Modifying existing contact behavior to include cohesive behavior 1

[vepawz]

Hello all,

I'm trying to model a welding problem between Cu-Al-Cu stack-up. Al melts before Cu and when that happens, I want to introduce cohesive contact behavior into the model. The model uses friction-less hard contact behavior until then.

I import material state without updating the reference configuration. This imports all the stresses, geometry and contact information.

So far, I've tried to delete existing contact pairs and introduce new contact pairs (both hard-contact and cohesive). I can only delete in *Step module and define new contact pairs before that. Effectively, I have to add new contact pairs before I delete existing ones but I need to delete before I add i.e. cannot overwrite.

Any way around this problem?

Thanks.

 

[FEA way]

All contact pairs must be created at the beginning of the analysis. However you could bypass this limitation and use the model change feature in such way that:
- first contact pair (without cohesive behavior) is created at the beginning of the analysis and then removed in selected step
- second contact pair (with cohesive behavior) is created, removed right at the start of the analysis in the first step and then reactivated in the same step in which first pair is removed

These changes can be applied in the Interaction module or using keywords directly (*Model Change, Type=Contact Pair, Remove/Add).

 

[vepawz]

@FEA way, thanks for the advice. I tried as you said and with no success.

I'm trying to model Al melting b/w two Cu layers. So, I'm trying to model the portion of Al that melts using purely cohesive behavior (small sliding, surface-to-surface) and the portion that doesn't melt using frictionless-normal behavior (finite sliding, surface-to-surface). Currently, I've split the Al surface into two parts for the above two interactions.

I'm getting an "unexpected load libraryA error 193", no further details with the error message. Any suggestions on how to proceed?

Thanks.

 

[FEA way]

This error most likely isn't caused by interaction definitions. It looks more like a subroutine issue.

I checked this approach and it shouldn't cause any problems. Here's an example of how it should look like in the interaction manager:

You've mentioned that you use import capability. For what reason do you use it ? If you just want to switch contact properties between non cohesive and cohesive this way, try doing this without import, as I described.

 

[vepawz]

I'm trying to simulate a coupled thermal-electric-mechanical welding simulation as an axisymmetric case. Since Abaqus currently doesn't support elements for this type of simulation, I've had to perform mechanical (static) and coupled thermal-electric simulations for each time step and transfer results b/w them.
So, after every thermal-electric simulation, I need to import new temperatures and previous material state into a new mechanical simulation. After which, I import the new geometry and contact information, and previous temperatures into a new thermal-electric simulation and so on until the weld time is over.

I'm not using any sub-routines in the mechanical simulations, I even tried to remove all restart and output requests. I doubt the application of cohesive and non-cohesive contact properties on different parts of the same surface.

We talked before about this simulation regarding importing voltages and how Abaqus calculates power by averaging start and end voltages. You gave me a few suggestions on how to import voltages. Unfortunately, I believe it's currently not possible to import voltages as predefined variables (I tried to run a dummy step after a restart analysis to be able to import previous temperatures, but the imported temperatures never overwrote the temperatures calculated after the dummy step and since it's a coupled thermal-electric analysis the temperature increase at the end of dummy step would be artificial and wrong).