Highly Distorted Element Error

  • Last Post 2 weeks ago
  • Topic Is Solved
joepa_2017 posted this 3 weeks ago

I am working on a 2D model that involves applying a thermal condition and large tensile displacement. The thermal condition causes shrinkage and is applied in the first load step. The tensile load is applied in the second load step. I can see that the mesh is adequate for the thermal condition, but it doesn't quite make it to the end of the second load step (it comes very close though). The error that comes up says that an element has become highly distorted. When I look at the element, I see that it is in a curved region.

I am using a nonlinear mechanical physics preference. My elements are triangular and the element order is linear. I have tried refining the mesh many times to make some quite tiny elements at the trouble spot. This has involved refining all of the elements in the model and refining the elements near the distorted element without success, so I'm starting to wonder if refining the model will solve the problem. I also have large large deflection turned on and am using hyperelastic material properties. And, each load step consists of 100 substeps. So, I've considered the things that the error message lists.

To me, it seems like I need to make slight improvements to my mesh. And metaphorically speaking, I'd like to learn to fish rather than just be given a fish since this is an error I've encountered a few times. I'm wondering if there are general tips that can help with meshing issues involving highly distorted elements or even if you can point me to a good source for learning more advanced meshing techniques. That way, I can have a better sense for troubleshooting meshing issues in future analyses.


Order By: Standard | Newest | Votes
peteroznewman posted this 3 weeks ago

Have you tried Reduced Integration on the elements with the hyperelastic material? Here is a post from an older version of ANSYS. It is done differently in 19.2.

  • Liked by
  • joepa_2017
joepa_2017 posted this 3 weeks ago

I have not tried Reduced Integration on the elements. Is it true that it only applies for hexahedral elements? I read that in the manual for 17.2, and I am working with a 2D model.

peteroznewman posted this 3 weeks ago

If it said so in the 17.2 manual, then Reduced Integration doesn't apply to 2D, I didn't look that up to confirm.

When you say each load step consists of 100 substeps. Do you have Auto Time Stepping Off or On? 

Another suggestion: continue increasing the substeps with Auto Time Stepping On. Put Initial Substeps at 1000 and Minimum Substeps at 1000 and see if that helps.


sathya posted this 3 weeks ago

Hi, If it involved in contact regions make sure the contact settings are correct. If it is on part model,as peter suggested play with Substep.If you are not sure of the Sub steps to be defined and only interested at the result of final time , then keep minimum number of sub step as 100, initial number of sub step as 500 and maximum number of sub step as 1000. Can you share the convergence plots?

  • Liked by
  • peteroznewman
joepa_2017 posted this 3 weeks ago

I tried changing substeps to initial number of substeps as 1000, minimum number of substeps as 1000, and maximum number of substeps as 5000. It still hit the error at about the same point. It looks like it may be possible to use reduced integration after all (the B-bar method with plane 182 elements). I will see if I can put up some convergence plots.

peteroznewman posted this 3 weeks ago

Under Solution Information, make sure to type a non-zero number, say 3 or more, for Newton-Raphson Residual Plots. When the convergence fails, these plots are helpful to show where there is a force imbalance.

These plots are more useful when the convergence fails due to insufficiently small elements, not so much for highly distorted elements.

Also show us the mesh and the boundary conditions. I had examples where the BC could be redefined to remove the highly distorted element error.

joepa_2017 posted this 3 weeks ago

I still need to re-run the simulation. But I am curious, what kind of BC's could be redefined to remove the error? I am only using displacement boundary conditions. Is there another way to redefine a displacement BC?

peteroznewman posted this 3 weeks ago

Fixed support is often used on a flat face of an object when what might be more appropriate is a remote displacement that allows small rotations to occur. This is often seen in 3-point beam bending test simulations.

joepa_2017 posted this 2 weeks ago

Peter, I got around to trying reduced integration, and that gave me a solution without any highly distorted elements occurring. I was wrong about the reduced integration on 2D elements. It is listed in the keyopts for plane182, so I followed the steps from the link you provided in your first answer. I also changed to auto time stepping as suggested by Sathya. That didn't work until I used reduced integration, so reduced integration definitely helped get to a solution here. I have another question that I'd like to resolve, but I'll make a separate post. Thanks!