Unofficial ANSYS HOWTO for MEnet Machines

by Tim Langlais

1. The Right Way to Use ANSYS
2. How to Create an ANSYS Batch File
3. Running ANSYS Without Wasting Resources
4. Words of Wisdom (One Man's Opinions)
5. FAQ (last update Thu Mar 12 16:31:59 CST 1998)

The Right Way to Use ANSYS

You can access ANSYS both interactively, using menus, and through the UNIX command line with batch files. When users first begin to use ANSYS, interactively clicking through the menus is far easier than sifting through pages of cryptic batch file commands. But do not be fooled! Easier does not mean better or faster. It turns out that solely using interactive ANSYS has several disadvantages

• Interactive use requires the user to save the model geometry and mesh in a *.db file and the results in a *.rst file. The *.db files can get as large as 50MB or more. We all have limited quotas. You will get no sympathy from the systems staff (they have quotas too) so you need to learn to conserve space.
• Interactive use is slow if you need to repeat operations. Mouse clicks are great until you have to do them over and over and over again.
• For long jobs, interactive use ties up a console. If you aren't using the machine for something else while ANSYS is solving, you are wasting resources. Besides, it is against MEnet policy to start a job on the console and leave for more than 15 minutes.

The main disadvantage of using batch files is that the learning curve is steep. But I figured it out, so you can too. The main advantages of batch processing ANSYS jobs are many:

• An entire model, mesh, and solution description can be contained in a file of 10-100K.
• You can run niced background batch jobs any time. Submit a job, go grab a bite, come back and look at the results.
• Batch processing is highly modular. If you spend time creating batch files, changing dimensions and mesh densities is a snap.
• You can optimize or make several ANSYS runs without having to do everything (changing pars, etc.) by hand.

How to Create an ANSYS Batch File

A batch file is a simple ASCII file with a list of ANSYS commands. The *.log file that you generate during an interactive session can be used as the starting point for a batch file. So if you you feel the task of creating a batch file from scratch is too daunting, then start by looking in the *.log file. It is best to check the *.log file as you go along through the menus. You will learn which menu commands correspond to which ANSYS commands.

Creating the geometry is often the most difficult process to perform in a batch file. There are a few options

• For those who know Pro/E, draw the model in Pro/E where you can change dimensions easily. Export IGES from Pro/E and read into ANSYS. This will require work to segment lines and define volumes for meshing.
• Draw the part in ANSYS using the menus. Keep careful track of the log file and try to piece together a batch file, adding a command for every mouse action. This works some of the time, but not all of the time.
• Learn the commands to draw keypoints and lines. Learn the commands for area and volume creation. Build the batch file slowly. Check the file in an interactive session of ANSYS as you go along using \input,batch.file.

All right already! You want to see a batch file. I have a few examples. Feel free to run these and pilfer what you may. Remember that \eof anywhere in the file stops execution. You may wish to place an \eof before the solve command in these files.

• A batch file that uses command line args to set the type of loading. Creates the geometry within ANSYS, meshes, and solves. Batch file: tshaft . And the companion shell script that will run ANSYS for the two different loadings, package up the results and delete everything in the tmp working directory. Shell script: ansys.sh Don't forget to make the shell script executable (chmod +x ansys.sh) and nice it.
• A batch file that reads in an IGES file, segments lines, meshes, then solves. Batch file: thole . IGES file: tube1.igs .
• A batch file that creates the geometry within ANSYS, segements, creates areas and volumes, meshes, then solves. Batch file: plate95S
• A batch file that uses contact elements, nonlinear solver, and ANSYS design optimization (written with Dan Moore, Linda Pham, and Olga Ugorets). Batch file: input

Running ANSYS Without Wasting Resources

So now you have a batch file and you want to know how to run the file to get some answers... Here is an example of running a batch file from the UNIX command-line.

unix% nohup nice +20 ansys53 -P ANSYSRF -m 48 < thole > ans.out &

nohup -- UNIX command; "no hangup"; run in the background
nice +20 -- UNIX command; add 20 to process priority; this 
       means ANSYS will use spare CPU cycles and not steal from
       the console
ansys53 -P ANSYSRF -- ANSYS with the correct license
-m 48 -- provide 48 blocks of memory (RAM) for ANSYS

ANSYS has a nasty habit of creating large temp files when it is solving a problem. It continually writes and reads from these files as it is solving. It is most efficient to write these files to the local hard drive rather than to your home directory through the network. Thus, you should always run an ANSYS background job from the local scratch space. Some of the MEnet machines have large scratch spaces, others very small. Be aware and use

df -k

unix% cd /usr/tmp

Once you have made an ANSYS run in the temporary directory, you can open up ANSYS interactively to look at the results. Note that the only files you need are those labeled *.db, *.log, and *.rst. The rest of the files are temp files. Remove them as they take up gobs of space and are not needed. Once you are done looking at the results, you can throw away everything but the batch file used to create the results. You can recreate the results at any time. If you really, really must save your results and geometry files, then at least archive and compress them

unix% tar -cvf - file.db file.log file.rst | gzip -9 > file.tar.gz      

Words of Wisdom (One Man's Opinions)

General

• Use batch files. After the umpteenth run, you'll be glad you did.
• Be nice. Run your ANSYS jobs niced when you are logged in to another machine, even interactively (nice +20 ansys53 ....). Folks on the console should have priority.
• If you have several runs that you'd like solve, write a shell script that will run ANSYS several times.

Geometry/BC's

• Write your batch files to draw the geometry using variables for dimensions. After you have had to root through a batch file or clicked through a model to change some length from 0.5m to 0.45m for the third time, you'll understand why variables are your friends (LENGTH=0.034).
• Apply point loads far away from the area of interest. The answers close to an applied point load are wrong. Point loads don't exist in the real world.
• Avoid Boolean geometry operations. ANSYS crashes as often as not trying to perform Boolean ops.

Meshing

• If you care about the accuracy of your answers, use h-elements instead of p-elements.
• Unless you know what you are doing, use quadratic elements rather than linear elements.
• Never use linear triangles or linear tetrahedra in structural problems. The strain is constant across the entire element.
• Use quad/brick elements when you can. This is hard, but often worth it. You will need to split volumes and specify element divisions.
• When the geometry is so complicated that you have to use tri/tet elements, be certain that ANSYS creates elements that are not distorted.
• Always use a coarse mesh first to determine the areas of steepest gradient (in stress or whatever variable you are interested in). The absolute answers won't necessarily be correct, but the trends ought to be. This will guide you in your choice of where more elements (higher accuracy) are needed.

Solution

• Never trust the answers without first checking them against something. FEA IS NOT A BLACK BOX!
• Use the PCG solver. It is faster than the wavefront solver for large problems (eqslv,pcg).
• Check that the stresses on the free surface are plane stress. On a traction-free surface, the stress normal to the surface should be zero. In ANSYS one of the principals ought to be at least O(2) less than the other two (or one if uniaxial).
• Check the unaveraged stresses. If the stress gradient is too steep, the unaveraged stresses will change too quickly (visually, from red to blue). Add more mesh points near these areas.
• Check that the stresses in the nominal section agree with a simple hand statics analysis.
• Make a few line graphs (stress vs. distance) near the areas of interest. If any of the larger stresses do anything but vary smoothly, beware the answers!
• Use line contours instead of filled color contours. You will get a better feel for the gradients that way.
• Stress != F( color ).

FAQ

Q1: How do I use the PCG solver?

A1: Once you are in the solution submenu (/solu) you can type

  eqslv,pcg

  Solution -> Analysis Options.. -> Linear Options [EQSLV] -> Precondition CG

Q2: How do I check the unaveraged stresses?

A2: When an FEM package solves for the stresses, it does so on an element by element basis. Unless otherwise prompted, ANSYS will solve for the stresses at the Guass points and extropolate to the nodes. However, many elements share nodes. So ANSYS averages the nodal stresses computed from each of the adjacent elements. If your mesh is sufficiently small, the averaged stresses will not be very different from the unaveraged stresses---that is to say that stresses at a common node, computed from adjacent elements will not be very different. So if you plot the unaveraged stresses and the stress from one element to the next changes drastically, your mesh is not small enough. You will need to define an element table to plot the unaveraged stresses.

General Postproc -> Element Table -> Define Table

[PLETAB] Avglab -> No - do not avg

Q3: How do I make line/XY plots of stress vs. distance?

A3: Sure, color contours look cool, but there are often better ways of presenting data. Good old XY plots are still

To define a path in ANSYS, select

General Postproc -> Path Operations -> Define Path

General Postproc -> Path Operations -> Map onto Path ...

Q4: How can I get ANSYS to plot line contours rather than filled contours?

Q5: How can I magnify the keypoint/node/element numbers? They're too small to read!

A5: Use

  /dev,text,2,%

Q6: How do import a part from Pro/E?

A6: The easiest way to trasfer a part from Pro/E to ANSYS is through an IGES file. In Pro/E select,

  Part -> Interface -> Export -> IGES

Once you have the IGES file, you need to import it into ANSYS. From the commandline,

/AUX15  
IOPTN,IGES,0
IOPTN,MERG,1
IOPTN,SOLID,0   
IOPTN,GTOLER, DEFA  
IGESIN,tube1,igs,
finish

  File -> Import -> IGES

Q7: How do I mesh a part in Pro/E?

A7: You don't. ANSYS has much better mesh capabilities than does Pro/E. For one, Pro/E cannot mapped mesh a solid with bricks. Quadratic bricks are often the best elements for a given problem. Use the above procedure for transfering a solid model from Pro/E to ANSYS.

Q8: How do I mesh a part in ANSYS

A8: Meshing is one of the most difficult parts of doing an FEM analysis. When I get around to it, I'll write some of the guidelines I use.

Q9: How can I select certain nodes in a batch file (you can't pick them with the mouse, obviously)?

A9: The different slection commands (nsel, lsel, asel) will allow you to select items based on location or some other parameters. For example, say I wanted to select all nodes with an x location between 0.05 and 0.06,

  nsel,r,loc,x,0.05,0.06

But what if you want all the nodes between with an x location from 0.05 to 0.06 and a y location between 0.7 and 0.71. Just stack the node selections. Essentially, you select the nodes with y between 0.70 and 0.71 from the set of nodes with an x location between 0.05 and 0.06.

  nsel,r,loc,x,0.05,0.06
  nsel,a,loc,y,0.70,0.71

Q10: How can I get a count of the number of items I have selected ?

A10: The *get command will allow you to get just about any information you want about selected items and allow you to store the result in a parameter/variable. Here is an example that with count the selected nodes and put the result in NODECNT

  *get,NODECNT,node,,count

Q10: How can I add logic (i.e. if-thens, etc) to my ANSYS batch file?

A11: ANSYS has much of the functionality of a programming language. In fact, much of the functionality is based on the underlying FORTRAN (sad that people use such an archaic language). You can compute parameters by calling any of the usual mathematical functions

NOTCH_MD=sqrt(NOTCH_R*NOTCH_R-DUMMY2*DUMMY2)

As another example you can use if-then logic to apply a certain load if a certain paramater (AXIAL in this case) is set

*if,AXIAL,EQ,1,then
        ! apply the axial force
        allsel
        nsel,r,loc,x,TOTAL_L-SMALLE,TOTAL_L+SMALL_E
        *get,NODECNT,node,,count
        f,all,fx,FAXIAL/NODECNT
*endif

Back to Tim's World