How to remove tied contact pairs during a step?

[Mettyrial]

I am trying to simulate the behaviour of a crack in a residual stress field.
I already modelled the crack (crackfaces=doubled nodes with the same coordinates) with CAE
In the first step, I want to let the crack be closed (the upper crackface tied to the down crackface), so that the mapped residual stress field finds equilibrium.
In the second step the whole crack should open.

I defined contact pairs etc. as explained in thread799-132367
, so that the crackfaces are tied together during the first step, but it is not possible to remove these tied contact pairs as explained in the mentioned thread.
I get the following error message:

***ERROR: CONTACT PAIR (UPPERCRACKFACE, DOWNERCRACKFACE) IS A TIED CONTACT PAIR. *MODEL CHANGE CANNOT BE USED FOR TIED CONTACT PAIRS

Is there a possibilty to remove tied contact pairs?
Has somebody an idea to solve this problem otherwise?

Thanx

 

[ENGLIAO]

I am not sure if I understand your question clearly. But I suggest you try to deactive tie-interaction in the second step. Say, you construct a tie interaction in the first step, it will automaticallu propagate to next step, but you can make it deactive.

 

[bassmanjax]

Looks like you're out of luck Mettyrial - according to the ABAQUS Users Manual, section 29.2.6, removal and reactivation of contact pairs cannot be done with tied contact.

Could you fix the crack nodes in the first step with a kinematic boundary condition and then remove the boundary condition in the second step?

Regards

Martin

 

[mrgoldthorpe]

Mettyrial,

I contributed to the thread you mentioned. Having looked at the manual agree with Martin that the tied contact lasts for the entire simulation. Sorry for that.

Interestingly, I am working on a similar type of analysis to yours: introducing a crack progressively into a residual stress field. I was going to use *DEBOND and *FRACTURE CRITERION, and debond the slave and master surfaces with crack length growing as a function of time.

However, my model is 3D, so I don't think I can do that. If I can't, I may place stiff, elastic elements between the crack surfaces, with elastic modulus that varies according to field variables. To simulate crack growth, the element moduli can be reduced from large to negligible values by changing the field variables using *FIELD.

Any comments would be gratefully received.

 

[Mettyrial]

I found a solution for my problem:
Instead of using the TIED contact, I did the following:

*CONTACT PAIR, TYPE=SURFACE TO SURFACE, INTERACTION=INTTIED
Crackdown, Crackup
*SURFACE INTERACTION, NAME=INTTIED
*SURFACE BEHAVIOR, NO SEPARATION

--> Here you have to be aware that there acts a certain force on the surfaces

-->Then, in the step definition:
*MODEL CHANGE, REMOVE, TYPE=CONTACT PAIR
Crackdown, Crackup

That's it, and it works for my problem.
mrgoldthorpe, my problem seems to be simplier than yours, 'cause I am analysing a static crack and no crackgrowth

Thanks