Adding layers of wedge elements to tetrahedral mesh
boundaries
If you apply the free meshing technique and tetrahedral element shape to a
region, an Insert boundary layer toggle and
Assign Controls button are available in the
Mesh Controls dialog box.
If you add a boundary layer to multiple meshing cells,
Abaqus/CAE
temporarily fixes the seeding on any internal faces between the cells to
simplify creation of the boundary layer across these faces.
From the main menu bar, selectMeshControls.
(For detailed instructions, see
Assigning mesh controls.)
Note:
You must select a free tetrahedral mesh to include a boundary layer
of wedge elements.
Toggle on Insert boundary layer near the bottom
of the Mesh Controls dialog box, and click
Assign Controls.
Abaqus/CAE
displays the Boundary Layer dialog box.
Enter the Wall element height.
The wall element height sets the height or thickness of the first
layer of wedge elements against the boundary walls.
Enter the Growth factor.
Starting from the wall elements and moving inward, the height of each
successive layer is determined by multiplying the height of the previous layer
by the growth factor. The growth factor must be between
1.0 and 2.0,
inclusive, where 1.0 results in no growth and
2.0 doubles the thickness of each new layer.
Enter the number of wedge element layers in the boundary layer.
Abaqus/CAE
displays the total Boundary layer thickness based on your
entries in Step 3 through Step 5.
If desired, toggle on Inactive faces, and click
Edit to select faces that you do not want to include in
the boundary layer.
The inactive faces are expected to be approximately planar and
perpendicular to local flow directions or along a plane of symmetry.
Note:
The default selection method is based on the selection method you
most recently employed. To revert to the other method, click Select
in Viewport or Sets on the right side of the
prompt area.
If desired, toggle on Create set, and enter a set
name to save a set containing all the boundary layer elements.
Click OK to close the Boundary
Layer dialog box.
The boundary layer will be created when you mesh the regions.
If mesh generation fails due to problems in the boundary layers,
Abaqus/CAE
displays a preview of the boundary layer mesh along with a warning dialog box.
Before closing the warning dialog and deleting the mesh preview, look for
problems such as self-intersecting layers near sharp corners; the possible
failure modes are similar to those described for offset meshes in
Reducing element distortion and collapse during mesh offsetting.
Make the necessary corrections to the boundary layer controls and try to mesh
the regions again.