Rigid body contact

[helentan]

Hi everyone,

I have a question regarding rigid body contact. I have a biphasic solid that is in contact with two rigid bodies (top and bottom plate). I am trying to simulate unconfined compression of the biphasic solid. I want to have frictionless contact between the solid and the rigid bodies and so I have been using rigid contacts. The rigid constraints for my top plate is fixed in Rx, Ry, Rz, Ux and Uy and I have prescribed displacement for Uz. On the other hand, my bottom plate is fixed in all rotations and displacements. However, I observed that there is bulging of my biphasic solid and the results seem to suggest a tied contact between my solid and the rigid bodies.

My question is have I chosen the correct contact for my problem? If not, what is your suggestions of contact that I should be using?

Hope to hear from you soon. Thank you very much!


Best regards,
Helen Tan

[brandonz]

Hi Helen,

Rigid contact is used to connect a rigid body to a deformable mesh, so you are correct in that you basically have tied contact. For unconfined compression between rigid plates and a biphasic solid, you would want to use something like 'sliding-elastic' with the friction coefficient set to 0. This will give the desired frictionless contact.

As a side note, you will need to apply symmetry constraints for this to work. If you try to compress an unconstrained cylinder between two frictionless platens, it will just move laterally (which is exactly what would happen physically if you could somehow have frictionless contact). A quarter model (or wedge) would allow you to apply symmetry constraints to keep the biphasic solid from jumping laterally during compression.

Brandon

[helentan]

Hi Brandon,

Thank you for your reply! I understand now. Following your suggestions, I tried implementing sliding elastic contact for my model, but I'm not sure why I am getting a negative jacobian error now. Would it be possible for you to point out to me if I'm implementing the contact correctly?

Thank you in advance!

Best regards,
Helen

[brandonz]

Hi Helen,

As a general rule, when you have rigid-on-deformable contact, your primary surface should always be the deformable one. Another general rule is that your primary surface should be the one with the finer mesh, as you establish contact from integration points on the primary surface. Both of your contact interfaces have the rigid surface as the primary. I switched your primary/secondary surface designations and the model runs fine, although the contact enforcement is poor and the fluid pressure looks wrong.

It turns out you accidentally selected a number of nodes on the bottom surface of the cylinder and applied a zero fluid pressure boundary condition here as well. Once I corrected that, turned on auto-penalty, and changed your solver scheme to full Newton (setting max_ups=0 in the solver), your model runs much better.

Brandon

[helentan]

Hi Brandon,

Thank you so much for your help! I get it now!

Helen