Brittle Failure in Laminates

lpdotcom

Hi - I'm looking for a (cost effective) structural FEA package and came across Mecway - I've been playing around for a few weeks and think I have a handle on things but I just wanted to check.

I'm interested in looking at laminated materials where a brittle material surrounds a more ductile one. When the outer layer reaches fracture I'm looking for it to "fail" - no longer contribute strength or stiffness to the system. I've been looking at the laminate function with a failure criterion but this doesn't seem to do the trick for me. Does anyone have any thoughts?

Victor

You're right that the failure criteria won't help - they are only for calculating factors of safety.

The internal solver doesn't do progressive failure for composites.

The CCX solver looks like it can if you define the brittle material using a plastic stress-strain curve which drops to zero stress after the failure strain. Here's an example of a sandwich material. The solution shows that the stress in the brittle layers drops when they fail but not all the way to zero which is strange. So I'm not sure if this is quite right.

lpdotcom

Thanks Victor - it seems that the zero strength value for post yield strength causes a few headaches - by setting a low, non-zero value for post yield strength the model is more stable.

BTW I'm using the demo version - does the full version have the ability to change convergence tolerance for the CCX NL Dynamic solver?

Victor

Oh, good find.

The demo version has no missing features except being limited to 1000 nodes. It doesn't have any CCX convergence options in the UI but you can enter the CCX card for that (*CONTROLS) in CCX -> custom model definition.

lpdotcom

Hey Victor - I've been looking at materials where the material in the middle is weaker but more ductile than the harder outer layers. This seems to cause convergence issues that I can't seem to resolve without relaxing tolerances so much that I am getting nonsense answers - do you have any thoughts?

Victor

I got it two work in two ways:

A ) Changed the fixed support to get rid of the stress singularities at the ends. Might not really be practical for a real structure. (plastic composite v3.liml)

B ) Added another stress-strain point to the brittle material data to give it a small non-zero stiffness after yield. This seems to solve the convergence problem. I put it at a huge plastic strain of 1 so that there'll be some slope to the curve for all realistic strains. (plastic composite v4.liml)

I notice you have a zero-slope curve for the ductile material too. That's usually risky and it might fail in other cases although it seems to be OK here.

I think the reason the stress might not going to zero after failure could be that the values are extrapolated from the integration points and then averaged between elements so a single point failure could be disguised by the non-yielded points around it.