Stomp on a Bug in ANSYS Mechanical R14


Okay, so it’s not the ugly critter in the picture, (that on was found at my house), but the bug in ANSYS R14 can give you the willies just the same. ANSYS, Inc. is working very hard to get the situation remedied, and they will be sending out defect notices shortly.  They provided a quick-fix however, and we wanted to get it out to you as  quickly as possible. So I have done some screen captures while I ran through the fix.

The issue found is that if you close a Mechanical, or Meshing, session and then hit ‘Save’ on the project window, you may lose the contents of your Mechanical database.   The problem has arisen in R14 because ANSYS, Inc. has decreased the start up time of Mechanical by pre-loading it when Workbench is started. When you close Mechanical, it stays open in the background as an empty database. There is a 1-second ‘window of opportunity’ after you close the Mechanical editor and save the project file when the process threads are not fully synchronized.  If you save during this period, the blank session gets saved on top of the good session, and all data is lost.  If you wait longer than a second, there shouldn’t be an issue, but customers have been reporting longer times where they have still lost data.  ANSYS, Inc. is working with those customers to find out what is causing the longer times on their boxes.

Luckily the remedy is simple, and hopefully none of you will have to lose any data.  Since the issue is caused by the pre-loading of Mechanical, the remedy is to simply turn the pre-loading off.  This has to be done from  the Tools > Options menu on the Project window. Just uncheck the Pre-Load box in both the Mechanical and Meshing dialog boxes, and then close Workbench after hitting ‘OK’. The next time you open Workbench, the bug will be neutralized.

I just wish it was that easy for that creepy guy in the picture! Smile


How do I Know that my Download was Successful?

With the release of ANSYS 14.0, I thought it would be good to get this topic on the Focus blog. Quite often, we get tech support calls about installs that crash or hang. Most of the time it is traced back to the fact that the download was not complete or had an error that the user didn’t see at the time.  So how can you check that your download was successful before starting you install?  Easy. Check the md5sum.

When you go to download software from ANSYS, or many other locations, they post the md5sum hash table value as shown below.


Md5sum is an algorithm used to calculate an identifier that functions as a compact digital fingerprint of a file.  Most UNIX and LINUX systems have it as a built in function. The Wikipedia article on md5sum says that Windows has it too, but I have never found it. So I went out on the internet and found one. Many actually. Here is a direct link to get MD5Sums, a useful one at, a  reputable download site.

“Md5sums” is nice in that it is fast, taking only about 30 seconds for a 4GB file, and you can use it two ways.  As with most other executables, you can use it at a command line or in a script, like this:

md5sums –u *winx64* > checksums.txt

to get a file, “checksums.txt”, with formatted output like this for all the matching files in a directory.

9febae323d5df015187c84f373db7a45 *ansys140_winx64_dvd1.iso
c90e04fd5e5bd94d1a39101bcbe18258 *ansys140_winx64_dvd2.iso

But MD5sums also allows you to drag-n-drop files onto it in the file explorer  and it starts processing those files, or a whole directory, in pop-up window. 


Then you just compare the output to the md5sum values that ANSYS posted on the download page.  If they are not the same, then something happened during the download process.  You’ll have to download the bad file again, but at least you haven’t started the install yet.  

Happy Downloads!!!

Why You Need a Good Text Editor: Finding What Changed in Your Model

There seems to come a time in everyone’s career, at least once, but usually for me, once a week, where I have made a change to something and didn’t even know it.  I copied a model, or made what I thought was a copy, but the results are coming out different.  So how do you tell what’s changed?

Well, you can spend time checking individual boundary conditions, part names, material properties, etc.  This can take a long time, especially with interactive programs that have a different menu or dialog box for each one.  This is where a good text editor can save you hours of work and years worth of frustration and stress.

So what can a good text editor do for you? In such a case it can compare two files and show you quickly exactly what is different.  For my money, GVIM gets my vote as the best text editor available. (Partly because it’s free and didn’t take any of my money. )

The “Split Diff with…” option in GVIM will show multiple files, side by side, and highlight differences between them.  Lines that are different are highlighted pink, with the actual difference highlighted in red. Lines that are present in one file, but not in the other, are highlighted purple, while blank lines are added to the other file to keep the similarities lined up.


So how do you use this feature to compare ANSYS, CFX, or Fluent, or any other models?  Most analysis programs have an export or archive feature that rights the model out in text format. In ANSYS, you can write out a text archive, CDB file, with the CDWRTE command.  In CFX, as in this example, you can export a CCL file.  In this example, GVIM quickly highlights what different between two CCL files.

In this case, the option on one of the boundary conditions was different.


Another great thing about GVIM, is that it will also do the “Split Diff With…” on binary and Hex files, too. Now, you might not read hexadecimal, I don’t either, but at least you would know that the files differ somewhere.


There are a lot of good text editors out in the market these days. The key is to find one that you like, and learn it inside and out.  It can save you a lot of frustration and time in the long run.


  • You can learn more about Vim and download a copy at:
  • Other text editors with text comparison capabilities:
    • Notepad++: Notepad on steroids, it has a nice difference utility
    • Emacs is the other editor that came out of Unix that people swear by, if they are not Vim users.
    • SlickEdit is not free, $299 for a single user license, but it is one of PADT’s favorite paid text editors.
  • A comprehensive list of text editors can be found on Wikipedia:

Mid-side nodes: Do they really help?

Do those pesky mid-side nodes really do anything other than increase my node count and runtime?  Over the years, I have heard that question over and over. “Do I really need them?”  If you are using tetra elements, then the answer is absolutely, “Yes!”  They even do more than just give you nice curvature to follow your geometry.  For tetras, the midside nodes are necessary to predict proper stresses.  Lower ordered tetras are overly stiff and will under predict deflection and stresses.  Let’s look at the underlying equations that make up the shape functions in both element types.


Yeah, the equations for tetras are a little more complicated than that, but I really didn’t think you  wanted to go down that road. But I will remind you that low-order elements have linear shape functions, while high-order elements have quadratic shape functions. So let’s look at an example, instead, to show that lower-order tetras will give unconservative results.

For the example, I made a simply-supported, rectangular-cross-section plank.  It’s 100 inches long, by 10 inches wide, by 1 inch thick, with a 1 psi pressure load. I set the mesh size at 1 inch and solved with low-order tetras, high-order tetras, and also with low and high-order hex elements.  The results are tabulated below along with the hand-calculated solution from the 7th Edition of Roark’s Formulas for Stress and Strain, Table 8.1, case 2e.



  Deflection Def. % Diff Stress Stress  % Diff Nodes Elements
Roark’s -0.53864   7500.0 psi      
20-Node Hex -0.54159 0.55% 7527.0 psi 0.36% 7553 1,000
8-Node Hex -0.54142 0.52% 7529.5 psi 0.39% 2222 1,000
10-Node Tetra -0.54158 0.55% 7525.9 psi 0.35% 20661 11,998
4-Node Tetra* -0.27151 49.6% 2249.3 psi  –70.0% 3222 11,999

As you can see, the hex elements along with the 10-node tetras get close to the solution and provide conservative results.  The 4-node tetras, however, which are actually degenerate 8-node hex elements because ANSYS removed their 4-node tetra elements along time ago, show only half the deflection under the same load.   The extra stiffness also causes the modal frequencies to be higher. In this case, the frequencies of the low-order tetras were about 40% higher than the high-order tetras.  When you’re looking at operating ranges, this could also lead to unconservative conclusions.

Of course this is a pretty coarse mesh with only one element through the thickness. So how do the results change as the mesh is refined? We should only need to cut the element size by half to get the extra nodes and the same results, right? 

    Deflection Def. % Diff Stress Stress  % Diff Nodes Elements
Roark’s -0.53864”   7500.0 psi      
1”  -0.27151”


2249.3 psi


3,222 11,999
0.5” -0.39768”


4879.1 psi


17,624 77,612
0.3” -0.47582”


6069.5 psi


69,040 334,433
0.2” -0.51023”


6760.9 psi


213,122 1,105,641
0.1” -0.53345”


7309.6 psi


1,599,327 8,877,326

As you can see the answer is, “No.”  Because  the high-order elements have quadratic shape functions , it takes far more linear elements to make up the difference. Here is a little animation to show why. You can see the error left by each set of linear elements when try to match a quadratic function.JoeAnim1

For another example, I made a long square-cross-section bar with holes in it.  It is cantilevered with a shear load at the other end.  I set the Physics preference to Mechanical and the Relevance Center to ‘Fine’ and I got the mesh that you see below. (I’d say its not too bad for 15 seconds of works. )image


Just to make sure that my mesh was the same in both cases, I told Mechanical to Drop the midside nodes and then I added a Command Object in the high-order  case to convert the elements to Solid 187 tetras during the run. Since no geometry is sent from Mechanical, the midside nodes were added and the edges were kept straight, so no further curvature was picked up.  Here’s the command object to try out yourself.



By scoping the results to just the hole closest to the fixed end we can see the difference in the stress values for the two runs.  The low-order tetras yield results that are 12% lower for deflection and over 19% lower for stress than the same mesh with midside nodes.  (But look, Boss! I saved 4 seconds on the solve time!!!)

  Elements Nodes Total
SEQV Solver Runtime
Low-order 18383 4854 0.28744” 177.51 Ksi 6.677 Sec.
High-order 18383 31332 0.32633” 219.46 Ksi 10.951 Sec.




So how many low-order tetras are needed to get the same accuracy this time?   I used the Convergence Tool in Workbench to find out this time. The Convergence tool refines the mesh only for the scoped region of the results plot.  So the resultant mesh looks like this.





  Elements Nodes SEQV Solver Runtime



21.951 Ksi

349.785 Sec.




21.946 Ksi

10.951 Sec.

The last pass took just under 6 minutes to run (349.8 sec). The stress finally gets as high as it is with the high-order elements, but the deflection results are still incorrect because the model was only refined at the hole.  And say it with me, “If the deflection is wrong, then the stress ain’t gonna be right!!!”  So basically I’ve wasted a half an hour getting the wrong solution so that you won’t have to do the same. Just remember, mid-side nodes are your friends. And just like any good friend, take advantage of them when you can!