Dad, What Do You Do at Work?

I’m sure the question comes up for a lot of us from time to time, whether from one of our own offspring, another relative, or an acquaintance.  “Just what is it that you do, anyway?”  Typical answers might be something short and sweet, such as, “I’m an engineer.”  A more detailed response might be, “I use a technique called finite element simulation which is a computer tool we use to simulate the behavior of parts or systems in their real world environment.”

You’ll probably find that people’s eyes glaze over and they start looking for someone else to talk to by the time you get to the end of that second quote above.  In fact, I find that my extended family is much more interested in my brother-in-law’s surgery stories from the operating room than they are in my own triumphs and challenges in the engineering simulation world.  Maybe you’ve had that same sort of reaction.  You have probably noticed that there are a whole lot more medical dramas on TV at any one time than there are engineering dramas.  They’ve got many characters from Marcus Welby on up to Dr. Ross on ER, Jack on Lost, to Dr. Grey on Grey’s Anatomy, with more than I can count in between.

We’ve got, well, Scotty.  And even then I think Dr. McCoy got more air time.

So when my kids ask me what I do at work, I recall a scene from that late 1980’s to early 1990’s TV show The Wonder Years.  In the episode “My Father’s Office,” Kevin asks his dad what he does for a living.  His father responds in an angry tone, “You know what I do!  I work at NORCOM.”  As if that were a sufficient explanation.  I suppose it was his way of saying, “It’s complicated.  It can be high pressure.  You might find it boring.  It puts food on the table and a roof over our heads, though.”

Rather than reply that way, I’ve tried to come up with what is hopefully a better response.  In fact, this concept constitutes the first portion of our Engineering with FEA training class, written by Keith DiRienz of FEA Technologies with contributions by yours truly.

I can’t guarantee that your audience’s eyes won’t glaze over by the end, nor that you’ll become the hit of the party, but this is free and you get what you pay for.  This explanation can obviously be adjusted based on the audience, but it goes something like this:

Simple explanation:

–We have equations to solve for stresses and deflections in simply-shaped parts such as cantilevered beams.

–No such equations exist for complex shaped objects subject to arbitrary loads.

–So, using finite elements, we break up a complex part into solvable chunks, leading to a finite set of equations with finite unknowns.

-We solve the equations for the chunks, and that ends up giving us the results for the whole part.

If we want more details, we can use this:  As an example, here is a simple beam, fixed at one end with a tip load P at the other end.  We have an equation to calculate the tip deflection u for simple cases:


In the above equation E is the Young’s Modulus, a property of the material being used and I is the moment of inertia, a property of the shape of the beam cross section.

For more complex shapes and loading conditions, we don’t have simple equations like that, but we can use the concept by dividing up our complex shape into a bunch of simpler shapes.  Those shapes are called elements.


A useful equation for us is the linear spring equation, F=Kx, where F is the force exerted on the spring, K is the stiffness of the spring, and x is the deflection of one end of the spring relative to the other.  If we extend that concept into 3D, we can have a spring representation in 3D space, meaning the X, Y, and Z directions.  In fact, the tip deflection equation shown above for the beam fixed at one end can be considered a special case of our linear spring equation, solved for deflection with a known applied force.

By assembling our complex structure out of these 3D springs, or elements, we can model the full set of geometry for complex shapes.  The process of making the elements is called meshing, because a picture or plot of the elements looks like a mesh.

Using linear algebra and some calculus (stay in school kids!) we can setup a big  series of equations that takes into account all the little springs in the structure as well as any fixed (unable to move) locations and any loads on the structure.  The equations are too big to solve by hand by normal people so computers are used to do this.

When the computer is done solving we end up with deflection results in each direction for the corner points (called nodes) in each element.  Some elements have extra nodes too.

From those deflection results, the computer can calculate other quantities of interest, such as stresses and strains.  Further, other types of analyses can be solved in similar fashion, such as temperature calculations and fluid flow.

Here is an example using a familiar object that practically everyone can relate to.  This plot shows the mesh:


This is fixed in the blue region at the bottom and has an upward force on the left end.  The idea here is that someone is holding it tightly on the blue surface and is pulling up on the red surface.


After solving the simulation, we get deflection results like this:


The picture above shows that the left end of the paper clip has deflected upward, which is what we would expect based on common experience with bending paper clips.  Using our finite element method, we can predict the permanent deflection resulting from bending the paper clip beyond it’s ‘yield’ point, resulting in what we call plastic deformation.

Clearly there is a lot more to it than these few sentences describe, but hopefully this is enough to get the point across.

In sum, not as exciting as my brother in law’s medical stories involving nail guns or other gruesome injuries, but hopefully this makes the world of engineering simulation a little more accessible to our friends and family.

In the Wonder Years episode, Kevin ends up going to work with his father to see for himself what he does.  I won’t spoil the episode, but hopefully you’ll get the chance to show your family and friends what it is that you do from time to time.

I Have the Touch: Check Contact in Workbench Prior to Solving with the Contact Tool

Song quotes Peter Gabriel, “I Have the Touch”

The time I like is the rush hour, cos I like the rush
The pushing of the people – I like it all so much
Such a mass of motion – do not know where it goes
I move with the movement and … I have the touch

Looking back I can see a defining moment in my life when about a month after high school graduation two good friends and I drove four hours from home to see Peter Gabriel in concert.  It’s not that the concert was great, which it was, but it was the trip itself.  It was a first foray after high school, a sort of toe dipping into the freedom of adulthood while in a strange pause between graduating in a small town in the same school system with the same kids and starting engineering school in a big city in the Fall.

Wanting contact
I’m wanting contact
I’m wanting contact with you
Shake those hands, shake those hands

What does all that have to do with ANSYS, you ask?  Primarily, it’s hard to get Peter Gabriel’s “I Have the Touch” out of my head whenever I’m working with contact elements.  Someone once said that we are a product of the music of our youth.  While as I’ve gotten older and hopefully wiser I would hope that we are made up of much more than the product of listening to some songs, I do find it true that certain songs from years ago tend to stick in my head.  So, while Mr. Gabriel plays in my head, let’s discuss checking our contact status in Workbench Mechanical.

For those of us familiar with Mechanical APDL, the CNCHECK command has been a good friend for a lot of years now.  This command can be used to interrogate our contact pairs prior to solving to report back which pairs are closed, what the gap distance is for pairs that are near touching, etc.  More recently, this type of capability has become available in Workbench Mechanical by inserting a Contact Tool under the Connections branch.

Let’s take a look at that in version 13.0.  Here we have inserted a Contact Tool under the Connections branch.  It automatically includes the Initial Information sub-branch, with a yellow lightening bolt meaning no initial information has yet been calculated.


By right clicking on the Initial Information sub-branch, we can select Generate Initial Contact Results.  The resulting worksheet view provides significant information on all of the defined contact regions.  By default the information displayed for each contact region includes the name, contact/target side, type (fictionless, no separation, etc.), status, number of elements contacting, initial penetration, initial gap, geometric penetration, geometric gap, pinball radius, and real constant set number.  That last value is useful when reviewing the solver output, as it lists contact info per real constant set number of each contact pair (contact region).


Further, by right clicking on that table we have the option to display some additional data, or remove fields of data.  The additional fields that can be added are contact depth, normal stiffness, and tangential stiffness.  We can also sort the table by clicking on any of the headings. 

The colors in the table display four possible status values:

Red = open status for bonded and no separation types

Yellow = open for non bonded/no separation types

Orange = closed by with a large amount of gap or penetration

Gray = inactive due to MPC or Normal Lagrange or auto asymmetric contact


If we left click on one or more of the contact regions in the table, we can then right click and “Go to Selected Items in Tree.”  This is a convenient way to view a particular set of contact regions in the graphics view.

Any social occasion, it’s hello, how do you do
All those introductions, I never miss my cue
So before a question, so before a doubt
My hand moves out and … I have the touch

So, what do we do with this information?  Ideally it will prevent us from launching a solution that goes off and cranks for a few hours only to fail due to an improper contact setup.  For example, by viewing the initial status for each pair we can hopefully verify that regions that should be initially touching are in fact touching as far as ANSYS is concerned.  If there is an initial gap or penetration, correcting action can be taken by adjusting the contact settings or even the geometry if needed prior to initiating the solution.

Wanting contact
I’m wanting contact
I’m wanting contact with you
Shake those hands, shake those hands

The Contact Tool > Initial Information is another tool we can use to help us obtain accurate solutions in a timely manner.  If you haven’t had the opportunity to use it, please try it out.  I can’t guarantee that it will trigger fond memories, but maybe you’ll have an enjoyable song playing in your head.

ANSYS 13.0 Enhanced Modal Analyses with Linear Perturbation

“Rest, rest, perturbed spirit!”  – William Shakespeare

If you have ever performed a large deflection prestressed modal analysis in ANSYS Mechanical APDL prior to version 13.0, your spirit might have been perturbed as well.  The procedure was not very user friendly, to sum it up.  For example, unless you were careful, the modal results would over-write the static preload results.  Thankfully, at 13.0 we have a smoother and more capable tool for handling large deflection prestressed modal analyses.  This new procedure is called Linear Perturbation.

We’ll focus on modal analyses in this article, but be aware that linear perturbation also applies to linear buckling analyses at 13.0, but only following a linear preload solution, and only in Workbench.  The capability for modal analyses is supported in both Workbench and Mechanical APDL.  Also, the preload, or ‘base’ analysis has to have multiframe restart capability turned on.  This will happen by default for a nonlinear analysis but needs to be manually activated in MAPDL for a linear analysis by issuing the command RESCONTROL,LINEAR.

In fairly simple terms, the prestress effects are included in a modal analysis via the change in the stiffness matrix that occurs during the prestress (typically nonlinear static) analysis.  This is the method that has been used in ANSYS for years.  What’s new at 13.0 is that the program keeps track of different components of the augmented tangent stiffness matrix.  The five possible contributing components are material property effects, stress stiffening effects, load stiffening effects, contact element effects, and spin softening effects.

While the material effects must remain linear, the contact stiffness can be altered, if desired, in the subsequent modal analysis.  More on that later.

The typical Mechanical APDL procedure to perform a nonlinear static structural prestress run followed by a modal analysis which utilizes those prestress effects is as follows:

! With static model prepared

/solu                            ! enter solution module
antype,0                         ! specify static analysis type
nlgeom,1                         ! turn on large deflection effects (nonlinear)
pstres,on                        ! turn on prestress effects for subsequent modal
nsub,10,10,10                    ! specify substep range
save                             ! save the database
solve                            ! solve the nonlinear static prestress case
finish                           ! leave the solution module
/solu                            ! re-enter solution so we can do a new analysis
antype,,restart,1,10,perturb     ! specify restart option for linear perturbation
! from last substep in this case
perturb,modal                    ! specify modal as next analysis
solve,elform                     ! calculate element formulation with solve command
modopt,lanb,12                   ! specify modal options for solution
mxpand,12                        ! specify number of modes for results calc
solve                            ! solve the prestress modal analysis
/post1                           ! enter general postprocessor
INRES,ALL                        ! make sure we read in all results from file
FILE,’nonlinear_static’,’rstp’   ! specify special results file for modal results
set,first                        ! read in results for first mode
plns,u,sum                       ! plot mode shape
set,next                         ! read in results for next mode
/repl                            ! plot mode shape, etc.


Note that the linear perturbation (modal) analysis has its own results file, the .rstp file.  Because of this, the preload results are still available in their own .rst file as it does not get overwritten by the modal step.

Here is a table of frequency results for a simple test case.  Three modal analyses were run:

1.  No prestress at all.

2.  With a linear static prestress state.

3.  With a nonlinear static prestress state.


Here is the model used for these runs in its initial configuration.  The block at the base was fixed in all DOF’s and the preload applied was a pressure load on one side of the vane.


Here is the model with the deformed mesh due to the nonlinear prestress:


Here is a mode shape plot for mode 12:


The above example is all well and good but could have been done in prior versions of ANSYS using the old partial solve method.  What’s nice about the newer linear perturbation method is that it’s easy to get the mode shape plots relative to the deformed mesh from the prior prestress run, and you don’t need to worry about over-writing the prestress results with the modal results, since the corresponding results files are different.

Further, we can now perform modal analyses using different restart points in the static prestress run, assuming multiple restart points are available.

Finally, we can actually change some contact options between the static prestress solution and the modal solution.  For example, if the prestress analysis was run using frictional contact, the subsequent modal analysis can be run utilizing the prestressed state of the structure but with one of three contact states for the modal analysis: true status (that of the prior static analysis), force (to be) sticking, or  force (to be) bonded. The sticking option applies only to contact elements with a nonzero coefficient of friction. The bonded option will force contact pairs that are in contact in the static analysis to be bonded in the modal analysis.

The Mechanical APDL command sequence for this procedure would be something like this:


! first perform nonlinear static prestress run, then



perturb,modal,,BONDED,PARDELE                    ! pre-stress modal analysis, switch contact to bonded, delete

                                                                                              ! loads in case future MSUP

solve                                                                ! Generate matrices needed for perturbation analysis

! Next perform modal analysis


mxpand                    ! default expand in case of complex solution


! modal results are now available for postprocessing

In Workbench Mechanical, the appropriate command sequence is sent to the solver when we link a modal analysis to a prior prestress analysis.  If the model involves contact, then in the modal analysis we’ll have choices for how the contact should be treated in the Pre-Stress branch under the Modal branch in the Outline Tree.  For frictional contact in the static prestress analysis, the choices in the Details view for the Pre-Stress branch in the modal analysis will be Use True Stress, Force Sticking, or Force Bonded as described above.

Here are some example plots for this scenario:

Two 3D plates subject to in plane bending, fixed at right ends, frictional contact between them.


Resulting contact status for static run (sliding is occurring)


Resulting static deformation:



Mode 6 result, “true” contact behavior:



Mode 6 result, “force bonded” contact behavior:


Those last two images show a dramatic difference in modal results simply by changing the contact status behavior in the modal analysis.  In the first of those images, the contact status is set to ‘true’, meaning essentially the same as in the prestress analysis, subject to the linear nature of the modal analysis.  In this example, the frictional behavior in the static prestress run becomes no separation in the modal analysis, so the two plates can have mode shapes in which the plates slide relative to each other.  In the last plot, the contact status has been changed to ‘force bonded’ for the modal solution.  As the plot shows, mode shapes can only exist in which the two plates are bonded together.  Both modal analyses have the same prestress condition however.

Here is a frequency table comparing the first six modes of the two modal analyses.  Note that with the contact forced to be bonded we get a stiffening response as we might expect.


So, although on the surface it might initially appear to be a black art, linear perturbation is a nice enhancement in ANSYS 13.0 that gives us a more robust and capable method for performing modal analyses with prestress effects included.  The prestress run is typically a linear or nonlinear static analysis, but it will also work with a full transient analysis to define the prestress state.  The ANSYS 13.0 Help has more information (see section 9.2 of the Mechanical APDL Structural Analysis Guide and section 17.8 of the Theory Reference).  We also recommend you try out the procedure on your own models.

Licensing Tips and Tricks, R13 Version

image_thumb31To many users, licensing is transparent and is managed by a system administrator pretty much behind the scenes. For users at smaller companies, license management may be part of your tasks as an ANSYS user. No matter where you fall on that spectrum, user, user-administrator, or administrator of many products including ANSYS, this article will hopefully have some beneficial information. First, we’ll explain some basics and then look at some problem scenarios and how to resolve them.

But before we get into the nitty gritty please take a second to hear our own very special musical take on licensing:

I’ve Got those Licensing Blues

The Basics

Why licensing at all? Licensing is how ANSYS, Inc. makes sure that only those paying for software can use the software. Just like you wouldn’t walk out of Ray’s Music Exchange without paying for a guitar, you wouldn’t want folks using ANSYS without paying for their product.



ANSYS uses FLEXlm software to administer licensing of the ANSYS products. However, unlike other applications that also use FLEXlm, the ANSYS license manager has an additional component, the ANSYS Licensing Interconnect. The ANSYS Licensing Interconnect was new at version 12.0 and was previously discussed here:

The recommended way to install the ANSYS license manager is to install FLEXlm and the ANSYS Licensing Interconnect together. The ANSYS licenses are then administered with the ANSLIC_ADMIN Utility. To access this utility on Windows license servers, the menu pick would be

Start > All Programs > ANSYS, Inc. License Manager > Server ANSLIC_ADMIN Utility.

On Linux, the path is

/ansys_inc/shared_files/licensing/lic_admin and the executable is anslic_admin.


FLEXlm and the ANSYS Licensing Interconnect can also be installed separately so that one can administer the FLEXlm portion using tools like FLEXnet Manager, but the ANSYS Licensing Interconnect still needs to be administered using the ANSLIC_ADMIN Utility.

Once we launch the ANSLIC_ADMIN Utility, the first things we want to check is the status box at the lower left. There are three components to check, the Licensing Interconnect, the Licensing Interconnect Monitor, and FLEXlm. Ideally the status for all three should be ‘running’, like this:


If all three are listed as ‘not running’, the first thing to try is to click on the Start the ANSYS, Inc. License Manager button. If the license file is properly installed and all else is right, the status of each of the three components should change to ‘running’.

Once the status of all three is ‘running’, it’s a good idea to verify the license status by clicking on the View Status/Diagnostic Options button, then Display the License Status. If all is well, the resulting listing should show that the license server is UP, and there are licenses available. The client machine should now be able to check out ANSYS licenses, again if all is well.

Useful Tools

Besides the ANSLIC_ADMIN Utility, a couple of useful tools are the license.log file and the ansyslic_server.log file in the ANSYS licensing directory. These files often provide clues to problem situations. The ANSLIC_ADMIN Utility can be used to view these files with the View Status/Diagnostic Options button, or they can be opened in a text editor. Another useful tool is the troubleshooting section in the ANSYS Licensing Guide in the ANSYS Help.

Problem Scenario 1: License Server will not start.

A couple of things can cause this. First, if you have not installed the license file properly. To install a license file, use the Run the License Wizard button or the Install the License File button in the ANSLIC_ADMIN Utility. Second, you are using an expired license file (for leased products, for example), or the hostname or flexid in the license file are wrong. To check it, click on the Register License Server Machine Information button in ANSLIC_ADMIN and compare the results with the info in the license file. It should match. If you have a dynamic IP address, you’ll need the license file to be tied to the hard driver serial number rather than the IP address.

Problem Scenario 2: License Manager starts, but FLEXlm doesn’t start.

In this case, you get a message in the ANSLIC_ADMIN Utility stating not all of the licensing components have started, and it may take a several minutes for everything to work properly. The status portion of the ANSLIC_ADMIN Utility will show that the interconnect is up and the interconnect monitor is up, but FLEXlm is down. The license.log file may show messages like this:

0:01:18 (lmgrd) The TCP port number in the license, 1055, is already in use.
0:01:18 (lmgrd) Possible causes:
0:01:18 (lmgrd) 1) The license server manager (lmgrd) is already running for this license.
0:01:18 (lmgrd) 2) The OS has not “cleared” this port since lmgrd died.
0:01:18 (lmgrd) 3) Another process is using this port number (unlikely).
0:01:18 (lmgrd) Solutions:
0:01:18 (lmgrd) 1) Make sure lmgrd and all vendor daemons for this
0:01:18 (lmgrd) license are not running.
0:01:18 (lmgrd) 2) You may have to wait for the OS to clear this port.
0:01:18 (lmgrd) Retrying for about 5 more minutes
0:01:36 (lmgrd) Still trying…
0:01:54 (lmgrd) Still trying…


In this case, the port may clear on it’s own, or you may need to change the port number from the default of 1055 to something else. This is done by adding a port number to the VENDOR line in the license file, see the ANSYS Licensing Guide for more info. Or, in the worst case, you’ll need to restart the license server computer to free up the needed port.

Problem Scenario 3: The license is up and running, but the client can’t connect to the license server

The first thing to check is that the client machine (which can also be the server) is properly pointing to the license server, even if they are the same computer. To test this, on the client machine (if it’s different from the server machine), run the Client ANSLIC_ADMIN Utility (On Windows: Start > All Programs > ANSYS 13.0 > ANSYS Client Licensing > Client ANSLIC_ADMIN Utility). Click on the Specify the License Server Machine button. Make sure the port numbers and server specification (usually the hostname) are correct. If they are not, take corrective action.

If the above is correct, the second thing to check is if the client can ‘see’ the server on the network. A quick way to test that is to ‘ping’ the server from a command window or shell. Type

ping hostname

in a command window/shell where ‘hostname’ is the name or IP address of the server machine. It should report back that bytes of data have been received from the server. If not, take corrective action, which may be to resolve network problems.

The third thing to check is that the ports and licensing executables can pass through any firewalls. The default port numbers that need to pass are 1055 and 2325. The server machine should allow lmgrd.exe, ansyslmd.exe, ansysli_server.exe, ansysli_monitor.exe, and ansysli_client.exe to pass through any firewall. The client machine should also allow ansysli_client.exe through any firewall.

Most problems in scenario three are resolved by one of those three steps.

Certainly there are other problems that can crop up with licensing. For those we suggest you review the ANSYS Licensing Guide in the Help, or contact your ANSYS support provider.

Hopefully this information is helpful and will keep the users from pursuing you, you won’t feel like the target of a manhunt, and you won’t get Those Licensing Blues.


10 Things Every ANSYS Mechanical APDL (MAPDL) User Should Know:

Providing tech support to users of Mechanical APDL gives us a wide exposure to a varied set of users.  And through the years we have discovered that there are some simple, basic, but important things every MAPDL users needs to know.  The ten most important things every user shoudl know are:

1.    /SHOW,3D
2.    /EFACET,2
3.    Picking window reset button
4.    Hot Spots for Picking and Press and Hold
5.    Displaying More than 9 Results Contours
7.    Copy and Paste into Input Window
8.    /EOF for Input File Debugging
9.    Use the Log File
10.   Making Results Plot Files


This command tells ANSYS Mechanical APDL to use your computer’s video card to control dynamic rotations of your model, rather than use software to rotate the model.  The big difference is that you’ll see a shaded image of your model during dynamic manipulation of the view, rather than shaded > wireframe while rotating > shaded.  For some users, switching to this option is like getting a color TV after years of watching just black and white.

To active this option from the Mechanical APDL Product Launcher, go to the Customization/Preferences Tab and change the Graphics Device Name to 3D.
If you are running ANSYS from the command line, you can use the –d 3D option after the ANSYS executable specification.


If you are running with mid-side noded elements, you’ll most likely want to include results for the midside nodes, and also make results plots which include any curvature of the element edges.  The default, however, is to not include midside noded results in listings or plots and to only give one facet per element edge in results plots.  The fix for that is to set the number of facets to 2 (or even 4) on the /EFACET command.  Note that Powergraphics needs to be on for this to work.

Picking Window Reset Button

If you have spent a lot of time working interactively in ANSYS Mechanical APDL, you have probably encountered the scenario in which you click on a command that is supposed to activate a picking window, but no picking window shows up.  No matter how many times you click on the command, you won’t get the needed picking window.  My understanding is this is due to a glitch in the Tcl/Tk GUI language used by ANSYS, Inc. to create the Mechanical APDL user interface.  Earlier versions had a fix implemented which was somewhat primitive:  while in the ANSYS session, simultaneously press Control-Shift-Delete.  This would reset the picking window so we could click on the desired command again and successfully get the needed picking window.  The last couple of releases of ANSYS have had an improvement over that, namely the Reset Picking button.  This button resides near the upper right corner of the user interface, in between the Raised Hidden “Cheese Sandwich” button and the Contact Manager button.

Hot Spots for Picking and Press and Hold

This is really two things, but they are closely related so we’ll consider them as one.  Have you  ever have trouble using the mouse to pick the entity you want?  You click where you think you’ll be picking the desired entity but some other entity gets highlighted.  If this happens a lot, you’re probably not familiar with how ANSYS uses Hot Spots for picking, nor with the Press and Hold left mouse button behavior.

First we’ll discuss hot spots, which are locations on each geometric entity.  Areas and volumes each have one hot spot, at or very near the centroid.  Lines have three hot spots, one at the middle of the line and one close to each end.  When you click a location in the graphics window to select an entity, the entity which has a hot spot closest to the picking location is the one which gets picked.  Note that hot spots can be outside of an entity (think of an annulus, for example).  That means you might click on an entity, but another entity might have its hot spot closer to where you clicked, so that’s the one the is selected.  Thinking about where hot spots are can assist greatly in selecting the entities we want.

Second, another useful tool for ensuring we actually pick entities we want is to press and hold the left mouse button while picking.  If you press and hold, the entity that’s going to be picked will be highlighted.  If you press and hold and drag the mouse around in the screen, different entities can be highlighted, the idea being you press, hold, and drag until the desired entity is highlighted.  You then release the left mouse button and that entity is now picked.

Displaying More Than 9 Results Contours

By default results plots in /POST1 have 9 color contours.  Sometimes we want more.  If you are using the Win32 or X11 graphics drivers, you can obtain up to 14 color contours by issuing

/show,win32c,,,8  !or /show,x11c,,,8

Note that if you are using the 3D graphics driver (see above), you can display up to 128 color contours using the same /contour command.  There are other useful options on this command so check the ANSYS help for more info.


What did we do before CNCHECK?

We attempted a lot more contact debugging solves than are needed today, that’s for sure.  CNCHECK can be used to interrogate one or more contact pairs prior to solving to help us ensure that contact regions are setup appropriately.  Not only does it tell us which contact and target element sets are associated with each other, but it lists all of the ‘calculated’ settings such as the actual value of contact stiffness, penetration tolerance, etc.  If there is an initial gap, it will tell us the gap distance.  If a contact region is supposed to be initially touching but isn’t, CNCHECK will tell us.  We can then hopefully take corrective action before we start the solution.  This can be a huge timesaver.  CNCHECK has other useful capabilities, all discussed in the Help.

Copy and Paste into Input Window

If you work with ANSYS MAPDL commands a lot, you are hopefully familiar with copying commands from a text file or from an editor (PADT’s PeDal editor specifically created for ANSYS input files comes to mind) and pasting them into the ANSYS command window.  ANSYS, Inc. tells us this is not a supported feature, but we at PADT and other users have been doing this for years and it works great.  Whether you are building an input file to automate your process or just checking out a few commands from the Help, you can copy the desired command lines and paste them into the input window.  You then click the Enter key and all of those commands will be executed within ANSYS, in sequence from first to last.  Try it.

/EOF for Input File Debugging

If you routinely build ANSYS MAPDL input files or are just starting to work with them, you should be aware of the /EOF command.  You can place that anywhere in your file and the input will stop being read at that location.  If you have 2000 lines of APDL code and just want to debug the first 20 by reading only those lines in, you just place the line /EOF after those first 20 lines of code, save the file, and read it in.  The remaining 1980 lines will be ignored and you can easily verify the action of those first 20 commands.  You can then delete the /EOF command and place a new one farther down to work in the next section.  Hopefully you now see the value of /EOF.

Use the Log File

The log file (jobname.log) is a running list of all the MAPDL commands you have executed in your current ANSYS session.  It doesn’t matter if you typed them in, pasted them in, or used the GUI, they are there in the log file, sequentially from top to bottom.  Further, if you have multiple ANSYS MAPDL sessions in the same working directory using the same jobname, you’ll have a multiple-session history in your log file, each with its own time and date stamp.

How is this useful?  If you find yourself repeating your steps over and over, you should consider automating those steps using an input file.  An easy way to create an input file is to edit the log file, extract the portion you want to automate, save that into a new file, and perhaps do some further editing to get it to be robust and tailored to your specific application.  How to do all that is beyond the scope of this article (see our APDL training classes at, but a quick set of instructions is to execute a command once using the GUI, then view the bottom of the log file to see how it was used.  Combine that with the ANSYS Help and you are off and running in building your own MAPDL input files.

Making Results Plot Files

A quick way to make a result plot file is to get the plot and view setup the way you want on the screen, then click on Plotters > Hard Copy > To File.  There are several plot file formats available, such as .jpg and .png.  This command will automatically ‘reverse video’ meaning you get black text on a white background in your plot file.  There are other techniques for getting results plots into plot files, but this is a quick and easy way that you will hopefully find helpful.

—That’s 10!