ansys.net search results
quick file search:
    home » search results
 
 
Undocumented Features (56 entries)
 
*GET,,ACTIVE
  *GET,Parm,ACTIVE,0,SOLU,CNVG
You can also *GET the convergence indicator, where 0=not converged; 1=converged.
[permalink]
 
Average Rating: 10.0 (16 votes)  
Rate this item:
 
*GET,,COMMON
  *GET,parm,common,,stepcm,,int,1
Newton-Raphson option key
[permalink]
 
Average Rating: 10.0 (2 votes)  
Rate this item:
 
*GET,,COMMON
  *GET,parm,common,,stepcm,,int,69
Adaptive descent key
[permalink]
 
Average Rating: 7.5 (4 votes)  
Rate this item:
 
*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 (1 vote)  
Rate this item:
 
*GET,,COMMON
  *GET,parm,common,,soptcm,,int,66
Auto Solve Method
[permalink]
 
Average Rating: 10.0 (1 vote)  
Rate this item:
 
*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)  
Rate this item:
 
*GET,,COMMON
  *get,parm,comm,,stepcm,,int,30
Number of nodal diameters:
[permalink]
 
Average Rating: 6.7 (6 votes)  
Rate this item:
 
*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)  
Rate this item:
 
*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)  
Rate this item:
 
*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)  
Rate this item:
 
*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)  
Rate this item:
 
*GET,,COMMON
  *get,parm,common,,stepcm,,real,10
Get the DMPRAT value for constant damping ratio.
[permalink]
 
Average Rating: 10.0 (4 votes)  
Rate this item:
 
/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: 8.3 (3 votes)  
Rate this item:
 
/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)  
Rate this item:
 
/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)  
Rate this item:
 
/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)  
Rate this item:
 
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)  
Rate this item:
 
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)  
Rate this item:
 
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: 8.3 (9 votes)  
Rate this item:
 
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)  
Rate this item:
 
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)  
Rate this item:
 
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)  
Rate this item:
 
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)  
Rate this item:
 
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)  
Rate this item:
 
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)  
Rate this item:
 
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)  
Rate this item:
 
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)  
Rate this item:
 
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]
 
No rating yet  
Rate this item:
 
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)  
Rate this item:
 
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 (1 vote)  
Rate this item:
 
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)  
Rate this item:
 
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)  
Rate this item:
 
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)  
Rate this item:
 
jobname.solc
  Regarding the undocumented jobname.solc feature:
  1. 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.
  2. 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)  
Rate this item:
 
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 (6 votes)  
Rate this item:
 
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)  
Rate this item:
 
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)  
Rate this item:
 
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)  
Rate this item:
 
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)  
Rate this item:
 
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)  
Rate this item:
 
OUTEQ
  OUTEQ outputs all results from equilibrium iterations while in /SOLU.
[permalink]
 
Average Rating: 10.0 (3 votes)  
Rate this item:
 
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)  
Rate this item:
 
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)  
Rate this item:
 
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)  
Rate this item:
 
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)  
Rate this item:
 
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: 8.3 (12 votes)  
Rate this item:
 
RSYNC
  RSYNC,ON
Forces dump of buffer of element stresses after they are written.
[permalink]
 
No rating yet  
Rate this item:
 
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]
 
No rating yet  
Rate this item:
 
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)  
Rate this item:
 
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)  
Rate this item:
 
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)  
Rate this item:
 
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]
 
No rating yet  
Rate this item:
 
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)  
Rate this item:
 
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)  
Rate this item:
 
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)  
Rate this item:
 
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)  
Rate this item: