Low modulus linear elastic material convergence issues

[bebme]

Hello,
I am trying to run a 2D static contact analysis between a cylindrical rigid material and a flat low modulus linear elastic material (20 MPa) subjected to a fairly large force (2000 N). I have solved the excessive distorted element problems but am now having trouble with solution convergence. I can get it to run to completion work with a 200 MPa modulus but the more I lower the modulus, the harder it is to get the model to converge. Now my message file states that the force equilibrium have not been reached mainly due to the displacement correction not being acceptable (default settings). I have tried decreasing the step size and increasing the cutback limit. Has anybody else had similar problems and determined ways to solve them?

 

[bebme]

More Info -
It is a incompressible material and plain strain 2D

 

[rstupplebeen]

I deal with materials that are around 1MPa along side 1500MPa materials regularly and for these sorts of problems displacement control is usually more robust. You can dial the step size to get the desired force.

Adaptive remeshing may also be worthwhile. I would suggest running at the 200MPa do a couple of cycles of adaptive then try to lower the modulus.

What type of elements are you using? Can you post a picture of the mesh?

I hope this helps.



Rob Stupplebeen

 

[bebme]

Thanks Rob for the response. I have attached my undeformed mesh. I am using CPE8RH elements.

 

[bebme]

Here is my deformed mesh also

 

[dw21]

Hi there,

1. Are you using strict enforcement of your contact constraints? If so, you can try to use the penalty method instead.

2. Did you define surface-to-surface or node-surface contact? Try the former.

3. Frictionless contact?

4. Purely elastic, or elastic-plastic material model? Excessive yielding can cause convergence problems.

AL

 

[bebme]

Hello dw21,
Thank you for your response. I will try the penalty contact method. I was using surface-surface frictionless contact before and my material model is purely elastic.

I am also looking into adaptive meshing. In order to remesh, how would I import my deformed part for remeshing using ABAQUS/CAE after I have my other restart files available? Thanks


RS

 

[bebme]

Yo rstupplebeen,
What kind of loads and part shapes were you using to load your material? Also what stresses and strains did you obtain when running your low modulus materials (<100 MPa)? Also, what do you mean when you say dial down the step size? Why wouldn't displacement control be the same as force control?
Thanks

 

[rstupplebeen]

1. I design surgical equipment for cataract surgery. At the end is a link to a video of one of our products. The first one has no blood the second one does.
2. We have strains much higher than 50%.
3. I usually allow the step size to go down to 1e-8 and then decide if I need to kill an analysis from there. Depending on your loading this may be a better starting point than the default.
4. Displacement controlled tends to be more stable. Before contact occurs an infinitely small force will cause an infinite displacement and leads to convergence issues. Once contact occurs then there is not that much difference however.
5. A larger mesh size might help you out however be careful to do a convergence check. Through the thickness it appears that there is a very thin layer of elements. That is probably your issue.

I hope this helps.

Rob Stupplebeen

http://video.google.com/videosearch...enUS253US253&um=1&ie=UTF-8&sa=N&hl=en&tab=wv#

http://video.google.com/videosearch...-8&sa=N&hl=en&tab=wv#q=crystalens&hl=en&emb=0

Rob Stupplebeen