I have a running model in which I have used tet10 mesh for solid. Now based on my results I would like to refine (fine mesh) mesh on one solid object. Is there a way to do it without deleted the mesh on the body and remeshing it again?

Question

I have RBE2 and RBE3 connected to that solid geometry. If I deleted the mesh and mesh it again using small GEL value I get bad elements. (probably its picking up the RBE3 and RBE2 nodes already associated with that solid and creating bad elements.) Any way around for this?

Arthur Hickson · Accepted Answer

An alternative approach that can be useful for remeshing parts of a tet mesh is to use a tri element skin . the methodology goes like this:

1) create a group of the tet elements that you want to remesh and only post that.

2) create tri elements on the free surface of these tets using:

Create / Element / Edit :

Shape: Tri

Topology: Tria6 (assuming you're om tet10s)

Pattern: Elem Face

turn auto execute off, use existing midside noes on, and then use the "Free face of element" select icon and do a selct of all the tet elements on the screen. This should only select the outside (free face) of the tet and use them to make tri elements.

3) delete the selected tet elements.

4) modify the tri mesh if you want to increase the element density in certain areas. This can be done by editing/splitting elements or probably easier using Create/Mesh/On Mesh and using Feature recognition and Feature selection to preserve edges/nodes that you need to retain (interface nodes, RBE nodes etc). Where the original selected tet elements join other tet elements, the tria mesh can not be changed otherwise the refined model can not be joined (equivalenced) correctly to the other parts of the original mesh. When you are happy with the new tria mesh use it to make new tet elements.

5) create new tet elements: Create / Mesh / Solid (Tet/TetMesh/Tet10) use a Global Edge Length that reflects the new element size you want and in the "Input List" rather than using the "solid" select icon use the "tri element" select icon and select all the tri elements (these should define an enclosed volume, their element normals pointing outwards).

6)delete the tri elements and check equivalencing (though you should have preserved the interface nodes as you remeshed the tri elements so there should be no nodes to equivalence).

This approach is remeshing solid elements rather than remeshing the geometry, so you may want to Associate/Element/Solid if the association is something you use for LBCs/Properties.