Surface contact type between solid and shell for doubling plate

[Eland123]

Hello all,

I was working with some doubling plates today with some linear static analysis. I tried out 3 different contact types for a doubling plate (solid) on top of a shell model. Which resulted in 3 completely different results. I am wondering why.

Below I schematically drew the setups I tested.

A:

I have a shell surface 4mm thick plate. Offset is set in a way that the outside surface is modeled (solid blue line) and the 4mm plate is inward (blue dotted line)

On top my doubling plate solid with the structure connected to it. The stresses in the corner on top of the doubling plate are measured (blue arrow).

I offset bonded shell surface to the underside surfaces of the doubling plate.

B:

Situation B is the same as A, only I changed the contact type to bonded.

C:
In C I changed the shell and solid models.

I made the doubling plate 4mm thinker and made a hole in the surface model.

So now the edge of the surface model is touching the side on my solid model.

I made a surface - edge offset bonded contact between the two.

*10mm max act dist yields the exact same results

Geometry wise these 3 situations should behave similarly right?

However when I measure the stress in the corner with the blue arrow I get different results.

If A is 100MPa, then B is 250MPa and C is 300MPa.

Why does this happen? Which would be most accurate?

Thanks.

[John_Holtz]

Hi @Eland123 

Is the solid one piece or two pieces bonded with the same type of contact as used for the solid-to-shell contact?

In general, stress at a corner is difficult for a simulation to calculate accurately. Even if you have a model without contact, the mesh size can greatly affect the stress given at a corner. So the first thing to check is whether the mesh is the same in all three cases, or if a difference in the mesh is related to the difference in stress. (A and B could be the same mesh since the only change is the contact type, assuming you used the same mesh. 🙂)

I suggest you check the displacements to see if they are similar or different.

• If the displacements are similar, try finer meshes to see if the stress result is a singularity (the stress continues to rise with finer meshes) or if the random location of the mesh is affecting the stress.
• If the displacements are not similar but the mesh is similar, this would be contributing to the difference in stress.

If using manual contact (the type where the faces are selected to define the contact region), then offset bonded contact occurs over the area defined by the maximum activation distance. Bonded contact only creates contact between the nearest nodes.

Let us know what you find out.

John

[Eland123]

Hi John,

Thank you for the reply.

To address some of your questions:

The solid piece is actually one piece. (So not 100% accurate to reality if you would weld a plate on top of an other).

Yes, I did use the same mesh (settings) everywhere. And for A&B I did just change the contact type and run the simulation again.

I had a look at your suggestion. And indeed the displacements between A and B are different. Where the displacement in A is lower than B.

"If using manual contact (the type where the faces are selected to define the contact region), then offset bonded contact occurs over the area defined by the maximum activation distance. Bonded contact only creates contact between the nearest nodes."

All contacts were done manually

Given this explanation it could be that under setting A the activation distance causes (a lot) more nodes to be bonded together compared to setting B? This changes the way the solid interacts with the shell, changing the stress and displacement as a results?

@John_Holtz : I'm bad at replying 😉 and replied to the topic instead of your comment