The fixed support must hold down the body it is set on at least. I would not trust the result from the modal analysis it if shows all bodies moving, and you should diagnose by other means. Do both of the zero modes show the same behavior?
I am confused about the simplified model. It seems to show 2 bodies, but you have frictional contact set up on what looks to be all surfaces of one body where there are no other bodies contacting. Are the other bodies just hidden? Or are they suppressed?
Are there any substeps converged? If even one substep is converged you can view a deformation result to see what is happening. You may be able to get a converged substep by specifying a very small initial time step, and then view its behavior. Also, set some nonzero value for newton raphson residuals, and view the problem locations.
I do not know the mesh sizes you have used but you may need to set some smaller mesh sizes.
The noninear adaptive region can be tricky to use and will make convergence problematic if not understood and applied well. Try it without the adaptive region first. You may get some converged substeps and you can view the model behavior at a time far before your end time. You can make sute the model is behaving properly for a time before the deformation gets too large, causing high element distortion error and requiring a remesh.
For the nonlinear adpative region, you need a body with enough bulk volume. Thin bodies may not allow enough room to refine the mesh. Your model looks to have thin bodies. Have it remesh early and often, before the body gets too deformed, or else it may not remesh with an acceptable quality. The purpose of nonlinear adaptive region is to repair a distorted mesh in order to overcome convergence problems caused by the distortion. It is effective only when the mesh distortion is caused by a large, nonuniform deformation. Nonlinear adaptive region cannot help if divergence occurs for any other reason such as unstable material, unstable structures, or numerical instabilities.
Check to see if your hyperelastic material properties are a cause of the problem. Choose a simpler material model to see if convergence is easy and the model behaves correctly. You could try the neoprene rubber material from the hyperelastic materials library.
Also, consider taking a section cut through the model and creating surfaces to analyze in 2D first. Rubber gaskets with high deformation can be very difficult models to get to converge and behave correctly. Make sure you know how to get it to run and behave reasonably in a 2D model first. 2D models have a quick turnaround time to run and make changes for another run. Symmetric contacts work better in these kind of analyses. You can lower the normal stiffness factor, and choose an option for the update stiffness frequency, such as update each iteration, or the agressive setting.
You are navigating away from the AIS Discovery experience