To add nodes to the mesh without specifying the faces, you can create a boundary zone in the boundary mesh (in the program that created it) just for this purpose, then you can introduce the nodes associated with these faces.
This feature is useful for clustering nodes (and therefore cells) in a controlled manner. Figure 14.9: Mesh Generated Using Isolated Nodes to Concentrate Cells shows a mesh that was generated using this method to cluster the nodes behind the wedge. A mesh that was generated for the same geometry without clustering is shown in Figure 14.10: Mesh Generated Without Using Isolated Nodes. You can follow either of the two procedures to insert isolated nodes into a mesh:
Delete the face zone before meshing.
Introduce the nodes using face zones after meshing.
This procedure is as follows:
Delete the face zone, but leave the associated nodes. Disable Delete Nodes in the Manage Face Zones dialog box to retain these nodes.
Note: By default, the unused nodes are deleted when the faces of the zone are deleted.
Disable Delete Unused Nodes in the Tet dialog box and generate the volume mesh.
Note: By default, unused nodes will be deleted during the automatic meshing.
The nodes will be introduced when you initialize the mesh. When you use this procedure, all nodes must be inserted into the mesh or the initialization will fail.
Warning: Do not place isolated nodes too close to the boundary or to other nodes.
This procedure is as follows:
Create a subdomain that does not include the face zones used to control the mesh density.
Create the volume mesh using the subdomain.
Activate the global domain.
Introduce the additional nodes using the text command: /mesh/modify/mesh-nodes-on-zone.
Important: The /mesh/modify/mesh-nodes-on-zone command will delete the faces associated with the face zone.