ansys.net search results
quick file search:
    home » search results
 
 
Undocumented Features (29 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,,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)  
Rate this item:
 
*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)  
Rate this item:
 
*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)  
Rate this item:
 
*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: 6.7 (12 votes)  
Rate this item:
 
*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 (7 votes)  
Rate this item:
 
*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 (5 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:
 
/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)  
Rate this item:
 
/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)  
Rate this item:
 
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]
 
No rating yet  
Rate this item:
 
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 (7 votes)  
Rate this item:
 
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:
  1. Flag surface or volumetric data to export by an "interface number" with the VAL2 argument of SF,,FSIN,,val2 or BFE,,FVIN,,val2 commands
  2. Use EXUNIT command to specify units for export.
  3. 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)  
Rate this item:
 
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:
  1. Flag surface or volumetric data to export by an "interface number" with the VAL2 argument of SF,,FSIN,,val2 or BFE,,FVIN,,val2 commands
  2. Use EXUNIT command to specify units for export.
  3. 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)  
Rate this item:
 
FSUM
  FSUM,,CONT
Sums contact forces only for CONTA171-174 (at 5.6.1)
[permalink]
 
Average Rating: 9.1 (16 votes)  
Rate this item:
 
FTST
  FTST,SEQV
Uses equivalent stress in fatigue calculations. Issue prior to FTCALC command. [5.4]
[permalink]
 
Average Rating: 6.6 (16 votes)  
Rate this item:
 
FTST
  FTST,SINT
Uses stress intensity in fatigue calculations. Issue prior to FTCALC command. [5.4]
[permalink]
 
Average Rating: 10.0 (9 votes)  
Rate this item:
 
NFORCE
  NFORCE,CONT
Calculates nodal contact forces only for CONTA171-174 (at 5.6.1)
[permalink]
 
Average Rating: 10.0 (8 votes)  
Rate this item:
 
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)  
Rate this item:
 
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)  
Rate this item:
 
PLOT33.F
  (ANSYS, Inc.)
  Old source code (ANSYS 5.4?) for PLOT33 program to read GRPH files (ANSYS Graphics Files)
[permalink]
 
No rating yet  
Rate this item:
 
PLVECT
  PLVECT,S,1
Plots only first principal stress instead of plotting all three vectors at once.
[permalink]
 
Average Rating: 10.0 (5 votes)  
Rate this item:
 
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: 7.5 (4 votes)  
Rate this item:
 
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]
 
No rating yet  
Rate this item:
 
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: 7.1 (7 votes)  
Rate this item:
 
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)  
Rate this item:
 
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)  
Rate this item:
 
TFUN
  TFUN,reference,variable,psd_table,name
Plot transfer function.
See Section 6 of the PSD Postprocessing Tip for details on this usage.
[permalink]
 
No rating yet  
Rate this item:
 
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)  
Rate this item: