Tied Contacts making overly stiff simulation results

[tsims]

Hello everyone,

My group and I are working on a breast cancer simulation project, Originally we were using a single model with a compartments for skin and adipose tissue to run our simulations, but generating these meshes result in ~1.5 million elements, which results in simulations that take quite a long time to run. As a result of this, we wanted to try using different meshes for the adipose tissue and using a tied contact between the two meshes. This results in meshes that are much more reasonable, ~500k elements. However, when we do this we get very different results even using the same material properties, int the contact problem the skin ends up being too stiff.

The all in one mesh:
Screenshot 2020-10-28 130316.png

The two meshes with a tied contact:
Screenshot 2020-10-28 125350.png

We are wondering if there is some configuration setting we set up incorrectly, or if there is something we aren't accounting for? These two simulations are the same except for the tied contact.

Thanks!

[ateshian]

Hi,

There are three tied interfaces for elastic materials in FEBio, which one are you using? What are your contact settings?

Best,

Gerard

[tsims]

Hi!

We are using a tied node-on-facet contact. I added our parameters below if that would help as well. The tissue makes the primary surface and the skin has the secondary surface.

Screenshot 2020-10-29 093629.png

[ateshian]

Hi,

Would you mind trying the tied-elastic contact interface instead? Please turn on auto-penalty, use a penalty of 100 (like you did before), and try it with two-pass. If it fails, try it with single-pass and/or reduce the penalty to 10. Let me know if you get more reasonable results in that case. Remember to use a non-symmetric stiffness matrix for the solver (and Broyden or full-Newton iterations), which gives better convergence for this tied-elastic interface.

Best,

Gerard

[tsims]

Hi Gerard,

Thank you so much for your help! It is very much appreciated.
I just ran two simulations with the settings you suggested, There wasn't much of a difference in the first simulation with two-pass, and with single-pass, the simulation resulted in an error about 93% through. (images below)
Do you have any idea what we could be doing wrong?

two-pass, penalty 100:
unknown.png

one-pass penalty 10:
unknown2.png

Thanks again
~Tres

[ateshian]

Hi Tres,

Thanks for trying this out. Would you please clarify what do you feel is not calculated properly in the tied-elastic analysis with two-pass and penalty=100? You said "There wasn't much of a difference in the first simulation with two-pass", do you mean in comparison to the results of the node-on-facet tied contact? If so, are you still concerned with "...when we do this we get very different results even using the same material properties, int the contact problem the skin ends up being too stiff."? If the skin ends up being too stiff, it could be because you coarsened the mesh and ended up with fewer elements through the skin stiffness, is that the case? Are you using tet4 elements with an uncoupled material? If so, you may be getting mesh locking. Please consider using tet10 elements instead.

Best,

Gerard

[Fluvio]

Gerard,

Thank you for following up! Discussing earlier with Tres we realized that we wrote this a little vague. Let me shed some light onto what we are expecting.

First, a few weeks back I posted on applying contact on folding surfaces (figures below). I followed your advice and we got some convergence, but the number of equations for a 1.5M tet mesh + the small search distance makes the simulation time very very long.

P69_STATE0.PNG P69_STATE1.PNG

In the meantime, Tres has been looking into ways of reducing the tet count on the original mesh. In the original model, the two compartments shared the nodes and the facets (we make this mesh using Cleaver2). One of the initial thoughts was to separate the skin from the adipose tissue and use a tied-contact condition to simulate their interaction. Following this approach, we get a mesh of 500K elements and, yes, they are all tet4 (...we will look into tet10 and mesh-locking next). After simulating with the same stiffness values for all compartments, Tres' model did not deform like the original model.