×
INTELLIGENT WORK FORUMS
FOR ENGINEERING PROFESSIONALS

Log In

Come Join Us!

Are you an
Engineering professional?
Join Eng-Tips Forums!
  • Talk With Other Members
  • Be Notified Of Responses
    To Your Posts
  • Keyword Search
  • One-Click Access To Your
    Favorite Forums
  • Automated Signatures
    On Your Posts
  • Best Of All, It's Free!
  • Students Click Here

*Eng-Tips's functionality depends on members receiving e-mail. By joining you are opting in to receive e-mail.

Posting Guidelines

Promoting, selling, recruiting, coursework and thesis posting is forbidden.

Students Click Here

Jobs

Shell to Solid Modeling

Shell to Solid Modeling

Shell to Solid Modeling

(OP)
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.

RE: Shell to Solid Modeling

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.

RE: Shell to Solid Modeling


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.

RE: Shell to Solid Modeling

(OP)
Thanks all.

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

Bye.

Carlos A. Medeiros
Structure Engineer, MSc.

RE: Shell to Solid Modeling

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

Red Flag This Post

Please let us know here why this post is inappropriate. Reasons such as off-topic, duplicates, flames, illegal, vulgar, or students posting their homework.

Red Flag Submitted

Thank you for helping keep Eng-Tips Forums free from inappropriate posts.
The Eng-Tips staff will check this out and take appropriate action.

Reply To This Thread

Posting in the Eng-Tips forums is a member-only feature.

Click Here to join Eng-Tips and talk with other members!


Resources