Ansys Employee

This is getting too involved for a forum post. You should submit a service request and attach the archive of your workbench model.

I will only add a few more points, some of which are reiterating what I said previously:

  1. Using linear tetra elements is definitely a problem. Set to quadratic.
  2. There is also a message stating that the nonlinear adpative region will not apply because it needs to be scoped to a region with quadratic tetrahedral elements. So switching to midside node elements will allow the adaptive region to work. However, as I stated previous, see if you can get some substeps converged first to see how the model is behaving before using an adaptive region. The model has to behave as expected before you can reasonably apply the adaptive region for later substeps that have too much defrormation to use the original mesh. 
  3. The unconverged solutuon is not reliable. It's usually just junk, so don't take anything from that. Don't try to look at the end time 1 sec. Did it even get one substep converged that you can look at?
  4. Restatement: Your substeps are definitley not enough for a problematic model. As I said in my previous message set a small initial time step as this may get a initial time step to converge and you can view that result to see what's happening. Try 1000 initial substeps, 100 min, and a max of 1e5. If that can't converge the substep, try even more initial substeps. The model would probably take a long time to solve a few substeps and never make it to the end since it's not behaving right. But even if the model is not behaving right you can interrupt the solution after you get a converged substep and then look at a result to see what's happening. Or if it can't converge that 1st substep, you can quickly abort and change something in the setup, instead of waiting all night just to see that no substeps converged.
  5. Restatement: I can not state this enough: large deformation gasket models (hyperelastic materials) may look simple but can be decievably hard to work with. For this reason, you should take a section cut and analyze as 2D model first. Get that to run the full time so that you can understand how the rubber is deforming, and this will help you set up the 3D model if still needed. Many times, you can undestand what you need just from this 2D model, and this will run faster and save you a lot of time.
  6. Some of your contacts appear to have some of the same geometry selections. This may confuse it a bit. Make sure your face selections are unique for each contact. Also, I see you have a frictional contact with zero coefficient. Try setting this to frictionless.
  7. Restatement: Symmetric contacts work better in these kind of analyses. To help convergence, you can also lower the normal stiffness factor, and choose an option for the update stiffness frequency, such as update each iteration, or the agressive setting.

Beyond these suggestions, this is getting too complex for a forum post. You should submit a service request with your model if you need further help. We cannot transfer files through forum posts.