ANSYS Command File Creation and Execution

Generating the Command File

There are two choices to generate the command file:
  1. Directly type in the commands into a text file from scratch. This assumes a good knowledge of the ANSYS command language and the associated options.

    If you know what some of the commands and are unsure of others, execute the desired operation from the GUI and then go to File -> List -> Log File. This will then open up a new window showing the command line equivialent of all commands entered to this point. You may directly cut and paste from here to a text editor, or if you'd like to save the whole file, see the next item in this list.

  2. Setup and solve the problem as you normally would using the ANSYS graphic user interface (GUI). Then before you are finished, enter the command File -> Save DB Log File This saves the equivalent ANSYS commands that you entered in the GUI mode, to a text file. You can now edit this file with a text editor to clean it up, delete errors from your GUI use and make changes as desired.

Running the Command File

To run the ANSYS command file,

GUI Command File Loading

To run this command file from the GUI, you would do the following:

Command Line File Loading

Alternatively, you can also read in the command file right from the ANSYS command line. Assuming that you started ANSYS using the commands...
   /ansys52/bin/ansysu52
and then entered
   /show,x11c
This has now started ANSYS in the text mode and has told it what graphic device to use (in this case an X Windows, X11c, mode). At this point you could type in /menu,on, but you might not want to turn on the full graphic mode if working on a slow machine or if you are executing the program remotely. Let's assume that we don't turn the menu mode on...

If the command file is in the current directory for ANSYS, then from the ANSYS input window, type

   /input,frame,cmd
and yes that is a comma (,) between frame and cmd. If ANSYS can not find the file in the current directory, you may need to point it to the proper directory. If the file was in the directory, /myfiles/ansys/frame for example, you would use the following syntax
   /input,frame,cmd,/myfiles/ansys/frame
If you want to rerun a new or modified file, it is necessary to clear the current model in memory with the command
   /clear,start
This full procedure of loading in command files and clearing jobs and starting over again can be completed as many times as desired.

ANSYS Command Groupings

ANSYS contains hundreds of commands for generating geometry, applying loads and constraints, setting up different analysis types and post-processing. The following is only a brief summary of some of the more common commands used for structural analysis.

Category Command Description Syntax
Basic
Geometry
k keypoint definition k,kp#,xcoord,ycoord,zcoord
l straight line creation l,kp1,kp2
larc circular arc line
(from keypoints)
larc,kp1,kp2,kp3,rad
(kp3 defines plane)
circle circular line creation
(creates keypoints)
see online help
spline spline line through keypoints spline,kp1,kp2, ... kp6
a area definition from keypoints a,kp1,kp2, ... kp18
al area definition from lines a,l1,l2, ... l10
v volume definition from keypoints v,kp1,kp2, ... kp8
va volume definition from areas va,a1,a2, ... a10
vext create volume from area extrusion see online help
vdrag create volume by dragging area along path see online help
Solid Modeling
(Primitives)
rectng rectangle creation rectng,x1,x2,y1,y2
block block volume creation block,x1,x2,y1,y2,z1,z2
cylind cylindrical volume creation cylind,rad1,rad2,z1,z2,theta1,theta2
sphere spherical volume creation sphere,rad1,rad2,theta1,theta2
prism
cone
torus
various volume creation commands see online help
Boolean Operations aadd adds separate areas to create single area aadd,a1,a2, ... a9
aglue creates new areas by glueing
(properties remain separate)
aglue,a1,a2, ... a9
asba creat new area by area substraction asba,a1,a2
aina create new area by area intersection aina,a1,a2, ... a9
vadd
vlgue
vsbv
vinv
volume boolean operations see online help
Elements &
Meshing
et defines element type et,number,type
may define as many as required; current type is set by type
type set current element type pointer type,number
r define real constants for elements r,number,r1,r2, ... r6
may define as many as required; current type is set by real
real sets current real constant pointer real,number
mp sets material properties for elements mp,label,number,c0,c1, ... c4
may define as many as required; current type is set by mat
mat sets current material property pointer mat,number
esize sets size or number of divisions on lines esize,size,ndivs
use either size or ndivs
eshape controls element shape see online help
lmesh mesh line(s) lmesh,line1,line2,inc
or lmesh,all
amesh mesh area(s) amesh,area1,area2,inc
or amesh,all
vmesh mesh volume(s) vmesh,vol1,vol2,inc
or vmesh,all
Sets &
Selection
ksel select a subset of keypoints see online help
nsel select a subset of nodes see online help
lsel select a subjset of lines see online help
asel select a subset of areas see online help
nsla select nodes within selected area(s) see online help
allsel select everything
i.e. reset selection
allsel
Constraints dk defines a DOF constraint on a keypoint dk,kp#,label,value
labels: UX,UY,UZ,ROTX,ROTY,ROTZ,ALL
d defines a DOF constraint on a node d,node#,label,value
labels: UX,UY,UZ,ROTX,ROTY,ROTZ,ALL
dl defines (anti)symmetry DOF constraints on a line dl,line#,area#,label
labels: SYMM (symmetry); ASYM (antisymmetry)
Loads fk defines a fk,kp#,label,value
labels: FX,FY,FZ,MX,MY,MZ
f defines a force at a node f,node#,label,value
labels: FX,FY,FZ,MX,MY,MZ