Creating the boundary mesh for a bottom-up region

When you create a bottom-up mesh for a geometric region, the meshing process consists of two phases:

  1. A boundary mesh of quadrilateral elements is generated on the source side—and on the connecting sides of a swept mesh if they are included.

  2. Abaqus/CAE generates a hexahedral mesh using the quadrilateral elements as faces of the hexahedral elements.

Context:

Creating a boundary mesh allows you to preview the first phase of producing the bottom-up mesh. Viewing the boundary elements can help you identify problems that may prevent generating a bottom-up mesh. The boundary mesh functions for geometric faces of bottom-up mesh regions are identical to the tetrahedral boundary mesh capabilities in Abaqus/CAE except that a bottom-up boundary mesh is composed of quadrilateral elements instead of tetrahedral elements (for more information on tetrahedral boundary meshes, see What is a tetrahedral boundary mesh?, and What can I do with a boundary mesh?).

To create the boundary mesh for faces of a bottom-up region you must use the top-down region meshing process.

  1. From the main menu bar, select MeshRegion.

  2. Toggle on Preview boundary mesh in the prompt area.

    Abaqus/CAE automatically switches the default selection option from Regions to Faces.

  3. Select the geometric faces of a bottom-up region for which you want to create the boundary mesh.

  4. Click Done in the prompt area.

    Abaqus/CAE creates a two-dimensional mesh on the selected faces.

When the Mesh defaults color mapping is selected, Abaqus/CAE displays a boundary mesh using white to represent the quadrilateral elements, which is in contrast to the cyan color that Abaqus/CAE uses to represent the final solid mesh. When you query the bottom-up boundary mesh, Abaqus/CAE refers to the two-dimensional boundary elements as Quad boundary elements. In contrast, when you query the final mesh, Abaqus/CAE refers to the three-dimensional solid elements as Linear hexahedral elements.