Jump to content
Sign in to follow this  
JJJ

Connecting beam and sheel elements

Recommended Posts

Dear friends,

 

Good morning, I have a situation and I don't know how to solve. I think you can have a solution.

 

I have a structure composed of beams and surfaces (beams are in the same planes than surfaces). I want to consider the connection between the two components: at this time I have meshed yet beam elements (so I have their nodes in the model), but now I want to do the next: that surfaces will be meshed and their nodes will be coincident with beams' Also I want to know if this is the only thing that I have to do to consider the connection between beams and shells or if I have to define something else.

Thank you very much for your attention. Best regards,

JJJ

altair-question.jpg

Share this post


Link to post
Share on other sites

Hi,

 

use Geometry>edit>nodes>associate

The Associate subpanel creates an association between the selected nodes and a selected piece of geometry. Nodes are projected to the geometry, provided the distance to the selected geometry is within the search tolerance. The tolerance is used to create a search sphere at each of the selected nodes. If the selected geometry is found within that search sphere, the node is projected to the closest point on the geometry. An association is made within the database between the nodes (and corresponding elements) and geometry, so any subsequent selection routines can reference either entity; for example, if creating a boundary condition (such as a force, pressure, or constraint) on the geometry, the boundary condition will be applied to the nodes and or elements upon export.

Share this post


Link to post
Share on other sites

Dear Hyperman,

 

Thank you very much for your rapid response. Once that I have associated nodes from beams elements to shell elements, how I can define the 2D meshing for that these elements will be coincident? When I mesh the 2D surface (as you can see in the figure attached) 2D nodes are not coincident with 1D nodes. And one more question: with this operation, then beam and shell elements will be "welded", or is it necessary to define in Hypermesh? Thank you very much.

2.jpg

Share this post


Link to post
Share on other sites

It turns out the proposed approach will not work- sorry about that. Node association only works when meshing with keep connectivity option and uses the existing nodes on any shared boundary edges (not interior nodes).

 

First workaround:

  • mesh 1D and 2D elements
  • remesh 2D elements with automesh and pick 1D nodes as anchor nodes (you can pick all 1D element nodes in one go by double-clicking nodes selector>by collector>1D elements component)

 

Second workaround:

  • mesh 1D elements
  • Geometry>edit>nodes>associate
  • geom>surface edit>trim with nodes>multiple nodes>select surface + 1D element nodes
  • mesh 2D elements

 

Anchor nodes: Designate nodes that will remain and be re-used in the new mesh.  Anchor nodes are "fixed" so that the automesher cannot move or replace them; in essence, they are exceptions to the re-meshing operation, and the new mesh must utilize them.

beam.jpg

After this operation, beam and shell elements should be "welded" and all degrees of freedom coupled (beam and shell elements both have 6 DOF per node, unlike solid elements that only have 3 translation DOFs). Verify connectivity in edge panel(F3)>preview equiv

Share this post


Link to post
Share on other sites

Join the conversation

You can post now and register later. If you have an account, sign in now to post with your account.

Guest
You are posting as a guest. If you have an account, please sign in.
Reply to this topic...

×   Pasted as rich text.   Paste as plain text instead

  Only 75 emoji are allowed.

×   Your link has been automatically embedded.   Display as a link instead

×   Your previous content has been restored.   Clear editor

×   You cannot paste images directly. Upload or insert images from URL.

Sign in to follow this  

×
×
  • Create New...