XFEM crack growth fails to converge

[s57_s2k]

I have created XFEM crack on cell partition I followed Abaqus documentation, but the problem is as soon as the crack initiate the iteration fail to converge. I have lowered minimum iteration step but it didn't solve the problem. I think that I need to create XFEM crack growth interaction but I can not see it under "create interaction" ( I have selected step: intial tap ) but still didn't see it.

What do I need to do ?

by the way my mesh is bad I am not use to work with tetrahedral mesh I find it very hard to create a mesh with out bad elements.

 

[FEA way]

XFEM introduces very large nonlinearity. You may need to use damage stabilization. Also it is advised to change default solution controls. Turn on discontinuous analysis and increase I_A to 20. Automatic stabilization with constant damping factor that can be turned on in the step definition may also aid convergence.

XFEM crack growth interaction (*Enrichment activation) is used to activate or deactivate crack propagation within the step. You may also add contact property to the crack definition to account for potential contact between crack surfaces.

 

[s57_s2k]

Thank you FEA way , it worked I changed I_A to 20 . damage stabilization and contact property did not help. I did not know how to turn on discontinuous analysis. also I think in CAE 2019 dassault removed XFEM crack growth interaction. The result is not what I expected but maybe it could be improved. I thought XFEM crack was going to cut ( shear off ) my spot weld but it did not.

 

[FEA way]

Discontinuous analysis option can be found in the same menu as I_A (General Solution Controls). Check Specify and then Discontinous analysis box in the Time Incrementation tab. XFEM crack growth interaction is still there. You can find it in the Create Interaction menu (select Initial step). But it's only needed to modify the status of crack growth ability in a step.

Did you request PHILSM output variable ? It's needed to visualize the crack.