Distortion and Convergence Problems with Simple Elastic Plate

  • Last Post 18 May 2020
  • Topic Is Solved
mskr posted this 13 May 2020

I have a simple plate made of a linearly elastic material, that is fixed on top and has a force acting on it from the side. I want to have a very soft material and large deformation.

For quicker testing, I used a very coarse mesh.

I need to use fixed time step. I tried out some step sizes.

With step size 0.01 sec, this error occurs instantly:

Element 1 located in Body "SYS\Solid" (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.


Also the solution has not converged. Total Deformation output:

With step size 0.0001 sec, the simulation stops converging at step 167.

The shape has not even much deformed yet. Shown below is Total Deformation of latest result.

With step size 0.00001 sec, it stops converging after step 4238 and still not much deformation.


So I now reach 0.042 real time seconds instead of 0.017, but I have a ten times smaller step size and the simulation took about half an hour instead of ten minutes. It did not seem reasonable to me to keep reducing the step size.

I have Large Deflection turned on.

Please take into account that I am a complete novice and may have set an unphysical material or loading or such a bad mesh that it can not work.

How can I know, how small does the time step have to be?

Are there other ways to improve stability of the simulation?

Can I expect a case like this to simulate one real time second in less than ten minutes on a 2018 AMD Ryzen 6 Core processor?

If the error is in my setup: Can one calculate from the linearly elastic material what force is needed for a certain amount of deflection?

Order By: Standard | Newest | Votes
peteroznewman posted this 14 May 2020

Your elements are way too large!

Set the default element size to 1/2 that size and rerun. Then set it to 1/4 that size and rerun. Compare the results between the two runs.

mskr posted this 14 May 2020

Ok this is 1/2 element size:


Step size 0.01 sec and 0.001 sec: Still high distortion error in first step.

Same goes for 1/4 element size and above step sizes. I don't understand, why the mesh distorts like this.

1/2 element size and step size 0.0001 sec makes a new error appear after step 88:

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.

Could some constraint or measure to account for the non-linearity be missing from my setup?

1/4 element size and step size 0.0001 sec: high distortion error after step 27. Force convergence stopped like this:

I did not try step size 0.00001 sec yet because such a small step cannot be tested quickly anymore.

How can I know, how fine my mesh has to be for transient case and linearly elastic material?

EDIT: For now, the best I can do is simulate with step size 0.00001 sec up to only 0.001 sec real time, but I need much more deformation than what is happening during this time. See this gif: https://imgur.com/a/kjC8WIv. This now uses the direct solver instead of iterative.

EDIT 2: After doing more time steps, the solution stops converging again.

The last image looks like I may need stiffer material in the upper part. Although I am not sure how to do that. Might that be one thing to try?

peteroznewman posted this 14 May 2020

 Thanks for the GIF, that was helpful.

The problem is the combination of the Fixed Support and the straight geometry, which together cause high distortion in the first element attached to the fixed face.  You can resolve this problem by either changing the Fixed Support to allow some deformation to occur there, while still holding the part. That means deleting the Fixed Support and replacing it with a Remote Displacement on that same face.  In the Remote Displacement, set all six constraints to 0. Most importantly, at the bottom of the Details window, on the Behavior line, change the behavior to Deformable.

Another approach is to keep the Fixed Support, but change the shape of your part so that the first fixed element doesn't experience so much deformation. That means a shape like this.

  • Liked by
  • mskr
  • KhizerKhan
mskr posted this 14 May 2020

Thank you too for your support.

Here is my result using your tip with fixed support and altered shape: https://imgur.com/a/NfIDac4

With step size 0.001 sec, I simulated 76 steps until it stops converging. That is a progress as I was only able to achieve that with smaller steps before.

Deformation is happening now at the bottom first, resulting in a smooth bending that I wanted to achieve.

However the deformation is still very small at the time it stops. I hoped for at least a 45 degree angle between the direction of the bottom end and the fixed support. Is there an approach that you would try to achieve that?

Note: I changed the force magnitude to be the function expression "time", to avoid sudden changes in loading. 

EDIT: I also changed the force location to the lower left edge, which was the main reason it looked smooth. When I don't do this, and else have the same settings in above gif, I get a highly distored element error after 200 steps and this result: https://imgur.com/Tp7fsIw. I do not understand why a force acting on the whole left lower face, causes this and it seems like I am non the wiser.

peteroznewman posted this 15 May 2020

Deformations as large as you want are generally not achieved using linear elastic material models.

There are two ways that large deformation is accomplished: Plasticity or Hyperelasticity.

Plasticity is used for metals that get permanently deformed during a large load and stay bent when the load is removed.

Hyperelasticity is for elastomer or rubber compounds that take a large deformation and spring back to the original shape when the load is removed. I think this is what you want. Go into the Engineering Materials database to find some Hyperelastic materials in the Engineering Sources you can try, such as the Elastomer Sample (Mooney-Rivlin). The solver should easily make it to the 45 degree angle you want to achieve.  There are some other settings that help convergence, but first let me know if this is the direction you want to go.

  • Liked by
  • mskr
mskr posted this 18 May 2020

Nice, this explains the problems I faced.

Now, I still wonder where this limitation comes from. Is it from the theory of linear elasticity or rather the mesh-based solver implementation? If it comes from the mesh, alternative solvers might be another option.

Thanks for the other suggestions, but I need to use linear elasticity.

peteroznewman posted this 18 May 2020

You can get 45 degrees of deformation in a linear elastic material model. Here is an example.  The limitation in your model is more about the boundary conditions and the distorted elements caused by high rate of change in the deformation.