Hello everyone, I was trying a very simple model in order to understand if perfectly plastic material model works correctly. I made an aluminum (E = 69000MPa) tensile specimen adopting symmetry on middle planes, applied 2000N force and simulated it using elastic material as well as elasto-plastic perfectly plastic material, setting an arbitrary yield stress at 20 MPa:
Elastic Material
The model works without any issue, delivering stress results on the middle section in accord with theory (2000N / 19.5mm^2 = 102.65 MPa)
Elasto-Plastic, perfectly plastic material
In this case, the maximum stress is slightly higher than the 20 MPa: the difference can be attributed to interpolation errors from integration points to nodes. The issue is that the model fails at around 20% of solution: the deformation is still very limited, and I really don’t understand why, since the mesh is quite fine and there are no contacts or high deformations involved:
You don’t need two points to define perfect plasticity, it can be just yield stress vs 0 plastic strain. The solver will extrapolate it as a constant yield stress value.
The thing is that perfect plasticity is bad for convergence when a significant part of the model yields and it should often be avoided because of that. In fact, it’s particularly bad for convergence when combined with Nlgeom and tension. Not only in CalculiX, it’s the same e.g. in Abaqus. One way to aid the convergence in such cases (apart from adding some hardening) is to replace force load with prescribed displacement.
Thank you very much for the tip. I know that imposing displacement would help: I made this simple model to understand why another (more complex) one, where contacts are involved, had the same problem. In that case displacement is imposed but I didn’t get convergence anyway. I’ll give a try with some hardening to see if situation improves
With a bar in tension that has a perfectly plastic material, any additional stress (load) above the yield point cannot be supported by the cross-section, because by definition the material has zero stiffness for that additional stress.
Your model is exhibiting exactly the correct behavior: at around 20% of the load (~20 MPa), the cross section has completely yielded and has no additional stiffness to support the load further. Therefore it does not and can not converge.
