Learning Forum

[Jared McFadden]

Hello,

I have a question regarding the force and displacement convergnece plots in the solver output section.

In one of my analyses, I noticed that both the force and displacement convergence lines were below the criterion line, but the step would not converge. This would occur for multiple iterations until it would finally converge. Why does this happen and is this indicating an issue in my model/setup?

Thank you,

Jared McFadden

[peteroznewman]

Hello Jared,

There are other requirements that must be satisfied to achieve convergence. For example contact elements that have too much penetration, incremental plastic strain that is too large, etc. 

Look at the Solution Output file in the Solution Information folder and read the text so see what is delaying convergence in your model.

Regards,

Peter

[Jared McFadden]

Hello Peter, 

Thank you for the clarification. The only messages I am seeing that stand out say "Multiple constraints have been applied on degree of freedom 1 of contact node of 30539. The program will remove certain internal MPCs. Please check the model carefully." and "The contact staus has changed at 29 contact points."

Could either of these be the cause of the issue?

[peteroznewman]

Yes, the number of contact points changing status should go down to a small number or zero for that increment to be considered to have converged.

You can reduce the number of iterations needed to achieve this by softening the contact. In the Details for a Frictional Contact, set the Normal Stiffness to a Factor and set the Factor to 0.1 instead of the default 1.0

[Jared McFadden]

Peter,

Thank you for the information! This is very helpful.

[Erik Kostson]

Just to add, there are quite a few nice videos on contact and convergence:

Convergence and contact

Hope this helps

Erik