Hi everyone, currently I’m working on a project which requires to know the value of the tensions generated by the contact between a flat punch with rounded edges and a flat surface and I can’t get a value which is aligned with the analytic results found here: The influence of rounded edges on indentation by a flat punch
I’m working with a 2D plane deformation model made of 3 pieces. On the top there is a holder, which is in contact with the punch, constrained on the y-axis. The bottom one has a force applied to it which represents the preload of a bolt and it represents the flat surface. The punch material is S255, for the other two pieces we have 18CrMo4. On both side surfaces there is a symmetry constraint. Slave contact surfaces are assigned to the punch.
The model converges without any problem but, has I said, I’m not satisfied with the results values.
In particular the tensions and cpress values varies with the contact stiffness and so I’m not sure if what I’m seeing is correct especially since they are far of in respect to the analytical ones. Do some of you have any tips on how to select the correct K value?
I also did a sensitivity study on the contact stiffness in relation to cpress hoping to find the right K value. There is convergence for the value of the mid node but the node with the maximum pressure does not seem to converge. I though this was a mesh problem but I pushed the min mesh dimension to 0.05mm and the problem is still there (punch width is 8mm), since the simulation time is still very quick I could go lower.
Looking at various tutorial the hard contact was used but in my case this would produce an irrealistic pressure distribution with a peak on the contact edges of over 4000MPa.
Looking at the normalised pressure distribution shape it seems ok but the values are of in respect to the analytical solution (fig.2 reference paper). I don’t remember for which K value this graph is generated.
Is it true scale or automatically scaled deformation ? Check the contact outputs - not just CPRESS, but also COPEN which shows where contact is active. You could also request output of contact elements.
You could also try with mortar contact, it should be more accurate than penalty contact, but may cause convergence issues. And it requires 3D elements, so you would have to extrude this 2D model to a single layer of 3D solid elements. PaStiX may work better than Pardiso in this case.
Surface-to-surface contact may show this kind of behavior due to how contact is enforced in an averaged sense.
In CalculiX, 2D elements have many limitations and issues/bugs, so it’s often better to extrude them to a single or more layers of 3D solid elements. One layer here will still be almost as efficient as a 2D model.
Mortar contact uses Lagrange multipliers, can simulate true hard contact and might be a good choice when accurate contact results are needed. Poor convergence is the biggest disadvantage, but it should be better in CalculiX 2.23 (you may need to change the solver binary because PrePoMax still uses ccx 2.22).
For penalty contact, you could also try exponential or even tabular definition if you need more control over the pressure-overclosure relationship.
The paper evaluates both frictionless and frictional contact (partial slip and full sliding), but the model here seems to be purely hertzian contact in the normal direction.
Might be worth discussing with the CalculiX team to be sure. Btw. Abaqus also has CSTATUS that directly shows the state of contact - sticking, slipping or open. And you can extend the range up to which COPEN is calculated.
