7 Replies Latest reply on Jul 29, 2015 4:07 AM by Stephen White

    Nonlinear Analysis with large displacement and contact

    Raoul Jansen

      Hello,

       

      I am trying to simulate geometry behavior of rubber like material under compression in a 2d nonlinear analysis. I am getting an error that the solver has numerical difficulties (see first appendix). If I suppress the contact sets it will solve completely however the part will interfere with itself. So my assumption is that it has to do with the large deformations in combination with a lot of surface contact. Does anyone have an idea to solve this issue?

       

      Thanks,


      Raoul

        • Re: Nonlinear Analysis with large displacement and contact
          Stephen White

          Hi Raoul,

           

          The time step looks rather large - you are displacing it quite a bit, so if the time step  is too large it wont be able to converge successfully. I modifed the time step to be intiail 0.01 and maximum 0.01 to force the solution step to be smaller and it solves for a bit longer (50%) but the model seems to be buckling in the small fillets. Using

           

          Might I suggest a smaller mesh size around the fillets and self contact on the fillet edges themselves (if you are using 2015) to try and stop this happening;

           

           

          I ran it again and altered the step size once it got towards the 'buckling' area too 0.001 and this has solved a lot further, however there are multiple buckling areas as the solutions progresses, so these need to be dealt with in the same way. This is how far I got it to go (61.8%)

           

           

          So the furst issue was fixed on the leftmost fillet but the next fillet along then buckles;

           

           

          And because there is no contact set on it, the mesh folds in on itself and eventually the solution fails.

           

          So in summary;

           

          1 - Change the time step to fully accommodate the buckling of the filleted areas (I used 0.001 time step)

          2 - Add self contact (if you are using 2015) on the fillets so that when they fold in on themselves they do not simply overlap

          3 - Apply mesh control around the fillets to help the contacts get resolved

          4 - Use the restart option - The first 3mm of displacement dont need a step size of 0.001, so if you run 0 - 0.3 with a step size of 0.01, and then stop the solver, it can be restarted with a smaller step size;

           

           

          5 - If it fails, have a look at the last time step and the strain in that area, this is most likely the area that caused the problem.

           

          I can keep giving it a go, but this should give you enough to have a go with.

           

          Cheers

           

          Steve