Learning Forum

[Nooka Susmitha]

Hi, I am trying to perform compression test upto to a certain percentage of strain. My material is ABS and using bilinear material model. I am doing static structural analysis.
These are the errors I am encountering:
1. "The solver engine was unable to converge on a solution for the nonlinear problem as constrained.  Please see the Troubleshooting section of the Help System for more information."
2. "Element 31 located in Body "Solid Body 1(External Model)" (and maybe other elements) has become highly distorted.  You may select the offending object and/or geometry via RMB on this warning in the Messages window.  Excessive distortion of elements is usually a symptom indicating the need for corrective action elsewhere.  Try incrementing the load more slowly (increase the number of substeps or decrease the time step size).  You may need to improve your mesh to obtain elements with better aspect ratios.  Also consider the behavior of materials, contact pairs, and/or constraint equations.  If this message appears in the first iteration of first substep, be sure to perform element shape checking. Named Selections for the offending element can be created via the Identify Element Violations property on the Solution Information Object."


And following are the warnings:
1. The solution failed to solve completely at all time points. Restart points are available to continue the analysis. 
2. One or more objects may have lost some scoping attachments during the geometry update. You can identify these tree objects by activating the Scoping Wizard in the Selection Toolbar, or by filtering the tree using the Scoping option set to Partial.


Earlier I tried my increasing the no.of sub- steps. But still I got the same error.
I have attached the screenshots of my simulations.

[Nooka Susmitha]

Remaining Screenshots.

[peteroznewman]

Change the Initial and Minimum Substeps to 100 and the Maximum Substeps to 1000 and solve.  Does the first substep converge?  If not add a zero to the end of each of those and try to solve again.  If the solution still fails on the first substep, there is something wrong with the model.  It is helpful to type a 3 or 4 into the Newton-Raphson Residuals box and a 1 in the Identify Element Violations box.

Assuming the first substep converges, it is likely that the solution will fail to converge again at a later time.  When that happens, show the Newton-Raphson Force Residual Convergence Plot under the Solution Information folder.

[Nooka Susmitha]

I tried but the solver is really taking 15hrs and still the simulation is 30% completed but have not got any errors. I tried the same settings for a single unit cell and got the results thank you for helping me with that..

Can you suggest me any way to speed up my simulation process.
My laptop specs: 8GB Ram, i5 processor and i have set 4 cores in ANSYS Licensed version.

Please help me out.

[peteroznewman]

If you followed my advice and typed a number for the Newton Raphson Residuals, there are plots to look at under the Solution Information folder. They show were the solver is struggling to find a force equilibrium. Usually, making the elements smaller in the neighborhood of the peak values of the Newton Raphson Residual will help the solver to converge.

The structure has a thin wall compared with the overall size. You can reduce solution time if you replace the solid model of the structure with a midsurface model.  Check the Solution Output to see if the solver is running incore or out-of-core memory. If it is the latter, then installing more RAM in your computer will reduce solution time.

[Nooka Susmitha]

I have tried to run the simulation in different laptop which has higher no.of cores available than mine and then the simulation ran succesfully. Thanks a lot!
Instead of importing a solid model I assigned thickness to a shell structure thinking that it would reduce the meshing and solving time.
If I want to assign thickness of 0.5mm, should I increase the layers? if not after meshing each element seems like a cuboid and I wonder should I consider any ratio while assigning thickness to a shell structure?  
If I have to increase the layers please tell me where can I find that option ins ANSYS. I worked in prepomax but did not find the option in ANSYS. Also please tell me about the ratio of the width and height of element, whether should I consider that strictly (Incase if it wont give accurate results)

[peteroznewman]

It is much better to have a surface to get a shell mesh and assign a thickness.  The shell element calculates stress through the thickness internally and uses a default number of integration points through the thickness. You would only need to increase the number of integration points if you were doing something like a nonlinear materal model with plasticity for example. Integration points in a shell element are like layers of solid elements, but much more efficient in terms of solution time.

Ansys will keep track of the element thickness to curvature ratio and issue a warning if the ratio exceeds a threshold.  If you see that warning, you should reduce the size of the elements so there is less curvature over each element. I don't think there is a warning about element width to thickness.

[Nooka Susmitha]

Where can I exactly change the no. of integration points? I am doing my analysis in ANSYS static structural.