Shell to Solid Modeling

[CA]

Hi! Experts.

Anyone knows how to performance a shell to Solid FE modeling in ANSYS ?

My scenarios is,
I want to connect a support modeled by solid Elements to a Shell structure using ANSYS.
I am worry about the compatibility between shell (6 dof - 3translation and 3rotation per node) and solid (3 dof – only translations per node) elements.
As far as I know, some commercial FE, like ADINA, have interface elements that link a solid element to a shell, but I really do not know how to do this by ANSYS.

I’d appreciate your Tips.
Carlos


Carlos A. Medeiros
Structure Engineer, MSc.

 

[GBor]

Here's a cheap way of taking care of it:

Extend your shell elements into the first row of bricks, but give the shell elements relatively low stiffness or make them extremely thin. This resolves the "hinge" effect from putting a 3DOF element adjacent to a 6DOF element.

 

[EricZhao]

I don't remember Ansys has dedicated interface elements that link a solid element to a shell. But you can do it manually in Ansys.

To connect a Shell element model with a brick element model, you have to first make sure the mesh at the boundary are compatible (nodes are one-to-one coincident). No mid-side nodes should be present. You should use 8 nodes brick element and 4 node shell element. Merge the coincident nodes by preprocessor>>numbering control>>merge items.

Up to this point your shell is simply supported, no rotation can be trasfered between the shell and the brick. Then you have to manually put trust element at the inner-coner of the connection point. Like this:

---------_____ single shell
| single | /
| brick | / single truss element
| | /
---------/

Make the truss element as stiff as possible. Of course stress close to the connection is no longer trustable. But displacement should be very accurate, and so is the stress far from the connection.
I bet ADINA did it the similar way.

 

[CA]

Thanks all.

Great tips that could help me. I'll try do that.

Bye.



Carlos A. Medeiros
Structure Engineer, MSc.

 

[cbrn]

Hi,

in addition to what have been said, I'd recommend you take a close look on the "Constraint Equations". There are some chapters in Ansys' Help which describe the connection "problems" between different element types:
chapter 2.5 for example.

Regards