Simulating compression of a silicone subject

  • Last Post 29 April 2020
aa02068 posted this 22 April 2020


I hope this finds you well.

I am attempting to simulate the compression of a silicone test subject. The silicone subject is cylindrical in shape, 50mm tall with a fillet of 15mm and a radius of 45mm. 

The model can be seen below:

I am using pure penalty contact, nodal-normal from target. 

I am solving a 30mm lubricated compression in 40 steps.

Here are the settings I am using:

simulation settings

I have attempted to use other hyperelastic materials to simulate such as Mooney-rivlin 3 parameters and Yeoh 1st order, however the simulation fails at 12 steps.

There is no specific error that I am receiving. Instead in the solution output I am getting a message saying the solution failed to converge.

I have attempted to use higher order elements but that makes the solution fail earlier. I've attempted to refine the mesh of both the plates and the silicone subject respectively with no change in the output.

I have attached the archive of the project.

Attached Files

Order By: Standard | Newest | Votes
peteroznewman posted this 22 April 2020

I have not looked at your model, but you can download an elastomer model here.

Pay attention to the Command Object under the Surface in the Geometry branch of the Outline.

Copy those commands and use them on your model.  It has two keyops that help hyperelastic materials to converge.  Suppress them and see how far the solution gets without them!

Click on the Geometry branch. In the Details window is Element Control. Set that to Manual as I have done.


aa02068 posted this 23 April 2020

Thank you very much Peteroznewman. 

I have applied the keyops as you suggested and am progressing further than without. 

At the moment, the solution is failing to converge at 23 steps out of the 40 steps I have selected.

I believe it is due to my PC not containing enough VRAM to run the simulation as I have received an error pertaining to that, although I am not certain.

peteroznewman posted this 23 April 2020

Getting a memory error is not failing to converge. Let's be clear on what is going wrong. How much RAM do you have?

Attach a new Archive of the model and I will run it on a computer with more RAM.  Say what version of ANSYS you are using.

aa02068 posted this 24 April 2020

I am using a laptop with 512MB of VRAM and am using Ansys Workbench 2020.

Thank you for offering to run the simulation. Please find it attached.


Attached Files

peteroznewman posted this 24 April 2020


I changed the Solve Process Settings to use less memory.

But the error you have is not due to memory, it is due to Element Distortion.

 Type a 1, 2 or 3 into the highlighted box below.

 The problem element is the top right corner.

The corrective action is to make a small radius on the top corner.

  • Liked by
  • aa02068
aa02068 posted this 28 April 2020

Thank you PeterNewman

I rounded the edge by 2mm and refined the mesh on the plates doing the compression and ran the simulation to completion for the majority of the hyperelastic models I am testing.

At the moment, I'm having trouble running Yeoh 2nd and 3rd order models which run to 33 and 37 steps respectively. 

I'm incrementing the mesh until the majority of the element quality is surrounding 1.0 on the element quality graph, but the mesh seems to fail in places with high element quality.

peteroznewman posted this 29 April 2020

Do you have material experimental measurements on standard tests for the hyperelastic materials?

What value of strain do your measurements go out to?

What value of strain does the Yeoh 2nd and 3rd order models have a good fit to the experimental data?

What value of strain does the model go to?