It’s a matter of convergence - complicated topic but basically you should mainly focus on the changes of the increment size (which are not visible here but in the Status tab) - based on that you can judge whether the model converges well or not. If the increment size decreases and reaches very low values then the convergence is less likely. If it increases and is not so low when compared with step time then the convergence is more likely.
Let’s also clarify the nomenclature. CalculiX uses incremental-iterative Newton-Raphson (NR) method for nonlinear implicit calculations and thus the following terms are used:
- steps - analysis procedures forming part of the loading history - multiple steps can be used in a single simulation to represent its different stages
- increments - load within a step is divided into smaller pieces called increments so that the whole nonlinear equilibrium path can be gradually followed by the solver (for example, an increment of 0.1 s in an analysis with total step time of 1 s means that 10% of load is applied)
- iterations - the solver performs iterations within each increment to find equilibrium (by comparing external and internal forces and calculating the difference between them called residual until it reaches a value lower than the tolerance set for the solver)
- attempts - those are the selections of the increment size - if the solver can’t reach convergence within a current increment then the attempt is considered unsuccessful (marked with U) and the solver can make another attempt by selecting a smaller increment size
The rest of what you see in the job monitor window applies to residuals and corrections. If you want to dig deeper, I recommend the chapter “Equilibrium iterations and convergence in Abaqus/Standard” in Abaqus documentation. There it’s explained much more comprehensively than in CalculiX’s manual.
There are several ways of aiding convergence in nonlinear problems. Usually, nonconvergence is caused by contact, often due to initial rigid body motions occuring before contact can be established. It often helps if you use displacement control instead of load control. In general, you have to make sure that boundary conditions are sufficient and the structure is not underconstrained. More specific tips usually require taking a look at a particular model.
After ensuring good convergence you can try to reduce the time necessary to solve the analysis. Either reduce the mesh density (but perform a convergence study to make sure that the mesh is sufficiently refined) or simplify the model using available assumptions such as symmetry (planar, axial or cyclic), plane stress/strain and so on.