How to find gaps in the mesh when the Tetramesher fails

Rahul_P1

When meshing with Tetra Elements, HyperMesh fails with the error message 'Volume Analysis failed'. There remains a 'tmp_2d_for_tetra'-Component. However there are not hints, where the mesh is incomplete or corrupt. I suppose there is a small gap in the mesh, which I can not see. Is there a way to find the critical areas for tetrameshing?

Rahul_P1

There are a few ways to find out about critical areas in the 2D surface mesh, which is generated automatically by HyperMesh, when the Tetramesher fails. The 2D mesh is found in the component tmp_2D_...

If there are gaps in the model, you will find them with:
Mesh > check > component > edges, option 'free edges'

If there are duplicate or t-connected edges, use
Mesh > check > component > edges, option t-connections

Both functions will highlight the critical areas with red plot elements within a temporary component '^edges'. Display only the edges component (model browser) and use 'unmask adjacent' in the 'Display' toolbar to isolate the critical area.

If there are elements with bad quality, use
Mesh > check > elements > check elements to find e.g. elements with skew angle >80°. Use save failed, Hide All (model browser) and the 'find' button to isolate the area

All critical 2D areas can be repaired either by cleaning the geometry in the area or by element editing

Rahul_P1

Basically this error usually means there are problems with you geometry. Some things to look for include:

* Two lines on the volumes surface that are too close together -- suppress on of the lines.
* There is a section of the volume with a much smaller cross-sectional area than other sections -- try and use the proximity option and/or change element size.
* There are free edges on the volume -- lines on the surface of the volume colored red.

Please refer to the Hypermesh tutorials covering geometry and 3-D Volume meshing for more information on the possible techniques to solve this problem.