Hello,
I want to arrange a crack propagation in a screw thread (s. picture). Therefor I use two dimensional axissymmetric elements in Abaqus 6.12-3 (it is the first version, that allows XFEM in axissymmetric models). The boundaries of the screw thread are on the one hand the symmetry axis, on the other hand the contact to a nut thread. Thus, there are two nonlinear problems: 1.) the contact problem and 2.) the XFEM crack growth.
1.) Arranging the analysis of the contact problem without crack growth works thoroughly.
2.) The XFEM crack propagation itself also works, when there is no contact (the screw thread is hold at the bottom). But it just works with problems (after a few little propagation steps, the analysis stops with the error:"ERROR: TOO MANY ATTEMPTS MADE FOR THIS INCREMENT"). The problem is that the tolerance f is exceeded.
3.) The connection of the XFEM crack growth with the contact is not possible. The analysis stops with the warning:"WARNING: DISPLACEMENT INCREMENT FOR CONTACT IS TOO BIG.". There is of course an expansion of the first carrying pitch of screw thread, but this condition I cannot change.
Has someone an idea, what I can do? How can I increase the number of attempts of an not working increment in CAE?I read, that the standart number is 5, but that is much to less. The minimum increment size is less enough (1e-12).
Greets,
Thomas
Go to Step>solution controls turn on default values and change IA = 5 to 20 in the time incrementation tab this will work
Yes, this function I found in the meantime. Thank you for help. The crack propagation itself works now fantastic for case 2.) (in just the screw thread).
With connection to the nut thread, there is still the problem achieving a convergence. I get now the error message:"There are 2 unconnected regions in the model", although it works fantastic without XFEM crack.
The steps are small enough 1.e-012 and IA=50.
What could be the solution? I have no idea.
Is it generally possible to use XFEM crack propagation in connection withcontact problems? I think, nothing should argue against.
you can ofcourse use xfem in connection to complex contact problems and contact has nothing to do with damage since contact would just compute and tansfer the forced to the node for strain calculations.
2 unconnected regions - is it an error or warning? i think its warning and you can leave it.
That sounds very good. The contact conditions are just between screw thread and nut thread and therefore just something like a boundary condition. There is of course no load in the crack flanks. I think, first the version 6.14 can handle the problems with crack flanks and crack tip under pressure.
In the message area, I get the message:
"Error in job Erstanalyse: Time increment required is less than the minimum specified
Job Erstanalyse: Abaqus/Standard aborted due to errors." ==> I have meshed very fine and the minimum increment step is in the meanwhile 1.e-020.
In the msg-file, I get several warnings:
***WARNING: THERE ARE 2 UNCONNECTED REGIONS IN THE MODEL. (it is obviously, how you said, just a warning)
***WARNING: SOLVER PROBLEM. NUMERICAL SINGULARITY WHEN PROCESSING NODE
SCHRAUBE-1.469 D.O.F. 2 RATIO = 13.4067E+12 .
***WARNING: DISPLACEMENT INCREMENT FOR CONTACT IS TOO BIG. (in the visualization, the nut "flies" in the opposite direction away. However, the direction of the load is correct. Without crack, the contact problem is solved correctly.)
***WARNING: THERE IS ZERO FORCE EVERYWHERE IN THE MODEL BASED ON THE DEFAULT
CRITERION. PLEASE CHECK THE VALUE OF THE AVERAGE FORCE DURING THE
CURRENT ITERATION TO VERIFY THAT THE FORCE IS SMALL ENOUGH TO BE
TREATED AS ZERO. IF NOT, PLEASE USE THE SOLUTION CONTROLS TO RESET
THE CRITERION FOR ZERO FORCE.
TIME INCREMENT MAY NOW INCREASE TO 4.336E-19
***ERROR: TIME INCREMENT REQUIRED IS LESS THAN THE MINIMUM SPECIFIED
==> when the minimum increment size is further decreased (1.e-100), I get:
***ERROR: SYSTEM ERROR IN TIMEUP. DTIME=ZERO
In other forums, some people say, the mesh is too fine (I cannot imagine). Others say, the minimum increment step is too low, that also stumps me.
hi
this videos can help
1/ https://www.youtube.com/watch?v=hleGKlOAeK0
2/ https://youtu.be/eEtVxAhExJA
Thomas Havelka have you solve your error:
ERROR: SYSTEM ERROR IN TIMEUP. DTIME=ZERO???
I have the same problem as you, and I dont know how to solve it.
I have been looking in the internet and wasn't able to find any reliable information about this.
Best regards, Ricardo Dias
The problem was in my case that I modeled the crack flanks not very precisely. Some of them were not in contact in the initial step and had no plane contact at the beginning. After modelling the parts again, the problem could be solved with help of the advices in Researchgate (i. e. increase IA up to 50 like above).
I don't know, why it didn't worked before. Actually, the calculation should have runned through nonetheless. Maybe, there were other problems in the model. Have you checked a simple model like the on in the videos of Brahami Abdessamad?
Unfortunately, I couldn't solve the problem of the determination of the stress intensity factors with XFEM. Therefore, I went for the typical solution with contour integral. For predicting the path, I took FRANC2D. My goal was the prediction of the life expectancy of a structure not just the path. If you find a solution of extracting the SIFs with Abaqus (linear elastic), you can publish it here. I am interested.
Simple example of crack propagation calculated with the help of XFEM method
The element is in tension and the direction of the crack changes becoming perpendicular to the dominant permanent tension principal stress.
You can try:
1. Increase IA (Step-Other-General solution control-edit step-specify-Time increment-more- change IA to the maximum value 30)
2. Refine the mesh in the contact regions to reduce the percentage of elements flipping in and out of contact.
3. Using mass scaling in Dynamic/Explicit to control the stable time increment.
- Badges
- Science topic