Hi,
I'm trying to model the failure mode of an simple rectangular FRP sheet with Hashin damage criteria, but I couldn't get the element deletion initiated, even though the HSNFTCRT (hashin damage criteria) for some elements has already become 1. Following are some clues and details for my modelling so far:
1) A homogeneous shell planar part was chosen so there's no much choice for the orientation, but the part is meshed in its fibre direction. Since the fibres are all unidirectional I don't think composite shell would make much difference.
2) For the material properties I entered elastic lamina properties with fail stress and strain, followed by Hashin damage criteria and damage evolution.
3) I tried Mesh > Element Type > Element Deletion ON, but the deletion could still not be initiated. Standard or Explicit didn't make too much difference.
4) When applying the load I chose a static, general step with a displacement load on one edge of the sheet. Changing the displacement value didn't make much difference since the job would abort close to the failure stress/strain from material properties.
5) I turned on STATUS, DAMAGEFT and HSNFTCRT in field output request, and for the results, the STATUS always gives an output of 1 and DAMAGEFT mostly gives 0, even though for some elements the HSNFTCRT gives 1, meaning the fibre tension failure criteria has been reached.
6) I realised it might be too perfect if a pure rectangular model is created, so I also tried to model a 'necked' sheet (like an hourglass shape rotated 90 degrees), but the jobs still get aborted due to 'too many attempts' or 'time increment less than minimum'. I think it's because that no element deletion is happening, and so the solution is not convergent.
I have searched for videos, tutorials and some other similar questions, but the results aren't too helpful. Therefore, I tried to make my situation above as detailed as possible. I appreciate for any ideas provided about this question, and for any other information I didn't mention above, I will try my best to check often and reply ASAP. Thank you very much.
Dear @Jiahui Wang
It seems that your problem is too complex to be solved by Static, general procedure. Hashin damage evolution contains material softening that makes the problem unstable that leads to solving error when Static, general procedure is used. Instead of Static, general, I recommend you quasi-static explicit analysis using Dynamic, explicit procedure. You can read below link to get more information.
https://www.researchgate.net/post/Implicit_static_Analysis_VS_Quasi-Static_Implicit_in_static_loading_condition
There is another way to make Static, general to be converged using "Viscous regularization". You could search about it to get more information.
About element erosion problem, in Abaqus/standard an element will be removed when damage variables for all damage modes reach 1.0 while in Abaqus/explicit an elemen will be removed when tensile or compressive damage variable for fiber failure modes reach 1.0. Therefore you should check DAMAGEFT, DAMAGEFC, DAMAGEMT, DAMAGEMC, DAMAGESHR values and DAMAGEFT, DAMAGEFC values for Abaqus/standard and Abaqus/explicit, respectively.
Regards,
M. Khodaei
Hi Meysam Khodaei
Thank you very much for the reply! I will contact you if there's any further question.
Dear Jiahui Wang
I have the same problem. If you solved it, Could you tell me how to solve it ?
- Badges
- Science topic