Microsoft Word - Document1

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

Plot -> Lines

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

keypoint
definition

k,kp#,xcoord,ycoord,zcoord

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

area definition
from keypoints

a,kp1,kp2, ... kp18

area definition
from lines

a,l1,l2, ... l10

volume
definition from
keypoints

v,kp1,kp2, ... kp8

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

defines element
type

et,number,type
may define as many as required; current
type is set by

type

set current
element type
pointer

type,number

define real
constants for
elements

r,number,r1,r2, ... r6
may define as many as required; current
type is set by

real

sets current real
constant pointer

real,number

sets material
properties for
elements

mp,label,number,c0,c1, ... c4
may define as many as required; current
type is set by

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

defines a DOF
constraint on a
keypoint

dk,kp#,label,value
labels:
UX,UY,UZ,ROTX,ROTY,ROTZ,ALL

defines a DOF
constraint on a
node

d,node#,label,value
labels:
UX,UY,UZ,ROTX,ROTY,ROTZ,ALL

defines
(anti)symmetry
DOF constraints
on a line

dl,line#,area#,label
labels: SYMM (symmetry); ASYM
(antisymmetry)

Loads

defines a

fk,kp#,label,value
labels: FX,FY,FZ,MX,MY,MZ

defines a force at
a node

f,node#,label,value
labels: FX,FY,FZ,MX,MY,MZ