votes)
|
|
|
| |
|
LARGE_ROTAT
|
| |
Sheldon Imaoka (CSI)
|
| |
Input file demonstrating large rotation (beam). Also shows that line search takes longer CPU time.
[permalink]
|
| |
|
Average Rating: 10.0 (25 votes)
|
|
|
| |
|
Large-Area, High-Transparency Extraction System for Negative Ions
|
| |
B. Heinemann, J. Bucalossi, P. Frank, R. Riedl, A. Simonin, E. Speth, O. Vollmer
|
| |
(Thermal analysis)
[permalink]
|
| |
|
| |
|
LCOLOR
|
| |
Jimmy Carlsson (AF Group)
|
| |
This macro colors lines as follows:
- Red: Line connected only to one of selected areas
- Yellow: Line connected to two of the selected areas
- Blue: Line connected to three or more selected areas
- Magenta: Line is not connected to any of the selected areas
[permalink]
|
| |
|
Average Rating: 5.0 (4 votes)
|
|
|
| |
|
Legend Example
|
| |
Bob Weathers (Trane)
|
| |
Example of customizing legend with annotations. See "Read Me" file for details, along with AVI animation.
"Essentially, I turn off the legend and write annotations into this area. It gives me considerable control over what appears there. I have also found that I can better communicate results to my customers by, say, having a legend that's reads 1.23 mils rather than 0.123E-02 inches or by referencing drawing and revision numbers, test results, material properties, and so on."
"You might need to change some of the character size and line spacing
dimensions in the macros. Again, though, they work just fine for my
hardware."
[permalink]
|
| |
|
Average Rating: 10.0 (7 votes)
|
|
|
| |
|
License monitoring and reporting [PDF]
|
| |
Sheldon Imaoka (CSI)
|
| |
Information on license monitoring and reporting for Elan (ANSYS 5.4-5.6). At 5.7, licensing has reverted back to FlexLM, and this document is not applicable.
[permalink]
|
| |
|
Average Rating: 10.0 (4 votes)
|
|
|
| |
|
LISTCM
|
| |
Sheldon Imaoka (ANSYS, Inc.)
|
| |
At 7.0, the CMLIST command only lists selected components rather than all existing components in the database (pre-7.0 behavior). This macro provides a listing of all components in the database, regardless of their selection status. May be useful to get pre-7.0 behavior of CMLIST.
[permalink]
|
| |
|
Average Rating: 10.0 (7 votes)
|
|
|
| |
|
LISTTYPE
|
| |
Sheldon Imaoka (ANSYS, Inc.)
|
| |
Macro used to list all unique combinations of element type, real constant, section type, and material properties of currently selected elements. Useful, for example, when importing mesh from Workbench or other software into ANSYS and confirming settings.
[permalink]
|
| |
|
Average Rating: 10.0 (6 votes)
|
|
|
| |
|
LKPZERO
|
| |
(ANSYS, Inc.)
|
| |
SCOPUS #7401
A failed AMESH/VMESH may generate lines with keypoints zero and zero at 5.6.0. This macro clears up the database and fixes this problem.
[permalink]
|
| |
|
Average Rating: 9.3 (15 votes)
|
|
|
| |
|
LMER |
| |
LMER,line1,line2,etc.
"Glues" lines together. Same command as LGLUE. See LGLUE for details on the usage of this command.
[permalink]
|
| |
|
| |
|
Load vs. displacement control in contact problems [PDF]
|
| |
Karen Dhuyvetter (CSI)
|
| |
Discussion on load vs. displacement control for contact problems.
[permalink]
|
| |
|
Average Rating: 10.0 (18 votes)
|
|
|
| |
|
Local Approximation Estimators For Algebraic Multigrid
|
| |
Jan Mandel
|
| |
"We are concerned with the development of Algebraic Multigrid (AMG) for symmetric, positive definite linear systems arizing from finite element discretization of elliptic partial differential equations. AMG methods attempt to create coarse levels from the algebraic system automatically, using no or only a minimum of additional information. The basic idea of the multigrid algorithm is that fine level error on which the smoothing process is not effective should be reduced by the coarse correction. Therefore, a-priori estimates of the approximation of fine level functions by coarse level function are important to guide the design of robust AMG methods."
[permalink]
|
| |
|
Average Rating: 10.0 (2 votes)
|
|
|
| |
|
Long Parameter and Component Names at 6.0 [ZIP]
|
| |
Sheldon Imaoka (ANSYS, Inc.)
|
| |
"Starting from version 5.7, strings have been introduced to replace character arrays. Strings allow
for up to 128 characters for APDL purposes, instead of the 8-letter limit of character parameters. The
/INQUIRE command as well as string manipulation functions (see *GET online help) extend the
usefulness of strings to retrieve and manipulate data. *VWRITE has also been enhanced to support C-format statements, useful in writing out long strings."
"At 6.0, the 8-character limitation on parameters, components, and /POST26 variables has been
removed. Users can now specify up to 32 character for these items, allowing for much more
descriptive names. In /POST26, variables can also be referred to by name when plotting or listing."
(Week 16, week of 01/28/02.)
[permalink]
|
| |
|
Average Rating: 10.0 (4 votes)
|
|
|
| |
|
Low Creep and Hysteresis Load Cell Based on a Force to Liquid Pressure Transformation
|
| |
Robert A.F. Zwijze, Remco J. Wiegerink, Theo S. J. Lammerink, and Miko Elwenspoek
|
| |
"Important problems in load cells are creep and hysteresis. Expensive high grade steels are used in order to reduce these effects. In this paper a load cell design based on a force to liquid pressure transformation is presented. The design is insensitive to hysteresis and creep and can be made at very low costs. Analytical, numerical and experimental results are in very close agreement with each other." (FLUID79)
See related paper
[permalink]
|
| |
|
Average Rating: 10.0 (5 votes)
|
|
|
| |
|
LPROJ
|
| |
John Crawford (Honeywell)
|
| |
Here is a macro I wrote several years ago that projects lines onto the working plane. It's a little crude, but works okay. I use it all the time to project IGES geometry onto the working plane (placed at global Z=0) to straighten lines that are slightly bent or not at Z=0. You still have to recreate your areas and all that sort of stuff, which is kind of a pain.
[permalink]
|
| |
|
Average Rating: 10.0 (6 votes)
|
|
|
| |
|
LREGEN
|
| |
John Crawford (Honeywell)
|
| |
Recreates selected lines by fitting b-splines through points on line. Useful with some imported IGES geometry
[permalink]
|
| |
|
Average Rating: 10.0 (3 votes)
|
|
|
| |
|
LS-DYNA Simulations of Thermal Shock in Solids
|
| |
Goran Skoro
|
| |
PowerPoint presentation on thermal shock on rod.
[ANSYS LS-DYNA, version unspecified]
[permalink]
|
| |
|
Average Rating: 10.0 (2 votes)
|
|
|
| |
|
LSAR |
| |
LSAR
Selects all lines associated with currently active areas.
[permalink]
|
| |
|
| |
|
LSLE |
| |
LSLE,s,1
Selects lines based on selected elements. See ASLE undocumented command (or NSLL documented command) for usage.
[permalink]
|
| |
|
Average Rating: 10.0 (1 vote)
|
|
|
| |
|
LSLN |
| |
LSLN,s,1
Selects lines based on nodes. See ASLE undocumented command (or NSLL documented command) for usage.
[permalink]
|
| |
|
Average Rating: 10.0 (2 votes)
|
|
|
| |
|
LSPA |
| |
LSPA,line,area
Project a line onto an area. It appears that the line must be directly over the area, and the area needs to be flat.
[permalink]
|
| |
|
| |
|
LSSOLVE |
| |
LSSOLVE,lsmin,lsmax,lsinc,,,,,,1
The ninth argument, when set to 1, solves load steps lsmin to lsmax with element shape checking disabled. (For related command, see SOLVE undocumented option.)
[permalink]
|
| |
|
Average Rating: 10.0 (5 votes)
|
|
|
| |
|
LSTDBDOC
|
| |
Chris Kennedy (Think PEAK, Inc.)
|
| |
This macro finds all :LBL constructs in the database. A :LBL can be any valid Ansys characters following a colon ":". Therefore you can have different labels for different aspects of your model, such as :MAT for material info, :REAL for real constant information, :INFO for general notes about the analysis, etc. Labels can be repeated.
[permalink]
|
| |
|
Average Rating: -5.0 (1 vote)
|
|
|
| |
|
LSTR |
| |
LSTR,p1,p2,ndiv,space
LSTR is documented, NDIV and SPACE are not. Analogous to the L command, you can put number of divisions and spacing ratio.
[permalink]
|
| |
|
Average Rating: 8.3 (3 votes)
|
|
|
| |
|
LSx() |
| |
LSx(line number, unit distance)
*GET functions for the slope of a line for LSX, LSY, LSZ where unit distance is between 0 and 1 (0 is slope at keypoint 1, 1 is slope at keypoint 2)
[permalink]
|
| |
|
Average Rating: 10.0 (4 votes)
|
|
|
| |
|
M55TO54
|
| |
(ANSYS, Inc.)
|
| |
Converts 5.5 CDB file to 5.4 format (for backwards compatibility).
[permalink]
|
| |
|
Average Rating: 10.0 (4 votes)
|
|
|
| |
|
MAKEMESH
|
| |
John Crawford (Honeywell)
|
| |
This macro is from John's article, "Meshing Complex Solids" from ANSYS Solutions Vol 4 No 1. The input file creates the geometry, then meshes it using steps outlined in his article (e.g., mapped meshing, sweep meshing, transition meshing).
[permalink]
|
| |
|
Average Rating: 10.0 (6 votes)
|
|
|
| |
|
Manipulating FE Mesh [ZIP]
|
| |
Sheldon Imaoka (ANSYS, Inc.)
|
| |
"There are some special situations where a user may be required to generate or manipulate a
database consisting mainly of finite element entities without solid model geometry. With some
careful planning, dealing with mesh-only databases can prove to be relatively easy.
Typical situations that may arise include the following:
- Import of mesh from Workbench Simulation or AI*Environment/ICEM CFD
- Generation of repetitive geometry
This memo hopes to cover these situations in more detail."
(Week 31, week of 10/02/05.)
[permalink]
|
| |
|
Average Rating: 7.7 (15 votes)
|
|
|
| |
|
Manual Calculation of Strain Energy Density [ZIP]
|
| |
Sheldon Imaoka (ANSYS, Inc.)
|
| |
"Output of elastic, plastic, and creep strain energy densities (SEND) was introduced in ANSYS 6.0, although this is limited to 18x elements in nonlinear analyses. Users whose models include core elements with plasticity and creep may also wish to obtain these quantities, and this memo hopes to review this procedure."
(Week 22, week of 12/22/02.)
[permalink]
|
| |
|
Average Rating: 10.0 (19 votes)
|
|
|
| |
|
MAPME
|
| |
Sheldon Imaoka (ANSYS, Inc.)
|
| |
General macro used to map one set of values & (x,y,z) coordinates to another. Uses *MOPER,,,MAP.Example input file can be found here which uses this macro. In this input example, *VPUT is used to compare mapping UX, UY, and UZ from one mesh to another. This can be used to map pressures, heat flux, convection, etc. from CFD codes to ANSYS, for example.Alternate macro also available here.
[permalink]
|
| |
|
Average Rating: 10.0 (28 votes)
|
|
|
| |
|
Mass property calculation methods [PDF]
|
| |
Sheldon Imaoka (CSI)
|
| |
This memo covers some ways to determine mass properties of an ANSYS model.
[permalink]
|
| |
|
Average Rating: 9.6 (12 votes)
|
|
|
| |
|
MASSPROP
|
| |
Bill Bulat (CSI)
|
| |
Calculates accurate mass properties via inertial relief method.
[permalink]
|
| |
|
Average Rating: 10.0 (6 votes)
|
|
|
| |
|
MATLAB
|
| |
Rick Morgans (Adelaide University)
|
| |
"On this subject, I've been meaning to post these for ages -> we've
been using these macros to transfer variables between ansys and matlab
for yonks. They write and read variables from ansys and matlab -> you
can check them out to see how they do it (i.e. I cant remember off of
the top of my head) -> I think they write out a format header then
write the rest of the variable as a single column.
varread.m
read variable into matlab
varread.mac
read variable into ansys
varreadc.m
read 2 column ansys variable into matlab as a complex variable
varreadcp.m
read "packed" 2 column variable into matlab as complex variable
varreadp.m
read "packed" variable into matlab
varreadp.mac
read "packed" variable into ansys
varwrite.m
write a variable from matlab
varwrite.mac
write a variable from ansys
varwritep.mac
write a variable from ansys in "packed" format using a vmask"
[permalink]
|
| |
|
Average Rating: 10.0 (16 votes)
|
|
|
| |
|
MAVGTEMP
|
| |
Joe Metrisin (Florida Turbine Technologies, Inc.)
|
| |
"Here is a macro to calculate the mass average temperature of the selected elements."
[permalink]
|
| |
|
Average Rating: 10.0 (7 votes)
|
|
|
| |
|
Maximization Of The Design Of A Scleral Expansion Band Segment For The Reversal Of Presbyopia
|
| |
Andrew J. Bax, Ronald A. Schachar
|
| |
"The focusing ability of the human eye declines universally with age. This age related decline in the amplitude of accommodation results in difficulty in reading at a normal working distance in the 40's and is called presbyopia. Conventionally, bifocals, reading glasses or bifocal contact lenses are used to facilitate reading in presbyopic patients. A new method for correcting presbyopia involves placing an implant, a scleral expansion segment, in the sclera (white of the eye) to alter the position of the underlying ciliary muscle." (Contact, Hyperelasticity, Mooney-Rivlin) From 2000 Conference
[permalink]
|
| |
|
Average Rating: 10.0 (2 votes)
|
|
|
| |
|
Meeting the Cost/Performance Requirements of Flex-Based Chip-Scale Packages
|
| |
Randy D. Schueller, Elizabeth A. Bradley, and Paul M. Harvey
|
| |
"An ANSYS two-dimensional, mechanical stress/strain model was created to compare a 12-mm flex BGA structure directly to the E-CSP in a board-level condition." (Nonlinear, plasticity)
[permalink]
|
| |
|
Average Rating: 10.0 (2 votes)
|
|
|
| |
|
Memory management and configuration [PDF]
|
| |
Sheldon Imaoka (CSI)
|
| |
Memo on memory management and configuration, especially in conjunction with the PCG solver and options in linear static analyses.
[permalink]
|
| |
|
Average Rating: 9.0 (10 votes)
|
|
|
| |
|
Mesh Discretization Error and Criteria for Accuracy of Finite Element Solutions
|
| |
Chandresh Shah
|
| |
"Any finite element analysis performed by an engineer is subject to several types of errors that can compromise the validity of the results. These errors can be broadly classified under the following categories: 1) user error - incorrect usage of FE software or input by the FE analyst, 2) errors due to assumptions and simplifications used in the model and 3) errors due to insufficient mesh discretization. User errors can be prevented by developing and utilizing a comprehensive pre and post processing checklist and by appropriate training in the basics of finite element analysis and usage of FE software. Errors due to modeling assumptions and simplifications can be alleviated by adding complexity to the model so that it better represents the physics of the problem being analyzed. Errors due to the inadequacy or coarseness of the mesh are often overlooked by the analyst. These errors due to mesh discretization can be fixed by evaluating the quality of the mesh and by developing and utilizing criteria that characterize the accuracy of the FE solution. This paper describes the source of mesh discretization error and presents several criteria that can be used by an FE analyst to evaluate the accuracy of the FE solution."
[ANSYS 5.7, 2002 Conference]
[permalink]
|
| |
|
Average Rating: 10.0 (4 votes)
|
|
|
| |
|
Meshing in Workbench [PDF]
|
| |
Sheldon Imaoka (ANSYS, Inc.)
|
| |
"Mechanical users have long enjoyed access to a variety of powerful meshing tools
inside of ANSYS to generate high-quality shell, tetrahedral, and swept meshes. During
the past several years, meshing in ANSYS Workbench Simulation has not only grown to
encompass traditional meshing algorithms in ANSYS but has also developed many
features requested by ANSYS users as well as integrated meshing technologies from
ANSYS CFX and ANSYS ICEM CFD."
(Week 43, week of 03/02/08)
[permalink]
|
| |
|
Average Rating: 9.2 (25 votes)
|
|
|
| |
|
Meshing papers presented at the 1998 Conference
|
| |
Various ANSYS staff and CMU students
|
| |
10 Papers on meshing algorithms
[permalink]
|
| |
|
Average Rating: 8.7 (16 votes)
|
|
|
| |
|
Methods for Modeling Bolts in the Bolted Joint
|
| |
Jerome Montgomery
|
| |
"Modeling bolts for three-dimensional finite element applications have, and still continue to raise questions. The limitations on model size sometimes make modeling of solid bolts impractical. Therefore, many analysts choose other methods to model bolts. Line elements with coupled nodes and line elements with spider beams are a couple of alternative approaches. This paper looks at a few methods for modeling pretension bolted joints using the finite element method (ANSYS 5.7). Pretension is modeled using ANSYS pretension elements (PRETS179) which can be used on solid or line element types. Surface-to-surface contact elements are used to account for varying contact distribution along flanges. Bolt head and nut behavior is modeled by, coupled nodes, beam elements, rigid body elements (RBE3), or solids. Bolt stud is modeled by solid elements, beam elements, pipe elements, or link elements. The choice of line elements versus solid elements is determined by the degree of complexity sought. The pros and cons of different simulations are also discussed."
[permalink]
|
| |
|
Average Rating: 9.3 (54 votes)
|
|
|
| |
|
MG
|
| |
John Crawford (Honeywell)
|
| |
Zooms in, out or autoscales images then does a replot
"When I want to zoom in by a factor of two I enter MG,2. If I want to zoom out I enter something like MG,.1. If I want to autoscale I just enter MG. It replots the last display, which is usually what I want to do anyway."
[permalink]
|
| |
|
Average Rating: 10.0 (4 votes)
|
|
|
| |
|
Micromachined Piezoelectric Ultrasonic Transducers Based On Parylene Diaphragm In Silicon Substrate
|
| |
Cheol-Hyun Han and Eun Sok Kim
|
| |
"This paper describes the techniques used in fabricating the transducers, their performance characteristics, and finite element analyses (FEA) with ANSYS 5.6. With ANSYS, we have calculated the stress and strain (under a static pressure load) and the dynamic mode shapes over a certain frequency range. Also, with appropriate piezoelectric matrices incorporated into the ANSYS batch model, a piezoelectric coupled-field analysis has been performed." (MEMS)
[permalink]
|
| |
|
Average Rating: 8.8 (12 votes)
|
|
|
| |
|
MICROOVEN
|
| |
Steve Groothuis (Micron Technology, Inc.)
|
| |
"The following input stream worked just fine in ANSYS 6.0 beta with no errors (1 warning for having both solid model and FE model BCs). Please try this file as I had to change your previous input file significantly. This input file should be generic enough to run in ANSYS 5.6. The bigger challenge will be having the appropriate electrical HF excitation model."
[permalink]
|
| |
|
Average Rating: 9.1 (22 votes)
|
|
|
| |
|
Microsystem Design Using Simulator Coupling
|
| |
S. Wünsche, C. Clauß, P. Schwarz, F. Winkler
|
| |
"A methodology for simulating the performance of complex microsystems using simulator coupling is presented. The technique is based on the coupling of the FEM program ANSYS with the circuit and system simulator SABER."
[permalink]
|
| |
|
| |
|
MIDSTRES
|
| |
Peter Budgell (Innovative Steam Technologies)
|
| |
From Analysis Solutions article "MIDSTRES: An ANSYS macro to aid mid-plane shell stress and load flow evaluation", Vol. 2 Issue 4 pg. 14. Useful for postprocessing shells, modifies results such that mid-plane stresses (or load/length) is copied to shell exterior. Used with PowerGraphics averaging/noaveraging.
[permalink]
|
| |
|
Average Rating: 10.0 (2 votes)
|
|
|
| |
|
Miners-Rule
|
| |
Larry Bryant
|
| |
"I have attached a script to compute a Miners Rule summation of structural
results from three different data bases.
It is not general for any case, however, one can see the logic and apply this
to their specific case as required.
I also have a simple script here that can be used to dump out a table of results
for an independent check of your results."
[permalink]
|
| |
|
Average Rating: 3.3 (3 votes)
|
|
|
| |
|
MK_MWRITE
|
| |
Matt Sutton (PADT, Inc.)
|
| |
This is a macro to write out arrays of user-specified width. Usually, when writing a macro, one has to specify the format of *MWRITE beforehand. This is a technique of a macro writing a macro for formatting purposes.
The history of this is from XANSYS on the following post (search for "mk_mwrite").
[permalink]
|
| |
|
Average Rating: 10.0 (1 vote)
|
|
|
| |
|
MKWEB
|
| |
Mark Krueger (Goodrich Corporation)
|
| |
"Macro to connect a single node by a 'web' of beams using an area"
Be sure that you have defined the beam element type and made it active (TYPE, REAL/SECNUM, MAT) prior to using this macro.
[permalink]
|
| |
|
Average Rating: 10.0 (1 vote)
|
|
|
| |
|
Modal Cyclic Symmetry Enhancements at 6.0 [PDF]
|
| |
Sheldon Imaoka (ANSYS, Inc.)
|
| |
"At ANSYS 6.0, the modal cyclic symmetry procedure has been significantly improved. New commands, CYCLIC and CYCOPT, replace the older CYCGEN and CYCSOL macros and provide more flexibility and ease-of-use."
(Week 12, week of 12/31/01.)
[permalink]
|
| |
|
Average Rating: 7.1 (12 votes)
|
|
|
| |
|
Modeling an Electrostatically Actuated MEMS Diaphragm Pump
|
| |
James Nabity
|
| |
"The recent advent of microelectromechanical systems (MEMS) or micro-devices has generated excitement in many diverse fields. In the area of micro-fluidics liquid pumps are highly desirable for fluid transport and atomization. A recent and popular example of this is the inkjet, which self-aspirates ink from a reservoir and then transports it to a chamber for expulsion as a single droplet during the printing process. Extending this technology to other potential applications requires analytical and computational tools for design. Several computational software packages are commercially available, such as CoventorWare™, FLUENT™, and ANSYS™, but each is difficult to use and to date only ANSYS has been able to solve this fully coupled multi-physics problem. Thus, simplified analytical models are attractive for preliminary design and analysis. This paper describes a quasi one-dimensional model developed for the design and analysis of an electrostatically actuated diaphragm pump. The attributes and assumptions of this model will be presented. Finally, performance results obtained for a MEMS diaphragm pump will be compared to ANSYS three-dimensional time-accurate results."
[ANSYS Multi-field Solver, Flotran, Structural, version unspecified]
[permalink]
|
| |
|
Average Rating: 10.0 (2 votes)
|
|
|
| |
|
Modeling Approach for CVD-Diamond-based Mechanical Structures [PDF]
|
| |
P. Schmid, M. Adamschik, S. Ertl, P. Gluche, and E. Kohn
|
| |
Analysis of diamond-based MEMS devices (instead of silicon) with ANSYS.
[permalink]
|
| |
|
Average Rating: 10.0 (3 votes)
|
|
|
| |
|
Modeling Diesel Engine Cylinder Head Gaskets using the Gasket Material Option of the SOLID185 Element
|
| |
Jonathan Raub
|
| |
"The modeling of diesel engine cylinder head gasket joints is complicated by the nonlinear response of the head gasket’s materials. Linearization of these material responses can lead to significant errors in the solution’s results. The 1-dimensional nonlinear approximation made by the Gasket material option of the SOLID185 element sufficiently captures the response of the nonlinear gasket materials while maintaining practical solution times for the large model sizes associated with multi-cylinder head gasket joint models. This paper will give an overview of the model building and assembly process used to create a head gasket joint model, describe the nonlinear nature of the materials used in the model, and present comparisons of the model’s results with experimental measurements."[STI: There is a gasket-specific material & element in 6.1, not available at the time of the writing]
[permalink]
|
| |
|
Average Rating: 9.2 (26 votes)
|
|
|
| |
|
Modeling MEMS Resonant Devices Over a Broad Temperature Range [PDF]
|
| |
Russell DeAnna, Shuvo Roy, Christian A. Zorman, Mehran Mehregany
|
| |
(from ANSYS Solutions magazine, volume 1, #2) (MEMS)
[permalink]
|
| |
|
Average Rating: 10.0 (1 vote)
|
|
|
| |
|
Modeling Of Aluminum Reduction Cells Using Finite Element Analysis Techniques
|
| |
Imad Tabsh, Marc Dupuis
|
| |
"This paper summarizes the authors' experience in using FEA to model Hall-Héroult reduction cells. FEA capabilities necessary to adequately simulate thermo-electric, electro-magnetic and stress fields within the cell are identified." (Used ANSYS 4.4A and 5.0)
Available is an older, related paper on Thermo-Electric Coupled Field Analysis of Aluminum Reduction Cells Using the ANSYS Parametric Design Language.
[permalink]
|
| |
|
Average Rating: 9.0 (5 votes)
|
|
|
| |
|
Modeling of the Piezoelectric Micropump for Improving the Working Parameters [PDF]
|
| |
Oana Tatiana Nedelcu, Victor Moagar-Poladian
|
| |
A piezo micropump. Used ANSYS for analysis of deflection of pump. (MEMS)
[permalink]
|
| |
|
Average Rating: 10.0 (9 votes)
|
|
|
| |
|
Modeling preloaded bolts [PDF]
|
| |
Sheldon Imaoka (CSI)
|
| |
Modeling preload in bolts via contact offset, thermal contraction, or the new pretension elements PRETS179.
PRELOAD1, PRELOAD2, and PRELOAD3 input files
[permalink]
|
| |
|
Average Rating: 10.0 (12 votes)
|
|
|
| |
|
Modeling Viscous Behavior [ZIP]
|
| |
Sheldon Imaoka (ANSYS, Inc.)
|
| |
"Amorphous solids or solids at elevated temperatures may exhibit viscous behavior. It
may be difficult for some users to determine how best to model such behavior. This
memo hopes to describe some available options in ANSYS and to differentiate between
viscoelastic and viscoplastic constitutive models."
(Week 36, week of 12/03/06.)
[permalink]
|
| |
|
Average Rating: 10.0 (10 votes)
|
|
|
| |
|
Modelling and Experimental Investigations on Degradation of Microcomponents in Power Cycling
|
| |
M. Thoben, W. Staiger, J. Wilde
|
| |
"Thermomechanical damage is one of the principal failure causes of microcomponents and microsystems. Often the basic defect mechanisms are crack initiation and subsequent crack propagation in interfaces or materials. The fatigue behavior of microcomponents can in many cases be described by the Manson-Coffin-Formula. This model is well-suited for comparison of different designs relative to each other but it will fail when a realistic lifetime prognosis is expected. Therefore we worked out a concept which is based on the computation of the strain range distribution in the interconnection by finite elements simulations and subsequent calculation of the cyclic crack propagation rate. Using this method in combination with calibration measurements it is possible to predict the lifetime of electronic assemblies with significantly improved precision compared to the Low-Cycle-Fatigue approaches."
[permalink]
|
| |
|
Average Rating: 10.0 (9 votes)
|
|
|
| |
|
MODESHAP
|
| |
Sheldon Imaoka (CSI)
|
| |
Plots four modes on screen and annotates plots
[permalink]
|
| |
|
Average Rating: 10.0 (8 votes)
|
|
|
| |
|
MODIFY |
| |
MODIFY, SET, LSTEP, ITER, CUMIT, TIME, Ktitle
Fields LSTEP, ITER, CUMIT, and TIME accept the value of "-1" to retain current values.
Fields LSTEP, ITER, and CUMIT also accept the value of "0" to retain current values, although TIME does not.
For an example, see the tip on changing the title of the results file.
[permalink]
|
| |
|
Average Rating: 10.0 (2 votes)
|
|
|
| |
|
MOPT |
| |
MOPT,STAT,ALL
Shows ALL meshing controls available to user
[permalink]
|
| |
|
| |
|
MOPT |
| |
MOPT,TSMO,OFF
Turns off smoothing if errors cause mesh smoothing failure [5.3]
[permalink]
|
| |
|
Average Rating: 10.0 (2 votes)
|
|
|
| |
|
MOPT |
| |
MOPT,LSMO,ON
Turns on line smoothing option [off by default at 5.3]. Causes locations of nodes on the boundary to be optimized as part of the smoothing option.
[permalink]
|
| |
|
| |
|
MOPT |
| |
MOPT,VSSM,OFF
Below describes an option for controlling "node relaxation" when using the VSWEEP command. This is needed when using VSWEEP with volumes that are axisymmetric, where you might have previously used VROT. The purpose of this option is to ensure that the nodes on opposite sides of the volume are positioned with identical radial and axial coordinates. When you create couples for cyclic symmetry, your nodes will match up precisely.
By default node relaxation is turned on. If you see that the source and target area are identical, you can issue the command.
If you have it turned off and you try to sweep a volume that changes in cross section, then you'll probably get bad quality elements.
[command available in 5.5.1 and above]
[permalink]
|
| |
|
Average Rating: 7.5 (4 votes)
|
|
|
| |
|
MOR for ANSYS
|
| |
Jan G. Korvink (University of Freiburg) and Evgenii B. Rudnyi (CADFEM)
|
| |
MOR for ANSYS (formerly mor4ansys) is "Model Order Reduction for ANSYS", useful to speed up transient or harmonic analyses.
[permalink]
|
| |
|
Average Rating: -5.8 (6 votes)
|
|
|
| |
|
MPC_GEN
|
| |
Ted Harris (PADT)
|
| |
Creates MPC184 elements between a master node and the other selected nodes. Can be modified for other 2-node line element types. Example of the use of *VMASK.
[permalink]
|
| |
|
Average Rating: 9.6 (12 votes)
|
|
|
| |
|
MPSCALE
|
| |
(CAEAI)
|
| |
Macro to scale linear material property and put into new material number.
[permalink]
|
| |
|
Average Rating: 10.0 (2 votes)
|
|
|
| |
|
MSHDVOLS
|
| |
Bob Weathers (Trane)
|
| |
Selects meshed volumes.
[permalink]
|
| |
|
Average Rating: 10.0 (2 votes)
|
|
|
| |
|
MUFFLER
|
| |
Sheldon Imaoka (ANSYS, Inc.)
|
| |
This memo provides basic instruction on performing acoustic analyses in Workbench Mechanical 14.0. An example of calculation of transmission loss in a muffler is demonstrated.
[permalink]
|
| |
|
Average Rating: 8.9 (27 votes)
|
|
|
| |
|
Multi-Criteria Shape Optimization of a Funnel in Cathode Ray Tubes Using Response Surface Model
|
| |
Tae Hee Lee, Kwangki Lee, Kwang Soon Lee
|
| |
"The ultimate goal of simulation that represents the behaviour of structures is to optimize their response performances within the specific requirements and needs with respect to the design variables. The first step of the design of cathode ray tubes is to design the glass geometry, called funnel geometry, to endure the vacuum stress because it is a main structure of cathode ray tubes. In order to create 3-dimensional funnel geometry in the cathode ray tubes, higher order response surface model is used instead of NURBS (non-uniform rational B-splines) or Bezier curve because it is more robust for understanding the geometry change in finite element analysis. By combining finite element analysis, response surface model and sequential quadratic programming within the process integration framework, the shape optimization of a funnel is successfully performed and the maximum stress is reduced to almost half of the current one."
[permalink]
|
| |
|
Average Rating: 7.1 (7 votes)
|
|
|
| |
|
Multiframe Restarts [PDF]
|
| |
Sean Harvey (CSI)
|
| |
Memo covering the multiframe restart capability (RESCON) in ANSYS.
Accompanying input file
[permalink]
|
| |
|
Average Rating: 4.5 (10 votes)
|
|
|
| |
|
MULTIPRO
|
| |
(ANSYS, Inc.)
|
| |
SCOPUS #6743
Gets rid of "Unknown Expression in input line" msg
[permalink]
|
| |
|
Average Rating: 10.0 (16 votes)
|
|
|
| |
|
MULTIPRO |
| |
Useful means of prompting user for input for multiple variables (a cleaner alternative to *ASK).
The MULTIPRO macro is located in the "docu" directory (e.g., /ansys55/docu). This allows a user to specify a dialog box to prompt a user for several pieces of info (better alternative than several *ASK commands). View the MULTIPRO.MAC macro in a text editor to see how to use this command.
(Another nice use for MULTIPRO is a simple OK/Cancel dialog box)
Also, there is the Tcl version of the MULTIPRO macro with a Test macro.
Lastly, there is also a ANSYS and Tcl (10/20/99) package by John Swanson which covers a lot of applications of Tcl, including multiprompt.tcl.
[permalink]
|
| |
|
Average Rating: 10.0 (3 votes)
|
|
|
| |
|
MULTP2
|
| |
Sean Harvey (CSI)
|
| |
Macro that facilitates importing multiple parts using the Connection product for Pro/E at 5.5.x. Note that from 5.6.1, importing of Pro/E assembly is supported (it is a beta feature in 5.6.0)
[permalink]
|
| |
|
Average Rating: 3.3 (3 votes)
|
|
|
| |
|
MULTREAD
|
| |
Sean Harvey (CSI)
|
| |
Macro that facilitates importing multiple part iges files into ANSYS at 5.5.x
[permalink]
|
| |
|
Average Rating: 10.0 (3 votes)
|
|
|
| |
|
MVSUM
|
| |
Alex Ng (ASM Assembly Automation Ltd.)
|
| |
Calculates total mass of selected volumes.
[permalink]
|
| |
|
Average Rating: 6.7 (3 votes)
|
|
|
| |
|
MWRITE
|
| |
Matt Sutton (PADT)
|
| |
Macro to write arrays to file. This macro actually uses Tcl/Tk to write another macro, which is then invoked.
[permalink]
|
| |
|
Average Rating: 9.2 (13 votes)
|
|
|
| |
|
MY_ROT
|
| |
Peter Budgell (Innovative Steam Technologies)
|
| |
A quick and dirty animation of rotation
[permalink]
|
| |
|
Average Rating: 10.0 (6 votes)
|
|
|
| |
|
MYANIM
|
| |
Peter Budgell (Innovative Steam Technologies)
|
| |
The following simple animation macro has worked for me with user-set contour level values. The user indicates the time delay for each frame, and the number of substeps to plot.
[permalink]
|
| |
|
Average Rating: 10.0 (5 votes)
|
|
|
| |
|
NameContactsByParts
|
| |
(ANSYS, Inc.)
|
| |
Macro to change all contact regions in Workbench to names of its contact parts.
[permalink]
|
| |
|
Average Rating: 10.0 (13 votes)
|
|
|
| |
|
NAS2ANS
|
| |
Diego Gorriz (Skycross Engineers)
|
| |
Example of a macro to convert Nastran input to ANSYS input. Works on shells only, so it should be used as an example.
[permalink]
|
| |
|
Average Rating: 10.0 (13 votes)
|
|
|
| |
|
NASTEXP
|
| |
Barry O'Donnell (ODCS Ltd.)
|
| |
"The macro uses logic (primariliy extracted from a previously published
macro) to identify the unique combinations of ETYPE, REAL and MAT for
non-section based elements and ETYPE, SECTYPE and MAT for secrion based
elements. It then gathers the relevant data into arrays (primarily vector
based arrays), and outputs the following NASTRAN cards:
CONM2 (mass21 element)
PSHELL (based on real data only, i.e. shell63)
CTRIA3 (shell63 degenerate elements recognised)
CQUAD4 (shell63 elements)
PBAR (beam4 element or beam188 element, A/Iyy/Izz supported)
CBAR (beam4 element or beam188 element, orientation node exported if it
exists and default vector of <0 1 0> exported otherwise)
CELAS2 (combin14, spring option, linear 2 node version only)
PROD (link180 element, A supported)
CROD (link180 element)
PSOLID (solid element property definition card, fully supported)
CHEXA (solid 185 and solid 45 fully supported, solid 186 & solid 95 not
working correctly)
CPENTA (solid 185/45/186/95 fully supported, degenerate elements recognised)
CTETRA (solid 185/45/186/95 & solid 186 & 95 fully supported)
GRID (nodal coordinates, note: nodal csys = 0)
MAT1 (E, nu, dens supported - non temp dependent, initial value supported
only)"
[permalink]
|
| |
|
Average Rating: 9.0 (10 votes)
|
|
|
| |
|
NAT_CONV3D
|
| |
Sheldon Imaoka (CSI)
|
| |
Simple natural convection problem of chip on board, 3D hex.
[permalink]
|
| |
|
Average Rating: 10.0 (11 votes)
|
|
|
| |
|
NBETWEEN |
| |
NBETWEEN,n1,n2,nnew,type,value
identical to KBETWEEN - generates a node between two other nodes
[permalink]
|
| |
|
Average Rating: 10.0 (2 votes)
|
|
|
| |
|
NDGROUP
|
| |
John Crawford (Honeywell)
|
| |
From the author:
"ndgroup.mac a macro which creates a macro of nsel commands for the currently selected nodes. this group of nodes can be recovered by running the macro that this macro creates.
The macro will prompt the user for the name of the file which will be created. The default name is 'ndgrp1.mac'.
You might check the implementation of *ASK to see if it works okay. I think they changed the way *ASK uses character parameters a few revisions ago and I may not have updated this macro. There is a chance that it will always create a file named "fname.mac" regardless of the name you entered at the *ASK prompt."
[permalink]
|
| |
|
Average Rating: 10.0 (1 vote)
|
|
|
| |
|
NDGROUP2
|
| |
Joe Woodward (PADT)
|
| |
"A macro which creates a macro of nsel commands for the currently selected nodes. this group of nodes can be recovered by running the macro that this macro creates. The macro will prompt the user for the name of the file which will be created. The default name is 'ndgroup.mac'."
Original macro by John Crawford, vectorized by Joe Woodward.
[permalink]
|
| |
|
Average Rating: 10.0 (2 votes)
|
|
|
| |
|
Neighborhood-based Element Sizing Control for Finite Element Surface Meshing [PDF]
|
| |
Steven Owen, and Sunil Saigal
|
| |
"A method is presented for controlling element sizes on the interior of areas during surface meshing. A Delaunay background mesh is defined over which a neighborhood based interpolation scheme is used to interpolate element sizes."
[permalink]
|
| |
|
Average Rating: 10.0 (1 vote)
|
|
|
| |
|
NELEM |
| |
NELEM
Selects the nodes attached to the currently active elements.
[permalink]
|
| |
|
Average Rating: 9.0 (10 votes)
|
|
|
| |
|
Nested macros, local parameters, trailing underscores
|
| |
Martin Herrenbruck (Technische Universität München)
|
| |
"A macro file is a file which contains Ansys commands. If you save your macro in your working directory or in the macro directory (see /PSEARCH command) you just enter the macro name in the command line and all these commands will be executed. You can even nest macros: from your main file you call e.g. zzmacro1 which again calls zzmacro2. The only problem is that a macro could change - and you would probably not notice that - the value of a parameter you are using in your main input file. This will be the case if the same parameter name is used accidentally in both the macro and your main input. Let's see how one can avoid these nasty errors - just click on the link!"
[permalink]
|
| |
|
Average Rating: 10.0 (1 vote)
|
|
|
| |
|
NFIXDEL
|
| |
John Crawford (Honeywell)
|
| |
"A macro that removes the selected nodes that are mistakenly associated with nonexistent geometry in ANSYS."
[permalink]
|
| |
|
Average Rating: 6.2 (4 votes)
|
|
|
| |
|
NFORCE |
| |
NFORCE,CONT
Calculates nodal contact forces only for CONTA171-174 (at 5.6.1)
[permalink]
|
| |
|
Average Rating: 10.0 (8 votes)
|
|
|
| |
|
NIP
|
| |
Dave Lindeman (3M)
|
| |
Example analysis of a head/media/roller NIP (structural nonlinear). Shows use of *VWRITE to write out an ABAQUS input deck.
[permalink]
|
| |
|
Average Rating: 6.7 (9 votes)
|
|
|
| |
|
NLIST |
| |
NLIST,all,,,xyz
Shows more significant digits for node listings.
[permalink]
|
| |
|
Average Rating: 10.0 (4 votes)
|
|
|
| |
|
NO_WEAK_SPRINGS |
| |
Set variable "no_weak_springs" to "1" to disable use of weak springs in DesignSpace, if you do not want this feature.
"(DS will add weak springs for several reasons. First it will add them if it detects that your model is underconstrained. Secondly it will add them if it finds contact conditions other than bonded. This is because
although you are specifying no-separation, the parts may still slide relative to one another. Weak springs are added in case you do not provide
adequate constraint to prevent free sliding. Assuming you have real life loads and adequate constraints to stop free sliding, the weak springs should have no affect on your answer and the message can be ignored.)", Al Hancq (ANSYS, Inc.)
[permalink]
|
| |
|
Average Rating: 10.0 (18 votes)
|
|
|
| |
|
NOD2KP
|
| |
(EMI)
|
| |
This is an ANSYS macro to move an existing node to the location of an existing keypoint. User picks single node to be moved, then picks single keypoint to move it to.
[permalink]
|
| |
|
Average Rating: 6.7 (3 votes)
|
|
|
| |
|
Non-Linear Elastic Properties of the Lingual and Facial Tissues Assessed by Indentation Technique: Application to the Biomechanics of Speech Productio
|
| |
J.M. Gerard, J. Ohayon, V. Luboz, P. Perrier, Y. Payan
|
| |
"This paper aims at characterizing the mechanical behavior of two human anatomical structures, namely the tongue and the cheek. For this,
an indentation experiment was provided, by measuring the mechanical response of tongue and cheek tissues removed from the fresh cadaver
of a 74 year old woman. Non-linear relationships were observed between the force applied to the tissues and the corresponding displacements.
To infer the mechanical constitutive laws from these measurements, a finite element (FE) analysis was provided. This analysis aimed at
simulating the indentation experiment. An optimization process was used to determine the FE constitutive laws that provided the non-linear
force/displacements observed during the indentation experiments. The tongue constitutive law was used for simulations provided by a 3D FE
biomechanical model of the human tongue. This dynamical model was designed to study speech production. Given a set of tongue muscular
commands, which levels correspond to the force classically measured during speech production, the FE model successfully simulated the
main tongue movements observed during speech data."
[ANSYS Nonlinear, version 5.7]
[permalink]
|
| |
|
Average Rating: 10.0 (3 votes)
|
|
|
| |
|
Non-linear Finite Element Modeling of the Titanium Briquettes Hot Extrusion Process
|
| |
Alexey I. Borovkov, Denis V. Shevchenko
|
| |
"In this paper the mathematical model is developed to perform mathematical simulation of the hot extrusion process. The model makes it possible to observe the influence of various system parameters on the extrusion process. All researches were carried out with the use of the ANSYS 5.6 RFS FE-software system. During the research the modeling and analysis of various events that can be observed (material dead zone appearing, capsule crimping, capsule damage etc.) was successfully carried out. The mathematical model was created on the basis of contact thermo-mechanics relations with physical and geometrical non-linearities."
[permalink]
|
| |
|
Average Rating: 10.0 (11 votes)
|
|
|
| |
|
Non-Linear Problems Of Steel Civil Engineering Structures
|
| |
Milan Vasek
|
| |
"The civil engineering structures are today designed with respect to the limit state of serviceability and limit states of the strength and stability. The design of more efficient and light structures leads to the nonlinear analysis of deflections and stresses. Some parts of structure could reach the yield point under the design load. Some parts of structure could lose their local stability. These complex problems of a different nature are possible to solve by FEM methods."
[permalink]
|
| |
|
Average Rating: 8.0 (37 votes)
|
|
|
| |
|
Nonlinear Contact Analysis Techniques Using ANSYS
|
| |
(ANSYS, Inc.)
|
| |
Presentation on various aspects of 17x contact technology (part of the "Advanced Analysis with ANSYS" seminar during the 2002 User's Conference).
[permalink]
|
| |
|
Average Rating: 10.0 (20 votes)
|
|
|
| |
|
Nonlinear Mechanics of Suspension Beams for a Micromachined Gyroscope
|
| |
W. O. Davis and A. P. Pisano
|
| |
"We present a method for the calculation of the coefficients of cubic stiffening for tether-suspended micromachined systems. The analysis is based on a nonlinear rod theory, and enables the prediction of the maximum achievable motion amplitude prior to the onset of nonlinear behavior. The analysis is applied in detail to a microgyroscope. Comparisons with a finite element model and experimental data are used to validate the analysis, and issues pertaining to the optimal design of the gyroscope's suspension are investigated." (MEMS)
[permalink]
|
| |
|
Average Rating: 10.0 (1 vote)
|
|
|
| |
|
Nonlinear Models of Reinforced and Post-tensioned Concrete Beams
|
| |
P. Fanning
|
| |
"Commercial finite element software generally includes dedicated numerical models for the nonlinear response of concrete under loading. These models usually include a smeared crack analogy to account for the relatively poor tensile strength of concrete, a plasticity algorithm to facilitate concrete crushing in compression regions and a method of specifying the amount, the distribution and the orientation of any internal reinforcement. The numerical model adopted by ANSYS is discussed in this paper. Appropriate numerical modelling strategies are recommended and comparisons with experimental load-deflection responses are discussed for ordinary reinforced concrete beams and post-tensioned concrete T-beams." (Concrete SOLID65)
[permalink]
|
| |
|
Average Rating: 9.6 (23 votes)
|
|
|
| |
|
Nonlinear monitoring [PDF]
|
| |
Sheldon Imaoka (CSI)
|
| |
Memo covering the benefits of the jobname.mntr file and the MONITOR command in nonlinear analyses.
[permalink]
|
| |
|
Average Rating: 10.0 (9 votes)
|
|
|
| |
|
Nonlinear Stress Analysis and Optimization of a Welded Plate Steel Pro/ENGINEER Assembly
|
| |
Andrew J. Bax, Chris Andersen, Shane Vander Kooi
|
| |
From 1996 Conference
[permalink]
|
| |
|
Average Rating: 8.4 (37 votes)
|
|
|
| |
|
Nonlinear Submodeling [ZIP]
|
| |
Sheldon Imaoka (ANSYS, Inc.)
|
| |
"Submodeling is often used to efficiently obtain solutions at local areas. Although submodeling
may be commonly thought of as being applicable to linear static structural solutions, it can also be
applied to nonlinear and transient analyses, as well as other disciplines. This memo hopes to cover
the specific case of nonlinear static structural submodeling."
(Week 14, week of 01/14/02.)
[permalink]
|
| |
|
Average Rating: 9.7 (19 votes)
|
|
|
| |
|
Nonlinear-Time-Dependent Analysis of Micro Via-in-Pad Substrates for Solder Bumped Flip Chip Applications
|
| |
John H. Lau, S. W. Ricky Lee, Stephen H. Pan, and Chris Chang
|
| |
"An elasto-plastic-creep analysis of a low-cost micro via-in-pad (VIP) substrate for supporting a solder bumped flip chip in a chip scale package (CSP) format soldered on a PCB is presented in this study." (Nonlinear, Anand)
[permalink]
|
| |
|
Average Rating: 1.7 (3 votes)
|
|
|
| |
|
Novel Horn Designs for Ultrasonic/Sonic Cleaning Welding, Soldering, Cutting and Drilling
|
| |
S. Sherrit, S.A. Askins, M. Gradziol, B.P. Dolgin, X. Bao, Z. Chang, and Y. Bar-Cohen
|
| |
"In this paper we will present a variety of novel horn
designs, which overcome some of the limitations discussed above. One particular design that has been found to overcome
these limitations is the folded horn. In this design the horn elements are folded which reduce the overall length of the
resonator (physical length) but maintain or increase the acoustic length. In addition initial experiments indicate that the tip
displacement can be further adjusted by phasing the bending displacements and the extensional displacements. The
experimental results for a variety of these and other novel horn designs will be presented and compared to the results
predicted by theory."
[ANSYS Piezoelectric, version unknown]
[permalink]
|
| |
|
Average Rating: 10.0 (3 votes)
|
|
|
| |
|
NROPT |
| |
NROPT,FULL,,ON,,A1,B1,C1,A0,B0,C0
A1,B1,C1 are for the first substep
A0,B0,C0, are for all other substeps
A=starting value for the descent parameter on this substep
B=multiplication factor for decreasing descent parameter
C=number of consecutive iterations with decreasing convergence value before multiplication factor is applied
Settings that have been good to me for some contact analysis problems have been nropt,full,,on,,,,1,0.7,5 This essentially would allow the contact elements to hold together longer by adaptive descent when physically they should not be contacting. They are slowly released for improved stability and convergence.
[permalink]
|
| |
|
Average Rating: 10.0 (4 votes)
|
|
|
| |
|
NS_From_Unique_Names
|
| |
(ANSYS, Inc.)
|
| |
In Design Simulation 8.0, Named Selections can be imported from Pro/E. However, only one surface is given a name...
"Attribute transfer from Pro/E is particularly limited since each entity within a part needs to have a unique name. That means that our processing for named selections becomes particularly ineffective since we group entities of like name (exact match only) for named selections. These same attributes can be imported as general attributes and then "grouped" by a different paradigm with the use of the script attached.
Here the expectation is that user would create a common naming structure (beginning with NS, though this could be modified with a simple script change) for the entities that would belong to a named selection and make them unique based on a "_N" suffix. N here is meant to be some counting number though it could be any unique string."
[permalink]
|
| |
|
Average Rating: 8.3 (3 votes)
|
|
|
| |
|
NUMCMP |
| |
NUMCMP,NODE,EORD
NUMCMP,ELEM,ELEM
These commands will cause the nodes and elements to be renumbered, after compression, to match the sequence in which they will be processed by the solver. This should be done after the WAVE command to (a) put the nodes in the element order and (b) put the elements in the new order.
[permalink]
|
| |
|
Average Rating: 10.0 (5 votes)
|
|
|
| |
|
Numerial Implementation of Multiaxial High-Cycle Fatigue Criterion to Structural Optimization
|
| |
Miroslaw Mrzyglód, Andrzej P. Zielinski
|
| |
"Modern multiaxial high-cycle fatigue criteria were investigated with respect
to their application in structural optimization procedures coupled
with finite element codes. As a result of tests carried out for several fatigue
criteria, the Dang Van hypothesis was used for the detailed numerical
study. A way of respective adapting the high-cycle load history was also
suggested. The complete algorithm of the fatigue optimization was illustrated
by applying the proposed procedures to vehicle parts which are
subject to high-cycle loadings. The finite element code ANSYS was
used in the structural modeling."
[ANSYS Structural, version 8.1]
[permalink]
|
| |
|
Average Rating: 5.0 (4 votes)
|
|
|
| |
|
Numerical Analysis of Plastic Encapsulated Electronic Package Reliability: Viscoelastic Properties of Underfill Resin
|
| |
Man-Lung Sham, Jang-Kyo Kim, Joo-Hyuk Park
|
| |
"The reliability and mechanical performance of electronic integrated circuit (IC) package is studied based on the finite element analysis."
ANSYS Nonlinear, version 5.7.
[permalink]
|
| |
|
| |
|
Numerical And Analytical Modeling Of The Piezoelectric Transformer And Experimental Verification [PDF]
|
| |
S. Hallaert , E. Sarraute and B. Le Pioufle
|
| |
Use of ANSYS for modal analysis of miniature piezo transformer. (MEMS)
[permalink]
|
| |
|
Average Rating: 7.0 (5 votes)
|
|
|
| |
|
Numerical Evaluation of Thermal Cycling Reliability of High Performance Flip-Chip Package Assembly Using Submodeling Analysis
|
| |
Chin-Li Kao, Yi-Shao Lai, and Tong Hong Wang
|
| |
"This paper applies the submodeling technique in analyzing thermal cycling reliability
of high performance flip-chip ball grid array package assemblies. The packages
have one-piece tunnel-type heat spreaders with different lead widths, connected
to chips using different thermal interface materials. The global model contains no
solder bumps to simplify the analysis. The calculated displacement field of the global
model is then interpolated on the boundary of the submodel that contains the critical
solder bump. The submodel is solved using the prescribed displacement boundary
conditions together with external thermal loads to evaluate thermomechanical reliability
of the critical solder bump."
ANSYS Nonlinear (Anand Model), version 7.0
[permalink]
|
| |
|
Average Rating: 9.0 (5 votes)
|
|
|
| |
|
Numerical Modeling for Systematization of Line Heating Process
|
| |
Jong-Gye Shin, Won-Don Kim, and Jang-Hyun Lee
|
| |
"In this paper, we first propose a conceptual configuration for ship production system of plate forming. It is necessary to integrate lofting and plate forming activities for minimum thermal energy in line heating process. The modeling of heating torch, water cooling, and plate to be formed is proposed for the finite element analysis after the mechanics of line heating is studied. A three-dimensional 8-node solid elements of ANSYS were chosen for analysis." (Thermal-Stress)
[permalink]
|
| |
|
Average Rating: 10.0 (6 votes)
|
|
|
| |
|
Numerical Simulations of Flat-walled Diffuser Elements for Valveless Micropumps [PDF]
|
| |
Anders Olsson, Goran Stemme, and Erik Stemme
|
| |
Use of ANSYS/Flotran for analysis of micropump. (MEMS)
[permalink]
|
| |
|
Average Rating: 10.0 (4 votes)
|
|
|
| |
|
NUMTOG
|
| |
John Crawford (Honeywell)
|
| |
A macro that toggles ID numbers off and on for keypoints, lines, areas, volumes, nodes, and elements.
[permalink]
|
| |
|
Average Rating: 10.0 (2 votes)
|
|
|
| |
|
Off-Axis Loads Cause Failure of the Distal Radius at Lower Magnitudes than Axial Loads: A Finite Element Analysis
|
| |
Karen L. Troy and Mark D. Grabiner
|
| |
"Distal radius fractures are among the most
common fall-related injuries in older
women. Numerous studies have quantified
upper extremity fall biomechanics with the
goal of identifying possible interventions to
reduce the peak force on the wrists, thereby
reducing the number of fractures.
Fracture initiation depends both on the force
applied to the bone and upon the strength of
the bone itself; thus, poor bone quality has
been implicated as a factor in distal radius
fractures. Generally, an intervention to
improve bone quality (such as antiresorptive
therapy) is considered successful
if bone mineral density (BMD) can be
increased by 2-4%.
Cadaver and finite element studies have
previously quantified the force required to
cause a distal radius fracture. To date,
however, only simple axial loads on the
radius have been considered. Because most
falls onto the hands result in off-axis loads,
we considered the possibility that a
combination of loading modes would
significantly influence the fracture strength
of the distal radius. Here, we used a
validated finite element model of the distal
radius, scaphoid, and lunate, to explore the
effects of loading direction and changes in
BMD on predicted fracture strength."
[ANSYS Structural, version 10.0]
[permalink]
|
| |
|
Average Rating: 3.3 (3 votes)
|
|
|
| |
|
OFFSET
|
| |
Sheldon Imaoka (ANSYS, Inc.)
|
| |
Shows difference between geometric offset and contact offset (CNOF real constant), useful in interference fit problems (so you don't have to modify geometry iteratively).
[permalink]
|
| |
|
Average Rating: 8.7 (19 votes)
|
|
|
| |
|
On Stress Analysis For a Hyperelastic Material [PDF]
|
| |
Xiao-Yan Gong and Riyand Moe
|
| |
Paper using ANSYS 5.5 for characterizing hyperelastic materials with Mooney-Rivlin
[permalink]
|
| |
|
Average Rating: 10.0 (12 votes)
|
|
|
| |
|
OPFACT |
| |
OPFA,3LEV
To perform a 3-level BOX-BEHNKEN factorial analysis:
OPTYP,FACT
OPFA,3LEV
[permalink]
|
| |
|
Average Rating: 10.0 (1 vote)
|
|
|
| |
|
OPNCONTROL |
| |
OPNCONTROL,OPENUPFACTOR,opnvalue
For automatic time-stepping, this controls the factor by which the timestep is increased if convergence is attained easily. The value of opnvalue defaults to 1.5 (it was 2.0 in older releases of ANSYS) and should be greater than 1.0. (see related undocumented CUTCONTROL,CUTBACKFACTOR command.)
[STI: now documented in latest ANSYS releases.]
[permalink]
|
| |
|
Average Rating: 0.0 (2 votes)
|
|
|
| |
|
Optimal Design of Computer Experiments for the Generation of Microsystem Macromodels Using IMSET and Non-Parametric Fitting
|
| |
Selden B. Crary, Peter Cousseau, David Armstrong, David M. Woodcock, Olivier Dubochet, Philippe Lerc
|
| |
"We present a new and unique software program, IMSET, capable of finding optimal designs for computer experiments. A finite-element simulation of a micro-machined flow sensor was used to illustrate macromodel generation and to compare the quality of the IMSET design with other approaches."
[permalink]
|
| |
|
| |
|
Optimization in high-precision glass forming
|
| |
M. Sellier
|
| |
"The question of interest in the present study is the inverse problem
for high precision glass forming, i.e. "How to design the mould and the temperature
regime so that at the very end of the forming process we will get at room temperature
a prescribed glass geometry with a precision in the order of the Micron?" The aim
is to eliminate from the manufacturing process the costly and time-consuming postprocessing
when the final shape does not conform precisely to the desired one."
[permalink]
|
| |
|
| |
|
Optimization of a Circular Piezoelectric Bimorph for a Micropump Driver
|
| |
Christopher J. Morris and Fred K. Forster
|
| |
"Piezoelectric bimorph actuation has been successfully used in numerous types of microdevices, most notably micropumps. However, even for the simple case of circular geometry, analytical treatments are severely limited. This study utilized the finite-element method to optimize the deflection of a circular bimorph consisting of a single piezoelectric actuator, bonding material and elastic plate of finite dimensions. Optimum actuator dimensions were determined for given plate dimensions, actuator-to-plate stiffness ratio and bonding layer thickness." (PLANE13)
[permalink]
|
| |
|
Average Rating: 2.0 (5 votes)
|
|
|
| |
|
Optimizing Board-level Reliability of an Underfilled, Stacked Chip Scale Package
|
| |
Zane E. Johnson, Nathan R. Schneck
|
| |
"Previously benchmarked finite-element (FE) models of a stacked chip scale package (CSP) are used to identify optimum underfill material properties under drop-impact and accelerated temperature cycling (ATC) stress conditions. The simulation sets indicate that an underfill having a modulus of 2–6 GPa and CTE of 25 ppm/K maximizes drop life and does no harm to ATC performance for both Sn63Pb37 and SAC305 solder joints. The methodology described can be applied to other package styles, material sets, and stress conditions."
[permalink]
|
| |
|
Average Rating: 10.0 (1 vote)
|
|
|
| |
|
Optimizing Linux Clusters for ANSYS 11
|
| |
Joshua Bernstein and Arend Dittmer (Penguin Computing)
|
| |
Introduction from paper:
"In many organizations design engineers perform FEA (Finite Element Analysis) based simulations on personal desktop systems. Even though increasing hardware performance has enabled the solution of complex problems on desktop systems, this approach has limitations. Interactive design work on the desktop is interrupted by compute intensive simulation runs, negatively affecting productivity. Moreover this approach requires high-powered desktop systems that are not shared with other users and therefore only fully utilized for relatively short periods of time. An approach, where simple simulations are run on desktop systems and more complex problems are solved on shared 'back-end' compute systems is more efficient. Due to their excellent price/performance ratio, Linux based clusters of commodity systems have become the dominating platform for these 'back-end' computations. While Linux-based clusters are a cost effective way to address the always increasing demand for compute cycles, the concept of achieving high performance through interconnected systems introduces performance and manageability challenges. This paper introduces how the choice of a cluster architecture and the selection of hardware components can impact cluster manageability and ANSYS application performance."
[permalink]
|
| |
|
| |
|
Optimum Design of a Ceramic Tensile Creep Specimen Using a Finite Element Method
|
| |
Z. Wang, C. K. Chiang, and T. J. Chuang
|
| |
"An optimization procedure for designing a ceramic tensile creep specimen to minimize stress concentration is carried out using a finite element method." (Optimization, Creep, Contact)
[permalink]
|
| |
|
Average Rating: 8.8 (4 votes)
|
|
|
| |
|
Options for ADAMS.MAC
|
| |
Sheldon Imaoka (ANSYS, Inc.)
|
| |
The ADAMS.MAC macro enables ANSYS users to generate MNFs for flexible bodies for use in ADAMS. The user can set an environment variable MDI_MNFWRITE_OPTIONS that can reduce the size of the MNF, as well as provide other options also available through the ADAMS/Flex Toolkit The temporary directory where the MNF is written can also be specified by the user.
[permalink]
|
| |
|
Average Rating: 10.0 (3 votes)
|
|
|
| |
|
OUTEQ |
| |
OUTEQ outputs all results from equilibrium iterations while in /SOLU.
[permalink]
|
| |
|
Average Rating: 10.0 (3 votes)
|
|
|
| |
|
OUTRES
|
| |
Sheldon Imaoka (ANSYS, Inc.)
|
| |
This is a simple example of using OUTRES with an array parameter to define at what time points results will be saved.
This is useful if you want to control exactly when results will be stored, even with the automatic timestepping algorithm present.
[permalink]
|
| |
|
Average Rating: 10.0 (2 votes)
|
|
|
| |
|
OUTS |
| |
OUTS,value
Controls writing of the jobname.stat file every value minutes (default is 6 minutes). The jobname.stat file is written in batch mode, and it provides the status (analogous to status bar in interactive mode) for some commands which may take a while. For example, for the SOLVE command, it will write out element formation, element solution, and PCG information every value minutes in batch mode. Can be issued in /PREP7 or /SOLU.
[permalink]
|
| |
|
Average Rating: 10.0 (2 votes)
|
|
|
| |
|
Overview of Reliability Models and Data Needs
|
| |
Ahmer Syed
|
| |
"Workshop on Modeling and Data Needs for Lead-Free Solders" (Amkor Presentation) Note that FEA pictures in presentation are ANSYS plots - Darveaux's data is based on Anand's Model (TB,ANAND), although ANSYS also allows for use of common creep laws such as hyperbolic sine and power law.
[permalink]
|
| |
|
Average Rating: 10.0 (2 votes)
|
|
|
| |
|
P |
| |
P,node1,node2,value,,,,node3,node4
Applies pressure of "value" to element face defined by node1-node4. An alternative to SF command since this command does not require selection of nodes and element faces prior.
[permalink]
|
| |
|
Average Rating: 10.0 (3 votes)
|
|
|
| |
|
P_DIRLBL
|
| |
Chris Kennedy (Think PEAK, Inc.)
|
| |
From the author:
You can use the attached macro. This is supplied without warranty, etc.
It places the directory, date, time, hostname at the top of the graphics window.... There are additional args that can also extract and post the jobname. Read the macro (at least the top of it.)
P_LOGO2 is a macro that places my company logo on the screen. You can remove that command.... unless you want it! :-)
[permalink]
|
| |
|
Average Rating: 10.0 (2 votes)
|
|
|
| |
|
P_NLIST
|
| |
Chris Kennedy (Think PEAK, Inc.)
|
| |
A special version of NLIST to list nodes in the active coordinate system.
[permalink]
|
| |
|
Average Rating: 10.0 (1 vote)
|
|
|
| |
|
P_PROTEC
|
| |
Chris Kennedy (Think PEAK, Inc.)
|
| |
Used as a "wrapper" for SAVE and RESUME in Toolbar, so one doesn't inadvertantly overwrite stuff in memory.
[permalink]
|
| |
|
| |
|
PARA-2
|
| |
Mike Rife (CSI)
|
| |
Creates parabola, ellipse, or hyperbola.
[permalink]
|
| |
|
Average Rating: 8.8 (12 votes)
|
|
|
| |
|
Parameter Studies For Enhanced Integrity Of Reciprocating Compressor Foundation Blocks
|
| |
Jayant S. Mandke, Anthony J. Smalley
|
| |
"The model development and analyses of reinforced concrete block used the ANSYS finite element program."
[permalink]
|
| |
|
Average Rating: 9.7 (34 votes)
|
|
|
| |
|
Parametric Studies in ANSYS [PDF]
|
| |
Sean Harvey (CSI)
|
| |
Automated parametric studies in ANSYS (generating and using parametric input files).
Example input file.
[permalink]
|
| |
|
Average Rating: 10.0 (7 votes)
|
|
|
| |
|
Patient Specific Spine Models - Development Of A Laboratory Intervertebral Disc For Validation Of The Models
|
| |
A. Mohsen, D. J. Siddall, P. Gillespie, S. Julian and M. J. Fagan
|
| |
"This research project is aimed at evaluating the feasibility of the modelling technique through the development of an artificial validation spine. The validation spine will be tested under controlled laboratory conditions and the results used to verify those found from analysis of the computer model. The intervertebral disc is the most critical component in the spine. Thus, the initial aim of this research was to develop a representative artificial disc. Concurrent development of a finite element model of the disc permits development theories to be analysed and laboratory results to be verified."
[permalink]
|
| |
|
Average Rating: 10.0 (3 votes)
|
|
|
| |
|
PDF file summarizing beta contact features at 5.6.1 [PDF]
|
| |
Sheldon Imaoka (CSI)
|
| |
Presentation on the thermal contact and fluid pressure capabilities of the surface-to-surface contact elements. This was written when these capabilities were beta at 5.6. Thermal capabilites are documented at 5.7.
Accompanying thermal contact example and fluid pressure example
[permalink]
|
| |
|
Average Rating: 10.0 (5 votes)
|
|
|
| |
|
PDS |
| |
For info on the Probabilistic Design System, which is beta at 5.6 (released at 5.7), contact your ASD.
[permalink]
|
| |
|
Average Rating: 10.0 (5 votes)
|
|
|
| |
|
PDS and Nonlinear Runs [ZIP]
|
| |
Sheldon Imaoka (ANSYS, Inc.)
|
| |
"The Probabilistic Design System (PDS) of ANSYS provides a very powerful tool in understanding the effect of uncertainties in one’s design.
The details of PDS are covered in the online help, so this memo will discuss the specific case of setting up serial and parallel PDS runs as well as performing nonlinear analyses with PDS."
(Week 23, week of 03/14/04.)
[permalink]
|
| |
|
Average Rating: 10.0 (6 votes)
|
|
|
| |
|
PENNY3D
|
| |
Sheldon Imaoka (ANSYS, Inc.)
|
| |
Simple example using ANSYS Workbench 12.0 to show one way to generate a penny-shaped crack (3D crack) for fracture mechanics (using CINT command to evaluate J-integral and stress intensity factors).
[permalink]
|
| |
|
Average Rating: 9.8 (25 votes)
|
|
|
| |
|
Performance of SOLID92 vs. Degenerate SOLID95
|
| |
Sheldon Imaoka (CSI)
|
| |
Discussion on why there are differences in run times of SOLID92 and the degenerate tetrahedra form of SOLID95. (From XANSYS posting)
[permalink]
|
| |
|
Average Rating: 7.3 (13 votes)
|
|
|
| |
|
PERI3D
|
| |
(EMI)
|
| |
This is an ANSYS macro that creates periodic boundary conditions for a 3D model. It is a modified version of Peri.mac that automatically determines the DOF per node and active coordinate system, therefore it can be used to couple structural symmetry model boundaries as well as FLOTRAN periodic boundaries.
[permalink]
|
| |
|
Average Rating: 9.7 (18 votes)
|
|
|
| |
|
Physics first, using ANSYS to define the design: Real-life examples from the automotive supplier company Mannesmann VDO
|
| |
Zlatko Penzar
|
| |
"In many non-standard engineering development applications it strongly pays off to invest an effort into understanding the physics of the problem prior to undertaking complex numerical simulations. The better the knowledge of the leading physical effects in a complex system, the simpler and more cost-efficient the analytical model can be. Moreover, the understanding of the most important physical driving effects often enables one to build a simplified, closed-form mathematical effective model. Such models usually give insight into the interplay of various parameters governing the physical behavior of the complex system. In this way, a fast pre-optimization of the desired features is often possible. Subsequently, the rich arsenal of ANSYS multiphysics capabilities can be used to refine the judgements and obtain the desired quantitative solutions."
[permalink]
|
| |
|
Average Rating: 8.3 (15 votes)
|
|
|
| |
|
PICKER
|
| |
Chris Masterson (University of Toronto)
|
| |
A while back I asked Bill Bulat for a pointer to a macro that could be used for meshing skin depths. He gave me some good pointers. I have since been working on a skin depth macro myself. I now have a first working beta". It is currently pretty crude since I'm relatively new to ANSYS, my geometry is pretty simple and the expansion algorithm I worked out is very simple. It will only mesh a line of rectangular prisms oriented with the current coordinate system. The end result is something similar to what a straight VSWEEP command could accomplish but with the difference that the user can specify exactly the thickness of the skin depth (or boundary layer if it suits) and how many layers of mesh should be contained in that skin depth. Suits my purposes for now so I thought that maybe somebody else might find a use as well. There are actually three macros: skin.mac - the main macro, and sorter.mac and picker.mac that are called from the main macro. The other caveat I guess is to mention that I wrote them for Ansys 5.5 and so some of the command names may be changed or obsolete (which includes jumping to a label which was already technically obsolete in 5.5) in newer versions."
"I posted some skin depth meshing macros to the Ansys egroup that you reproduced on your ansys.net page. Since then I have updated the macros significantly to make them more usable and a lot less buggy. The macro is now able to mesh full planes of rectangular prisms, instead of just a line of prisms. With the use of an extra coordinate system I use it to expand the mesh in both directions away from the surface of interest. The macros are now updated to Ansys version 5.6 as well (and in fact won't work in 5.5 due to VSWEEP no longer requiring source and target areas). Just thought I would send the new improved versions to save frustration if anyone ever uses them."
[permalink]
|
| |
|
Average Rating: 8.1 (8 votes)
|
|
|
| |
|
PIPE_PML
|
| |
Sheldon Imaoka (ANSYS, Inc.)
|
| |
Example of using PML (perfectly matched layers) with acoustic elements, which is a feature new in version 13.0 (for 3D FLUID30, FLUID220, FLUID221 only). The model is a simple pipe with a planar wave - the wave should propagate through the pipe without loss of amplitude, which demonstrates the use of PML in this case.
[permalink]
|
| |
|
Average Rating: 5.0 (8 votes)
|
|
|
| |
|
PIPE20 |
| |
NMISC 101 through 104 are S1max, S3min, SINTMAX, SEQVMAX for Node I (NMISC 105 through 108 for Node J).
[permalink]
|
| |
|
Average Rating: 10.0 (5 votes)
|
|
|
| |
|
PIPE60 |
| |
NMISC 104 through 107 are S1max, S3min, SINTMAX, SEQVMAX for Node I (NMISC 108 through 111 for Node J).
[permalink]
|
| |
|
Average Rating: 8.3 (3 votes)
|
|
|
| |
|
PLANE13 |
| |
KEYOPT(1)=1 (VOLT only)
KEYOPT(1)=5 (AZ, TEMP)
[permalink]
|
| |
|
| |
|
PLANE2
|
| |
PLANE2 "2-D 6-Node Triangular Structural Solid" was undocumented at ANSYS 11.0. It should be replaced by PLANE183 with KEYOPT(1)=1.
[permalink]
|
| |
|
Average Rating: 10.0 (1 vote)
|
|
|
| |
|
PLANE55, PLANE77 |
| |
Supports planar with thickness with KEYOPT(3)=3
Use real constant to specify thickness
ET,2,55
KEYOPT,2,3,3
R,2,THICK
Above sets planar with thickness for PLANE55 as element type 2.
Thickness of "THICK" parameter specified as real constant 2.
[STI: Note that for PLANE55, this has become a documented option from ANSYS 8.1 onwards.]
[permalink]
|
| |
|
Average Rating: 10.0 (9 votes)
|
|
|
| |
|
Plastic Deformation and Loss of Joint Force by Creep in High Current Joints
|
| |
Josef Kindersberger, Helmut Löbl, Stephan Schoft
|
| |
"The mechanical stress distribution in aluminum busbar joints is calculated using the Finite Element Method. Based on the physical fundamentals of creep in aluminum the reduction of the joint force by creep depending on the temperature of the joints as well as on the initial joint force and on the washer is simulated." (Creep)
[permalink]
|
| |
|
Average Rating: 10.0 (5 votes)
|
|
|
| |
|
Plasticity Hardening Rules [ZIP]
|
| |
Sheldon Imaoka (ANSYS, Inc.)
|
| |
"ANSYS has a wide range of constitutive models and element technology available to the user. In this memo, the basics of isotropic and kinematic hardening for plasticity will be discussed, specifically related to proportional/non-proportional, monotonic/cyclic loading, and finite strain applications."
(Week 11, week of 12/17/01.)
[permalink]
|
| |
|
Average Rating: 9.3 (23 votes)
|
|
|
| |
|
PLATE_CMS
|
| |
Sheldon Imaoka (ANSYS, Inc.)
|
| |
Example showing how to use CMS (component mode synthesis) with Response Spectrum analysis (single-point response spectrum).
The non-superelement ("full model") input is here, so you can compare the results to see that they are essentially the same.
[permalink]
|
| |
|
Average Rating: 7.5 (2 votes)
|
|
|
| |
|
PLESOL |
| |
PLESOL,ENER,work
PRESOL,ENER,work
PLNSOL,ENER,work
PRNSOL,ENER,work
ESOL,var,elem,node,ENER,work (/POST26)
At 5.7, this will plot energy of elements. Specifically, "work" should be "elwk", "plwk", or "crwk" for elastic, plastic, and creep strain energies, respectively. This is available in 5.7 only.
For example, issue:
PLESOL,ENER,ELWK
to view elastic strain energies (at integration points).
[STI: Note that this is for 5.7/5.7.1 only. At 6.0, PLESOL,SENE has been introduced instead, so this output is no longer valid.]
[permalink]
|
| |
|
Average Rating: 10.0 (7 votes)
|
|
|
| |
|
PLESOL |
| |
PLESOL,NL,CREQ
PRESOL,NL,CREQ
Plots (or lists) cumulative creep strain. Similar to NL,EPEQ which is cumulative plastic strain.
[permalink]
|
| |
|
Average Rating: 10.0 (1 vote)
|
|
|
| |
|
PLOT_MAT_AS_TEMP
|
| |
Przemyslaw Siedlaczek (MESco)
|
| |
Macro to plot material properties as temperatures. (Note that this macro will apply boundary conditions to your model, so save your model first prior to using this macro.)
[permalink]
|
| |
|
Average Rating: 8.3 (3 votes)
|
|
|
| |
|
PLOT_TAG
|
| |
Mark Tate (Hamilton Sundstrand)
|
| |
This macro will tag your plots with directory and jobname.
[permalink]
|
| |
|
Average Rating: 10.0 (1 vote)
|
|
|
| |
|
PLOT33.F
|
| |
(ANSYS, Inc.)
|
| |
Old source code (ANSYS 5.4?) for PLOT33 program to read GRPH files (ANSYS Graphics Files)
[permalink]
|
| |
|
| |
|
Plotting Entities and Graphs in Multiple Windows [PDF]
|
| |
David Haberman (CSI)
|
| |
ANSYS 5.4 through 5.6 allow users to plot multiple entities (keypoints, lines, areas, volumes, nodes, and elements) in a given window. Prior to ANSYS 5.4, a user was required to plot entities on top of one another, like transparencies. Furthermore, multi-plotting also allows a user to generate graphs. The following memo discusses how the ANSYS multi-plotting feature works.
[permalink]
|
| |
|
Average Rating: 8.8 (4 votes)
|
|
|
| |
|
PLRV
|
| |
Rick Fischer (Marconi Communications)
|
| |
"This macro reduces the number of vectors plotted so that a velocity vector plot on a model with a fine mesh will be more ledgible. It works great for plotting velocity in the middle of a flat rectangular duct on a plane of symmetry. It creates a grid of points in the active coordinate system, finds an element that contains that point, and plots a velocity vector from that element's centroid."
[permalink]
|
| |
|
Average Rating: 5.0 (5 votes)
|
|
|
| |
|
PLVECT |
| |
PLVECT,S,1
Plots only first principal stress instead of plotting all three vectors at once.
[permalink]
|
| |
|
Average Rating: 10.0 (5 votes)
|
|
|
| |
|
PLVLN
|
| |
Mike Yaksh (NAC Int'l)
|
| |
Macro for displaying vector plots with element outline overlay.
[permalink]
|
| |
|
Average Rating: 10.0 (4 votes)
|
|
|
| |
|
Post Refinement Element Shape Improvement for Quadrilaterial Meshes [PDF]
|
| |
Matthew L. Staten and Scott A. Canann
|
| |
"This paper presents techniques for improving the quality of quadrilateral meshes after Schneiders' refinement. Improvement techniques use topology and node valence optimization rather than shape metrics. Hence, improvement is computationally inexpensive."
[permalink]
|
| |
|
Average Rating: 9.0 (5 votes)
|
|
|
| |
|
Postprocessing Harmonic Results [ZIP]
|
| |
Sheldon Imaoka (ANSYS, Inc.)
|
| |
"In harmonic analyses, due to the fact that results may not be in phase, postprocessing quantities of interest can pose a challenge. Users may need to review non-sinusoidal results, such as equivalent stresses, at different locations, so accounting for phase information may be required.
This memo hopes to cover some of the more important points regarding postprocessing
structural harmonic analysis results in both the General and Time-History Postprocessors."
(Week 30, week of 07/17/05.)
[permalink]
|
| |
|
Average Rating: 10.0 (22 votes)
|
|
|
| |
|
POW2MAT
|
| |
Carl Olsard (noiseboard.com)
|
| |
"This is a simple program written in Turbo pascal which I find very useful for converting the output from ANSYS (prvar, prnsol, etc) into columns, while removing the headers at the start and between the page listings. The program is used at a DOS prompt and one types in: pow2mat col filein fileout , where col are the number of columns in the output, filein MUST have an extension .val and fileout WILL have an extension .txt. You do NOT type in the extensions, they are default. For example, you would type pow2mat 7 nodelist nodelist which would extract 7 columns from the file nodelist.val and write a stripped file called nodelist.txt . If you have several files to convert, you can use the DOS FOR command as follows:
FOR %I IN (*.val) DO pow2mat 3 %~nI %~nI"
[permalink]
|
| |
|
Average Rating: 10.0 (2 votes)
|
|
|
| |
|
PowerGraphics vs. Full Graphics
|
| |
John Crawford (Honeywell)
|
| |
This article describes the differences and features of PowerGraphics vs. Full Graphics in ANSYS.
PDF Version Here.
[permalink]
|
| |
|
Average Rating: 8.9 (9 votes)
|
|
|
| |
|
Predicting Human Thermal Comfort in a Transient Nonuniform Thermal Environment
|
| |
J.P. Rugh, R.B. Farrington, D. Bharathan, A. Vlahinos, R. Burke, C. Huizenga, and H. Zhang
|
| |
"The National Renewable Energy Laboratory (NREL) has developed a suite of thermal comfort tools to assist in the development of smaller and more efficient climate control systems in automobiles. These tools, which include a 126-segment sweating manikin, a finite element physiological model of the human body, and a psychological model based on human subject testing, are designed to predict human thermal comfort in transient nonuniform thermal environments such as automobiles. The manikin measures the heat loss from the human body in the vehicle environment and sends the heat flux from each segment to the physiological model. The physiological model predicts the body’s response to the environment, determines 126 segment skin temperatures, sweat rates, and breathing rate, and transmits the data to the manikin. The psychological model uses temperature data from the physiological model to predict the local and global thermal comfort as a function of local skin and core temperatures and their rates of change. Results of initial integration testing show the thermal response of a manikin segment to transient environmental conditions."
[ANSYS Thermal, version unknown]
[permalink]
|
| |
|
Average Rating: -5.0 (1 vote)
|
|
|
| |
|
Prediction of Thermal Fatigue in Tooling for Die-casting Copper via Finite Element Analysis
|
| |
Amit Sakhuja, Jerald R. Brevick
|
| |
"Recent research by the Copper Development Association (CDA) has demonstrated the feasibility of diecasting
electric motor rotors using copper. Electric motors using copper rotors are significantly more energy
efficient relative to motors using aluminum rotors. However, one of the challenges in copper rotor die-casting is low tool
life. Experiments have shown that the higher molten metal temperature of copper (1085 °C), as compared to aluminum
(660 °C) accelerates the onset of thermal fatigue or heat checking in traditional H-13 tool steel. This happens primarily
because the mechanical properties of H-13 tool steel decrease significantly above 650 °C. Potential approaches to
mitigate the heat checking problem include: 1) identification of potential tool materials having better high temperature
mechanical properties than H-13, and 2) reduction of the magnitude of cyclic thermal excursions experienced by the
tooling by increasing the bulk die temperature. A preliminary assessment of alternative tool materials has led to the
selection of nickel-based alloys Haynes 230 and Inconel 617 as potential candidates. These alloys were selected based
on their elevated temperature physical and mechanical properties. Therefore, the overall objective of this research work
was to predict the number of copper rotor die-casting cycles to the onset of heat checking (tool life) as a function of bulk
die temperature (up to 650 °C) for Haynes 230 and Inconel 617 alloys. To achieve these goals, a 2D thermo-mechanical
FEA was performed to evaluate strain ranges on selected die surfaces. The method of Universal Slopes (Strain Life
Method) was then employed for thermal fatigue life predictions."
[permalink]
|
| |
|
Average Rating: 8.8 (4 votes)
|
|
|
| |
|
prefs.contourCount |
| |
Add this line to your script file to be able to set the number of legend contours:
prefs.contourCount = 4; // sets the number of contours to 4
[permalink]
|
| |
|
Average Rating: 10.0 (4 votes)
|
|
|
| |
|
PRESSURE
|
| |
Imad Tabsh (CompuSIM Inc.)
|
| |
Applies pressure from an equation onto a node or an area. User must modify macro with their own equation.
[permalink]
|
| |
|
Average Rating: 10.0 (7 votes)
|
|
|
| |
|
Pressure Load Macro [ZIP]
|
| |
Sheldon Imaoka (ANSYS, Inc.)
|
| |
"In ANSYS, pressure loading via the SFx family of commands allows users to apply a force per unit area in a direction normal to the surface. Structural surface effect elements SURF153 and SURF154 extend pressure loading capabilities by allowing users to specify normal, tangential, or arbitrary distributed loading. In fact, for an arbitrary ‘distributed loading vector,’ the full or projected area may be used, with or without the tangential component of load. This type of loading can be useful in mimicking a bearing load (include tangential component) or wind loading (no tangential component), to name a couple of examples.
"Because of the fact that the vector-type of pressure loading can be based on full or projected area, with or without the tangential component, trying to determine an appropriate value for the loading can be cumbersome. The author has written a simple macro which can be used as an example in utilizing surface effects more effectively by allowing the user to specify the total force instead of pressure – the macro calculates the appropriate pressure value to be applied on the surface effect elements."
(Week 27, week of 07/04/04.)
[permalink]
|
| |
|
Average Rating: 8.9 (18 votes)
|
|
|
| |
|
Pressure Mapping Example
|
| |
Bob Weathers (Trane)
|
| |
An example which demonstrates mapping between dissimilar meshes and element types.
At the bottom of the macro is an example of how to apply the mapped results from the first model onto the second using a TABLe. The TABLe uses the second model's node numbers (sorted and stored in ascending order) to index into the TABLe. This results in a very efficient way to map boundary conditions that's fast and uses minimum memory.
[permalink]
|
| |
|
Average Rating: 7.9 (12 votes)
|
|
|
| |
|
PRESSURE_MAC
|
| |
Hursha Narayan (Robert Bosch Corporation)
|
| |
"I have written a macro that calculates the total force along the three axes from applied pressure. I find this macro to be useful just to make sure that the pressure I'm applying on a curved surface is accurate and also it gives a feel for the mesh discretization where the pressure is applied. The user has to basically identify the elements with a particular magnitude of pressure and save the list file (SFELIS.lis). The macro does everything else automatically. The downside to the macro is:
1. Right now it only handles 10 node tet elements.
2. The pressure has to be uniform
The user will have to modify some of the fields in the macro as well as the c-shell file prescalc."
[permalink]
|
| |
|
Average Rating: 7.9 (7 votes)
|
|
|
| |
|
PRETEN_BOLT
|
| |
Sheldon Imaoka (CSI)
|
| |
Example demonstrating pretension (bolt) element PRETS179.
[permalink]
|
| |
|
Average Rating: 9.9 (38 votes)
|
|
|
| |
|
Preventing Rigid-Body Motion in Contact Problems [ZIP]
|
| |
Sheldon Imaoka (ANSYS, Inc.)
|
| |
"In contact problems run in a static manner, controlling rigid-body motion may sometimes be an issue under the following circumstances: (a) force-controlled systems or (b) multiple bodies with some parts unconstrained."
"This memo hopes to address some ways of controlling rigid-body motion in contact problems through the use of options available with the surface-to-surface contact elements."
(Week 2, week of 10/03/01.)
[permalink]
|
| |
|
Average Rating: 9.7 (18 votes)
|
|
|
| |
|
Principles of Simulating Contact Between Parts using ANSYS
|
| |
David H. Johnson
|
| |
"The ANSYS finite element analysis (FEA) program offers a variety of elements designed to treat cases of changing mechanical contact between the parts of an assembly or between different faces of a single part. These elements range from simple, limited idealizations to complex and sophisticated, general purpose algorithms. FEA analysts are frequently faced with modeling situations where changing contact cannot be assumed negligible and ignored. Finding the best choices for contact elements, element options, solver, and solution options can drastically improve the model’s performance and reduce the analyst’s frustration with a contact simulation model."
[permalink]
|
| |
|
Average Rating: 9.3 (14 votes)
|
|
|
| |
|
PRINGET
|
| |
Mike Yaksh (NAC Int'l)
|
| |
"This macro computes the principle stresses and SI for the maximum node number or for the stress input by the input arguements."
[permalink]
|
| |
|
Average Rating: 10.0 (2 votes)
|
|
|
| |
|
PRNWP
|
| |
James Kosloski (CAEAI)
|
| |
"Macro to align working plane with principal stress directions at a node"
[permalink]
|
| |
|
Average Rating: 9.6 (12 votes)
|
|
|
| |
|
Probabilistic Design System (PDS): A Realistic Approach of Finite Element Modelling for Capacitive Micro-machined Ultrasonic Transducers (cMUTS)
|
| |
Vamshi Kommareddy, Manoj Kumar, Ying Fan, James Barshinger
|
| |
"This paper represents a realistic approach for modeling a cMUT device.
CMUTs have become very popular over the last decade because of the comparable
bandwidth, sensitivity and dynamic range with its piezoelectric counterparts. The
ease of fabrication is an added advantage. Modeling of CMUT is a coupled physics
problem, which involves solving Electrostatics-Structural-Fluid interactions
simultaneous. Finite Element models of the CMUT are constructed using the
commercial code ANSYS (10.0). In the standard approach of modeling, from
existing literature assumes deterministic values for design parameters, however
fabrication of the device introduces some amount of variation in the design
parameters. In this paper, the PDS FEM approach is discussed to account for the
variability in fabrication. The results from the PDS approach on the performance
characteristics like resonance frequency; collapse voltage and electromechanical
coupling coefficient will be discussed."
[ANSYS PDS, version 10.0]
[permalink]
|
| |
|
Average Rating: 8.0 (5 votes)
|
|
|
| |
|
PRONY
|
| |
John Thompson (ANSYS, Inc.)
|
| |
Macro to do curve-fitting for TB,PRONY constants for given relaxation data.
[STI: Note that, at 8.0 and above, curve-fitting of TB,PRONY is directly available in ANSYS with the TBFT command.]
[permalink]
|
| |
|
Average Rating: 10.0 (4 votes)
|
|
|
| |
|
PSD Calculation Efficiency [PDF]
|
| |
Sheldon Imaoka (ANSYS, Inc.)
|
| |
"A very common use of PSD analyses is to look at the response of a system under a single base
excitation, such as the case with many aerospace and civil applications. The default PSD settings are very general in nature and may consequently be inefficient for such a situation. This memo hopes to outline some ways in which the user may obtain more efficient PSD solutions for the specific instance of single base excitation with relatively flat spectrum (although some techniques may be extrapolated for other cases)."
…An older doc I recently reanimated and updated…
(Week 25, week of 06/13/04.)
[permalink]
|
| |
|
Average Rating: 9.2 (13 votes)
|
|
|
| |
|
PSD Postprocessing [ZIP]
|
| |
Sheldon Imaoka (ANSYS, Inc.)
|
| |
"PSD, or random vibration, analyses present some interesting challenges in postprocessing due to the nature of the assumptions related to the analysis. This memo hopes to address some of these
items, including evaluation of derived stresses and calculation of response power spectral density."
…An older doc I recently reanimated and updated…
(Week 26, week of 06/27/04.)
[permalink]
|
| |
|
Average Rating: 9.6 (13 votes)
|
|
|
| |
|
PSD Postprocessing of Relative Displacement [ZIP]
|
| |
Sheldon Imaoka (ANSYS, Inc.)
|
| |
"PSD users may wish to determine the relative 1-sigma results between two points.
This memo covers three methods to perform this operation, in hopes that
it will give users more familiarity with PSD postprocessing in ANSYS."
(Week 53, week of 03/07/09)
[permalink]
|
| |
|
Average Rating: 10.0 (7 votes)
|
|
|
| |
|
PSD results and RSYS
|
| |
Sheldon Imaoka (ANSYS, Inc.)
|
| |
Some tips on postprocessing random vibration analyses - specifically, RSYS,SOLU and PSD results as well as cases with rotated nodes.
[permalink]
|
| |
|
Average Rating: 10.0 (2 votes)
|
|
|
| |
|
PSDOUT
|
| |
Jeff Strain (PADT)
|
| |
"psdout.mac retrieves PSD data, in G^2/Hz, at picked nodes and stores them as variables in the Time History postprocessor as well as the array parameter PSDDATA. PSDDATA excludes data for modes lying outside the input PSD spectrum. The user also has the options of plotting the PSD curves and/or exporting the data to the text file, psddata.txt.
Usage: psdout,dir,plot,list where dir = 'x', 'y', or 'z' (defaults to 'x'); plot = 1 to plot the PSD curves in ANSYS (defaults to 0); and list = 1 to export the data to psddata.txt (defaults to 0).
Acceleration results (load step 5) must be available for this macro to work."
Example output plot as PNG file
[permalink]
|
| |
|
Average Rating: 10.0 (9 votes)
|
|
|
| |
|
PSDRES |
| |
PSDRES,Lab,RelKey,WriteRPSD
The PSDRES command has an undocumented 3
rd argument which, when set to “ON”, will
write an .rpsd file containing modal response PSDs. The contents of the file may be viewed
in /AUX2, although the format is not documented.
[permalink]
|
| |
|
Average Rating: 10.0 (1 vote)
|
|
|
| |
|
PSTRES |
| |
To perform a prestressed "full" harmonic analysis, simply issue PSTRES,ON during the static analysis and PSTRES,ON during the harmonic analysis (similar to prestressed modal). Prestressed modal superposition and reduced harmonic are documented in the manuals.
[STI: I think that this may be documented at 5.7]
[permalink]
|
| |
|
Average Rating: 8.5 (13 votes)
|
|
|
| |
|
Purple colormap
|
| |
Bryan Baskin (Bell Helicopter Textron, Inc.)
|
| |
Color map (contours) which ranges from purple to red. Use /cmap,plot7.cmap to read in file.
[permalink]
|
| |
|
Average Rating: 7.8 (9 votes)
|
|
|
| |
|
PUT_AMP
|
| |
Mike Yaksh (NAC Int'l)
|
| |
Applies J to selected elements for a specified current input (A). Model is assumed to be in SI units.
[permalink]
|
| |
|
Average Rating: 10.0 (1 vote)
|
|
|
| |
|
Pyramid Elements for Maintaining Tetrahedra to Hexahedra Conformability
|
| |
Steven Owen, Scott Canann, and Sunil Saigal
|
| |
[Click here for PDF file]
This is a feature added in ANSYS 5.5 to automatically define transitional pyramids between hex- and tet-meshed volumes (e.g., with SOLID95)
[permalink]
|
| |
|
Average Rating: 10.0 (2 votes)
|
|
|
| |
|
PZT Actuated Micromirror For Nano-Tracking Of Laser Beam For High-Density Optical Data Storage [PDF]
|
| |
Youngjoo Yee, Hyo-Jin Nam, See-Hyung Lee, Jong Uk Bu, Young-Sam Jeon, and Seong-Moon Cho
|
| |
A piezo-actuated micromirror. Used ANSYS for stress and modal analysis of mirror. (MEMS)
[permalink]
|
| |
|
Average Rating: 5.0 (4 votes)
|
|
|
| |
|
QCLEAR
|
| |
Rod Scholl (PADT)
|
| |
Does a /CLEAR without prompting the user for an OK.
[permalink]
|
| |
|
Average Rating: 10.0 (2 votes)
|
|
|
| |
|
QR Damped and Unsymmetric Stiffness [ZIP]
|
| |
Sheldon Imaoka (ANSYS, Inc.)
|
| |
"There have been significant enhancements to the QR Damped eigenvalue extraction method in
the past several releases of ANSYS. At 8.0, the capability of including unsymmetric damping [C]
matrix was introduced, along with support of damping defined via the DMPRAT and MDAMP
commands.
ANSYS 8.1, the material-based constant damping ratio MP,DMPR allowed users to
specify constant damping ratios per material ID in mode-superposition harmonic analyses, when
used with the QRDAMP eigensolver. With the release of 9.0, QRDAMP also supports unsymmetric
stiffness [K] matrix, output of complex eigenvectors, and the use of the PSOLVE command.
This memo hopes to cover the use of QR Damped eigenvalue extraction method in friction
problems, where an unsymmetric stiffness [K] matrix may be present. An example of this type of
problem is brake squeal analyses, where the combination of ANSYS 17x contact elements and the
QRDAMP eigensolver provide an easy-to-use, efficient means of determining unstable modes."
(Week 29, week of 01/09/05.)
[permalink]
|
| |
|
Average Rating: 9.4 (16 votes)
|
|
|
| |
|
QR Damped Modal Analysis [PDF]
|
| |
Sheldon Imaoka (CSI)
|
| |
Presentation on different damped eigenvalue extraction methods in ANSYS, focusing on the newer QR Damped method.
Input files in zip format
[permalink]
|
| |
|
Average Rating: 10.0 (10 votes)
|
|
|
| |
|
Quad-Morphing: Advancing Front Quad Meshing Using Triangle Tranformations
|
| |
Steven Owen, Matthew Staten, Scott Canann, and Sunil Saigal
|
| |
[Click here for PDF file]
This is the new Q-morph quad mesher added in ANSYS 5.5
"Quad-morphing is a new technique used for generating quadrilaterals from an existing triangle mesh. Beginning with an initial triangulation, triangles are systematically transformed and combined. An advancing front method is used to determine the order of transformations. An all-quadrilateral mesh containing elements aligned with the area boundaries with few irregular internal nodes can be generated."
[permalink]
|
| |
|
Average Rating: 5.0 (1 vote)
|
|
|
| |
|
Quality Based Design and Design for Reliability of MEMS Using Probabilistic Methods [PDF]
|
| |
Stefan Reh, Paul Lethbridge, Dale Ostergaard
|
| |
Presented at MSM 2000. (MEMS)
[permalink]
|
| |
|
| |
|
Quality Based Design from Probabilistic Methods [PDF]
|
| |
Stefan Reh, Paul Lethbridge, Dale Ostergaard
|
| |
(from ANSYS Solutions magazine, volume 2, #2) (MEMS)
[permalink]
|
| |
|
Average Rating: 10.0 (1 vote)
|
|
|
| |
|
QZMULTI
|
| |
Peter Budgell (Innovative Steam Technologies)
|
| |
The following APDL code can do a stress plot for a Working Plane slice on top of a capped hidden display of the underlying elements. You will need to change the two /TYPE commands if you want to use a Z-Buffer approach. You may want to add a /TYPE command at the end to change back to a conventional hidden surface method. You have to be in /POST1 before calling this macro, and have defined the position of your Working Plane inside the body of your model. Customize as you wish.
[permalink]
|
| |
|
Average Rating: 10.0 (3 votes)
|
|
|
| |
|
RADAIRGAP
|
| |
Sheldon Imaoka (ANSYS, Inc.)
|
| |
Some users wish to define a region with conduction and allow radiation within that region (such as modeling conduction across an air gap). The attached is a simple example showing use of Radiosity solver (left-side model) and contact element radiation (right-side model).
Comparison with a thermal resistance network is done to ensure results are correct.
(The solution takes a while to solve because of the segregated solution technique with the radiosity solver. The radiation option of contact elements does not require many iterations, but it only assumes radiation in the normal direction, which may be sufficient for thin gaps.)
[permalink]
|
| |
|
Average Rating: 10.0 (6 votes)
|
|
|
| |
|
Radiation article in ANSYS Solutions Magazine [PDF]
|
| |
Dave Looman (ANSYS, Inc.)
|
| |
Overview of ANSYS's radiation capabilities, including a discussion on the radiosity solution method.
[permalink]
|
| |
|
Average Rating: 8.0 (10 votes)
|
|
|
| |
|
Radiosity Solver [PDF]
|
| |
Sheldon Imaoka (CSI)
|
| |
Information on radiation capabilities of ANSYS, focusing on the radiosity solution method.
Accompanying input files 1, 2, 3 and 4
[permalink]
|
| |
|
Average Rating: 9.6 (13 votes)
|
|
|
| |
|
RANDOM
|
| |
Jeff Strain (PADT)
|
| |
"Performs PSD base excitation analysis on a component in units of G^2/Hz.
Execute random,1 to perform a modal analysis prior to the PSD analysis. Execute random with no arguments to run the PSD solution only.
Apply constraints before running this macro"
[permalink]
|
| |
|
Average Rating: 10.0 (9 votes)
|
|
|
| |
|
Random Vibration Analysis of a Circuit Board [PDF]
|
| |
Sean Harvey (CSI)
|
| |
Example of random vibration analysis of a circuit board in ANSYS.
Input files in zip format
[permalink]
|
| |
|
Average Rating: 9.8 (48 votes)
|
|
|
| |
|
RANDSEED
|
| |
Stefan Reh (ANSYS, Inc.)
|
| |
"All random number generators are only pseudo-random number generators. They use what is called a "seed" value to calculate a random number. The result is only pseudo-random because with the same seed value you will always end up with the same "random" number. So whenever you start ANSYS it initializes the seed value. If you start generating random numbers then you will always get the same sequence of "random" numbers. The solution to this problem is to randomize the seed value itself using the system-time. Enclosed is the macro "randseed" that will exactly do that. You will get "real" random numbers after you run "randseed". You might want to run this macro every time before you start with your random number generation. You can also include the macro in your "start.ans" procedure so it will be executed each time you start ANSYS."
It effectively randomizes
the seed by executing the RAND an arbitrary number of times.
[permalink]
|
| |
|
Average Rating: 5.6 (9 votes)
|
|
|
| |
|
Ratcheting Simulations with Modified Abdelkarim-Ohno Cyclic Plasticity Model
|
| |
Radim Halama
|
| |
"In a search for a constitutive model for ratcheting simulations in rolling contact fatigue domain, the models by Chaboche and AbdelKarim-Ohno and the modificiation of AbdelKarim-Ohno model have been evaluated against a set of uniaxial and biaxial ratcheting responses of steel CS1026. It is difficult to simulate simultanously the uniaxial and multiaxial ratcheting responses with the AbdelKarim-Ohno model. This problem has been removed by modification described in the paper. The proposed model was implemented into the FE code Ansys using Fortran user‘s subroutine. The proposed cyclic plasticity model simulates all solved cases very well."
[ANSYS nonlinear, version 8.0]
[permalink]
|
| |
|
Average Rating: 6.7 (3 votes)
|
|
|
| |
|
RCS2ICS
|
| |
Mark Troscinski (ANSYS, Inc.)
|
| |
"Macro RCS2ICS transforms FLOTRAN velocities, computed in a rotating coordinate system (or frame of reference), into an inertial coordinate system, for post-processing purposes."
[permalink]
|
| |
|
Average Rating: 10.0 (1 vote)
|
|
|
| |
|
RCYL
|
| |
Steve Hale (CAEAI)
|
| |
"A macro has been developed that calculates the actual radial and tangential displacements for a large rotation analysis in ANSYS. The macro, named RCYL.MAC , stores the actual radial and circumferential displacements in the following results quantities:
EPTOT,XY = radial displacement
EPTOT,YZ = circumferential displacement
The macro is valid for up to 180 degrees of rotation and it correctly handles the case when a node rotates from one quadrant to the next. Full Graphics mode must be used when plotting these results because a *VPUT command is used in the macro."
[permalink]
|
| |
|
| |
|
READSI
|
| |
David Gross (Dominion Engineering, Inc.)
|
| |
Example of a macro for stress intensity extraction. Dumps results of PRSECT to file, then *VREADs results into array.
[permalink]
|
| |
|
Average Rating: 10.0 (3 votes)
|
|
|
| |
|
REASSIGN
|
| |
Sheldon Imaoka (CSI)
|
| |
Example of reassigning matrix scratch files to another directory. For this example, I also differentiate between the platform type when specifying a scratch directory since Windows and UNIX file systems are assigned differently.
Requires jobname macro.
[permalink]
|
| |
|
| |
|
Reduced Order Modeling of Fluid Structural Interactions in MEMS Based on Modal Projection Techniques
|
| |
Jan Mehner, Wolfram Doetzel, Bernd Schauwecker, Dale Ostergaard
|
| |
This paper provides useful background information on the modal projection technique available in ANSYS with FLUID136 elements (RMFLVEC, DMPRAT, and ABEXTRACT macros). Although the ROM140 element has not been officially released (it is undocumented), this paper introduces that element as well.
[permalink]
|
| |
|
Average Rating: 10.0 (1 vote)
|
|
|
| |
|
REFORMAT
|
| |
Sheldon Imaoka (CSI)
|
| |
Provides a longer format listing for /POST1 (PRxxxx commands) with longer "pages". Makes for nicer-looking listings to import into third-party spreadsheets or programs such as Excel or Tecplot.
[permalink]
|
| |
|
Average Rating: 10.0 (7 votes)
|
|
|
| |
|
Reliability Study of Underfill/Chip Interface Under Accelerated Temperature Cycling (ATC) Loading
|
| |
Y.L. Zhang, D.X.Q. Shi, W. Zhou
|
| |
"Interface reliability issue has become a major concern in developing flip chip assembly. The CTE mismatch between different material layers may induce severe interface delamination reliability problem. In this study, multifunctional micro-moire´ interferometry (M3I) system was utilized to study the interfacial response of flip chip assembly under accelerated thermal cycling (ATC) in the temperature range of 40 C to 125 C. This in-situ measurement provided good interpretation of interfacial behavior of delaminated flip chip assembly. Finite element analysis (FEA) was carried out by introducing viscoelastic properties of underfill material. The simulation results were found to be in good agreement with the experimental results. Interfacial fracture mechanics was used to quantify interfacial fracture toughness and mode mixity of the underfill/chip interface under the ATC loading. It was found that the interfacial toughness is not only relative to CTE mismatch but also a function of stiffness mismatch between chip/underfill."
ANSYS Nonlinear (Viscoelasticity), version 6.1.
[permalink]
|
| |
|
| |
|
RENAM
|
| |
John Swanson (SAS, Inc./ANSYS, Inc.)
|
| |
Renames files in working directory. For example, using "renam,'tif',_1" renames all TIF files in working directory and adds prefix "_1". Useful to rename graphics files. (Note: At 5.6.1, the undocumented command /DIRGET which this macro uses does not work on Windows and will result in an abort.)
[permalink]
|
| |
|
| |
|
RESVEC
|
| |
Sheldon Imaoka (ANSYS, Inc.)
|
| |
This input file is a simple demonstration of the usefulness of the residual vector method in capturing accurate higher-frequency response in mode-superposition analyses.
In the input file, change the first two parameters as follows:
- For results with many modes included and no residual vector, set MY_FREQUENCY = 1 and MY_RESVECTOR = 0
- For results with few modes included and no residual vector, set
MY_FREQUENCY = 0 and MY_RESVECTOR = 0
- For results with few modes included and with residual vectors, set MY_FREQUENCY = 0 and MY_RESVECTOR = 1
By performing the above, one will see that even at the higher-frequency response, the residual vector method will give results comparable to including many modes even if the user has a smaller set of modes. An Excel spreadsheet is also available, which tabulates the results (notice the difference in results for higher frequencies - this is where, without residual vector method and fewer modes, one may not accurately capture higher-frequency response).
Note that the residual vector method includes stiffness of higher frequencies, but one should still have enough modes to characterize the mass of the structure (i.e., it's not a panacea for insufficient modes). Also, use of ANSYS 11.0 or higher is required.
[permalink]
|
| |
|
Average Rating: 9.3 (7 votes)
|
|
|
| |
|
RESWRITE |
| |
RESWRITE,filename,load step, substep, time
Three additional fields are available in RESWRITE to specify the load step, substep, and time values. Basically, this will append results to the results file - it is a shorthand for using FILE and RAPPND, although the above undocumented options for RESWRITE give the user control over the substep number as well.
[permalink]
|
| |
|
Average Rating: 8.0 (5 votes)
|
|
|
| |
|
Returning Values in a Macro
|
| |
Primoz Cermelj
|
| |
An example on returning values from a macro. This uses a parameter name as an argument which can then be modified and returned back for use in ANSYS.
[permalink]
|
| |
|
Average Rating: 10.0 (11 votes)
|
|
|
| |
|
Reverse Video Color colormap
|
| |
Sheldon Imaoka (ANSYS, Inc.)
|
| |
Colormap file to have reverse black and white. Use /cmap,reverse.cmap to read this file in.
(This is the same colormap you get when you use "Utility Menu > PlotCtrls > Style > Color > Reverse Video")
[permalink]
|
| |
|
Average Rating: 7.8 (9 votes)
|
|
|
| |
|
Reverse Video Grayscale colormap
|
| |
Sheldon Imaoka (ANSYS, Inc.)
|
| |
Colormap file to have reverse black and white with grayscale colors (dark=blue, light=red). Use /cmap,reverse_gray.cmap to read this file in.
[permalink]
|
| |
|
Average Rating: 9.2 (12 votes)
|
|
|
| |
|
Review of Anisotropy, Yield Criteria, Failure Criteria [PDF]
|
| |
Sheldon Imaoka (ANSYS, Inc.)
|
| |
"This memo hopes to serve as a review of the basics of anisotropy, yield criteria, failure criteria, and the ANSYS procedure related to these topics."
(Week 15, week of 01/21/02.)
[permalink]
|
| |
|
Average Rating: 8.8 (20 votes)
|
|
|
| |
|
REVOLVE
|
| |
Sheldon Imaoka (ANSYS, Inc.)
|
| |
Simple example showing a disk loaded with initial velocity. Disk rotation is defined by MPC184, so this must be run in version 7.0 and above. (Disk rotation could have been defined by other methods such as deformable-rigid contact, but this was meant to illustrate a particular technique.)
[permalink]
|
| |
|
Average Rating: 9.8 (41 votes)
|
|
|
| |
|
RFOR_TOTAL
|
| |
Adam Shinbrot (Zimmer Spine)
|
| |
"For a selected nodal set, macro creates vector r_f of dimension arg1 x 1 and fills it with successive values of reaction forces in y for successive time steps, the total number of which is specified by arg1.
"This macro assumes ultimate time step is number 1; this is easily changed, however."
[permalink]
|
| |
|
Average Rating: 3.3 (6 votes)
|
|
|
| |
|
RIGID_MOMENTS |
| |
Set DesignSpace variable "rigid_moments" to "1" if you want to use DesignSpace v5 moment application in DesignSpace v6.
"(In DesignSpace 5, when applying moments to a surface, this was done through stiff springs. This also made the surface act rigidly.
In DesignSpace 6, force couples are used instead to apply the moment, allowing the surface to deform. This is more representative of what happens when a moment is applied, as an applied moment should not make the surface act rigidly.
If the user wants to use the older DesignSpace 5 method of applying moments, setting the above variable will do so. This would also produce same answers in DesignSpace 6 as in 5, if the user saw a discrepancy between revisions.)"
[permalink]
|
| |
|
Average Rating: 10.0 (11 votes)
|
|
|
| |
|
RIGIDBODY_ROTATION
|
| |
Sheldon Imaoka (ANSYS, Inc.)
|
| |
This is a very simple example of using RBE3 or force-distributed type of surface constraint to track an averaged sense of the rotation or translation of a part within an assembly.
By listing the displacements or rotations at the pilot node, one can obtain these quantities. (Remember that rotations are reported in radians, not degrees.)
[permalink]
|
| |
|
Average Rating: 9.0 (5 votes)
|
|
|
| |
|
RISK |
| |
RISK,A1,A2,A3,A4,A5,A6,A7,A8,A9
Scatter, failure, or design analysis of SEQV or SINT from PSD analysis.
See Section 2.4 of the PSD Postprocessing Tip for details on this usage.
[permalink]
|
| |
|
| |
|
rlnext() |
| |
RLNEXT(R)
Next defined real set having a number greater than R. (*GET inline function)
[permalink]
|
| |
|
Average Rating: 10.0 (2 votes)
|
|
|
| |
|
RMXPORT |
| |
RMXPORT,ATOV
Translate ANSYS ROM into Verilog-A
RMXPORT,VTOA
Translate Verilog-A into ANSYS ROM
[permalink]
|
| |
|
| |
|
ROLLER
|
| |
Sheldon Imaoka (ANSYS, Inc.)
|
| |
Simple example of a hollow metal pipe being bent by rollers. Rigid-deformable contact, metal plasticity, use of Joints (MPC184) are in the Workbench Mechanical 12.1 model.
An animation of this can be found on the gallery page.
[permalink]
|
| |
|
Average Rating: 8.2 (11 votes)
|
|
|
| |
|
ROTATE
|
| |
Joe Metrisin (Florida Turbine Technologies, Inc.)
|
| |
Here's a UIDL function (Granule file) I wrote a while back to rotate any geometric or finite element entity about any local or global coordinate system axis.
[permalink]
|
| |
|
Average Rating: 10.0 (6 votes)
|
|
|
| |
|
ROTV
|
| |
John Crawford (Honeywell)
|
| |
A macro to rotate the currently selected volumes about an axis.
[permalink]
|
| |
|
Average Rating: 10.0 (3 votes)
|
|
|
| |
|
ROUND
|
| |
Gordon May (Rolls Royce Compressor Key System)
|
| |
Macro to round a parameter to a specified number of digits.
[permalink]
|
| |
|
Average Rating: 10.0 (3 votes)
|
|
|
| |
|
RPAREA
|
| |
(CAEAI)
|
| |
"This macro uses the ASUB command to replace/repair old areas with new areas to repair them in preparation for meshing."
[permalink]
|
| |
|
Average Rating: 5.0 (1 vote)
|
|
|
| |
|
RPnnn |
| |
RPnnn, vinc1, vinc2, ...
The RPnnn command works similar to *REPEAT,nnn. For example, instead of using *REPEAT,3 to repeat the previous commands a total of 3 times, one can use RP3 instead. The second argument (value increment) of RPnnn is the same as the third argument of *REPEAT.
[permalink]
|
| |
|
Average Rating: 10.0 (2 votes)
|
|
|
| |
|
RSYNC |
| |
RSYNC,ON
Forces dump of buffer of element stresses after they are written.
[permalink]
|
| |
|
| |
|
RSYNC |
| |
RSYNC,filename
"Filename" is created when the load set is complete on the results file. The file will have one line giving the appropriate SET command to process that results set.
[permalink]
|
| |
|
| |
|
Running batch jobs on UNIX and on Windows
|
| |
Sheldon Imaoka (CSI)
|
| |
Discussion on creating C-shell scripts to run batch jobs on UNIX. Also discussion on writing DOS scripts to run batch jobs on Windows. (From XANSYS posting)
[permalink]
|
| |
|
Average Rating: 8.8 (4 votes)
|
|
|
| |
|
RV_BA
|
| |
David Haberman (CSI)
|
| |
Example of random vibration, base acceleration.
[permalink]
|
| |
|
Average Rating: 8.8 (29 votes)
|
|
|
| |
|
RV_BA_MP
|
| |
David Haberman (CSI)
|
| |
Example of random vibration, base acceleration in two directions.
[permalink]
|
| |
|
Average Rating: 6.8 (19 votes)
|
|
|
| |
|
RV_LMM
|
| |
David Haberman (CSI)
|
| |
Example of random vibration, large mass method.
[permalink]
|
| |
|
Average Rating: 10.0 (8 votes)
|
|
|
| |
|
RV_NF
|
| |
David Haberman (CSI)
|
| |
Example of random vibration, nodal forces.
[permalink]
|
| |
|
Average Rating: 8.2 (11 votes)
|
|
|
| |
|
RV_PRESS_FM
|
| |
David Haberman (CSI)
|
| |
Example of random vibration, pressure loading.
[permalink]
|
| |
|
Average Rating: 7.8 (9 votes)
|
|
|
| |
|
RV_PRESS_RM
|
| |
David Haberman (CSI)
|
| |
Example of random vibration, pressure loading (reduced modal).
[permalink]
|
| |
|
Average Rating: 10.0 (8 votes)
|
|
|
| |
|
RWRITE |
| |
Write out real constant tables (jobname.real)
[permalink]
|
| |
|
Average Rating: 10.0 (4 votes)
|
|
|
| |
|
SASEL
|
| |
Sheldon Imaoka (ANSYS, Inc.)
|
| |
Macro used to select areas based on the value of the area itself (=length^2). Can be used to select all areas of a certain surface area or a range of surface area (with tolerance).
[permalink]
|
| |
|
Average Rating: 10.0 (4 votes)
|
|
|
| |
|
SCOPY
|
| |
Dave Rea (ANSYS, Inc.)
|
| |
Macro used to copy a meshed sector to a full 360 degree model. Copies meshed solid model and merges nodes (can also edit to merge keypoints). Also, an example file is supplied.
[permalink]
|
| |
|
Average Rating: 10.0 (1 vote)
|
|
|
| |
|
Seismic Simulation Of The Motorola SC4812ET RF And Power Cabinets Using Pro/Engineer and ANSYS
|
| |
Alan Herda, D. Allan Daggs
|
| |
"To prevent earthquake test failure and reduce cycle time, mechanical development engineering conducted seismic simulations in parallel with the design of a new outdoor cellular base station and accompanying battery cabinet. Finite element models of the Motorola SC4812ET RF (Radio Frequency) and Power Cabinets, weighing 1400 pounds and 3500 pounds respectively, were built and subjected to Bellcore Zone 4 earthquake loading using ANSYS finite element analysis software."
[permalink]
|
| |
|
Average Rating: 8.6 (14 votes)
|
|
|
| |
|
SELECT_HEXPYRA
|
| |
Sheldon Imaoka (ANSYS, Inc.)
|
| |
Simple example to unselect tetrahedral and wedge-shaped SOLID164 degenerate elements, leaving only hexahedral and pyramid SOLID164 selected.
While this macro has limited usefulness by itself, it can be used as an example of selecting certain element shapes by nodal connectivity - very useful if you have a single element type but multiple degenerate element shapes and want to differentiate between them in your model.
[permalink]
|
| |
|
Average Rating: 10.0 (1 vote)
|
|
|
| |
|
SelectBodysByMaterial
|
| |
Przemyslaw Siedlaczek (MESco)
|
| |
Workbench macro selects all bodies with the same material as the selected body.
[permalink]
|
| |
|
Average Rating: 10.0 (4 votes)
|
|
|
| |
|
Selecting Items in the Graphics Window |
| |
Sheldon Imaoka (ANSYS, Inc.)
|
| |
This one is mainly for new users... When selecting items with the mouse in the ANSYS graphics window, click and hold down the left mouse button and move your cursor. You'll see that as you move your cursor on the screen, different objects will be highlighted, based on which object's centroid is closest to your mouse. This allows you to pick specific objects [areas, lines, elements, etc.] more easily rather than 'guessing'. Also, while in select mode with the picking dialog box on your left, you can use your right mouse button to toggle between "pick" and "unpick", and your middle mouse button acts as an "apply" command. Note that if you only have two mouse buttons, using both buttons acts like the middle mouse button.
[permalink]
|
| |
|
| |
|
SELLOC
|
| |
Don Shaffer (Siemens Westinghouse Power Corp)
|
| |
"This is a utility tool to speed up selection of model entities by location." Please read the comments in the macro file for more details on usage.
[permalink]
|
| |
|
Average Rating: -5.0 (4 votes)
|
|
|
| |
|
SELTOL |
| |
SELTOL,value
Sets selection tolerance to value prior to xSEL commands.
SELTOL,1e-2
NSEL,S,LOC,X,1000
SELTOL
Above example selects nodes at x=1000+/-1e-2, then resets selection tolerance to 0.005xVMIN
[permalink]
|
| |
|
Average Rating: 9.6 (12 votes)
|
|
|
| |
|
Semiconductor Package Simulations: Assembly, Test, and Reliability [PDF]
|
| |
Steven Groothuis
|
| |
This is a presentation which demonstrates various types of analyses ANSYS can perform which are applicable to the semiconductor industry.
[permalink]
|
| |
|
Average Rating: 7.5 (8 votes)
|
|
|
| |
|
SEQV_MAX
|
| |
Adam Shinbrot (Zimmer Spine)
|
| |
"For a selected nodal set, macro creates vector s_eqv of dimension arg1 x 1 and fills it with successive values of SEQV (Von-Mises stress) max for successive time steps, the total number of which is specified by arg1.
"This macro assumes ultimate time step is number 1; this is easily changed, however."
[permalink]
|
| |
|
Average Rating: 10.0 (1 vote)
|
|
|
| |
|
SET |
| |
SET, Lstep, SBSTEP, FACT, KIMG, TIME, ANGLE, NSET, ORDER
For the KIMG argument, the words phase or ampl can be used to plot or print phase angles or amplitude in /POST1 for a damped system.
[permalink]
|
| |
|
Average Rating: 7.5 (8 votes)
|
|
|
| |
|
SET_L
|
| |
(ANSYS, Inc.)
|
| |
At 5.6, SET in GUI results in dialog box rather than text listing as in 5.5. This provides short results set summary (equivalent to SET,LIST in 5.5).
[permalink]
|
| |
|
Average Rating: 10.0 (6 votes)
|
|
|
| |
|
SET_L2
|
| |
(ANSYS, Inc.)
|
| |
At 5.6, SET in GUI results in dialog box rather than text listing as in 5.5. This provides long results set summary (equivalent to SET,LIST,2 in 5.5).
[permalink]
|
| |
|
Average Rating: 9.4 (8 votes)
|
|
|
| |
|
setLegend
|
| |
Al Hancq (ANSYS, Inc.)
|
| |
"The macro below will set the legend of the current result in DesignSpace. (Note that this and any legend setting will get wiped out after a resolve)"
- put the contents below into a script file (like setLegend.js), setting the legend min/max as desired
- select your desired result.
- run this macro via Tools->Run Macro
"You can make this macro to be more elaborate such as walking down the tree
and setting all result legends at once."
"I have verified this macro in DesignSpace 6.0.1 but it should work in DesignSpace 6.0 as well."
[permalink]
|
| |
|
Average Rating: 10.0 (5 votes)
|
|
|
| |
|
setScale
|
| |
Sheldon Imaoka (ANSYS, Inc.)
|
| |
"Attached is a quick hack of a macro to change the scaling for the deformed shape in DesignSpace v6. Edit the file and put in the scale factor you want, then use "Tools > Run Macro..." to run this.
Please note that your Results toolbar will not be updated with this macro, and it will show whatever you had previously (like "0.5:1
Automatic"). What I'd suggest doing is changing to 'undeformed' and then running this macro, so you know that it's your own specified scale factor, even though the Results toolbar says 'undeformed.'"
[permalink]
|
| |
|
Average Rating: 10.0 (6 votes)
|
|
|
| |
|
Setting Windows "HOME" Directory |
| |
Sheldon Imaoka (ANSYS, Inc.)
|
| |
On UNIX, the user can create a user-specific "start60.ans" file in his/her home account directory (~/start60.ans).
On Windows, the user can create two environment variables: HOMEDRIVE and HOMEPATH to specify his/her 'home' directory. For example, to make D:\docs\start60.ans your startup file location, set the environment variables HOMEDRIVE=D: and HOMEPATH=\docs\ and place the start60.ans in that directory. The author prefers this method since, if the user modifies the start60.ans in the ANSYS 6.0 "docu" subdirectory, and if the user needs to reinstall ANSYS, this customized start60.ans file might be overwritten unintentionally.
Note that the startup file was called start5x.ans or start.ans for prior version of ANSYS 5.x.
[permalink]
|
| |
|
Average Rating: 10.0 (1 vote)
|
|
|
| |
|
SFMAP
|
| |
(CAEAI)
|
| |
"This macro is used to map pressure from a CFD mesh onto a structural mesh. The point XYZ locations from the CFD analysis must exist in an array called cfdxyz(npts,3). A corresponding array called "cfdpres" must be exist also. This array contains the pressure values corresponding to the point locations."
Useful example of the use of *MOPER,,,MAP.
[permalink]
|
| |
|
Average Rating: 6.9 (16 votes)
|
|
|
| |
|
Shape Memory Alloy
|
| |
Sheldon Imaoka (ANSYS, Inc.)
|
| |
Short PDF describing differences between the superelastic and shape memory effect options for Shape Memory Alloy (SMA) material model. Simple input file can be downloaded here.
[permalink]
|
| |
|
Average Rating: 9.5 (11 votes)
|
|
|
| |
|
Shaping Optimization of Turbine Disk and Bearing Seal
|
| |
Shen-Yeh Chen
|
| |
Example of use of in-house optimization code with ANSYS to produce optimization of structures without parametric geometric information.
[permalink]
|
| |
|
Average Rating: 9.6 (13 votes)
|
|
|
| |
|
SHELL_CONT
|
| |
Sheldon Imaoka (CSI)
|
| |
Input file demonstrating plasticity, contact, finite strain. Also shows benefit of line search activated.
[permalink]
|
| |
|
Average Rating: 9.1 (45 votes)
|
|
|
| |
|
SHELL-ABD
|
| |
Sheldon Imaoka (ANSYS, Inc.)
|
| |
Simple example showing how to calculate the A, B, D, and E matrices for general shell input for a single layer (homogenous) shell.
The A, B, D, and E matrices are the shell membrane, coupling, bending, and transverse shear stiffness relationships.
[permalink]
|
| |
|
Average Rating: 6.0 (5 votes)
|
|
|
| |
|
SHELL131RDSF
|
| |
Sheldon Imaoka (ANSYS, Inc.)
|
| |
Simple input file demonstrating use of SHELL131 (thermal shell element which allows for in-plane as well as through-thickness conduction) with the Radiosity Solution method.
[permalink]
|
| |
|
Average Rating: 8.3 (9 votes)
|
|
|
| |
|
SHELL143
|
| |
SHELL143 "4-Node Plastic Small Strain Shell" was undocumented at ANSYS 11.0. It should be replaced by SHELL181 with KEYOPT(3)=2.
[permalink]
|
| |
|
Average Rating: 10.0 (1 vote)
|
|
|
| |
|
SHELL43
|
| |
SHELL43 "4-Node Plastic Large Strain Shell" is undocumented at ANSYS 12.0.1, namely because SHELL181 has a richer set of features. Use SHELL181 instead of SHELL43.
[permalink]
|
| |
|
Average Rating: 10.0 (1 vote)
|
|
|
| |
|
SHELL51
|
| |
SHELL51 "Axisymmetric Structural Shell" was undocumented at ANSYS 11.0. It should be replaced by SHELL208.
[permalink]
|
| |
|
Average Rating: 10.0 (1 vote)
|
|
|
| |
|
SHELL91
|
| |
SHELL91 "Nonlinear Layered Structural Shell" became undocumented at ANSYS 12.0.1 in order to simplify the shell element offerings. One should use SHELL281 instead since SHELL281 is a current technology element that has layered capabilities.
[permalink]
|
| |
|
Average Rating: 10.0 (3 votes)
|
|
|
| |
|
SHELL93
|
| |
SHELL93 "8-Node Structural Shell" became undocumented at ANSYS 12.0.1 in order to simplify the shell element offerings. One should use SHELL281 instead since SHELL281 is a current technology element with many more features compared with SHELL93.
[permalink]
|
| |
|
Average Rating: 10.0 (2 votes)
|
|
|
| |
|
SHELL99
|
| |
SHELL99 "Linear Layered Structural Shell" became undocumented at ANSYS 12.0.1 in order to simplify the shell element offerings. One should use SHELL281 instead since SHELL281 is a current technology element that has layered capabilities.
[permalink]
|
| |
|
Average Rating: 10.0 (4 votes)
|
|
|
| |
|
SHELLCONTACT
|
| |
Bob Weathers (Trane)
|
| |
Shows a simple example of contact with shells, shell offset key, and pretension elements.
[permalink]
|
| |
|
Average Rating: 8.9 (44 votes)
|
|
|
| |
|
Short Truss Tutorial
|
| |
(Ryerson University)
|
| |
A lab exercise of doing a truss model in ANSYS 9.0.
[permalink]
|
| |
|
Average Rating: 7.1 (7 votes)
|
|
|
| |
|
SHOWNRES
|
| |
Hursha Narayan (Robert Bosch Corporation)
|
| |
"This macro takes an result parameter as input and shows the value at the corresponding group of nodes selected in the model."
[permalink]
|
| |
|
Average Rating: 10.0 (3 votes)
|
|
|
| |
|
SILICON
|
| |
Steve Groothuis (Micron Technology, Inc.)
|
| |
Although strictly not an input file, the "silicon.mat" file contains temp-dependent properties of silicon. See this email from S. Groothuis for more informaiton.
[permalink]
|
| |
|
Average Rating: 7.9 (12 votes)
|
|
|
| |
|
Simple APDL Implementation of a 3D FEM Simulator for Mutual Capacitances of Arbitrarily Shaped Objects Like Interconnects [PDF]
|
| |
Andreas Hieke
|
| |
Alternative download link here or here
See other publication by A. Hieke. I can't recall if this or the above article is referenced in ANSYS 5.6 Theory Manual. A variant article "Tiny Devices, Big Problems: Computation of Capacitance in Microelectric Structures" was published in the ANSYS Solutions magazine Vol 2 No 3.
[permalink]
|
| |
|
Average Rating: 10.0 (2 votes)
|
|
|
| |
|
Simulation Of An Ultrasonic Piezoelectric Transducer
|
| |
David Johnson, Dharmendra Pal
|
| |
"This paper presents the piezoelectric, coupled field capability of the ANSYS/Multiphysics product in both linear and nonlinear simulations. A piezoelectric transducer assembly is modeled, including a discussion of vendor-supplied property data as it relates to the ANSYS material input requirements. A cylindrical geometry is treated as an axisymmetric model using the PLANE13 element type. The transducer model is used in modal and harmonic analysis solutions to understand its mechanical behavior and to aid in design modifications to optimize its weight, performance, and electrical power consumption."
[permalink]
|
| |
|
Average Rating: 9.4 (17 votes)
|
|
|
| |
|
Simulation of Bellcore Testing of Electronics Cabinets for the Telecommunications Industry [PDF]
|
| |
Chris Andersen
|
| |
Various Bellcore tests performed with ANSYS.
[permalink]
|
| |
|
| |
|
Simulation of Brake Block Induced Corrugation on Railway Wheels
|
| |
Ulf Sellgren
|
| |
"Railway wheels that are equipped with cast-iron brake blocks generate significantly more
rolling noise than wheels with other types of braking devices or block materials. The
roughness of the treads on cast-iron block-braked wheels has typically a peak at a wavelength
around 6 cm. The complex interaction between quasi-static and dynamic mechanical behavior
and thermal, chemical, and metallurgical effects in the block-wheel contact combined with the
rolling and sliding situation in the wheel-rail contact has made it difficult to get an
understanding of the causes from field measurements. Coupled transient thermal and quasi-static
mechanical FE simulations with ANSYS show that thermoelastic instability (TEI) may
be a major cause for the roughness initiation."
[permalink]
|
| |
|
Average Rating: 8.8 (8 votes)
|
|
|
| |
|
Simulation of the Retroglossal Fluid-Structure Interaction During Obstructive Sleep Apnea
|
| |
Franz Chouly, Annemie Van Hirtum, Pierre-Yves Lagr´ee, Jean-Roch Paoli, Xavier Pelorson, and Yohan P
|
| |
"A method for computing the interaction between the airflow
and the soft tissue during an Obstructive Apnea is presented. It
is based on simplifications of the full continuum formulation (Navier-
Stokes and finite elasticity) to ensure computation time compatible with
clinical applications. Linear elasticity combined with a precomputation
method allows fast prediction of the tissue deformation, while an asymptotic
formulation of the full Navier-Stokes equations (Reduced Navier-
Stokes/Prandtl equations) has been chosen for the flow. The accuracy of
the method has already been assessed experimentally. Then, simulations
of the complete collapsus at the retroglossal level in the upper airway
have been carried out, on geometries extracted from pre-operative radiographies
of two apneic patients. Post-operative geometries have been
also used to check qualitatively if the predictions from the simulations
are in agreement with the effects of the surgery."
[ANSYS Structural, version unspecified]
[permalink]
|
| |
|
| |
|
Sine sweep simulation [PDF]
|
| |
David Haberman (CSI)
|
| |
Discussion on harmonic sweeps, either via the direct displacement method or the large mass method.
Direct displacement method example input file and Large mass method example input file
[permalink]
|
| |
|
Average Rating: 8.5 (26 votes)
|
|
|
| |
|
SIRESUME
|
| |
Sheldon Imaoka (CSI)
|
| |
Use this for the RESUM_DB abbreviation in the Toolbar to prevent accidental resuming (which clears contents of current database). This macro will not prompt user for confirmation is database is blank. Otherwise, it will prompt user to verify that he/she wants to resume.
[permalink]
|
| |
|
Average Rating: 10.0 (2 votes)
|
|
|
| |
|
SIYSDCAP
|
| |
Sheldon Imaoka (ANSYS, Inc.)
|
| |
Tip on visualizing the Drucker-Prager Cap model yield surface.
[permalink]
|
| |
|
Average Rating: 8.4 (16 votes)
|
|
|
| |
|
SKIN
|
| |
Chris Masterson (University of Toronto)
|
| |
A while back I asked Bill Bulat for a pointer to a macro that could be used for meshing skin depths. He gave me some good pointers. I have since been working on a skin depth macro myself. I now have a first working beta". It is currently pretty crude since I'm relatively new to ANSYS, my geometry is pretty simple and the expansion algorithm I worked out is very simple. It will only mesh a line of rectangular prisms oriented with the current coordinate system. The end result is something similar to what a straight VSWEEP command could accomplish but with the difference that the user can specify exactly the thickness of the skin depth (or boundary layer if it suits) and how many layers of mesh should be contained in that skin depth. Suits my purposes for now so I thought that maybe somebody else might find a use as well. There are actually three macros: skin.mac - the main macro, and sorter.mac and picker.mac that are called from the main macro. The other caveat I guess is to mention that I wrote them for Ansys 5.5 and so some of the command names may be changed or obsolete (which includes jumping to a label which was already technically obsolete in 5.5) in newer versions."
"I posted some skin depth meshing macros to the Ansys egroup that you reproduced on your ansys.net page. Since then I have updated the macros significantly to make them more usable and a lot less buggy. The macro is now able to mesh full planes of rectangular prisms, instead of just a line of prisms. With the use of an extra coordinate system I use it to expand the mesh in both directions away from the surface of interest. The macros are now updated to Ansys version 5.6 as well (and in fact won't work in 5.5 due to VSWEEP no longer requiring source and target areas). Just thought I would send the new improved versions to save frustration if anyone ever uses them."
[permalink]
|
| |
|
Average Rating: 10.0 (2 votes)
|
|
|
| |
|
SKNDPTH
|
| |
Bill Bulat (CSI)
|
| |
Used to calculate skin depth. Prompts for resistivity, relative permeability, and frequency.
[permalink]
|
| |
|
Average Rating: 10.0 (3 votes)
|
|
|
| |
|
SLICEPLN
|
| |
Don Shaffer (Siemens Westinghouse Power Corp)
|
| |
"This macro moves the working plane origin to the specified keypoint and orients it with wz normal to the specified cartesian axis with x=1,y=2 and z=3."
[permalink]
|
| |
|
| |
|
Small Pivot Terms
|
| |
David Gross (Dominion Engineering, Inc.)
|
| |
Description of what small pivot terms of the stiffness matrix are during solution. (From XANSYS posting)
[permalink]
|
| |
|
Average Rating: 9.3 (14 votes)
|
|
|
| |
|
Smart Materials for Silent Alarms
|
| |
Mostafa Hedayatnia (Philips Consumer Communication)
|
| |
"Piezoceramic materials can produce motion by receiving electric potential across their polarized surfaces. Using finite-element analysis and optimization, engineers at Philips Corp. in Sunnyvale, Calif., have developed a miniature vibrator/piezo-bender that consumes only 8 milliamperes."
[permalink]
|
| |
|
Average Rating: 5.0 (4 votes)
|
|
|
| |
|
Smartsizing: Automatic Boundary Sizing for 2D and 3D meshes [PDF]
|
| |
Alexandre L. Cunha, Sunil Saigal, Scott A. Canann
|
| |
"We present in this paper a simple technique, called smart sizing, which automatically computes high quality initial element sizing on curves for triangular, quadrilateral and tetrahedral elements."
[permalink]
|
| |
|
Average Rating: 10.0 (5 votes)
|
|
|
| |
|
SMDT |
| |
SMDT,option,value
Change tolernace for solid modeling conditions. Affects all solid modeling operations, so be careful when using these values.
List of options:
1 - Tolerance for tesselation
2 - Tolerance for line on line
3 - Approx. tolerance
4 - Tolerance for point coincidence (default 1e-5 or 1e-4 -- e.g., can make tighter to very small dimensions)
5 - Tolerance for NURBS knot coincidence (default 1e-7, may be difficult to use)
6 - Tolerance for angle (default 1e-6, may be difficult to use)
7 - Machine precision tolerance
...up to 17...
[permalink]
|
| |
|
Average Rating: 8.0 (5 votes)
|
|
|
| |
|
SOLID191
|
| |
SOLID191 "3-D 20-Node Layered Structural Solid" has become undocumented in ANSYS 12.0.1 to simplify the element offerings. SOLID186 has layered capabilities along with many more features than SOLID191, so use that element type instead.
[permalink]
|
| |
|
| |
|
SOLID45 |
| |
Keyoption 7 for solid45
Toggles between temperature property evaluation between centroid and integration points.
[permalink]
|
| |
|
Average Rating: 10.0 (13 votes)
|
|
|
| |
|
SOLID46
|
| |
SOLID46 "3-D 8-Node Layered Structural Solid" has become undocumented in ANSYS 12.0.1 to simplify the element offerings. SOLID185 and SOLSH190 both have layered capabilities along with many more features than SOLID46, so use those elements instead.
[permalink]
|
| |
|
Average Rating: 10.0 (3 votes)
|
|
|
| |
|
SOLID5, SOLID98 |
| |
KEYOPT(1)=3 for Piezo option (UX, UY, UZ, VOLT) instead of using KEYOPT(1)=0 for PIEZO.
[STI: Documented in 5.6.]
[permalink]
|
| |
|
Average Rating: 10.0 (10 votes)
|
|
|
| |
|
SOLID64
|
| |
SOLID64 "3-D Anisotropic Structural Solid" was undocumented at ANSYS 11.0. It should be replaced by SOLID185.
[permalink]
|
| |
|
Average Rating: -10.0 (1 vote)
|
|
|
| |
|
SOLID65 |
| |
KEYOPT(10)=1 is an undocumented keyoption for SOLID65, available starting from ANSYS 12.1.
Depending on the input concrete constants, the failure surface may have a hole in the transition from compression-compression-compression state to the compression-compression-tension state. This keyoption attempts to patch this hole in the failure surface to help achieve convergence.
[permalink]
|
| |
|
Average Rating: 10.0 (4 votes)
|
|
|
| |
|
SOLID72
|
| |
SOLID72 "3-D 4-Node Tetrahedral Structural Solid with Rotations" was undocumented around ANSYS 5.7 because of the fact that many users incorrectly assumed that the rotational DOF of the solid element was compatible with those of beam or shell elements. There is no replacement except to use higher-order SOLID92 or SOLID187 instead.
[permalink]
|
| |
|
Average Rating: 0.0 (2 votes)
|
|
|
| |
|
SOLID73
|
| |
SOLID73 "3-D 8-Node Structural Solid with Rotations" was undocumented around ANSYS 5.7 because of the fact that many users incorrectly assumed that the rotational DOF of the solid element was compatible with those of beam or shell elements. There is no replacement except to use lower-order SOLID45/185 or higher-order SOLID95/186 instead.
[permalink]
|
| |
|
Average Rating: 10.0 (3 votes)
|
|
|
| |
|
SOLID92 and EMAT Files
|
| |
Sheldon Imaoka (CSI)
|
| |
Discussion on when EMAT files are written when using SOLID92. Preventing writing of EMAT files to disk may decrease overall solution times on some hardware. (From XANSYS posting)
[permalink]
|
| |
|
Average Rating: 10.0 (3 votes)
|
|
|
| |
|
SOLVE |
| |
SOLVE,,,,,NOCHECK
Solves without checking elements. Useful to force ANSYS to solve despite elements which produce shape testing errors. It is assumed that the user is able to determine that this is appropriate for his/her situation
[STI: This arises when "bad" elements exist, most commonly from imported meshes of 3rd party products since ANSYS 'fails to mesh' instead of generating error elements, by default]
[permalink]
|
| |
|
Average Rating: 10.0 (10 votes)
|
|
|
| |
|
SORT2D
|
| |
Ashok K. (EACoE, Bangalore)
|
| |
Ansys macro to sort a given numeric array (2d)
I usually get all the nodal coordinates into an array (call it NodeInfo) with
node numbers in col 1;
X,Y and Z coords in columns 2, 3 and 4 respectively.
Then lets say I want to sort by the Z- coord followed by the X-coord and then
the Y-coord I call the macro
sort_by_cols, 'NodeInfo', 4,2,3
The tolerance is something which you may or may not need. Depends on your application. If you just want to compare upto full decimal accuracy leave the tolerance
value at zero.
[permalink]
|
| |
|
Average Rating: 6.2 (4 votes)
|
|
|
| |
|
SORTED
|
| |
Gordon May (Rolls Royce Compressor Key System)
|
| |
Example of sorting arrays using *MOPER.
[permalink]
|
| |
|
Average Rating: 6.7 (6 votes)
|
|
|
| |
|
SORTEM
|
| |
Rick Fischer (Marconi Communications)
|
| |
Another similar example of sorting arrays using *MOPER.
[permalink]
|
| |
|
Average Rating: 10.0 (3 votes)
|
|
|
| |
|
SORTER
|
| |
Chris Masterson (University of Toronto)
|
| |
A while back I asked Bill Bulat for a pointer to a macro that could be used for meshing skin depths. He gave me some good pointers. I have since been working on a skin depth macro myself. I now have a first working beta". It is currently pretty crude since I'm relatively new to ANSYS, my geometry is pretty simple and the expansion algorithm I worked out is very simple. It will only mesh a line of rectangular prisms oriented with the current coordinate system. The end result is something similar to what a straight VSWEEP command could accomplish but with the difference that the user can specify exactly the thickness of the skin depth (or boundary layer if it suits) and how many layers of mesh should be contained in that skin depth. Suits my purposes for now so I thought that maybe somebody else might find a use as well. There are actually three macros: skin.mac - the main macro, and sorter.mac and picker.mac that are called from the main macro. The other caveat I guess is to mention that I wrote them for Ansys 5.5 and so some of the command names may be changed or obsolete (which includes jumping to a label which was already technically obsolete in 5.5) in newer versions."
"I posted some skin depth meshing macros to the Ansys egroup that you reproduced on your ansys.net page. Since then I have updated the macros significantly to make them more usable and a lot less buggy. The macro is now able to mesh full planes of rectangular prisms, instead of just a line of prisms. With the use of an extra coordinate system I use it to expand the mesh in both directions away from the surface of interest. The macros are now updated to Ansys version 5.6 as well (and in fact won't work in 5.5 due to VSWEEP no longer requiring source and target areas). Just thought I would send the new improved versions to save frustration if anyone ever uses them."n
[permalink]
|
| |
|
Average Rating: 9.2 (6 votes)
|
|
|
| |
|
Space-Time Finite Element Approximation and Numerical Solution of Hereditary Linear Viscoelasticity Problems
|
| |
J. Orlik, A. Ostrovska
|
| |
"In this paper we suggest a fast numerical approach to treat problems
of the hereditary linear viscoelasticity, which results in the system
of elliptic partial differential equations in space variables , who’s coefficients
are Volterra integral operators of the second kind in time. We
propose to approximate the relaxation kernels by the product of purely
time- and space-dependent terms, which is achieved by their piecewisepolynomial
space-interpolation. A priori error estimate was obtained and
it was shown, that such approximation does not decrease the convergence
order, when an interpolation polynomial is chosen of the same order as
the shape functions for the spatial finite element approximation, while the
computational effort is significantly reduced."
[ANSYS Nonlinear, version unknown]
[permalink]
|
| |
|
| |
|
Sparse Solver (Memory and Performance Information)
|
| |
Gene Poole (ANSYS, Inc.)
|
| |
Discussion on memory requirements and performance of the sparse solver in ANSYS. (From XANSYS posting)
[permalink]
|
| |
|
Average Rating: 8.8 (4 votes)
|
|
|
| |
|
Sparse Solver Improvements [PDF]
|
| |
Sheldon Imaoka (ANSYS, Inc.)
|
| |
"There have been various sparse solver improvements in each release of ANSYS. This memo hopes to cover some general information on the solvers available in ANSYS as well as performance improvements between ANSYS 5.6 and 6.0 related to linear static analyses."
(Week 4, week of 10/15/01.)
[permalink]
|
| |
|
Average Rating: 10.0 (1 vote)
|
|
|
| |
|
Sparse vs. PCG Solvers
|
| |
Gene Poole (ANSYS, Inc.)
|
| |
Thorough discussion on the differences in performance between sparse and PCG solvers.
[permalink]
|
| |
|
Average Rating: 6.9 (8 votes)
|
|
|
| |
|
Spatially-Varying Pressure Loading in Workbench Simulation [ZIP]
|
| |
Sheldon Imaoka (ANSYS, Inc.)
|
| |
"Workbench Simulation 11.0 allows users not only to apply constant pressure loads or force vectors per unit area but also to utilize hydrostatic pressure loads and line pressure loads (force per unit length), and these can be defined as a function of time. Moreover, fluid pressures can be mapped from a steady-state or transient ANSYS CFX solution.
Despite these options, there may be situations where a user may want to import a predefined, spatially-varying pressure field from an external text file. This can be accomplished through the use of a “Commands” object and APDL tables, which this
memo will introduce."
(Week 38, week of 07/01/07.)
[permalink]
|
| |
|
Average Rating: 8.5 (20 votes)
|
|
|
| |
|
SPEC_ACC
|
| |
David Haberman (CSI)
|
| |
Example of running a sprectrum analysis in ANSYS.
Acceleration Sprectrum.
[permalink]
|
| |
|
Average Rating: 8.7 (16 votes)
|
|
|
| |
|
SPEC_ACC_VEL_MPT
|
| |
David Haberman (CSI)
|
| |
Example of running a sprectrum analysis in ANSYS.
Multipoint input sprectrum (acceleration and velocities).
[permalink]
|
| |
|
Average Rating: 7.7 (11 votes)
|
|
|
| |
|
SPEC_PULSE2
|
| |
David Haberman (CSI)
|
| |
User can modify the 1/2 sine input amplitude and duration.
ANSYS will calculate the fft and give you an input spectrum for later use in a spectrum analysis.
[permalink]
|
| |
|
Average Rating: 8.7 (15 votes)
|
|
|
| |
|
SPHERE
|
| |
Sheldon Imaoka (CSI)
|
| |
Example of acoustic radiating sphere. Comparison w/ hand calculations.
[permalink]
|
| |
|
Average Rating: 8.8 (154 votes)
|
|
|
| |
|
SPIDER
|
| |
Marco Perucchi (Delta JS AG)
|
| |
"I have a macro that might be useful for you. It creates spider webs between 1 center and a group of surrounding nodes. Before starting the macro you have to collect the center node in one component and the group of surrounding nodes in another component. If you are able to do that with your model you should be able to create the link elements without problems."
[permalink]
|
| |
|
Average Rating: 10.0 (8 votes)
|
|
|
| |
|
SPIDER2
|
| |
Donald Cummings (GE Transportation Systems)
|
| |
"This macro creates a spider-web that connects a center node with a group of surrounding nodes on the inside surface of a hole with line elements (beam or link). The modeling objective is to provide attachment of a single point to the inside surface of a hole for the transfer of loads or boundary conditions to the model. This is an approximate method of modeling a shaft support in a hole."
[permalink]
|
| |
|
Average Rating: 10.0 (2 votes)
|
|
|
| |
|
SPIDER3
|
| |
Barry O'Donnell (ODCS Ltd.)
|
| |
"I attach the macro which I was working on, for which I recieved help from the group for. It is called as:
spider,arg1,arg2
where arg1 is the washer diameter and arg2 is the centre node number. It is intended to connect all the nodes on the attached area that are within the
washer diameter (arg1) to the central node (arg2) using RBE3 eleemnts. Useful if you haven't specific areas which correspond to the bolt head
dimension etc. It would be easy to modify, though currently it is intended for bolts aligned with the global x-axis."
[permalink]
|
| |
|
Average Rating: 9.4 (8 votes)
|
|
|
| |
|
SPIRAL
|
| |
Keith DiRienz (PADT)
|
| |
A macro to generate a spiral.
[permalink]
|
| |
|
Average Rating: 7.1 (7 votes)
|
|
|
| |
|
SPLOT |
| |
SPLOT,area_min,area_max,area_inc,mesh
where 'area_min' is beginning area number, 'mesh' is the amount of lines to put on the surface (like a wireframe tesselation). I think this 'mesh' argument is what J. Crawford referred to as 'contour lines'. (That's a better description, actually) [6.0]
By default, if you just issue SPLOT with no arguments, it plots all surfaces with a 'surface mesh density' (wireframe tessellation density) of 4, I think.
Plot surfaces ANSYS uses for basis for geometric areas (similar to surface/face analogy in CADfix); works in 5.4 but will cause 5.5-5.7.0 to crash. Reintroduced at 5.7.1 and 6.0.
With the improvements to the solid modeling capabilities in ANSYS 6.0, the SPLOT command became more relevant in detecting potential problems with geometry.
[permalink]
|
| |
|
Average Rating: 10.0 (4 votes)
|
|
|
| |
|
SPLTARCS
|
| |
John Crawford (Honeywell)
|
| |
A macro that splits the selected arcs into two pieces. this is done to avoid problems when using NUMM,KP with circles made from two 180 degree arcs..
[permalink]
|
| |
|
Average Rating: 10.0 (4 votes)
|
|
|
| |
|
SPOKES
|
| |
Pat Cunningham (CAEAI)
|
| |
"The macro will create a connection between a selected set of nodes and a master node typically located at the center of curvature of a line connecting the selected nodes."
Used for generating CERIG, MPC184, or RBE3.
[permalink]
|
| |
|
Average Rating: 10.0 (13 votes)
|
|
|
| |
|
SPOKES_MPC
|
| |
R. Balasubramanian (Brakes India Ltd - TVS)
|
| |
"This Macro forms a 'spider web' like Multipoint constraint for a given set of nodes. The user has to just place the clusters of nodes in separate components by names 'NODES1','NODES2'..etc.,
The macro automatically finds the 'centre-node' for each node cluster and links it with the surrounding nodes in the cluster to form a 'spokes' pattern using MPC 184 elements with 'Rigid-beam' option
(the element option can be changed by user for his/her requirements)."
[permalink]
|
| |
|
Average Rating: 7.5 (12 votes)
|
|
|
| |
|
SPOPT |
| |
SPOPT,PSD,NMODE,Elcalc,FRATIO,SIGNIF,IntKey,IntArr,NUME
“FRATIO,” or “frequency ratio for modal coupling,” limits covariance cross-terms by
allowing the user to provide a ratio of the frequency of two modes to be included. For
example, specifying FRATIO as “1” will only include diagonal terms of the covariance
matrix. This only works in conjunction with numerical integration method, discussed next.
For numerical integration, the last four arguments apply. The last argument should be
“NUME” to activate numerical integration. The other three options relate to the “integration
significance level,” “integration key (value of 1 to 6),” and “work array length (value of 100
to 500),” although these are optional and need not be specified. Note that if numerical
integration is used, the RPSD calculations in /POST26 will not work properly.
[permalink]
|
| |
|
Average Rating: 10.0 (1 vote)
|
|
|
| |
|
SPRING
|
| |
Dave Lindeman (3M)
|
| |
Attached is an input file that sets up and runs an analysis for a variable radius (hyperbolic) compression spring. You should be able to modify it for your needs.
[permalink]
|
| |
|
Average Rating: 8.7 (31 votes)
|
|
|
| |
|
SPRS_MPRS
|
| |
Sheldon Imaoka (ANSYS, Inc.)
|
| |
The attached zip file includes a simple example demonstrating the procedure to perform a single-point response spectrum (SPRS), where the excitation in 3 direction is applied together (using SRSS combination), not independently.
The procedure for multi-point response spectrum (MPRS) is included as well for the same situation.
An Excel spreadsheet shows that the results obtained for this simple model is the same for both methods (compare the mode coefficients for each squared mode in the spreadsheet).
[permalink]
|
| |
|
Average Rating: 9.6 (14 votes)
|
|
|
| |
|
SRCS |
| |
SRCS, NTURN, CURR, FREQ, PSYM, CSYM
NTURN: Number of turns in the coil winding. Input the total number of windings regardless of the symmetry used in the model.
CURR: Current per turn applied to the coil. Required only for a three-dimensional analysis (the value is calculated for a two-dimensional analysis and is returned as the parameter IWIND).
FREQ: Harmonic frequency of coil current (in Hertz). Required only if terminal voltage (VLTG) is to be calculated. Assumes that eddy currents are neglected.
PSYM: Planar symmetry factor. Used when a symmetric model is used through the cross-section of the coil. The factor is applied to the terminal parameter calculations. For example, if an axisymmetric coil is modeled with symmetry about the X-axis, the symmetry factor would be 2. Defaults to 1.
CSYM: Circumferential symmetry factor. Used only for three-dimensional analysis when a circular-symmetric model is used. For example, if a 90 degree sector is modeled, the symmetry factor (to scale to a full 360 degree model) would be 4. Defaults to 1.
Undocumented at ANSYS 5.7, SRCS is a macro that is still available in the "apdl" subdirectory in ANSYS 11.0. SRCS is limited to linear models. The LMATRIX command, however, is applicable to both linear and nonlinear models, so LMATRIX should be used instead of SRCS.
[permalink]
|
| |
|
Average Rating: 10.0 (4 votes)
|
|
|
| |
|
ST_EX3
|
| |
Sheldon Imaoka (CSI)
|
| |
Simple example illustrating use of generating, using, and post-processing thermal surface effect elements.
[permalink]
|
| |
|
Average Rating: 10.0 (16 votes)
|
|
|
| |
|
Status Bar |
| |
*ABSET,title40,[BAR|KILL|BOTH]
Creates a customized status/progress bar for use during a macro to give feedback to the user as to what % complete the macro is at.
*ABCHECK,percent,newtitle
Updates the status bar to "percent" complete with information printed as "newtitle"
What is useful is to make "newtitle" a parameter (%PARAM%) as well.
It is recommended not to call *ABCHECK more than 20 times in a loop. Also, be sure to check _RETURN values prior to issuing this
*ABFINI
Removes status bar
[STI: See ALSM.MAC, VLSM.MAC, and JB_FORC.MAC macros in the Macros page for examples]
[permalink]
|
| |
|
Average Rating: 0.0 (2 votes)
|
|
|
| |
|
Steve Owen's Meshing Research Corner
|
| |
Steve Owen
|
| |
This is the best source to go for everything you wanted to know about meshing...but were afraid to ask.
[permalink]
|
| |
|
Average Rating: 10.0 (4 votes)
|
|
|
| |
|
STIICEMFLOTRAN
|
| |
Sheldon Imaoka (ANSYS, Inc.)
|
| |
MESH200 supports a 4-node tetrahedral option (KEYOPT(1)=8), but the node numbering is different from a degenerate 8-node tetrahedral element, such as FLUID142.
If a user exports a lower-order tetrahedral mesh using MESH200, conversion to an actual element, such as FLUID142, may be required. Use of this macro allows a user to perform this relatively easily (it is customized to convert 4-node MESH200 tetrahedral elements to Flotran FLUID142 tetrahedral elements, although the user can modify the macro to suit his/her needs).
[permalink]
|
| |
|
Average Rating: 10.0 (6 votes)
|
|
|
| |
|
STORE |
| |
STORE,PSD,num,1
The last argument, when set to 1, will use evenly-spaced points for RPSD calculations rather than automatically-generated points. (The default is automatic and recommended)
[permalink]
|
| |
|
Average Rating: 10.0 (1 vote)
|
|
|
| |
|
Stress vs Strain Experimental Curve
|
| |
Guoyu Lin (ANSYS, Inc.)
|
| |
Discussion on stress vs. strain curves, plasticity, element formulation, necking, and undocumented NLISO option.
[permalink]
|
| |
|
Average Rating: 9.4 (9 votes)
|
|
|
| |
|
Strings |
| |
*DIM,StrPar,STRING,nChar,[nString,{nPages]]
Defines strings (5.6)
strcat(Param1(1,1),Param2(1,1))
Concatenation of strings
Example:
*DIM,Param1,STRING,128
*DIM,Param2,STRING,128
*DIM,Param3,STRING,128
Param1(1,1) = 'THIS IS STRING 1'
Param2(1,1)=' THIS IS STRING 2'
Param3(1,1) = strcat(Param1(1,1),Param2(1,1))
This gives:
THIS IS STRING 1THIS IS STRING 2
strsub(Param1(1,1),location,numchr)
Gets substring of numchr long starting from location
strfill(Param1(1,1),Param2(1,1),location)
Fills in Param2 to Param1 starting from location
strleng(Param1(1,1))
Returns length of Param1 as a scalar number
strpos(Param1(1,1),Param2(1,1))
Returns location of Param2 substring in Param1 string as a scalar number
An example macro can be downloaded which illustrates some of the above points through examples.
[STI: Strings will be documented at 5.7]
[permalink]
|
| |
|
Average Rating: 10.0 (11 votes)
|
|
|
| |
|
STRNE
|
| |
Mike Rife (CSI)
|
| |
This macro sums the strain energy at every substep for a transient analysis and then plots the values versus time.
[permalink]
|
| |
|
Average Rating: 10.0 (9 votes)
|
|
|
| |
|
STRPLOT
|
| |
Peter Bastian (Darmstadt University of Technology)
|
| |
This macro displays results as continuos contours using the PLNSOL command. For the display of the numbers in the legend, you can define the number of contours and the number of digits after the decimal point, to be displayed. If you do not want any digits after the decimal point, you can define, how many places should be displayed with a "0". For example 2100 instead of 2123.
[permalink]
|
| |
|
Average Rating: 6.7 (6 votes)
|
|
|
| |
|
Structural and Thermal Analysis of a MEMS Angular Gyroscope
|
| |
Chris C. Painter and Andrei M. Shkel
|
| |
"This paper describes the structural and thermal modeling of a Micro Electro Mechanical System (MEMS) z-axis angular gyroscope. The gyroscope consists of a oscillating proof mass supported by a suspension made up of six concentric interconnected rings rigidly attached to an anchored frame. The device is capable of measuring angular displacement through precession of the proof mass line of oscillation in the presence of rotation induced Coriolis force. Using a strain energy method,a closed form solution for the effective stiffness of the suspension system is developed, which is confirmed using finite element modeling. A comparative study of the suspension with a commonly used serpentine spring suspension demonstrates that the studied device is robust to thermal fluctuations and residual stresses. A parametric analysis is used to identify an appropriate micromachining technology suitable for the fabrication of the angular gyroscope."
[permalink]
|
| |
|
Average Rating: 10.0 (7 votes)
|
|
|
| |
|
Structural Beam Elements Overview [PDF]
|
| |
Sheldon Imaoka (CSI)
|
| |
An overview of beam elements available in ANSYS, including the new BEAM188/189 elements and differences between thin and thick beams.
[permalink]
|
| |
|
Average Rating: 8.8 (17 votes)
|
|
|
| |
|
Structural Shell Elements Overview [PDF]
|
| |
Sheldon Imaoka (CSI)
|
| |
Overview of structural shell elements in ANSYS, including differences between thin and thick shells, drilling DOF, etc.
[permalink]
|
| |
|
Average Rating: 9.2 (20 votes)
|
|
|
| |
|
Structural Surface Effect Elements Intro [PDF]
|
| |
Sheldon Imaoka (CSI)
|
| |
Introduction to structural surface effect elements (SURF153/154).
BOLTLOAD input file
[permalink]
|
| |
|
Average Rating: 8.6 (7 votes)
|
|
|
| |
|
Structural surface Effect Elements, General Overview
|
| |
Sheldon Imaoka (ANSYS, Inc.)
|
| |
An overview presentation and example workshop on structural surface effect elements. This is an old presentation I did at ANSYS 5.6.1, so if you use later versions of ANSYS, some of the menus and dialog boxes may have changed.
[permalink]
|
| |
|
Average Rating: 9.5 (11 votes)
|
|
|
| |
|
SUBCONT
|
| |
Joe Metrisin (Florida Turbine Technologies, Inc.)
|
| |
"Attached is a macro I wrote years ago which automates substructuring with contact. Just build the complete model with contact elements included, and create the component names as described in the macro header. The macro puts all the linear elements into a superelement and iterates on the contact elements only."
[permalink]
|
| |
|
Average Rating: 10.0 (8 votes)
|
|
|
| |
|
Subject Specific Finite Element Modelling of the Levator Ani
|
| |
Su-Lin Lee1, Ara Darzi, Guang-Zhong Yang
|
| |
"Understanding of the dynamic behaviour of the levator ani is
important to the assessment of pelvic floor dysfunction. Whilst shape modelling
allows the depiction of 3D morphological variation of the levator ani between
different patient groups, it is insufficient to determine the underlying behaviour
of how the muscle deforms during contraction and strain. The purpose of this
study is to perform a subject specific finite element analysis of the levator ani
with open access magnetic resonance imaging. The method is based on a
Mooney-Rivlin hyperelastic model and permits dynamic study of subjects
under natural physiological loadings. The value of the proposed modelling
framework is demonstrated with dynamic 3D data from nulliparous, female
subjects"
[ANSYS Nonlinear, version unspecified]
[permalink]
|
| |
|
Average Rating: 10.0 (1 vote)
|
|
|
| |
|
SUBOPT |
| |
SUBOPT,,,,,,,,SubConvTol
Sets convergence tolerance for modal analysis w/ subspace method. SubConvTol defaults to 1e-5 [at 5.3] and can be tightened to 1e-12 or loosened to speed up convergence.
[permalink]
|
| |
|
Average Rating: 7.5 (4 votes)
|
|
|
| |
|
SUBSTR-FULLPOST
|
| |
Sheldon Imaoka (ANSYS, Inc.)
|
| |
Fictitious model used to demonstrate substructuring. SETRAN and SESYMM are used to translate and reflect a superelement. RSPLIT and RSTOFF are also used, and postprocessing of the entire model (superelements and non-superelements) is shown.
[permalink]
|
| |
|
Average Rating: 2.5 (4 votes)
|
|
|
| |
|
Super Elastic Alloy Eyeglass Frame Design Using the ANSYS Workbench Environment
|
| |
Peter R. Barrett and Patrick Cunningham (CAEAI)
|
| |
"Up front analysis at the concept stages of developing a device most often result in reduced time to market and a better more efficient product development cycle. Design Modeler (1) / DesignXplorer (2) and ANSYS Structural’s super-elastic material model (3) are used in this demonstration of a design process for an eyeglass frame. This example provides an illustration of using the parametric functionality of the ANSYS Workbench environment for a highly nonlinear application. The Workbench environment can be used to perform design iterations in conjunction with material laws only available in the standard ANSYS environment. A shape memory superelastic material law was formally included in ANSYS 8.0. The material law captures the super-elastic behavior of Nitinol (4) along with its unique hysteretic response under cyclic loading. In the demonstration, the eyeglass frame is subjected to crushing and cyclic loading events. Geometric design variables are varied in an attempt to increase the frame stiffness yet keep the peak strain levels in the frame below 10% strain, which is a typical elastic limit for Nitinol. The cyclic behavior of the material is also monitored under the design load to evaluate the potential of fatigue failure. The procedure demonstrates the ease in interfacing the suite of Workbench products with geometric, material and contact nonlinear analysis problems."
Presentation file also available here
[permalink]
|
| |
|
Average Rating: 3.3 (15 votes)
|
|
|
| |
|
Superelements in acoustic analyses
|
| |
Sheldon Imaoka (CSI)
|
| |
Using superelements in acoustic analyses. (From XANSYS posting)
[permalink]
|
| |
|
Average Rating: 7.7 (13 votes)
|
|
|
| |
|
SURF_TRACTION
|
| |
Sheldon Imaoka (CSI)
|
| |
Shows surface effect element for traction load application.
[permalink]
|
| |
|
Average Rating: 10.0 (6 votes)
|
|
|
| |
|
SURF19
|
| |
SURF19 "2-D Surface Effect" was undocumented around 5.6. It should be replaced with either SURF151 (thermal) or SURF153 (structural).
[permalink]
|
| |
|
| |
|
SURF22
|
| |
SURF22 "3-D Surface Effect" was undocumented around 5.6. It should be replaced with either SURF152 (thermal) or SURF154 (structural).
[permalink]
|
| |
|
Average Rating: 10.0 (2 votes)
|
|
|
| |
|
Surface Effect Elements, General Overview
|
| |
Sheldon Imaoka (ANSYS, Inc.)
|
| |
An overview presentation and example workshop on generating surface effect elements. This is an old presentation I did at ANSYS 5.6.1, so if you use later versions of ANSYS, some of the menus and dialog boxes may have changed.
[permalink]
|
| |
|
Average Rating: 9.2 (6 votes)
|
|
|
| |
|
SVSEL
|
| |
Sheldon Imaoka (ANSYS, Inc.)
|
| |
Macro used to select solids based on the value of the volume itself (=length^3). Can be used to select all volumes of a certain value or a range of values (with tolerance).
[permalink]
|
| |
|
Average Rating: 5.0 (3 votes)
|
|
|
| |
|
SWP
|
| |
Barry O'Donnell (ODCS Ltd.)
|
| |
"This macro extracts the peak worst
principal stress. The worst principal stress can be defined as:
max(S1,abs(S3)) and should be stored with the appropiate sign, e.g.
S1=100,S3=-70,SWP=100 & S1=100,S3=-170,SWP=170."
[permalink]
|
| |
|
Average Rating: 10.0 (2 votes)
|
|
|
| |
|
SXYZ
|
| |
John Crawford (Honeywell)
|
| |
It is often times nice to be able to get the stress at a specific location in space,whether a node is there or not. By some strange quirk of fate, I just happen to have a macro that does this. Here it is.
[permalink]
|
| |
|
Average Rating: 10.0 (38 votes)
|
|
|
| |
|
Tabular Boundary Conditions and Function Editor at 6.0 [PDF]
|
| |
Sheldon Imaoka (ANSYS, Inc.)
|
| |
"This tips and tricks is an introductory memo on the use of tabular and function boundary conditions. The use of the Function Editor is also discussed."
(Week 9, week of 12/03/01.)
[permalink]
|
| |
|
Average Rating: 8.9 (28 votes)
|
|
|
| |
|
TB,OGDEN |
| |
TB,OGDEN
Ogden Hyperelastic Material
similar to *MOONEY for Ogden constitutive law for HYPER56, 58, & 74.
[STI: Ogden material is available for 18x family of elements at 5.7, so it is strongly recommended to use those elements instead.]
[permalink]
|
| |
|
Average Rating: 9.0 (15 votes)
|
|
|
| |
|
TB,PRONY |
| |
For TB,PRONY, up to 10 pairs of constants can be input. [The documentation mentions only up to 6 pairs of constants for TB,PRONY.]
[STI: At 10.0, up to 100 pairs can be used and is documented.]
[permalink]
|
| |
|
Average Rating: 9.5 (10 votes)
|
|
|
| |
|
TCHG |
| |
TCHG, ELEM1, ELEM2, ETYPE2
Converts 20-node degenerate tets (e.g., SOLID95) to 10-node degenerate tets (e.g., SOLID92).
TCHG is documented in 5.5 and 5.6. It is undocumented but available at 5.4.
[permalink]
|
| |
|
Average Rating: 10.0 (1 vote)
|
|
|
| |
|
TCHKPLOT
|
| |
Sung-Chul Lee (Engineering Systems & Consulting, Inc.)
|
| |
Macro to create shell thickness plot into 8-color contour band by respecifying element color properties.
[permalink]
|
| |
|
Average Rating: 10.0 (5 votes)
|
|
|
| |
|
Techniques for Successfully Using ANSYS Contact Elements
|
| |
Rich Bothmann
|
| |
Presentation from the Midwest ANSYS User Group
[ANSYS Nonlinear, version 9.0]
[permalink]
|
| |
|
Average Rating: 9.4 (9 votes)
|
|
|
| |
|
TEGEN |
| |
TEGEN,inum,numincr,estart,eend,eincr
Generates/copies element temperatures.
inum is number of times to perform (>1)
numincr is element number increment
estart,eend,eincr is range of element numbers starting from estart to eend incremented by eincr (can use "all" for estart)
[permalink]
|
| |
|
| |
|
TEMPDELE.BAT
|
| |
Bram Weisman (SBM-IMODCO)
|
| |
"Caution: This batch file is very powerful. It searches the current folder
and all subfolders for known ANSYS temporary files and deletes them without
sending them to the recycle bin. Therefore I would recommend that you do
not execute this in the root folder of any drive which has program files.
It would be O.K. to execute this one folder down in a folder where you keep
your ANSYS project files. Also, you should familiarize your with the list
of file extensions which this batch files deletes and be sure you agree with
it. Do not run this in an ANSYS folder if you plan to do any RESTART from
existing results files."
[permalink]
|
| |
|
Average Rating: 7.5 (2 votes)
|
|
|
| |
|
Text and compression utilities [PDF]
|
| |
Sheldon Imaoka (CSI)
|
| |
Memo on text editors which support syntax highlighting, useful in editing input files and/or macros. Also discusses compression utilities to reduce filesize of database and results files. (Also see "bzip2" compression utility, not discussed in memo)
[permalink]
|
| |
|
Average Rating: 10.0 (3 votes)
|
|
|
| |
|
TEXT_UNIX
|
| |
John Swanson (SAS, Inc./ANSYS, Inc.)
|
| |
This macro launches a text editor and creates a file called "jobname.inp" in the current working directory. A similar macro for Windows is also available.
[permalink]
|
| |
|
| |
|
TextPad APDL Syntax File
|
| |
Bob Weathers (Trane)
|
| |
APDL Syntax definitions for use with TextPad on Windows. (Modified by Sheldon)
[permalink]
|
| |
|
Average Rating: 10.0 (5 votes)
|
|
|
| |
|
TFUN |
| |
TFUN,reference,variable,psd_table,name
Plot transfer function.
See Section 6 of the PSD Postprocessing Tip for details on this usage.
[permalink]
|
| |
|
| |
|
TGEN |
| |
TGEN,inum,numincr,nstart,nend,nincr
Generates/copies nodal temperatures.
inum is number of times to perform (>1)
numincr is node number increment
nstart,nend,nincr is range of node numbers starting from nstart to nend incremented by nincr (can use "all" for nstart)
[permalink]
|
| |
|
Average Rating: 10.0 (2 votes)
|
|
|
| |
|
The Building Blocks of Simulation: A New Family of Elements for Stress Analysis
|
| |
(ANSYS, Inc.)
|
| |
Presentation on 18x family of elements (part of the "Advanced Analysis with ANSYS" seminar during the 2002 User's Conference).
[permalink]
|
| |
|
Average Rating: 0.0 (2 votes)
|
|
|
| |
|
The Comparison of Biomechanical Breast Models: Initial Results
|
| |
C. Tanner, J.A. Schnabel, A. Castellano Smith, L.I. Sonoda, D.L.G. Hill, D.J. Hawkes, A. Degenhard,
|
| |
"We present initial results from evaluating the accuracy with which biomechanical breast models based on finite element methods can predict the displacements of tissue within the breast. We investigate the influence of different tissue elasticity values, Poisson’s ratios, boundary conditions, finite element solvers and mesh resolutions on one data set. MR images were acquired before and after compressing a volunteer’s breast gently. These images were aligned using a 3D non-rigid registration algorithm. The boundary conditions (surface displacements) were derived from the result of the non-rigid registration or by assuming no patient motion at the posterior or medial side. Three linear and two non-linear elastic material models were tested."
[permalink]
|
| |
|
Average Rating: 5.8 (6 votes)
|
|
|
| |
|
The Control Of The Thermal Environment Of Perimeter Spaces In Buildings To Prevent Cold Drafts
|
| |
Yuji Hukushima, Yasuo Utsumi, Hiroshi Kobayashi, Yoshimi Ishikawa, Mitsuo Suzuki, And Tatsuya Yamash
|
| |
"This paper is focused on the evaluation of simulation system using the experiment result and the configuration of pericounter which is the part of counter unit setting at bottom of window side with heat panel to avoid the influence of cold draft, utilizing simulation system. The simulation shows similar flow pattern to full scale experiment and consequent simulations indicate that cold draft does not flow into interior zone when the heat generation rate exceeds heat loss from the window in most cases. When the heat generation portion is 75% of heat loss from the window, some cases which have certain configuration of pericounter successfully avoids the influence of draft without fan."
[permalink]
|
| |
|
Average Rating: 10.0 (5 votes)
|
|
|
| |
|
The Numerical Analysis of Strain Behavior at the Solder Joint and Interface in a Flip Chip Package
|
| |
S.C. Chen, Y.C. Lin, C.H. Cheng
|
| |
"The aim of this study was to investigate the strain behaviors at the joint interface of a flip chip package during thermal cycling testing using
a numerical method. Because the underfill and solder bump material properties exhibit a large non-linearity in the higher temperature range,
the linear elastic assumption may lose accuracy during numerical analysis. This study compared the differences in interfacial stress or strain
between the linear and non-linear material property assumptions. The viscoplasticity of the solder bump and temperature-dependent underfill
properties were assumed in the non-linear analysis. The numerical results showed that the solder bump failure mechanism was a combination
of fatigue and creep actions dominated by plastic shear strain. The tensile stress due to shrinkage and hardening in the solder joints in the low
thermal cycle temperature dwell period could result in ablation at the joint interface."
ANSYS 5.6.1, Anand model
[permalink]
|
| |
|
Average Rating: 6.7 (3 votes)
|
|
|
| |
|
The Thermo-Mechanical Stress Issues in a Thermally Enhanced QFP
|
| |
Jack G. Hwang, T. J. Huang, and J. J. Lee
|
| |
"A finite element model with multiple load steps for different processes is used to predict the stresses in die in a thermally enhanced QFP (HQFP)."
[permalink]
|
| |
|
Average Rating: 10.0 (3 votes)
|
|
|
| |
|
THERM_CONT
|
| |
Sheldon Imaoka (CSI)
|
| |
Simple input file demonstrating thermal contact conductance with surf-to-surf contact elements (not all thermal features of contact elements shown). Note: Thermal contact for 169-174 elements are BETA at 5.6.
[permalink]
|
| |
|
Average Rating: 10.0 (31 votes)
|
|
|
| |
|
Thermal contact overview [PDF]
|
| |
Yongyi Zhu (ANSYS, Inc.)
|
| |
Presentation on the thermal contact capabilities of the surface-to-surface contact elements, beta at 5.6.
Input file for pressure-dependent thermal conductance
[permalink]
|
| |
|
Average Rating: 9.7 (17 votes)
|
|
|
| |
|
Thermal Finite Elements Analysis of the BaBar Silicon Vertex Tracker
|
| |
D. Barni, D. Giugni, F. Lanni, F. Palombo
|
| |
"In this note we present nite elements calculations of the thermal behavior of the BaBar silicon vertex tracker. Layers 1-2, 3 and 5 have been studied. Results show the adequacy of the cooling system in keeping the front-end chips into their optimal working condition. Thermo-mechanical results of layers 1-2 are also presented."
[permalink]
|
| |
|
Average Rating: 10.0 (4 votes)
|
|
|
| |
|
Thermal Modeling of the Infrared Reflow Process for Solder Ball Connect (SBC)
|
| |
H.V. Mahaney
|
| |
"A thermal model of the infrared reflow process
has been developed for an FR-4 card
populated with an array of Solder Ball Connect
(SBC) modules. The analysis of the three-dimensional, transient, finite element model
accounts for radiative exchange within the
infrared oven and for the heat conduction
(nonisotropic) within the modules and card.
Transient temperature profiles of selected
points and three-dimensional temperature
distributions at selected times are presented
to describe the primary heat-transport
mechanisms. Numerical predictions and
empirical data indicate that the SBC modules
are relatively isothermal throughout the
infrared reflow process. Therefore, every
solder ball within the array exhibits a nearly
identical thermal profile. This result is
fortunate, since the inner solder ball
connections cannot be visually inspected. The
influence of module spacing and the ability to
improve the reflow process by use of a high-emissivity cap coating are demonstrated."
[permalink]
|
| |
|
Average Rating: 8.3 (3 votes)
|
|
|
| |
|
Thermal Stress Analysis of Numi Baffle
|
| |
Bob Wands
|
| |
(Thermal-stress analysis)
[permalink]
|
| |
|
Average Rating: 10.0 (6 votes)
|
|
|
| |
|
Thermal Surface Effect Elements Intro [PDF]
|
| |
Sheldon Imaoka (CSI)
|
| |
Introduction to thermal surface effect elements (SURF151/152).
[permalink]
|
| |
|
Average Rating: 10.0 (9 votes)
|
|
|
| |
|
Thermal surface Effect Elements, General Overview
|
| |
Sheldon Imaoka (ANSYS, Inc.)
|
| |
An overview presentation and example workshop on thermal surface effect elements. This is an old presentation I did at ANSYS 5.6.1, so if you use later versions of ANSYS, some of the menus and dialog boxes may have changed.
[permalink]
|
| |
|
Average Rating: 9.5 (10 votes)
|
|
|
| |
|
Thermal-stress analyses using SHELL57 and SHELL93
|
| |
Sheldon Imaoka (CSI)
|
| |
Tips on performing thermal-stress analyses of shells, including temperature effects of SHELL93 and compatibility with SHELL57. (From XANSYS posting)
[permalink]
|
| |
|
Average Rating: 8.8 (20 votes)
|
|
|
| |
|
Thermomechanical Fatigue Failure of Interfaces in Lead-Free Solders
|
| |
M¨uge Erinc (Eindhoven University of Technology)
|
| |
"The European Union Waste Electrical and Electronic Equipment Directive (WEEE)
and Restriction of Hazardous Substances Directive (RoHS) banned lead from electronic
systems from July 1, 2006 onwards, which has led to much interest in leadfree
solders in the past years. Among several lead-free solder alternatives, SnAgCu
is a widely accepted replacement due to its better creep-fatigue resistance and microstructural
stability. SnAgCu has been extensively studied in the past decade,
however, there are still issues to be resolved concerning solder reliability, the underlying
mechanisms of thermo-mechanical fatigue failure, fatigue life predictions
and the overall effect of decreasing component size, driven by the ongoing miniaturization
trend. This thesis aims to scientifically contribute to this subject by a coupled
experimental-numerical approach."
[permalink]
|
| |
|
Average Rating: 10.0 (1 vote)
|
|
|
| |
|
THICKPLT
|
| |
Bram Weisman (SBM-IMODCO)
|
| |
"Plots shell element thickness by utilizing surface pressures. I recommend plotting nodes with a contour or outline plot of pressure for best results. Element plot can also be used, but pressure colors will conflict with element colors."
[permalink]
|
| |
|
Average Rating: 8.3 (3 votes)
|
|
|
| |
|
THICPLOT
|
| |
Bill Newland (Bell Helicopter)
|
| |
"This macro assigns pressures based on real constant thickness values of shell elements. The shell elements are then plotted with pressure contours having the same values as the thicknesses."
"Select the desired shell elements to be plotted before running macro. After running macro, DO NOT SAVE. Exit without saving as erronious pressures will be applied to model."
[permalink]
|
| |
|
Average Rating: 10.0 (1 vote)
|
|
|
| |
|
THOPT
|
| |
THOPT, Option, ReformTol, nTabPoints, TempMin, TempMax
Uses fast thermal solver option, beta at 5.6, released at 5.7.
The link above refers to the outline of the usage of THOPT.
[permalink]
|
| |
|
| |
|
THREAD
|
| |
Ernst Hustedt (Air New Zealand Engineering)
|
| |
"For what it's worth, here is a macro I made some years ago ('94) for doing thread profiles for axisym analysis. Looking at it now, I am not sure if the UN thread option works correctly, I can't remember that I actually used it, but the ISO should be O.K. You can spin the profile along Don's helix."
[permalink]
|
| |
|
Average Rating: 10.0 (2 votes)
|
|
|
| |
|
Three Dimensional Turbulent-Incompressible Fluid Flow Analysis Of A Ranger QCT Control Valve
|
| |
Joseph W. Smith, Keith Black
|
| |
"Cashco, Inc., desired to determine whether or not a Computational Fluid Dynamic (CFD) model could accurately predict the fluid flow through a Ranger QCT Control Valve. ANSYS Revision 5.4 was used to create the finite element mesh, apply loads, solve, and evaluate the results of the fluid analysis. The results of the fluid analysis showed that ANSYS predicted the Flow Coefficient and Pressure Recovery Factor to within 10% and 2% of their experimental values, respectively." (Flotran) From 2000 Conference
[permalink]
|
| |
|
Average Rating: 9.4 (39 votes)
|
|
|
| |
|
Three-Dimensional Modeling Of A Bolted Connection
|
| |
David Johnson, Richard Englund, Brian McAnlis, Kevin Sari, and David Colombet
|
| |
"Two-dimensional, axisymmetric models are used to study the interaction and stresses developed in the threads of a bolted connection. One problematic issue with this approach is that the 2D model simulates the threads as separate rings of material, not as the actual continuous helix. Therefore, two-dimensional modeling cannot simulate the conditions of joint tightening and sliding along the helical thread flanks when the nut is turned. In addition, the analyst must justify the 2D axisymmetric assumption as appropriate to this truly three-dimensional system. This paper presents the modeling technique used to create a "mostly-brick" meshed 3D model of a nut and bolt joint."
[permalink]
|
| |
|
Average Rating: 9.6 (28 votes)
|
|
|
| |
|
Time-Dependent Material Modeling for Finite Element Analyses of Flip Chips
|
| |
Frank Feustel, Steffen Wiese, Ekkehard Meusel
|
| |
"Finite element analyses (FEA) have established as effective method for reliability assessment of flip chip assemblies. The simulation results are significantly dependent on the selected material models. Regarding flip chip assemblies, this statement mainly applies to the tin lead solder of the flip chip joints and the encapsulant – the so-called underfill.
Comprehensive material data of eutectic solder were determined on real flip chip joints by TU Dresden. Based on these data three modeling approaches were evaluated (target platform was the FEA code ANSYS): viscoplasticity (Anand's model), power law creep (with 2 terms) + plasticity, and sinh law creep + plasticity (as user defined model in ANSYS)."
[permalink]
|
| |
|
Average Rating: 9.3 (7 votes)
|
|
|
| |
|
Timestep for VOF analyses
|
| |
Sheldon Imaoka (CSI)
|
| |
Information on the volume-of-fluid (VOF) time steps in Flotran.
[permalink]
|
| |
|
Average Rating: 9.7 (15 votes)
|
|
|
| |
|
TINTP |
| |
TINTP,,,,,,,npoint,ntol
By default, automatic time-stepping will target 20 points/cycle. The undocumented fields are "npoints" points/cycle with a tolerance of +/- "ntol" points/cycle.
[permalink]
|
| |
|
Average Rating: 10.0 (1 vote)
|
|
|
| |
|
Tip on 4D and 5D Tables
|
| |
Sheldon Imaoka (ANSYS, Inc.)
|
| |
Simple tip on defining the indices for 4D and 5D tables (*DIM,,TAB4 and *DIM,,TAB5) using *TAXIS or manually by specifying the proper indices.
[permalink]
|
| |
|
Average Rating: 10.0 (3 votes)
|
|
|
| |
|
Tip on Changing /TITLE in the results file (.rst)
|
| |
Bram Weisman (SBM Atlantia)
|
| |
Tip on changing the title (/TITLE) in the ANSYS results file using the MODIFY command.
[permalink]
|
| |
|
Average Rating: 0.0 (1 vote)
|
|
|
| |
|
tlbrlist61.ans |
| |
Although undocumented, tlbrlist61.ans can be used to create customized toolbars. Copy this configuration file to your home or working directory. The contents of "tlbrlist61.ans" contain filenames, and these can be changed to point to different files.
The actual toolbar information is contained in ANSYSSTANDARD.TLB (icon toolbar) and ANSYSABBR.TLB (abbreviation toolbar). These can be copied and modified to suit one's needs, although one should know some Tcl/Tk and ANSYS to do this.
[permalink]
|
| |
|
Average Rating: 3.3 (3 votes)
|
|
|
| |
|
TLSPRM |
| |
Macro performs s-parameter extraction for transmission line (HF Emag). Available in 6.1 in "docu" directory as a macro - see contents of macro file for usage.
[permalink]
|
| |
|
Average Rating: 10.0 (4 votes)
|
|
|
| |
|
TOGIF
|
| |
Charles Wong (Goodrich Corporation)
|
| |
"I have a macro that creates small high resolution GIF files for Windows only. It calls out a shareware program pvw32con.exe. GIF's are much smaller and higher quality than tiff or jpeg."
[permalink]
|
| |
|
Average Rating: 7.2 (9 votes)
|
|
|
| |
|
Tooling up for Micro Electro Mechanical Systems [PDF]
|
| |
Dale Ostergaard
|
| |
(from ANSYS Solutions magazine, volume 2, #1) (MEMS)
[permalink]
|
| |
|
Average Rating: 10.0 (4 votes)
|
|
|
| |
|
Topology Optimization in ANSYS
|
| |
Brian King (IMPACT Engineering Solutions, Inc.)
|
| |
Presentation from Midwest ANSYS User Group on Topological Optimization capability in ANSYS and Workbench Simulation.
[permalink]
|
| |
|
Average Rating: 5.0 (4 votes)
|
|
|
| |
|
TORSION3
|
| |
Deepak Ganjoo (ANSYS, Inc.)
|
| |
Example of ALE, squeeze-film damping calculations. Requires associated macros MVCONN and BOXMOVE.
[permalink]
|
| |
|
Average Rating: 8.5 (17 votes)
|
|
|
| |
|
Towards Automated Determination of USERMAT for the Nonlinear Constitutive Behavior of Composites
|
| |
J. Michopoulos, P. Mast, R. Badaliance, L. Gause, T. Chwastyk, R. Foerch
|
| |
"Recent advances in finite element techniques and design optimization integration technologies along with the parallel hardware and software evolution have directed the CMS group to turn its attention to utilizing "of the shelf" technology of achieving the same goals. Thus, the "Z-mat" and "Z-Optim" packages from Northwest Numerics, Inc., have been utilized to extract the non-linear constitutive response from the available experimental data in an integrated and automated manner and in conjunction with the ANSYS/Mechanical infrastructure. The automation lies on the fact that the process automatically generates the code of a "USERMAT" subroutine that it can be subsequently used with any geometry and loading specification definable within the limits of ANSYS' non-linear element library. The geometry of the single notched specimen of NRL's In Plane has been used for developing and verifying the process."
[permalink]
|
| |
|
Average Rating: 7.5 (8 votes)
|
|
|
| |
|
TR_LMM_ACC_MSPT
|
| |
David Haberman (CSI)
|
| |
Structural Transient
Modal Superposition
Large Mass Method
Acceleration vs. Time Acceleration:f=ma
[permalink]
|
| |
|
Average Rating: 8.2 (19 votes)
|
|
|
| |
|
TR_LMM_ACC_MSPT_2
|
| |
David Haberman (CSI)
|
| |
Structural Transient
Pre-Stressed Modal Superposition
Large Mass Method
Acceleration vs. Time Acceleration:f=ma
[permalink]
|
| |
|
Average Rating: 10.0 (9 votes)
|
|
|
| |
|
TR_LMM_ACC_MSPT_SIN
|
| |
David Haberman (CSI)
|
| |
Example of a transient modal supperposition
Large mass method applying acceleration vs. time
1/2 sine wave with 75 g peak over .006 sec
[permalink]
|
| |
|
Average Rating: 9.4 (16 votes)
|
|
|
| |
|
TR_LSM_EL_MSPT
|
| |
David Haberman (CSI)
|
| |
Structural Transient, mode superposition method
Element pressure vs. Time
[permalink]
|
| |
|
Average Rating: 9.3 (7 votes)
|
|
|
| |
|
TR_LSM_F_MSPT
|
| |
David Haberman (CSI)
|
| |
Structural Transient, mode superposition method
Nodal forces vs. Time
[permalink]
|
| |
|
Average Rating: 10.0 (8 votes)
|
|
|
| |
|
TR_LSM_PRESS_FT
|
| |
David Haberman (CSI)
|
| |
Structural Transient, full method
Element pressure vs. Time applied as load steps
[permalink]
|
| |
|
Average Rating: 10.0 (11 votes)
|
|
|
| |
|
TR_TB_PRESS_FT
|
| |
David Haberman (CSI)
|
| |
Structural Transient, full method
Element pressure vs. Time applied as tabular load
[permalink]
|
| |
|
Average Rating: 9.3 (35 votes)
|
|
|
| |
|
Transient Behavior of a Polymer Fill Material with Time Dependent Viscoelastic Properties
|
| |
John Thompson, Steven Groothuis, Hong Tang, Paul Koeneman
|
| |
"In an effort to simplify the implementation of viscoelastic material models into ANSYS, an ANSYS User-Programmable Feature (UsrFictive) has been modified to allow a more practical definition of viscoelastic material parameters. Standard ANSYS input of material data may be based upon temperature. Currently, ANSYS material data may not be a function of any other parameter. Many polymers used in industry are initially liquid and must be “cured” in a manufacturing process. This fact means that the properties will change over time. This application demonstrates one method of implementing a curing process simulation for a viscoelastic polymer."
[ANSYS Nonlinear, version 6.?]
[permalink]
|
| |
|
| |
|
Transient Thermal Analysis of Spot Welding Electrodes
|
| |
K. S. Yeung, P. H. Thornton
|
| |
"The accurate thermal simulation of a spot welding electrode cap could permit critical design parameters to be identified for improved electrode life. In this study, a parametric model has been developed to predict the transient thermal behavior of a typical spot welding electrode cap. The model employs the technique of conjugate heat transfer analysis to avoid the problem of estimating a value for the heat transfer coefficient that arises with conventional heat transfer analysis."
[permalink]
|
| |
|
Average Rating: 8.1 (27 votes)
|
|
|
| |
|
TRANSIENT2
|
| |
Thomas Jin-Chee Liu (National Cheng Kung University)
|
| |
Example input of thermal transient analysis with moving heat source.
[permalink]
|
| |
|
Average Rating: 9.1 (92 votes)
|
|
|
| |
|
Transmission of Mechanical Stresses within the Cytoskeleton of Adherent Cells: a Theoretical Analysis Based on a Multi-Component Cell Model
|
| |
Philippe Tracqui and Jacques Ohayon
|
| |
"We investigate here the spatial distributions of intracellular stresses when
adherent cells are probed by magnetic twisting cytometry. The influence of the cell nucleus
stiffness on the simulated nonlinear torque-bead rotation response is analyzed by considering a
finite element multi-component cell model in which the cell and its nucleus are considered as
different hyperelastic materials. We additionally take into account the mechanical properties of
the basal cell cortex, which can be affected by the interaction of the basal cell membrane with
the extracellular substrate. In agreement with data obtained on epithelial cells, the simulated
behaviour of the cell model relates the hyperelastic response observed at the entire cell scale to
the distribution of stresses and strains within the nucleus and the cytoskeleton, up to cell
adhesion areas. These results, which indicate how mechanical forces are transmitted at distant
points through the cytoskeleton, are compared to recent data imaging the highly localized
distribution of intracellular stresses."
[ANSYS Nonlinear, version 6.0]
[permalink]
|
| |
|
Average Rating: 5.0 (2 votes)
|
|
|
| |
|
TRIM1
|
| |
G.N.S. Prakash
|
| |
Macro entry for "APDL Guru" contest by PADT.
"Here is the scenario. I have a number of straight lines in the XY plane. I would like a macro that does the following:
- Allows me to select any two lines, but only two.
- If the two lines intersect, they are both divided at the intersection point and the resulting four lines are connected such that they share a common keypoint at the intersection point.
- If the lines do not intersect, the first line is extended until it is tangent to the second line.
The macro should be capable of handling the special case in which the second line needs to be extended in order for intersection to occur. If this case should occur, the macro should extend both lines to a common intersection point and then join the two lines together. However, if the second line does not require extension, then the macro should divide the second line at the intersection point and join the two pieces of the original second line together with the first line, which has been extended."
[permalink]
|
| |
|
Average Rating: 6.0 (5 votes)
|
|
|
| |
|
TRIM2
|
| |
Vlad Suprunov
|
| |
Macro entry for "APDL Guru" contest by PADT.
"Here is the scenario. I have a number of straight lines in the XY plane. I would like a macro that does the following:
- Allows me to select any two lines, but only two.
- If the two lines intersect, they are both divided at the intersection point and the resulting four lines are connected such that they share a common keypoint at the intersection point.
- If the lines do not intersect, the first line is extended until it is tangent to the second line.
The macro should be capable of handling the special case in which the second line needs to be extended in order for intersection to occur. If this case should occur, the macro should extend both lines to a common intersection point and then join the two lines together. However, if the second line does not require extension, then the macro should divide the second line at the intersection point and join the two pieces of the original second line together with the first line, which has been extended."
[permalink]
|
| |
|
Average Rating: 6.7 (3 votes)
|
|
|
| |
|
TRIM3
|
| |
Charles Wong
|
| |
Macro entry for "APDL Guru" contest by PADT.
"Here is the scenario. I have a number of straight lines in the XY plane. I would like a macro that does the following:
- Allows me to select any two lines, but only two.
- If the two lines intersect, they are both divided at the intersection point and the resulting four lines are connected such that they share a common keypoint at the intersection point.
- If the lines do not intersect, the first line is extended until it is tangent to the second line.
The macro should be capable of handling the special case in which the second line needs to be extended in order for intersection to occur. If this case should occur, the macro should extend both lines to a common intersection point and then join the two lines together. However, if the second line does not require extension, then the macro should divide the second line at the intersection point and join the two pieces of the original second line together with the first line, which has been extended."
[permalink]
|
| |
|
Average Rating: 10.0 (2 votes)
|
|
|
| |
|
TRIM4
|
| |
Navaneeth Bashyam
|
| |
Macro entry for "APDL Guru" contest by PADT.
"Here is the scenario. I have a number of straight lines in the XY plane. I would like a macro that does the following:
- Allows me to select any two lines, but only two.
- If the two lines intersect, they are both divided at the intersection point and the resulting four lines are connected such that they share a common keypoint at the intersection point.
- If the lines do not intersect, the first line is extended until it is tangent to the second line.
The macro should be capable of handling the special case in which the second line needs to be extended in order for intersection to occur. If this case should occur, the macro should extend both lines to a common intersection point and then join the two lines together. However, if the second line does not require extension, then the macro should divide the second line at the intersection point and join the two pieces of the original second line together with the first line, which has been extended."This macro won the above contest.
[permalink]
|
| |
|
Average Rating: 10.0 (2 votes)
|
|
|
| |
|
TRIM5
|
| |
Rod Scholl & Jeff Strain (PADT)
|
| |
Macro entry for "APDL Guru" contest by PADT.
"Here is the scenario. I have a number of straight lines in the XY plane. I would like a macro that does the following:
- Allows me to select any two lines, but only two.
- If the two lines intersect, they are both divided at the intersection point and the resulting four lines are connected such that they share a common keypoint at the intersection point.
- If the lines do not intersect, the first line is extended until it is tangent to the second line.
The macro should be capable of handling the special case in which the second line needs to be extended in order for intersection to occur. If this case should occur, the macro should extend both lines to a common intersection point and then join the two lines together. However, if the second line does not require extension, then the macro should divide the second line at the intersection point and join the two pieces of the original second line together with the first line, which has been extended."
[permalink]
|
| |
|
Average Rating: 3.3 (3 votes)
|
|
|
| |
|
TRNOPT |
| |
TRNOPT, Method, MAXMODE, Dmpkey, MINMODE, MCout
The MCout argument is undocumented, where it can take the values of "yes" or "no" (default). It writes out modal coordinates in an external text file called "jobname.mcf" for mode-superposition method.
[STI: from release 7.0 and above]
[permalink]
|
| |
|
Average Rating: 10.0 (4 votes)
|
|
|
| |
|
TRQ_MSP
|
| |
Bill Bulat (CSI)
|
| |
Used to calculate torque about global Z axis for 3D MSP analyses.
[permalink]
|
| |
|
Average Rating: 10.0 (5 votes)
|
|
|
| |
|
Turning off gradient background |
| |
Sheldon Imaoka (ANSYS, Inc.)
|
| |
Use of the command "/COLOR,PBAK,OFF" will turn off the default gradient blue background and use black instead. ("Utility Menu > PlotCtrls > Style > Background > Display Picture Background") However, you can add "/UIS,PBAK,OFF" in your start6x.ans file to use the black backgorund every time you start up ANSYS. (The reason why the command is /UIS rather than /COLOR is because the latter assumes that the GUI is already up, but /UIS is a configuration command which can be used before the ANSYS GUI is started.)
[permalink]
|
| |
|
| |
|
TV Panel Glass Forming and Annealing Process Model
|
| |
John Chumley
|
| |
"This article describes the modeling technique used in forming a TV glass panel from the formation of the droplet of molten glass (gob) delivered to the forming machine (ELP) through the pressing and cooling operations plus the annealing oven (lehr). To assure the continuity of the solution, the model also tracks the return of the empty mold parts to their initial position on the ELP. The complexity of the problem and variety of solution domains involved requires multiple solution techniques."
(VISCO89 and Flotran FLUID142)
[permalink]
|
| |
|
Average Rating: 10.0 (12 votes)
|
|
|
| |
|
Underfill Constraint Effects during Thermo-Mechanical Cycling of Flip Chip Solder Joints
|
| |
I. Dutta, A. Gopinath, and C. Marshall
|
| |
"The presence of an 'underfill' encapsulant between a micro-electronic device and the underlying substrate is known to substantially improve the thermal fatigue life of flip-chip solder joints, primarily due to load-transfer from the solder to the encapsulant. In this study, a new single joint-shear (SJS) test, which allows the measurement of the strain response of an individual solder ball during thermo-mechanical cycling (TMC), has been utilized to investigate the impact of the constraint imposed by the underfill on a solder-joint. Finite element modeling has been utilized to demonstrate that the SJS sample geometry captures most of the deformation characteristics of a flip-chip joint, and to provide insight into the experimental observations."
[permalink]
|
| |
|
Average Rating: 10.0 (4 votes)
|
|
|
| |
|
Understanding Accuracy and Discretization Error in an FEA Model
|
| |
Jon Pointer
|
| |
"The often-ignored topic of mesh discretization error is examined to identify a simple set of rules that the
average user can enlist to determine solution accuracy. The sources of discretization error are explained,
tools to quantify it are introduced and an example is given. The purpose is to bring an understanding of
these issues and usable tools to the common user who is not proficient in the mathematical basis of FEA."
[ANSYS 7.1, 2004 Conference]
[permalink]
|
| |
|
Average Rating: 10.0 (4 votes)
|
|
|
| |
|
Understanding Lagrange Multipliers [PDF]
|
| |
Sheldon Imaoka (ANSYS, Inc.)
|
| |
"Lagrange multipliers are a general term used in different areas of ANSYS, specifically contact and element formulation. This memo hopes to provide the user with a simplified introduction to the most important concepts in using elements with Lagrange multipliers, in hopes that some of the element options and solver selection can be better understood.
Currently, at ANSYS 6.0, the node-to-node gap element CONTA178 and the Mixed U-P formulation of the 18x elements (i.e., KEYOPT(6)>0) utilize Lagrange multipliers, so the discussion will focus on these elements."
(Week 7, week of 11/05/01.)
[permalink]
|
| |
|
Average Rating: 8.4 (16 votes)
|
|
|
| |
|
Understanding the Response Surface Method in DesignXplorer [PDF]
|
| |
Sheldon Imaoka (ANSYS, Inc.)
|
| |
"ANSYS DesignXplorer enables the user to perform optimization studies based on multiple objectives, to account for uncertainties in product design and use, and to determine how best to improve product reliability. These tasks are accomplished through the use of response surfaces, and this memo hopes to cover some of the basics of DesignXplorer operation."
(Week 32, week of 12/18/05.)
[permalink]
|
| |
|
Average Rating: 10.0 (9 votes)
|
|
|
| |
|
Undocumented Hyperelastic Material Models at 5.7-6.1 [ZIP]
|
| |
Sheldon Imaoka (ANSYS, Inc.)
|
| |
"From 5.7, the 18x series of elements support a variety of hyperelastic constitutive models, namely general polynomial, Mooney-Rivlin, Neo-Hookean, Arruda-Boyce, and Ogden. Four other models have been included in 5.7 onwards, although these are undocumented options for TB,HYPER. These four models consist of the Yeoh and Gent models for incompressible behavior and the Hyperfoam and Blatz-Ko options for compressible rubbers. This memo hopes to provide a summary of these material models and of the required input."
(Week 18, week of 03/11/02.)
[permalink]
|
| |
|
Average Rating: 8.0 (20 votes)
|
|
|
| |
|
Uniaxial and biaxial ratchetting in piping materials - experiments and analysis
|
| |
S.C. Kulkarni, Y.M. Desai, T. Kanta, G.R. Reddy, P. Prasad, K.K. Vaze, C. Gupta
|
| |
"The performance of the Chaboche kinematic hardening model has been evaluated in this paper to predict the ratchetting responses for a
broad set of uniaxial and biaxial loading histories. The investigations have been performed with reference to both uniaxial and biaxial
experimental data, viz. (a) strain and stress controlled uniaxial tests on tensile specimens; (b) biaxial tests on straight pipes with constant
internal pressure and cyclic bending load; and (c) a shake table test on elbow. The parameters of the Chaboche model have been calculated
from the uniaxial strain controlled stable hysteresis loop. Amongst the various parameters in the Chaboche model, it has been found that the
selection of the value of g3 plays a crucial role in achieving better simulation. The Chaboche model was observed to predict complete
shakedown for g3 ¼ 0: On the other hand, the model closely simulated the experimental results for g3 ¼ 9: The same parameters have been
used to analyze the biaxial loading condition. Ratchetting simulation studies by the Chaboche model have resulted in reasonably good
agreement with experiments."
[permalink]
|
| |
|
Average Rating: 10.0 (5 votes)
|
|
|
| |
|
Unofficial History of ANSYS
|
| |
Shen-Yeh Chen (Honeywell)
|
| |
This is an unofficial history of Dr. Swanson and ANSYS.
[permalink]
|
| |
|
Average Rating: 7.1 (19 votes)
|
|
|
| |
|
Unsymmetric MATRIX27
|
| |
Sheldon Imaoka (ANSYS, Inc.)
|
| |
There have been changes between ANSYS 10.0 and 11.0 regarding MATRIX27 unsymmetric input via real constants. This describes the change and provides a visual representation of the matrix input.
[permalink]
|
| |
|
Average Rating: 10.0 (2 votes)
|
|
|
| |
|
Use Of Finite Element Analysis To Simulate The Hyperelastic Behaviour Of Cardiovascular Tissue [PDF]
|
| |
S. Daly, P.J. Prendergast, F. Dolan, T.C. Lee
|
| |
Examination of Mooney-Rivlin.
[permalink]
|
| |
|
Average Rating: 8.1 (8 votes)
|
|
|
| |
|
User Implemented Nitinol Material Model in ANSYS
|
| |
Peter R. Barrett and Daniel Fridline
|
| |
"Nitinol is an acronym for NIckel TItanium Naval Ordinance Laboratory since the alloy was originally
developed at the Naval Lab. It is used to describe a family of materials, which contain a nearly equal
mixture of nickel and titanium. Nitinol alloys are attractive to the medical device industry because they are
biocompatible and when processed correctly, are at their optimum superelastic behavior at body
temperature.
"Nitinol exhibits a different stress-strain curve for loading and unloading that cannot be modeled with
existing material models in ANSYS. This paper describes the implementation of a unique user material
model in ANSYS that simulates the nitinol superelastic behavior. Example analyses are provided
demonstrating the application of this material model for medical implant devices called stents."
[ANSYS Nonlinear, version unspecified]
Note that TB,SMA allows users to access built-in shape memory alloy constitutive model in ANSYS.
[permalink]
|
| |
|
Average Rating: 7.5 (2 votes)
|
|
|
| |
|
User_Fatigue_PNEN13445-3
|
| |
Przemyslaw Siedlaczek (MESco)
|
| |
Workbench macro solves fatigue according to pressure vessel code PN EN 13445-3 and displays results as a User Defined Result.
[permalink]
|
| |
|
Average Rating: 10.0 (6 votes)
|
|
|
| |
|
User-Defined Creep Laws with USERCREEP [ZIP]
|
| |
Sheldon Imaoka (ANSYS, Inc.)
|
| |
"ANSYS provides 13 creep equations for use with implicit creep – these range from
the simple Norton law to the hyperbolic sine form to the Blackburn model to a rational
polynomial expression, to name a few – that can be used to model a range of creep
behavior for metals. The TBFT command provides curve-fitting functionality for the user
wishing to evaluate creep material parameters from test data. Also, the user can model
anisotropic creep as well as combine implicit creep with rate-independent plasticity to
model a wide range of complex material response.
Despite this wealth of features, however, one may wish to incorporate one’s own
creep law into ANSYS. For example, a company may have their own creep equation
with material parameters already defined and validated through testing. The built-in
creep laws in ANSYS assume creep used in design rather than failure analysis, so the
available creep laws are meant to model primary and secondary creep – consequently,
another need to incorporate a user-defined creep law would arise when a user wants to
include tertiary creep and/or to evaluate creep damage.
This memo will hope to address some aspects of writing one’s own user-defined
creep law with the USERCREEP.F subroutine to address this issue."
Example using Anand's model.
(Week 40, week of 10/07/07)
[permalink]
|
| |
|
Average Rating: 9.7 (18 votes)
|
|
|
| |
|
User-Defined Failure Criteria with USERFC [ZIP]
|
| |
Sheldon Imaoka (ANSYS, Inc.)
|
| |
"The FC command provides users with the ability to predict first-ply failure
using maximum strain, maximum stress, or Tsai-wu failure criteria. In
ANSYS 12.0.1, users can also take advantage of the userfc subroutine to
define up to nine different criteria.
This memo reviews the userfc subroutine, and a sample implementation
of the Hashin criterion is included."
(Week 54, week of 10/11/09)
[permalink]
|
| |
|
Average Rating: 9.5 (11 votes)
|
|
|
| |
|
User-Defined Hyperelasticity with USERHYPER [ZIP]
|
| |
Sheldon Imaoka (ANSYS, Inc.)
|
| |
"User-Programmable Features (UPFs) are an extremely useful feature for analysts that need
additional advanced functionality, especially in the area of constitutive modeling.
TB,HYPER allows users to include many incompressible and compressible hyperelastic
material behavior – Ogden, Arruda-Boyce, Gent, Yeoh, Blatz-Ko are but some of the
available models. However, for those wishing to use a customized strain energy function,
the USERHYPER.F subroutine is available."
(Week 39, week of 09/30/07.)
[permalink]
|
| |
|
Average Rating: 10.0 (4 votes)
|
|
|
| |
|
User-Defined Output with USEROUT.F [ZIP]
|
| |
Sheldon Imaoka (ANSYS, Inc.)
|
| |
"There are various situations where a user may wish to define specific type
of output to postprocess — this can range from simple evaluation of safety
factors to more involved damage calculations. While APDL, the ANSYS
command language, allows users to manipulate results in any manner one
sees fit, user-programmable features (UPFs) also provide a means for users
to calculate specific output results efficiently at the solution level."
Example of calculating fatigue and Cap (Extended Drucker-Prager) output.
(Week 48, week of 06/01/08)
[permalink]
|
| |
|
Average Rating: 10.0 (7 votes)
|
|
|
| |
|
USER01
|
| |
Sheldon Imaoka (ANSYS, Inc.)
|
| |
Very simple example showing use of user-defined command (USER01).
This UPF command simply reads and interpolates a defined table array. Use of the parevl() is also shown in this simple input.
[permalink]
|
| |
|
Average Rating: 10.0 (5 votes)
|
|
|
| |
|
USERELEMENT
|
| |
Roger Young (Industrial Research Ltd.)
|
| |
"This package contains a number of examples
of the Ansys user element <uel> which may
be further adapted for personal use. The
examples given here are for a 4-node planar
element USER101 with linear shape functions
similar to the Ansys element PLANE42. However
USER101 may easily be extended to a 3D 8-node
element and/or to quadratic shape functions
by changing the specifications in lib/PAR.NML.
In addition there is a simple extension to
general large strain non-linear deformation
which is illustrated in uel3/ex2."
[permalink]
|
| |
|
Average Rating: 1.7 (3 votes)
|
|
|
| |
|
USERMAT
|
| |
Document describing the USERMAT user material subroutine.
[permalink]
|
| |
|
Average Rating: 9.3 (46 votes)
|
|
|
| |
|
Using a Heat Transfer Analogy to Solve for Squeeze Film Damping and Stiffness Coefficients in MEMS Structures
|
| |
Dale Ostergaard, Jan Mehner
|
| |
This paper provides background information on using a heat transfer analogy to solve the Reynolds equation (squeeze film damping). Although ANSYS now has FLUID136 and FLUID138 to solve such problems, this paper can be useful in gaining a better understanding of these types of analyses.
[permalink]
|
| |
|
Average Rating: 10.0 (6 votes)
|
|
|
| |
|
Using Abbreviations to Customize the Toolbar [PDF]
|
| |
Sheldon Imaoka (ANSYS, Inc.)
|
| |
"The ANSYS Toolbar provides a useful means of accessing commonly-used functions, especially for users who use the GUI rather than typing in commands."
"This memo hopes to provide a brief introduction to the ANSYS Toolbar and, more importantly, how to assign macros or specific dialog boxes to the Toolbar buttons, including Fnc_ UIDL granules or ~eui Tcl/Tk dialog boxes."
(Week 3, week of 10/08/01.)
[permalink]
|
| |
|
Average Rating: 9.6 (12 votes)
|
|
|
| |
|
Using ANSYS-Based Aluminum Reduction Cell Energy Balance Models to Assist Efforts to Increase Lauralco's Smelter Productivity
|
| |
Marc Dupuis and Claude Fradet
|
| |
"State of the art ANSYS-based aluminum reduction cell energy balance models have been successfully used to assist efforts to increase Lauralco's smelter productivity by improving cell thermo-electric design."
From 1998 Conference
PDF version here
[permalink]
|
| |
|
Average Rating: 8.1 (8 votes)
|
|
|
| |
|
Using Birth and Death with Multiframe Restart
|
| |
Odd Einar Lindøe (Imenco Engineering)
|
| |
Tips on using element birth and death (EKILL/EALIVE) with multiframe restart (RESCONTROL). By default, one cannot use birth and death with multiframe restart since the .rdb file is resumed (and the latest information is in .db, not .rdb). This tip shows some methods of using birth and death with multiframe restart.
[permalink]
|
| |
|
Average Rating: 9.3 (15 votes)
|
|
|
| |
|
Using CMS in Workbench Simulation [ZIP]
|
| |
Sheldon Imaoka (ANSYS, Inc.)
|
| |
"At Workbench 11.0, the ANSYS Rigid Dynamics add-on module enables users to model complex kinematic assemblies, whereby system-level performance as well as accurate force loading on components can be obtained.
Although the parts in the assembly may initially be considered rigid, an interesting, related method is the use of component mode synthesis (CMS) to account for the flexibility of parts. This memo will attempt to cover a way in which users can incorporate CMS in their multibody analyses in Workbench Simulation."
[For version 12.0, use supplied "cms_use_v12.mac" instead of "cms_use.mac" - courtesy of D. Creech.]
(Week 37, week of 05/27/07.)
[permalink]
|
| |
|
Average Rating: 9.8 (28 votes)
|
|
|
| |
|
Using FTP/SFTP to Transfer Files
|
| |
Sheldon Imaoka (ANSYS, Inc.)
|
| |
There are many cases where you may need to transfer files outside of your company. FTP (and SFTP) is a popular mechanism to transfer large files — for big ANSYS models, the files can be quite huge — and here are some details on using FTP/SFTP.
[permalink]
|
| |
|
| |
|
Using PSOLVE [ZIP]
|
| |
Sheldon Imaoka (ANSYS, Inc.)
|
| |
Although most often used for large-deflection prestressed modal analyses, PSOLVE has other applications which make it attractive to use, especially for large models.
PSOLVE can be used for the following situations:
- Precise mass calculations
- Detailed listing of contact pair information
- Evaluation of tabular boundary conditions and loads
Since PSOLVE is a partial solution (namely, calculation of element matrices), it is usually much faster than performing an actual solution. Hence, the user may obtain any (or all) of the above three types of information prior to running an actual analysis, which can be a valuable way of verifying model input and settings prior to solution.
(Week 20, week of 07/14/02.)
[permalink]
|
| |
|
Average Rating: 8.1 (21 votes)
|
|
|
| |
|
Using RCP/SCP to Transfer Files
|
| |
Sheldon Imaoka (ANSYS, Inc.)
|
| |
Besides FTP, one can also use RCP or SCP to copy files between computers. This is an easier method that is well-suited for copying files on an internal network, especially if you were using a Windows PC for pre- and post-processing but solving remotely on a UNIX or Linux server/cluster.
[permalink]
|
| |
|
| |
|
Using the Radiosity Solver in Workbench Simulation [PDF]
|
| |
Sheldon Imaoka (ANSYS, Inc.)
|
| |
Please note that in Workbench Mechanical 12.1, surface-to-surface radiation (using the Radiosity Solution Method) has been introduced in the GUI, so this memo is obsolete if you use version 12.1 and higher.
"Radiation can play an important role in heat transfer analyses. In Workbench
Simulation 10.0, a “Radiation” load has been added to allow users to account for losses to
the surroundings, although this does not include radiation exchange between surfaces.
For users wishing to utilize the ANSYS surface-to-surface radiation capabilities, this
memo hopes to introduce an easy method to include these effects within Workbench
Simulation via Named Selections and Command objects.
This type of methodology can be extended to include any other advanced solution
feature of ANSYS which the user may wish to incorporate inside of Workbench
Simulation."
(Week 35, week of 11/05/06.)
[permalink]
|
| |
|
Average Rating: 9.1 (23 votes)
|
|
|
| |
|
Using the WB Simulation Remote Solution Manager [PDF]
|
| |
Sheldon Imaoka (ANSYS, Inc.)
|
| |
"Workbench Simulation has the ability to allow the user to solve multiple jobs locally or
remotely. These capabilities are defined within the “Solution” branch of WB Simulation as well as in the WB Remote Solution Manager.
"This memo hopes to introduce this capability, especially with regards to solving multiple jobs locally on a Windows machine."
(Week 33, week of 04/02/06.)
[permalink]
|
| |
|
Average Rating: 7.5 (10 votes)
|
|
|
| |
|
Using Windows file extension association for ANSYS files
|
| |
Sheldon Imaoka (CSI)
|
| |
How to associate jobname.db files with ANSYS under Windows, so one can double-click on them to launch ANSYS. (From XANSYS posting)
[permalink]
|
| |
|
Average Rating: 10.0 (2 votes)
|
|
|
| |
|
UVBREFRESH |
| |
UVBREFRESH updates the Main Menu (UIDL).
First, set the environment variable UIDLVB to 1. It can be set in your .cshrc file with "setenv UIDLVB 1".
In ANSYS, at the BEGIN level, type UVBREFRESH to re-index and re-read the granule files. Note that this doesn't work with the root menu MenuRoot.
[permalink]
|
| |
|
Average Rating: 10.0 (2 votes)
|
|
|
| |
|
V_BY_2A
|
| |
Michael W. Hiller (In2 Solutions, Inc.)
|
| |
Creates a volume by picking two opposed areas. From the author:
"It was meant for the case where you have two opposite areas each area having 4 lines (4 keypoints). It will automate volume creation from 2 areas, or you can modify it as necessary. It includes logic to (try to) avoid unnecessary twisting (bowtie)."
[permalink]
|
| |
|
Average Rating: 10.0 (4 votes)
|
|
|
| |
|
V2COMET
|
| |
Fern Thomassy (Southwest Research Institute)
|
| |
Creates a COMET/Acoustics results file of velocity results.
[permalink]
|
| |
|
Average Rating: 10.0 (1 vote)
|
|
|
| |
|
V2GLUE
|
| |
Eric Miller (PADT)
|
| |
Work around for standard VGLUE that avoids the "ungluing" that can occur
[permalink]
|
| |
|
Average Rating: 10.0 (7 votes)
|
|
|
| |
|
Validation of a General Fatigue Life Prediction Methodology for Sn-Ag-Cu Lead-Free Solder Alloy Interconnects
|
| |
David M. Pierce, Sheri D. Sheppard, Paul T. Vianco, Jerome A. Regent, J. Mark Grazier
|
| |
"A general fatigue life prediction methodology, based on a unified creep plasticity damage
(UCPD) model, was developed for predicting fatigue cracks in 95.5Sn-3.9Ag-0.6Cu
(wt %) solder interconnects. The methodology was developed from isothermal fatigue
tests using a double-lap-shear specimen. Finite element analysis model geometries, mesh
densities, and assumptions were detailed for both a full model (an octant-symmetry slice
of the entire ball grid array (BGA) assembly) and a submodel (the solder joint deemed
most likely to fail and the surrounding package layers) to facilitate fatigue prediction.
Model validation was based on the thermal mechanical fatigue of plastic BGA solder
joints (250-4000 thermal cycles, -55°C to 125°C, and 10°C/min). Metallographic
cross sections were used to quantitatively measure crack development. The methodology
generally underpredicted the crack lengths but, nonetheless, captured the measured crack
lengths within a +-2X error band. Possible shortcomings in the methodology, including
inaccurate materials properties and part geometries, as well as computational techniques,
are discussed in terms of improving both the UCPD constitutive model and the
fatigue life prediction methodology fidelity and decreasing the solution time."
[permalink]
|
| |
|
Average Rating: 10.0 (2 votes)
|
|
|
| |
|
Various MEMS Examples Using ANSYS [ZIP]
|
| |
(EPFL, The Swiss Federal Institute of Technology Lausanne)
|
| |
Tutorials on using ANSYS with various MEMS examples. This was originally taken from EPFL's website.
[permalink]
|
| |
|
Average Rating: 9.3 (28 votes)
|
|
|
| |
|
VARTHK
|
| |
(CAEAI)
|
| |
"This macro applies a varying shell thickness based on a given function."
[permalink]
|
| |
|
Average Rating: 10.0 (3 votes)
|
|
|
| |
|
Vector operations and commands [PDF]
|
| |
Sheldon Imaoka (CSI)
|
| |
Vector notation/functions in ANSYS allow the user to execute some of these *DO loops in a much more efficient manner. Instead of looping through individual functions, vector functions act upon arrays, resulting in faster execution times. This memo will provide some basic/introductory examples on the use of *VGET as well as the undocumented vector notation.
HTML Version here.
Accompanying input file, BUILDN1 macro, and BUILDN2 macro.
In the memo, in Section 2, please note that there is a typo. The section with the following lines:
*vget,NARRAY(1,1),node,1,u,x
*vmask,NMASK(1)
*vget,NARRAY(1,2),node,2,u,y
*vmask,NMASK(1)
*vget,NARRAY(1,3),node,3,u,z
should be replaced as follows:
*vget,NARRAY(1,1),node,1,u,x
*vmask,NMASK(1)
*vget,NARRAY(1,2),node,1,u,y
*vmask,NMASK(1)
*vget,NARRAY(1,3),node,1,u,z
[permalink]
|
| |
|
Average Rating: 8.2 (14 votes)
|
|
|
| |
|
VectorRotation
|
| |
Bob Weathers (Trane)
|
| |
"These macros rotate a matrix of vectors from one set of Euler angles to another. One macro creates the rotation matrix and a second does the rotation. To test the macros, a pressurized cylinder (or optionally a sphere) is built, meshed, and solved in 6 different coordinate systems. To check accuracy, results are rotated from one CSYS to another by the macros and then compared to ANSYS. Set your text editor's tab stops to 2 for macro readability."
In the zip file, "zTestRotationVector.mac" is the test model macro, and "zRotateVector.mac" is the main macro to rotate vectors.
Update 02/07/2009: correction to zRotateVector.mac provided by David Creech.
[permalink]
|
| |
|
Average Rating: 5.7 (7 votes)
|
|
|
| |
|
Verifying file integrity
|
| |
Sheldon Imaoka (ANSYS, Inc.)
|
| |
When sending large files (such as ANSYS database and result files) from one company to another (such as via ftp or sftp), ensuring that the file transferred correctly and that the file indeed came from the expected person can be important. Use of checksum programs such as cksum, md5sum, and sha1sum can be used to verify the file's integrity. GNU Privacy Guard (gpg) can not only perform a checksum but also include a PGP 'signature' to help validate the authenticity of the file as well.
[permalink]
|
| |
|
| |
|
VERT
|
| |
Rod Scholl (PADT)
|
| |
Generates a big long vertical line at specified location
[permalink]
|
| |
|
Average Rating: 10.0 (2 votes)
|
|
|
| |
|
VEXT |
| |
VEXT,NA1,NA2,NINC,DX,DY,DZ,RX,RY,RZ,spacing_ratio
Specifies spacing ratio in volume extrusion direction with "spacing_ratio" value. Specify number of divisions in extrusion direction with ESIZE,,ndiv.
[permalink]
|
| |
|
Average Rating: 10.0 (2 votes)
|
|
|
| |
|
VFOPT |
| |
VFOPT,none
Usually, radiosity solution method writes viewfactor file (jobname.vf) to disk, then also stores it in memory. This option prevents writing VF file and only stores viewfactors in memory. Note that, upon exiting ANSYS, viewfactors are not stored in database jobname.db, so it would have to be recomputed later.
Viewfactor file (jobname.vf) can be large, so this option prevents writing to disk, useful if you know you won't be needing the VF file to read from for subsequent sessions.
[permalink]
|
| |
|
Average Rating: 10.0 (3 votes)
|
|
|
| |
|
VFSM |
| |
VFSM,encl_num,1.0
Scales viewfactors to force the sum to be 1.0 with the Radiosity Solver.
For some situations of closed enclosures, the viewfactors may not add up to 1 (such as if the mesh may be coarse). This scales all viewfactors to force them to be 1, so no space node/temperature needs to be defined for the closed case.
Please note that VFSM is now documented at ANSYS 12.0.1, but the syntax of the command has changed, so please refer to the Commands Reference for details.
[permalink]
|
| |
|
Average Rating: 10.0 (3 votes)
|
|
|
| |
|
VGET_SUBS
|
| |
Kiran Sreeram (GE Power Systems)
|
| |
"This macro stores the information requested by the user for a selected set of nodes or elements in an array called RESULT_COMP. This information can be any thing that is in the command *vget,for nodes & elements. The reason for this macro is that when using *vget the node or elem numbers must be sequential, in order to get any information. This macro deals with that i.e. by using *vmask, one can always do this manually, however this macro is helpful when needed to use regularly.
This macro also creates a txt file for the requested information."
[permalink]
|
| |
|
Average Rating: 10.0 (15 votes)
|
|
|
| |
|
Vibration Prediction in Switched Reluctance Motors With Transfer Function Identification From Shaker and Force Hammer Tests
|
| |
Zhangjun Tang, Pragasen Pillay, and Avoki M. Omekanda
|
| |
"A vibration prediction model for the switched reluctance
motor is constructed in this paper. Shaker and force hammer
tests for vibration measurement are used for measuring crucial parameters
like modal frequency and damping ratio for the transfer
function. A detailed lookup table of normal force versus phase current
and rotor angle is constructed based on finite-element calculations.
The model is then verified by experiments, with acceptable
accuracy."
[ANSYS Low-Frequency Electromagnetics, version unspecified]
[permalink]
|
| |
|
Average Rating: 10.0 (6 votes)
|
|
|
| |
|
VIEWFACE
|
| |
Tim Atchison (IDAC)
|
| |
"This ANSYS macro orientates your model to view a selected geometry face parallel to the screen. This is a must for analysts who regularly need to instantly orientate models to positions other than the standard views allowed. Simply click the face you want to view."
[permalink]
|
| |
|
Average Rating: 10.0 (5 votes)
|
|
|
| |
|
VISCO106
|
| |
VISCO106 "2-D 4-Node Viscoplastic Solid" (Anand Model) has been undocumented at ANSYS 12.0.1 to simplify the element offerings. Consider using PLANE182 with TB,RATE,,,,ANAND instead.
[permalink]
|
| |
|
| |
|
VISCO107
|
| |
VISCO107 "3-D 8-Node Viscoplastic Solid" (Anand Model) has been undocumented at ANSYS 12.0.1 to simplify the element offerings. Consider using SOLID185 with TB,RATE,,,,ANAND instead.
[permalink]
|
| |
|
Average Rating: 10.0 (2 votes)
|
|
|
| |
|
VISCO108
|
| |
VISCO108 "2-D 8-Node Viscoplastic Solid" (Anand Model) has been undocumented at ANSYS 12.0.1 to simplify the element offerings. Consider using PLANE183 with TB,RATE,,,,ANAND instead.
[permalink]
|
| |
|
| |
|
VISCO88
|
| |
VISCO88 "2-D 8-Node Viscoelastic Solid" has been undocumented at ANSYS 12.0.1 to simplify the element offerings. Consider using PLANE183 with TB,SHIFT and TB,PRONY instead.
[permalink]
|
| |
|
Average Rating: 10.0 (1 vote)
|
|
|
| |
|
VISCO89
|
| |
VISCO89 "3-D 20-Node Viscoelastic Solid" has been undocumented at ANSYS 12.0.1 to simplify the element offerings. Consider using SOLID186 with TB,SHIFT and TB,PRONY instead.
[permalink]
|
| |
|
| |
|
Viscoelastic Properties of Filled Rubber. Experimental Observations and Material Modelling
|
| |
Bohdana Marvalova
|
| |
"The paper presents an application of a phenomenological material model for a viscoelastic stress
response at large strains. The model is used for the simulation of carbon-black filled rubber in
monotonic and cyclic deformation processes under isothermal conditions. The material stress response
is decomposed into two constitutive parts which act in parallel: an elastic equilibrium stress response
and a rate-dependent viscoelastic overstress response. The response of a particular filled rubber in the
cyclic and relaxation tests was measured experimentally. The parameters of the constitutive functions
are determined from the experimental data by an identification process employing nonlinear
optimization methods. The paper concludes with a simulation by FEM of the cyclic loading of a simple
rubber specimen."
[ANSYS Nonlinear, version 10]
[permalink]
|
| |
|
Average Rating: 10.0 (2 votes)
|
|
|
| |
|
Viscoelasticity
|
| |
(ANSYS, Inc.)
|
| |
Presentation on the viscoelasticity model, introduced in ANSYS 6.1, available for both hypo- and hyper-elasticity (part of the "Advanced Analysis with ANSYS" seminar during the 2002 User's Conference).
[permalink]
|
| |
|
Average Rating: 8.5 (23 votes)
|
|
|
| |
|
Viscoelasticity [ZIP]
|
| |
Sheldon Imaoka (ANSYS, Inc.)
|
| |
"Viscoelastic constitutive models allow users to analyze the time-dependent
relaxation or creep behavior of materials, including glass, polymers, solid
rocket propellants, to name a few. One may view viscoelastic materials as
containing an elastic and viscous component, similar to a spring and dashpot
in series. This memo will introduce viscoelastic input in ANSYS and as well
as cover curve-fitting procedures."
(Week 49, week of 06/08/08)
[permalink]
|
| |
|
Average Rating: 9.8 (23 votes)
|
|
|
| |
|
Viscoplastic Finite-Element Simulation To Predict The Solder Joint Fatigue Life Of Different Flash Memory Die Stacking Architectures
|
| |
Yong Je Lee
|
| |
"This thesis focuses on the viscoplastic finite-element simulation to predict the
solder joint fatigue life of different die stacking architectures for flash memory products.
Four different stacked package architectures were evaluated as follows: pyramid,
rotated, and spacer stacking, while interconnection (solder joint) was held constant.
Number of dies for all four stacking configurations were varied from three, five and
seven. To keep the package height constant, the die and die attach thickness were varied
and the resulting effects on the stresses were investigated. A quarter and half symmetry
model of stacked flash package are generated using ANSYS APDL script. The life cycle
of the resulting packages were simulated under accelerated temperature cycling
conditions (-40C to +125C, 15min ramps/15min dwells)."
[permalink]
|
| |
|
| |
|
Visualizing structural matrices in ANSYS using APDL
|
| |
Aaron Acton (ANSYS, Inc.)
|
| |
"This article presents a method of visualizing structural matrices used in finite-element analysis using ANSYS and the ANSYS Parametric Design Language (APDL). The information is intended to provide some insight into the nature of structural matrices used in finite-element codes. Some terms used in sparse-matrix arithmetic are discussed, and methods for calculating certain quantities are provided. A test model is constructed to demonstrate how the stiff ness, mass, and damping matrices may be visualized for various systems. The eff ect of element shape, element type (including superelements), element reordering, and equation reordering on structural matrices is briefly investigated."
[permalink]
|
| |
|
Average Rating: 9.3 (15 votes)
|
|
|
| |
|
VLSM
|
| |
John Crawford (Honeywell)
|
| |
I ended up writing a macro that selects/reselects/unselects meshed areas, and then copied it and modified it for doing the same with volumes.
[permalink]
|
| |
|
| |
|
VM256 with Workbench Mechanical
|
| |
Sheldon Imaoka (ANSYS, Inc.)
|
| |
Created a Workbench 12.0 version of VM256.
Useful for users who may wish to get a better understanding of implementing the CINT command inside of Workbench Mechanical for J-integral and stress intensity factor calculations.
[permalink]
|
| |
|
Average Rating: 6.4 (7 votes)
|
|
|
| |
|
VM267 with Workbench Mechanical
|
| |
Sheldon Imaoka (ANSYS, Inc.)
|
| |
Created a Workbench 12.0 version of VM267.
Useful for users who may wish to get a better understanding of implementing the CINT command inside of Workbench Mechanical for stress intensity factor calculations.
[permalink]
|
| |
|
Average Rating: 7.1 (7 votes)
|
|
|
| |
|
VMER |
| |
VMER,volu1,volu2,etc.
"Glues" volumes together. Same command as VGLUE. See VGLUE for details on the usage of this command.
[permalink]
|
| |
|
Average Rating: 10.0 (3 votes)
|
|
|
| |
|
VOL
|
| |
John Swanson (SAS, Inc./ANSYS, Inc.)
|
| |
Used to calculate total volume of selected elements.
[permalink]
|
| |
|
Average Rating: 10.0 (6 votes)
|
|
|
| |
|
VOLSATELEM
|
| |
Doug Scott (Honeywell)
|
| |
"This macro basically takes the selected elements (8-noded bricks), creates volumes at the elements, assigns the appropriate attributes to the volumes, and then deletes the selected elements."
[permalink]
|
| |
|
Average Rating: 10.0 (3 votes)
|
|
|
| |
|
VORTEX
|
| |
Mark Troscinski (ANSYS, Inc.)
|
| |
Example of setting up vortex shedding. This is not a complete input file but shows options necessary to set up the problem. Also, a Zipped AVI animation is available.
[permalink]
|
| |
|
Average Rating: 8.3 (30 votes)
|
|
|
| |
|
VRANGE
|
| |
Mitch Voehl (CEC Corporation)
|
| |
Macro which creates a mask vector for array values which fall between specified minimuim and maximum values. Will also return parameters containing the index location of the first and last array elements meeting the criteria, as well as the number of array elements which meet the criteria.
[permalink]
|
| |
|
Average Rating: 5.0 (1 vote)
|
|
|
| |
|
VSLE |
| |
VSLE,s,1
Selects volumes based on selected elements. See ASLE undocumented command (or NSLL documented command) for usage.
[permalink]
|
| |
|
Average Rating: 10.0 (3 votes)
|
|
|
| |
|
VSLM_BW
|
| |
Bram Weisman (SBM-IMODCO)
|
| |
Based on VLSM macro, created by John Crawford to select/reselect/unselect meshed volumes. Written to take advantage of vectors to execute faster.
[permalink]
|
| |
|
| |
|
VSLN |
| |
VSLN,s,1
Selects volumes based on nodes. See ASLE undocumented command (or NSLL documented command) for usage.
[permalink]
|
| |
|
Average Rating: 10.0 (3 votes)
|
|
|
| |
|
VTHICK
|
| |
Rick Fischer (Marconi Communications)
|
| |
"This macro sets variable shell thickness based on thicknesses at corners of a surface. Only problem is that the attributes are being applied as a real constant. But, rthick creates r cards, one for each element, with real numbers the same as the argument. This could overwrite the reals used for the attributes, depending on how the model is numbered."
[permalink]
|
| |
|
Average Rating: 10.0 (1 vote)
|
|
|
| |
|
WB OLD PRESTRESS |
| |
Workbench Mechanical 13.0 introduces a new way of performing prestressed modal analyses with the PERTURB command. To use the older method of prestressed modal analyses (PSTRES command), set the operating system environment variable "WB OLD PRESTRESS" to a value of 1. (On Windows, use the System control panel to define this environment variable.)
Note that in the Static Structural system, you need to save the MAPDL database under the "Analysis Settings" branch since the Modal analysis system needs to resume the database.
[permalink]
|
| |
|
Average Rating: 7.5 (8 votes)
|
|
|
| |
|
WELD
|
| |
Karen Dhuyvetter (CSI)
|
| |
Transient analysis of a weld (phase change analysis)
[permalink]
|
| |
|
Average Rating: 9.5 (103 votes)
|
|
|
| |
|
WFMIN107
|
| |
Jan Christian Anker (Anker-Zemer)
|
| |
Wavefront optimization. Original link can be found here on Anker-Zemer's website.
[permalink]
|
| |
|
Average Rating: 10.0 (5 votes)
|
|
|
| |
|
Windows file association for ANSYS files [PDF]
|
| |
Sheldon Imaoka (CSI)
|
| |
How to associate database, graphics, and input files with ANSYS under Windows, so one can launch ANSYS more easily without the ANSYS launcher.
[permalink]
|
| |
|
Average Rating: 9.7 (17 votes)
|
|
|
| |
|
Windows NT and Max Addressable Memory (-m)
|
| |
Chris Hawkins (ANSYS, Inc.)
|
| |
Discussion of memory management and max addressable memory in Windows and why only about 1.4 GB of RAM can be accessed (5.6).
[permalink]
|
| |
|
Average Rating: 8.3 (6 votes)
|
|
|
| |
|
Wire Bond Temperature Sensor
|
| |
Shivesh Suman, Michael Gaitan, Yogendra Joshi, George Harman
|
| |
"This work reports the first demonstration of a bond pad test structure with embedded thermopile sensors for
the measurement of the transient temperature response during the wire bonding operation. This paper will present the
design and operation of the bond pad test structure and show and discuss temperature measurements during the wire
bonding operation."
[ANSYS Thermal, version unknown]
[permalink]
|
| |
|
Average Rating: 10.0 (3 votes)
|
|
|
| |
|
WIREBOND
|
| |
Sheldon Imaoka (ANSYS, Inc.)
|
| |
Simple Workbench Mechanical 13.0 example of a ultrasonic wire bonding tool. The piezoelectric stacks are prestressed with a bolt and driven at a given frequency (in this case, resonance is around 59 kHz). Project includes prestressed modal and prestressed harmonic response analyses.
To run this analysis, be sure to set the environment variable WB OLD PRESTRESS first since piezoelectric elements are not supported with the newer PERTURB method.
[permalink]
|
| |
|
Average Rating: 9.0 (15 votes)
|
|
|
| |
|
WOOFER
|
| |
Sheldon Imaoka (ANSYS, Inc.)
|
| |
Fictitious example of an acoustic analysis of a speaker in an archived ANSYS Workbench 13.0 project. Voice coil is excited with unit force; pressure is measured in front of speaker.
In Workbench, turn on beta features in order to be able to postprocess acoustic pressure.
Instead of performing a harmonic sweep, an analysis of a single frequency is set up. The Workbench Parameter page is then use to run a frequency sweep, where the PML (perfectly matched layers) region and buffer region size, along with mesh density, is adjusted for each frequency. This is done because if a single mesh for a large frequency range is used, the PML region would need to be as large as to accommodate the lowest frequency of interest while the mesh needs to be fine enough to capture the response of the highest frequency of interest — a large domain and small element size would result in inefficient solution times. By using Workbench Parameters, the mesh can be adjusted uniquely for each frequency. Higher-order FLUID220 and FLUID221 are used.
[permalink]
|
| |
|
Average Rating: 9.7 (39 votes)
|
|
|
| |
|
Workbench XML Material Format
|
| |
(ANSYS, Inc.)
|
| |
ANSYS Workbench Engineering Data module (e.g., Workbench Simulation, Workbench FE Modeler) can import/export material data as XML files. These XML files utilize the MatML format, and this zip file contains an example. This can be useful for users wishing to generate their own material libraries in XML format outside of Workbench Engineering Data.
[permalink]
|
| |
|
Average Rating: 8.6 (25 votes)
|
|
|
| |
|
WRITEARR
|
| |
Carl Olsard (noiseboard.com)
|
| |
"One command that is severely lacking from ANSYS is a simple way to export a matrix to a file, so that it can be imported into MATLAB. This script writearr.mac should be used with the companion MATLAB script readansysarray.m to export a matrix from ANSYS and import the array into MATLAB. At the moment the script is written to export 2D arrays of MxN (don't need to specify the dimensions). The output file contains the data i,j,data(i,j) where i and j are the array indices. The usage of the macro is:
writearr,'array','filename','ext'"
Here is the companion MATLAB script:
READANSYSARRAY
"This is the second part of the script, which uses the file exported by writearr.mac. This matlab script will import the file, and reshape the matrix into the correct format. The function is used as follows:
1. load the file into MATLAB: load press.txt
2. convert the matrix into the correct format: press2=readansysarray(press);"
[permalink]
|
| |
|
Average Rating: 9.7 (18 votes)
|
|
|
| |
|
X_BCSLOPE
|
| |
Shen-Yeh Chen (Honeywell)
|
| |
"This macro will apply slope BC value on the selected nodes according to the active coordinate value in sepcified DOF."
[permalink]
|
| |
|
Average Rating: 10.0 (5 votes)
|
|
|
| |
|
X_CECYC
|
| |
Shen-Yeh Chen (Honeywell)
|
| |
"This macro will create CE for cyclic sysmtric sector, even if the mesh on the two sectors interfaces are dissimillar."
[permalink]
|
| |
|
Average Rating: 10.0 (3 votes)
|
|
|
| |
|
X_DEMO_VREAD
|
| |
Shen-Yeh Chen (Honeywell)
|
| |
"This macro will demonstrate how to read in a matrix ZREAD(ZNNODE,3) in one *VREAD command. The macro will get coordianates from the current model first, write them into the file x_demo_vread.tmp, and read the data from the file"
[permalink]
|
| |
|
Average Rating: 7.5 (6 votes)
|
|
|
| |
|
X_ESUM
|
| |
Shen-Yeh Chen (Honeywell)
|
| |
"Calculate and print the summary of (selected) elements area or volume, and centroid. The result will be saved in the parameter _ParName."
[permalink]
|
| |
|
Average Rating: 10.0 (4 votes)
|
|
|
| |
|
X_NFOR2F
|
| |
Shen-Yeh Chen (Honeywell)
|
| |
"I usually use the following macro to "extract" element force, add a negative sign, and transfer into nodal force. This can sometimes be used to get the cross-section force on the cutting face, and do a force-controlled (instead of displacement-controlled) sub-model."
[permalink]
|
| |
|
Average Rating: 9.5 (10 votes)
|
|
|
| |
|
X_NOFFST
|
| |
Shen-Yeh Chen (Honeywell)
|
| |
Copies nodes (and elements) by x, y, z offset. Example of the use of a vector command with NMODIF.
[permalink]
|
| |
|
Average Rating: 10.0 (2 votes)
|
|
|
| |
|
X_PLLDST
|
| |
Shen-Yeh Chen (Honeywell)
|
| |
"This macro will get/plot (reponse vs load level) graph on the screen."
[permalink]
|
| |
|
Average Rating: 10.0 (8 votes)
|
|
|
| |
|
X_SHL2SLD
|
| |
Shen-Yeh Chen (Honeywell)
|
| |
"This macro will sweep the currently selected or assigned SHELL elements into SOLID elements."
[permalink]
|
| |
|
Average Rating: 10.0 (11 votes)
|
|
|
| |
|
X_TH2ST
|
| |
Shen-Yeh Chen (Honeywell)
|
| |
"This macro transfers the temperature distribution from a thermal analysis into structural temperature load. Only pre-selected nodes are dumped. The output file name is x_th2st.tld." (Note that there is a built-in ANSYS command called LDREAD command which does similar functionality)
[permalink]
|
| |
|
Average Rating: 9.3 (14 votes)
|
|
|
| |
|
XMLOPT |
| |
XMLOPT,options
This ANSYS command allows to write current load step results in XML format for use in Workbench Simulation.
"Options" can be the following:
- ALL - all results
- DOFS - nodal results
- S - stress results at the nodes
- EPEL - elastic strain
- EPPL - plastic strain
- (EPTO - total strain: obsolete)
- CONT - contact results
- PARM - parameters
- RFOR - reaction forces
- TG - thermal gradients at the nodes
- TF - thermal flux at the nodes
- (RESULTS - convenience label to include the S, EPTO, TG, TF results: obsolete)
See also /XML undocumented command to write results to file.
[permalink]
|
| |
|
Average Rating: 7.5 (18 votes)
|
|
|
| |
|
xPSD
|
| |
(PADT)
|
| |
"One of the most important types of mechanical simulation is the prediction of a system’s behavior due to random vibration. Almost every type of machinery, from computer circuit cards to satellite sub-assemblies, undergoes some type of random vibration, and it is the job of the analyst to determine if the system can stand up to this loading. xPSD is a tool from PADT that allows a user to take the results of a standard modal analysis and conduct fast, flexible studies on the behavior of the structure under just such loading.
"xPSD uses the "large mass method" to capture the modal response of a system to random vibration, expressed in terms of a Power Spectral Density (PSD) input. The user can quickly specify many different PSD input curves and extract the response of the system. The goal of the tool is to provide a simple - but fast and accurate - way for users to carry out PSD analyses. In fact, on a typical model (300,000 DOFs, 200+ modes), nodal response and 1-sigma values can be calculated in a matter of just minutes."
Although it is recommended to download the latest version from PADT's website above, there is an alternative download here.
[permalink]
|
| |
|
Average Rating: 9.4 (8 votes)
|
|
|
| |
|
YONGYI
|
| |
Yongyi Zhu (ANSYS, Inc.)
|
| |
Example of pressure-dependent thermal contact (beta at 5.6).
[permalink]
|
| |
|
Average Rating: 8.7 (38 votes)
|
|
|
| |
|
YZCURV
|
| |
Bill Bulat (OMM)
|
| |
"Here's something I used recently (NOT FULLY TESTED!!). Edit as needed to obtain curvature in other global planes (I wrote this to obtain curvature in global yz plane - a symmetry plane in a half symmetry model I recently created). Also reports the average radius of curvature if you're inclined to ignore the speed control bumps. My intention was to make this applicable to arbitrarily large deformations."
[permalink]
|
| |
|
Average Rating: 8.8 (4 votes)
|
|
|
| |
