Greetings,
First, I want to thank the developing team for the introduction of the monitor graphs. It is much easier now to see how the computation progresses.
Back to the main topic. I want to ask those with experience in the field, how should I understand the drops and peaks of convergence in the same step as in the picture? Notice how between increment 1 and the last 58th, there are drops and increases both in the contacts, displacement and force criteria. My simulation doesn’t suggest anything like a motion over a sharp edge or sudden high deformation.
Does it have to do something with the mesh, the convergence criteria or anything else? Does it make sense to reduce the maximum time increment or the iteration size from 60 to lets say 30?
Thanks in advance 
PS - in the picture I meant to write iteration 1 and iteration 58, not increment.
When it comes to automatic incrementation and convergence criteria, everything is described in the CalculiX documentation and here: Stacked flow plates - model simplification - #26 by FEAnalyst
In short, the two main criteria are:
- residual force < 0.5% of the time average force
- displacement correction < 1% of the max displacement increment
The NR method applies a fraction (increment) of the load and iterates (also updating the stiffness matrix) to find equilibrium within the aforementioned tolerances. Often many iterations are needed to achieve that and if it fails then cutback (increment size reduction) is needed.
Automatic incrementation reduces the increment size when convergence gets worse and increases it when convergence improves. Otherwise, the increment size is kept constant.
2 Likes
Contact introduces severely discontinuous nonlinearity since its state may change rapidly from open to closed and from sticking to slipping (frictional contact is particularly bad for convergence). The NR method often struggles with that and shows the kind of behavior that you observe. It may also indicate contact chattering (erroneous repetitive changes in contact state).
In contact analyses, changes in the number of active contact elements are also monitored by the solver. The goal is to achieve the minimum penetration with the penalty method (penetrating nodes are pushed away) and release contact constraints subjected to tension.
Improving the mesh (and avoiding second-order elements), reducing the contact stiffness (hard contact is usually way too stiff), adjusting the incrementation settings (especially initial increment size) or solver controls (rarely needed) often helps.
When it comes to solver controls, you can safely increase the number of allowed iterations and attemps. Just be careful with adjusting the convergence criteria, it should be done as the last resort.
2 Likes
@FEAnalyst Many thanks for the practical advices. Indeed, reducing the precision from second to first order helped the most in reaching a convergence and dramatically shortening the time for calculation.
What worries me is that the use of first order elements leads to less reliable results overall, doesn’t it? Should I proceed with a submodeling simulation to make a better analysis of the critical parts?
Finally, to be honest, convergence plots (based on the data in the Status and Convergence tabs of the job monitor) are helpful to identify issues such as the aforementioned chattering, but ultimately, it’s crucial to have a closer look at the model’s behavior. You should locate the nodes mentioned as having the highest residual forces or corrections and see what happens with the model during the analysis, especially when it’s diverging.
1 Like
I mean only hexahedral meshes, those can usually consist of first-order elements (possibly C3D8R or C3D8I) if you have enough of them. Of course, not all parts can be hex-meshed and then second-order tetrahedrons are needed even if there’s contact.
Submodeling is a very useful technique to get more accurate results in specific areas of interest, e.g., near joints. Its particularly useful for large assemblies when you want to focus on such selected small regions. But it’s not always needed, proper meshing with local refinement in the global model is usually sufficient.
1 Like
