XFEM in Abaqus/Standard for 3D CFRP layup - nodal level set value error

[IcarusAero223]

Hi everyone! Any advice is greatly appreciated!

I'm trying to model a composite test coupon damage combining LaRC05 criterion and XFEM.
To get my job converge after first element experienced some damage (STATUSXFEM between 0 and 1, usually at 0.4) I had to define damping factor of 0.0002 in the Step module (completely eyeballed this value based on some superficial reading some time ago - constant throughout the analysis).
That enabled the model to converge but ended up with an error: The system error in std_findcutshape3d8_xfem -- nodal level set values might not be correct for element 85606 instance part-1-1, its philsm are -1.85580e-02, 0.17272, -3.78320e-02, -0.20095, 8.42569e-02, -0.27117, -5.87143e-02, 0.27912.
This model had 1 enrichment zone per layer.

I tried softening displacement amplitude, refining mesh, and making enriched zone smaller and defining 2 enrichment zones per layer (above and below the hole) but nothing really helped.

Is there anything else I could try that might help my model converge better or faster? Pictures attached are the first model with the error mentioned.

 

[FEA way]

This error is described in the DS Knowledge Base article "Abaqus/Standard XFEM Crack Propagation with Non-planar Cracks" (QA00000058422). If you can’t access it, I’ll try to summarize it here.

 

[IcarusAero223]

This error is described in the DS Knowledge Base article "Abaqus/Standard XFEM Crack Propagation with Non-planar Cracks" (QA00000058422). If you can’t access it, I’ll try to summarize it here.

I don't have access so that would be greatly appreciated.

 

[FEA way]

Ok but which version of Abaqus are you using - there are separate ways to handle this error for versions below and above/including 2019 FP.1906.

 

[IcarusAero223]

Ok but which version of Abaqus are you using - there are separate ways to handle this error for versions below and above/including 2019 FP.1906.

It's a 2022 version.

 

[FEA way]

Then check the NPOLY, ANGLEMAX and INISMOOTH parameters for the *FRACTURE CRITERION and *DAMAGE INITIATION keywords. They were introduced to handle such issues. Especially the angle one may help. Of course, they are described in the documentation.

 

[IcarusAero223]

Then check the NPOLY, ANGLEMAX and INISMOOTH parameters for the *FRACTURE CRITERION and *DAMAGE INITIATION keywords. They were introduced to handle such issues. Especially the angle one may help. Of course, they are described in the documentation.

Thank you very much. I checked the documentation and NPOLY and INISMOOTH parameters aren't available for LaRC05 so I'm just going to try ANGLEMAX which does look promising.

 

[FEA way]

I'm just going to try ANGLEMAX which does look promising.

Yes, it may help eliminate the issue of the crack becoming non-planar. This parameter allows you to limit the new crack propagation direction to be within a certain angle of the previous crack propagation direction.

 

[IcarusAero223]

Yes, it may help eliminate the issue of the crack becoming non-planar. This parameter allows you to limit the new crack propagation direction to be within a certain angle of the previous crack propagation direction.

With ANGLEMAX = 15 upper part of the crack connected nicely, while the lower part (even though its symmetrical layup) hasn't and that caused the original error. As the explanation of this parameter in the manual is a bit vague I'm not sure how the angle defined is measured.

 

[FEA way]

Did you try different values ? It's the angle between the subsequent crack propagation directions.

If it doesn't help, I would try changing the mesh.