For an university project, I'm simulating the behavior of an inflatable actuator made of silicone. I use solution 601,106. The simulation setup is done in NX10. The material is hyperelastic and the large strain option is activated. The model is meshed using CHEXA20 elements. There are some glue and contact regions.
In my simulation, I apply a linearly increasing pressure load to chambers inside the structure, which will cause the actuator to bend in one direction. However, I have trouble reaching convergance as soon as a certain level of load is reached. In the beginning, the energy convergance ratio curve has a negative slope and smoothly decreases. After about 5 to 10 iterations however, the slope will increase until it is positive. Then, the solution doesn't diverge and abort, but insted the curve will flatten and continiue with zero slope indefinitely. The longest run I did was 400 iterations, after which it was still flat. I've attached a screenshot of this.
I tried changing the element types (hexa and tetra), number of nodes and mesh density, but this behavior is consistend. I have no idea what could cause this, whether the geometry of the part contains some instability at high load, meshing or boundary condition or solver options are incorrect.
I'd appreciate any help or hints! I've also attached the model files.
Solved! Go to Solution.
I will try first to look at the unconverged solution (plots, animation,...) to figure out what's going wrong.
Also check your material defintions (curves). For nonlinear material simulaitons, the solver will follow the material curve. Try to use at the begining simple material models.
Always start with simple models and add complexity gradually (I'll start without contact at the beginning).
I think non linear behavior is realy complex and the numerical solution often only describe special parts of the problem.
I had for instance comparable problems everytime at the same deformation conture in former model. Afterwards I realized that it was a buckling problem with a leap in internal energy and deformation. My selected solution scheme in SOL601 didn't suit to determine that part of the problem. I can't remember which.
I also think that there are internal limitations for defomation of elements regardless of using hyperelastic material or not.
Check your problem with this recommendations.
Thanks for the suggestions. I still don't know what exatcly causes this behavior, while buckling sounds reasonable, I would expect it to cause divergence, and not this behavior. I did however manage to solve this particular problem. As shown in the original post, the error did not reduce until convergence, but rather stayed at a certain level. By using line-searches in the solution this does not happen because the error is reduced in an additional step after each iteration of the solver. So line search did improve convergence behavior enough to faciliate the solution of the model.