I’m having trouble getting my model to converge when I reduce the Youngs modulus of the material.
The model consists of an elastomer stator with a steel rotor inside of it. I’ve locked the rotation of the rotor and fixed the outside of the stator. I’ve then applied pressure to various cavities that should induce a moment reaction force in the rotor. There is initially a slight interference between the rotor and stator as well.
The model runs and converges as expected when I use a higher modulus, for example 2000MPA. But when I lower it to something more reasonable for rubber, like 20MPA, it fails.
I have also tried with a hyper-elastic model but have had similar failed results.
Does anyone have any suggestions to help the model converge with the lower modulus?
I tired both refining the mesh considerably and changing the surface behavior to linear and still no luck getting it to converge.
I’m not sure that I can swap to a displacement load rather then pressures. I could apply a rotation, but I would still need to have the pressure load in order to have the correct load applied to the elastomer.
I have also attempted to leave the pressure load off completely to test the material, and still can’t get it to converge with a low Youngs Modules.
Is it possible to start the model with a higher modulus and lower it in a second step?
when it has been adjusted, refined mesh and hyper-elastic material type also but still a problem. Probably it’s related to element type due to distortion occurs and volumetric locking. In this case, linear hexahedral with reduced integration (C3D8R) may fit and solvable. Recommended using at least four layer trough thickness since it’s only have one integration points at center.
check the contact status (*Contact file) as it progresses, if the the material is very soft the loading equilibrium changes and makes difficult for the implicit solver to converge, then maybe you have to go explicit. Also you can try first with no friction.
I seem to recall that the contact stiffness is based on the 1st material card in the input deck. If the first material is very stiff compared to the rubber-like material, then that would indicate that a higher contact stiffness is required. There is an old thread about this, but I can’t find it now.
You must find the right balance for your contact stiffness for rubber to metal contact. It is tricky, and it is best to run a few scenarios (surface-2-surface, node-2-surface, mortar contact, etc) to see what converges.
What a clever approach, to split the pressure on each chamber to induce the rotation. Thanks for sharing.
I have managed to run the file with some changes.
-I have remove the thermal effect to isolate the source of problems and be able to progress. That can be added later when everything works smooth.
-Hard contact doesn’t seem to work properly. I’m using elastic.
-Avoid including in the rigid body definition the contact surface. Too many things going on in the same place.
-You need to work on that mesh. I’m using linear elements to speed up the process. I have only reach 50% of final pressure but the rotation is completed.
-Hyperelasticity better later but I have tried Neo Hookean and it works.
C10 3.5868 Mpa
D1 0.0636 1/Mpa
-Solids doesn’t have rotational DOFS.
-I’m constaining
REF 3
ROT 1,2
You can play switching master and slave. I have changed the role and provide a wider supporting surface. I prefer the master to be the surface that moves the less.
