Using Shells from Surface Patches

[matt.knight]

Hi,

I'm having trouble creating a model which comprises of beams and shell elements created from surface patches. I create sketches by projecting lines from the master sketch bellow and use these to create surface patches.

When I transfer this into Nastran In-CAD I apply edge to surface bounded contacts.

However when I run the model the surfaces detach from the edges at seemingly random places.

How do I constrain these surfaces along all the edges, or is there a better was of creating this model? Any help would be really appreciated!

Thanks,

Matt

[John_Holtz · Accepted solution]

Hi Matt (@matt.knight)

I think the problem is that the contact is defined using "sketch segment". I typically see the contact defined using "edge". Therefore, I think the sketch segment used in the contact is not associated with the shell elements, so no contact is created. Please remove the sketch segments from the contact definition and select the edges (or you can select the two faces).

Here are some other things that you might need to investigate about the model setup. (You may have these done properly -- it is hard to know from the images.)

1. When connecting shells together, you probably want to use "offset bonded" instead of "bonded" contact. Offset bonded contact creates a moment connection; bonded contact creates a hinge connection.
2. Since you are working with a single part model, you can use the "Continuous Meshing" option to match the mesh between the shell faces. If you do this, you do not need to define contact. (You do not want to use continuous meshing in an assembly according to this article: Results indicate that constraints and loads are applied to extra edges in Nastran InCAD. This problem may be fixed in the release that comes out after version 2019.1.0.)
3. If you have beam elements along the edges of the shell elements, you may want to review this article: Nastran In-CAD: How to connect beam and shell elements. If I remember correctly, you do not want to use a sketch segment to define the beam elements along the "common edge" with the shell. You want to use the edge of the surface to define the beam elements along the common edge. When you use the edge to define the beam elements, the nodes will match with the shell mesh, and the beam and shell elements will be connected together.

[matt.knight]

Hi John,

Thanks for the advice. Making sure edges rather than sketch segments are selected and an offset bonded contact seems to have done the trick.

Thanks again,

Matt