Hi,
I am using XFEM framework in abaqus to model crack propagation at the notch region in the CT sample. The model consists of elastic phase inclusions in elastic-plastic metal matrix as shown in Figure 1. The crack propagates through the metal matrix by connecting those inclusions, so only the metal matrix is defined with XFEM enrichment. Initial crack is defined in the model as abaqus XFEM allows only one crack to propagate in an enrichment region. The crack propagates as expected with the influence of the inclusions, but as soon as it approaches one of the inclusions convergence is judged unlikely and simulation fails (figure 2). The inclusion debonds prior to crack approaching them and I am expecting to see crack growth by initiating crack on the other side of the inclusion. To help with the convergence I have change step increments to lower values (10e-15), tolerance, damping factors and general solution controls. I even tried increasing control parameters Rnα and Cnα to larger values to help convergence. But, it only helped slightly as convergence is still bothered at minimum step increment of 1e-15 and the crack cannot pass beyond the inclusion. It seems like the problem failed to converge at the fracture of the last element to connect the crack to the inclusion and also to initiate crack on the other side of the inclusion.
Common warnings in the simulation are:
***WARNING: THE STRAIN INCREMENT HAS EXCEEDED FIFTY TIMES THE STRAIN TO CAUSE
FIRST YIELD AT 8 POINTS
***WARNING: EXCESSIVE DISTORTION AT A TOTAL OF 4 INTEGRATION POINTS IN SOLID
(CONTINUUM) ELEMENTS
***WARNING: THE SYSTEM MATRIX HAS 1 NEGATIVE EIGENVALUES
***NOTE: ELEMENTS ARE DISTORTING EXCESSIVELY. CONVERGENCE IS JUDGED UNLIKELY.
***NOTE: THE SOLUTION APPEARS TO BE DIVERGING. CONVERGENCE IS JUDGED UNLIKELY.
Any of you have experience working on XFEM crack simulation and have idea on the problem I am having I will very much appreciate you effort to help me overcome this problem. Regarding damage criteria in XFEM I am defining as material property in the form of cohesive MAXPS ( also tried MAXPE) and evolution based on displacement.
I think most of the warning messages did not abort the simulation and the error is always TIME INCREMENT REQUIRED IS LESS THAN THE MINIMUM SPECIFIED. which is already quite.
Question to answer is whether your problem is inherently unstable or only numerically non-converging. Here are a few things to think about/check/try:
Is your problem load-controlled? if so, switch to displacement control.
Is any of your materials plastic? If so, check that there is sufficient hardening - ideal plasticity can cause problems.
If possible with XFEM (I'm not sure), switch to dynamic, analysis=quasistatic.
If this is not possible, add some automatic stabilization to your step.
Also check whether the problem persists if you refine the mesh locally where the crack runs.
Dear Martin,
Thank you very much for your suggestions.
I am trying to check whether the problem is unstable or only numerical convergence problem. So I tried to eliminate numerical convergence problem by setting tolerance and solution control parameters to higher values. After increasing those parameters, the force and moment are converging as they are defined with higher tolerance, but now the problem is EXCESSIVE DISTORTION OF ELEMENTS and still fails due to very small time increment requirement.
The experimental test was performed as load controlled and only load data were recorded accurately, so I am using load-controlled problem.
For the plastic properties, it is defined as table data (up to plastic strain =0.3) evaluated from power law expression fitted from the tensile test result. As the stress was higher than UTS at some points, I have slightly change plastic definition by defining power law till UTS point and thereafter adding a perfect plastic line.
Currently, XFEM is not available in abaqus Explicit. I have once tried with an implicit step but could not get much improvement. I will check this option in detail.
With these additional information, could you please help me to identify what may cause such error and such a small time increment.
Many Thanks,
"So I tried to eliminate numerical convergence problem by setting tolerance and solution control parameters to higher values. "
This will usually not suffice even if the problem is numerical. And it is of course highly dangerous because you may actually accept a wrong solution.
"thereafter adding a perfect plastic line."
Try adding more hardening to see whether this stabilizes.
Try also other ways to stabilize the problem (like automatic stabilization for the step).
And switch to displacement-control to see wether this converges, even if this is not what you want in the end. (Although, for most problems, it will be no problem to run the simulation displacmeent-controlled, read out the forces and then compare to experiment.)
Thank you Martin for your answers.
By using higher control parameters I was just trying to check whether that will solve the issue. In case of these changes solving the problem I would be checking accuracy and correctness of the solution. As you mention it seems they are not sufficient to overcome the problem.
The simulation converges with only elastic property defined. With the addition of plastic behaviour, the solution fails to converge. I have tried different material definitions like linear hardening, power law hardening and deformation plasticity. Hardening defined to larger plastic strain seemed to converge slightly more steps. But the problem is that it progress very slowly (increment=1e-12) and also the stress and strain values are observed to be larger than the fracture value at some part of the model.
I have enabled automatic stabilization (with tol=0.05), damping (0.0002) for step and damage stabilization and tolerance, but not much of help till now.
Haven't checked displacement controlled in detail. Tried some simulation but the problem did not converge completely. Need to check in more details.
Thanks,
XFEM is based on linear-elastic fracture mechanics LEFM and this is why it works perfectly in the linear elastic region, you have to change the numbers (trial and error) and trial applying the load using more than one step. you may use the Damage Stabilization Cohesive option when defining your material. a common number to start with would be less than the tolerance by 3 orders of magnitude.
- Badges
- Science topic