Geometry abstraction, polygon geometry, and convergent geometry > Creating polygon faces from meshes and face boundaries

Creating faces from existing meshes

Video: Creating faces from existing meshes

In some analyses, you may need to modify finite element models that either have no geometry or that are not associated to geometry. You can use the Face from Mesh command to create a new polygon face from a selected set of 2D elements, 3D element faces, or a 2D or 3D mesh. The elements or mesh that you select to create the new face become the initial mesh on that face. You can then make modifications to the new face or its associated mesh.

The Face from Mesh command is helpful when you need to:

Associate an existing finite element model to new geometry.
Connect shell meshes that are not associated to any geometry.
Locally refine a region of a mesh that is not associated to any geometry.
Create faces from manifold and non-manifold 2D meshes.

You can later modify the mesh on that face. For example, you could use the 2D Mesh command to regenerate the entire mesh on that face, or you could use the 2D Local Remesh command to refine a subset of those elements.

The following graphic shows a very simple use of the Face from Mesh command. (A) shows a FEM file that was created from Nastran bulk data. The model contains only 2D PSHELL elements. (B) shows the face that was created from those elements. Those elements become the initial mesh on that new face. (C) shows the new face (with the mesh display turned off).

Managing faces from meshes in the Simulation Navigator

The software places the containers for the new polygon bodies in the Polygon Geometry node in the Simulation Navigator. Because the software creates a different type of polygon bodies depending on whether you selected 2D elements, 3D element free faces, or a 2D or 3D mesh, the software uses a different icon to help you distinguish between them. For example:


Polygon Geometry
Polygon Body Created from 2D Elements
Polygon Body Created from 3D Element Free Faces
Polygon Body Created from 2D Mesh

Notice that the icon for polygon bodies for faces created from 3D element free faces contains a lock. Those types of faces are largely locked from modification. For more information, see Modifying faces created from existing meshes.

The selected elements become a geometry associative mesh for the new face

When you create a new face from elements or a mesh, the elements and their nodes become associated with that new face. The nodes and elements become the geometry-associative mesh for that face. Additionally, the software moves those elements into a separate mesh in the Simulation Navigator. You can use the geometry associative meshing commands, such as 2D Mesh or Mesh Controls to modify that mesh.

If you delete the face, the associated elements remain but become disassociated from the geometry. This changes the mesh from a geometry associative mesh to an orphan mesh.
If you delete the mesh, the face remains. You can then use any of the geometry associative meshing commands to create a new mesh on that face.

Creating faces from 3D meshes or 3D element free faces

You can use the Face from Mesh command to create faces from the following 3D element types only:

Linear and parabolic tetrahedral elements
Linear and parabolic hexahedral elements

Subdividing new faces along feature edges

Use the Add Feature Edges option to select element edges that define features you want to represent in the new face. When you generate the face from the mesh, the software creates a new polygon edge along these feature edges. With this option, you select a single element edge. The software uses the selected edge as a seed edge to automatically select the adjacent element edges that lie along the most tangent continuous path.

If the software does not select all the element edges that you want, you can also use the Connected Element Edges smart selection method and set the new Method option to Most Tangent Path. With this method, the software favors the most tangent continuous path that minimizes the edge angle between the first and last element edge you select.

In the Nastran environment, you can use the Add Feature Edge option to subdivide faces at the location of the following types of beam elements:

CBEAM
CBAR
CROD
CONROD

With these types of beam element, you must use Add Feature Edge to select all the element edges that are connected by the beam elements.

If the polygon edge that the software creates from the 1D elements completely bisects the new face, the software subdivides that face. If the 1D elements do not completely bisect the new face, the software creates the new edge as a scar on the face.

The software associates the 1D elements to the new face as a coating 1D mesh and stores them in a 1D_mesh_coat node in the Simulation Navigator. 1D coating elements affect the 2D meshes on adjacent faces.

Modifying the new faces or their associative meshes

Depending on whether you selected 2D elements, 3D element faces, or a 2D mesh to create the face, you can use the commands on the Model Cleanup commands to modify the face. For more information, see Modifying faces created from existing meshes.

Working with faces from meshes and CAD faces in the same model

You can have faces created from meshes and faces associated to CAD geometry in the same FEM file.

If the CAD geometry updates, the software updates the bodies, faces, and meshes associated with the CAD geometry. The software does not update the faces created from meshes.
You cannot create a Glue Coincident type of Mesh Mating Condition between a CAD associated body and a body created by the Face from Mesh command. If you need to connect the mesh on a geometry-based face to the mesh-based face, you must:Create a Free Coincident type of Mesh Mating Condition between the faces to create an imprint of the geometry-based face on the mesh-based face.Delete the geometry-based face.Choose Home tab→Polygon Geometry group→Stitch Edge to stitch the edges of the mesh-based face to the remaining edges of the geometry-based face.

Modifying a face created from a mesh

Once you use the Face from Mesh command to create a new face, you cannot modify that face. If you need to make changes to the face, you must first delete the face and then recreate it from the mesh:

In the Simulation Navigator, right-click the appropriate polygon body.
Select Delete.

You can then use the Face from Mesh command to recreate the face using different options.

For more information, see Tools for identifying and repairing polygon body problems.

Where do I find it?

Application	Pre/Post
Prerequisite	A FEM file as the displayed part and work part
Command Finder	Face from Mesh
Menu	Model Cleanup→Face from Mesh

Quick links

Command reference

Pre/Post video examples

Bulk Entry Descriptions

Simcenter 3D tutorials

Browse Simcenter 3D help by product area