Contact between plates

[GauthamBP]

Hello there!

I am conducting a simple simulation where I have placed 2 plates of equal dimension and thickness one upon another. I have pinned one corner and restricted motion in the z direction for the edge faces. I have applied an equal shear load on all the edge faces for both the top and bottom plate and have implemented a contact between the 2 plates. When I run the simulation, I find that the 2 plates don't deform the same, even though the boundary conditions and loading conditions are the same. What could be the reason for this behavior? Could it be due to the contact?

I have attached the inp file below. It takes barely 15-20 seconds to run. Do help in brainstorming!

 

[FEA way]

Could you also attach a picture of your model ? Did you try with tie constraint between the plates instead of contact ?

 

[Mustaine3]

You have a singular system with a possible rigid body motion for each part. So there isn't a unique solution.

 

[FEA way]

Your model only solves thanks to self-equilibrating load. Otherwise it would fail to converge due to rigid body motion - spinning around the fixed edge. You have to constrain this RBM first.

 

[GauthamBP]

Hello guys!

I had tried changing the mode of contact implementation. I was using a small sliding formulation with a node to surface discretization. I changed it to a finite sliding formulation and tested it for both node to surface and surface to surface discretization and it worked well!

@FEAway yes I do understand about the self-equilibrating load part of it. I initially tried to use a point load and the solver didnt converge at all. I didn't want to use a tie constraint and intentionally used a contact. I had posted a question last week about my composite plate with a hole rotating, and i was trying to solve a plate without a hole first. Changing the sliding formulation appears to have solved the rotation problem too! If you have any idea as to why that is so do let me know.

@Mustaine3 I am not exactly sure what that means. I will follow up on that if I find any issues in the simulations hereafter.

 

[Mustaine3]

You can't solve that problem until you create a statically defined model. So prevent the rigid body motion of your two parts by making sure they cannot rotate free about one axis. Add some more boundary conditions, or springs, or stabilization or run it quasi-static or whatever else would do it.

 

[FEA way]

Generally it is advised to use default finite sliding contact in the vast majority of analysis cases. Small sliding is only needed in specific situations when we are sure that sliding between contacting surfaces will actually be small. In such cases we may use small sliding assumption to speed up the analysis.

 

[IceBreakerSours]

Before running stress analyses, I personally run a modal analysis to quickly ensure my BCs are specified appropriately. The cost benefit ratio of this strategy is so low that it makes little sense not to do it. Besides, one also gains some insight into the lowest modes that will influence the results heavily.

*********************************************************
Are you new to this forum? If so, please read these FAQs:

http://www.eng-tips.com/faqs.cfm?fid=376

http://www.eng-tips.com/faqs.cfm?fid=1083