17.7.1 Overview

ABAQUS/CAE follows these basic steps to generate a mesh:

Generate a mesh on each region using the meshing technique currently assigned to that region. By default, ABAQUS/CAE generates meshes with first-order line, quadrilateral, or hexahedral elements throughout.
Merge the meshes of all regions into a single mesh. For more information, see “Meshing multiple three-dimensional solid regions,” Section 17.11.1.

Typically, ABAQUS/CAE merges the nodes along the common boundaries of neighboring regions into a single set of nodes. However, in certain cases ABAQUS/CAE creates tied surface interactions instead of merging these nodes; for example, along the common interface between hexahedral and tetrahedral meshes.

Meshes generated by ABAQUS/CAE conform to the geometry of the part or part instance they discretize, as shown in Figure 17–31:

Figure 17–31 The mesh conforms to the geometry of the part instance.

A node is generated at each geometric vertex.
A connected set of element edges is generated along each geometric edge.
A connected set of element faces is generated along each geometric face.
Nodes that are on the boundary of the mesh (including the midside nodes of second-order elements) are also on the boundary of the geometry.
Midside nodes of internal second-order elements are centered between the two corner nodes.

For detailed, step-by-step instructions on creating a mesh, see “Creating a mesh,” Section 17.14.1.