But something strange is happening. When I choose the default solver the models converges easily with and without frictional contact (default settings and hard behaviour). Nevertheless when I change the solver to one of the Iterative solvers there is a huge difference in solution time and convergence behaviour. Please check images below. The solution with friction has much more iterations and even the number of contact elements drops right in the second iteration. Do you have an explanation for this behaviour? Is there something special to pay attention when solving models with frictional contacts and iterative solvers?
My second question is about embedding in bolt connections. I want to investigate bolt connections regarding VDI2230 where emedding should be considered in models. Do you have any advice in doing this in PrePoMax/Calculix? From scratch my first idea was to do a calculation with one step and bolt load to check the deformation in the bolt to achiev this load. Then I restart the simulation with displacement control and in the second step I then substract an incremental of lets say 0,01 mm of the initial value. In ANSYS there is a mixed possibilty with load in the first step and then displacement incrementals in the second step to consider embedding before the general load is applied in the third step. I guess this mixed solution is not possible in PrePoMax/Calculix/Abaqus?
Regarding the first question, I wouldn’t recommend those uncommon solvers. The typically used ones (Pardiso, PaStiX, Spooles - in that order of robustness) are usually sufficient.
I’m not familiar with ANSYS or that VDI 2230 standard but from what I understand, embedding can be used to account for the loss of preload due to surface roughness, right ? CalculiX and Abaqus don’t have such an option but you could simulate it manually as you said. You can have one step with force load and then follow it by a displacement-controlled step. Although it’s usually done in the opposite way in other scenarios - displacement to established contact followed by force. This way you can avoid convergence issues.
Am I right that the 3 solvers you mentioned (Pardiso, PaStiX ans Spooles) are all direct solvers? Therefore I could run out of memory in certain cases with my limited machine.
Yes you are right embedding accounts for a loss in preload due to surface roughness.
Theoretically, iterative solvers may help with large, well-conditioned, blocky solid models (benchmark with a cube/cuboid may confirm that) but in practice, Pardiso is usually the best choice for large models and many threads here and on the CalculiX forum confirm that.
iterative scaling still can be useful for limited hardware and large models, but may not working well in contact analysis compared to PaStiX or Pardiso. Also model with shell element, but shown better for solid element, limited to ~800k equation or ~55k element and ~1300k equation or ~290k element respectively. In early before Pardiso and PaStiX implemented, i have been tested personally on Windows 32bit limited by maximum memory of 3Gb, below another test on 64bit reported from external references.
