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,

• save the ASCII text commands in a text file; e.g. frame.cmd
• start up either the GUI or text mode of ANSYS

GUI Command File Loading

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

• From the File menu, select Read Input from.... Change to the appropriate directory where the file (frame.cmd) is stored and select it.
• Now ANSYS will execute the commands from that file. The output window shows the progress of this procedure. Any errors and warnings will be listed in this window.
• When it is complete, you may not have a full view of your structure in the graphic window. You may need to select Plot -> Elements or Plot -> Lines or what have you.
• Assuming that the analysis worked properly, you can now use the post-processor to view element deflections, stress, etc.
• If you want to fix some errors or make some changes to the command file, make those changes in a separate window in a text editor. Save those changes to disk.
• To rerun the command file, you should first of all clear the current model from ANSYS. Select File -> Clear & Start New.
• Then read in the file as before File -> Read Input from...

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