I am running a modal analyis, where a component is placed over a plate which is fixed.
When I am seeing the results, the component is moving into the fixed plate(check the attached gif). How to avoid that, since it is not going to happen in the real time. I tried surface to surface contact but it is not solving the problem. Gluing works but that is not the real simulation.
How to solve this?
the nature of an eigenfrequency analysis is that is always performed about the current state in a linearized sense and that the frequencies are independent from the amplitude.
This means for your case: A contact situation that is "open" at the start of the eigenfrequency analysis will remain open, and a contact situation that is "closed" (glued contact or regular contact) will remain closed.
This is what you see: You defined contact, but this contact was open when you started the eigenfrequency analysis. This means that the contact is not taken into account and penetrations are possible (especially that the result is amplitude independent).
The only way to avoid that is to chose an analysis in the time domain (not eigenfrequency) and include contact, but that is magnitudes more CPU intensive than an eigenfrequency analysis.
Actually, I would use a STATSUB to have the contact surface taken into account, then run modes on the "contacted" parts... Works very nicely and it's very easily done in NX CAE as the SOL103 sim solution already has a branch for preload...