Most problems with the mesh generation process become manifest in the failure to generate an initial mesh. There are two sources of such problems:
An invalid surface mesh
Incorrect sliver size specified
Some of the common problems and suggestions for checking and fixing the mesh are described in this section.
To look at the nodes and faces that have not been meshed, enable Unmeshed in the Display Grid dialog box.
Some codes create multiple copies of the same node where two boundary curves or surfaces meet, resulting in a connectivity problem. This problem can be detected by reporting the number of free nodes or by drawing the free edges. If the geometry does not contain infinitely thin walls then there should not be any free nodes or edges. You can remove duplicate nodes using the /boundary/delete-duplicate-nodes command.
The presence of duplicate faces can be detected in one of two ways:
If the nodes of the duplicate faces are not shared by the non-duplicate faces, the duplicate faces may have free edges that can be displayed.
If the nodes are not distinct or have been merged, there will be multiply-connected edges.
Note: Duplicate faces can be handled, it is not necessary to remove them.
Nodes that are not used by any face are called unused nodes. The unused nodes can easily be found and deleted using the Merge Boundary Nodes dialog box, if those nodes are not required. However, there are cases where these additional nodes may be useful (see Inserting Isolated Nodes into a Tet Mesh). Extra faces can be identified and removed using the method described for duplicate faces.
To merge nodes that are not on a free edge, in the Merge Boundary Nodes dialog box disable Only Free Nodes in the Compare... or With... group box or in both group boxes. For example, if you read a hybrid mesh containing hexahedral cells (and quadrilateral boundary faces) and triangular boundary faces, there may be some duplicate nodes on adjacent quadrilateral and triangular boundary zones. To merge them, compare free nodes on both zones with all nodes on both zones (that is, select both zones in the Compare... and With... group boxes, and disable Only Free Nodes in one of them).
If there are intersecting faces in the mesh, you will not be able to generate a mesh until the problem faces are removed. Most intersecting faces can be located using the /boundary/mark-face-intersection command. If intersecting boundary faces are encountered during initialization, a message will be displayed.
After the meshing fails, the unmeshed faces can be drawn to see the problem area. Usually, because the intersecting face will have been meshed, it will not be drawn and some additional sleuthing will be required. Draw all the faces near the unmeshed faces by setting display bounds (by using the Display Grid dialog box). Click the button in the Intersect Boundary Zones dialog box to highlight the face intersection. Alternatively, you can use the command /boundary/mark-face-intersection to highlight the face intersection. When you set the Feature Angle, note that this specifies the minimum angle between the feature edges that should be preserved during retriangulation. All the edges in the zone having feature angle greater than the specified Feature Angle are retained. This option is useful for preserving the shape of the intersecting boundary zones. A value in the range of 10–50° is recommended; a large value may distort the shape of the intersecting boundary zones.
Some meshing problems can be caused by a poor quality surface mesh. The surface mesh may have highly skewed faces, or two or more boundaries in close proximity may have very different face sizes. In the latter case, the boundaries can be connected (for example, in a corner) or completely separate. Either way, the boundary mesh cannot be created without considering the impact of other nearby boundaries.
If the gap between two boundaries is D, the largest edge on a face should not exceed D. The mesh quality is extremely important when a coarse mesh is required in a small gap.
You can generate an initial mesh even if there is a hole in a boundary either due to missing faces or a gap between two zones. In this case, instead of having two separate zones on opposite sides of the boundary, you will have just one combined zone. This situation is evident because you will have very few zones.
If the hole is in the outer boundary, the cells outside the boundary will be combined with the cells inside, resulting in an error. The edges around the hole will be marked as free edges and therefore can be displayed.
If the problem is caused by a small gap between boundaries and the duplicate nodes have already been merged, increase the tolerance and perform additional merging.
The following command can be used to detect holes in the geometry by tracing the path between the two specified cells:
/mesh/tet/trace-path-between-cells
A path between the selected cells will be highlighted.
During refinement, a node may be placed too close to a boundary face, resulting in a highly skewed cell. You can detect this situation by displaying the highly skewed cells. You can then smooth the mesh to eliminate the problem.
If the interior node is constrained by the boundary faces, increase the Min Boundary Closeness (in the Tet Refine Controls dialog box) and regenerate the mesh.