I am currently incorporating a fatigue user defined material model (UMAT) within Abaqus to describe the constitutive behavior of a cohesive zone element. I know the required psuedo time (elapsed cycles) in order to effectively run the simulation. I intended to prescribe the corresponding time increment (according to a linear relation between elapsed cycles and simulation time) using the PNEWDT variable.
The problem is that prescribing the PNEWDT variable only has effect when the value is set equal to 1. In this case the initial time increment is used through the whole analysis. If however a smaller value (1) no effect is visible and the standard automatic time incrementation is used, i.e. progressing from the initial time increment to the max. time increment. The Abaqus manual relates this behavior to cases where "automatic time incrementation is not selected", but here it also seems to be the case.
Can anyone point me to the origin of this problem and possibly propose a general solution?
Any help will be much appreciated.
As usual, it is almost impossible to answer this question without seeing the model or at least the error message with which Abaqus aborts.
Many thanks for your replies,
@ Ridha: This seems to result in a fixed time increment, what I want to implement is a user controlled time step (which isn't constant by definition).
@ Martin: For some reason in developing a minimal working example of the UMAT to make the bug finding easier for you I actually made it work somehow. I'll start adding the additional features and routines and will get back to this post with my findings. At least I did find it is genuinely possible.
I do not know why it did not work previously, because also with the added functionality it works like a charm. Thanks again for considering this question.
Am I correct however in thinking that a value of PNEWDT larger than 1.5 no longer has any effect, i.e. that Abaqus will not increase the time incrementation by a factor larger than 1.5?
This is due to the fact that by default 1.5 is the maximum increase in a time increment from one inc to the next. You can change that with solution controls (*controls, parameters=time incrementation, second line, 7th parameter ), but it is rarely worth the bother, I think (the manual agrees...).
Dear Martin and others who might still feel like jumping in,
For some reason a PNEWDT value less than 1 has immediate effect in the first increment, however a value larger than 1 only influences the time increment in the second increment of the step. I can not find a control parameter in the "Keywords Reference Guide" which can make its effect already present in the first increment.
In order to allow you to think along I think this is a good moment to illustrate the intent of my model a little further.
The fatigue model for the user defined cohesive element constitutive behavior should ideally allow the fatigue crack to propagate a whole element within each increment. Which element is to be failed is determined by a global set of routines (uexternaldb, urdfil). The number of cycles required to fail the element is determined using the (stable) crack propagation Paris law (crack extension/cycle) which for example depends on the strain energy release rate within the element. This latter value is determined within the UMAT and consequently a number of cycles required to propagate the crack through the whole element can be derived. In order to efficiently simulate the crack propagation I want to enforce this number of cycles through a corresponding time increment. The amount of cycles is constant for constant crack propagation through a uniform mesh, but if the mesh is non-uniform or if the crack growth is non self-similar for example the required number of cycles can be quite different from one increment to the next. That prescribing the jump in cycles this way is numerically possible (and also very feasible) has already been shown through implementation into an in-house FEM code.
Can I also enforce time increments this explicitly within Abaqus? Please feel free to share your thoughts.
By the way:
Setting the control parameters in the input file as:
-----------------------------------------------------------------------------
*CONTROLS, PARAMETERS=TIME INCREMENTATION
,
,,,,,,2.0
-----------------------------------------------------------------------------
still gives an increase of 1.5 maximum, what am I doing wrong here?
@Steyn
"I can not find a control parameter in the "Keywords Reference Guide" which can make its effect already present in the first increment."
As far as I am aware, this is simply not possible in Abaqus. To increase the time increment, the heuristics of Abaqus demand that convergence was sufficiently good in two consecutive steps.
I don't know why the time increase does not exceed 1,5, probably one of the other parameters is responsible...
Thanks for your replies Martin,
Regarding the time increment I found that changing BOTH the second line, 7th parameter and the third line, 2nd parameter does the trick.
So:
2(7) - D_D, increase factor when two consecutive increments converge in a small number of equilibrium iterations.
3(2) - D_M, maximum time increment increase factor for all cases except dynamic stress analysis and diffusion-dominated processes.
ABAQUS mailing list
https://groups.yahoo.com/group/ABAQUS
http://imechanica.org/
- Badges
- Science topic