About Groups

If you are working with a part that you have meshed, associativity is maintained between the geometry of the part and the mesh. For example, you can select a face as the support for a pressure load, and the associativity applies the load to the underlying element faces.

In other cases, you must select a region of the mesh as the support because suitable geometry does not exist or is not available. For example, no geometry is available when you are working with a mesh part imported from an Abaqus^® input file or a Nastran bulk data file. As a result, you must select a region of the mesh as the support for, say, a pressure load or a concentrated force. However, you cannot directly select a region from the mesh as the support. You can select a mesh group that defines the region. For example, you can select a mesh group containing the element faces to which the pressure load is applied. For a video overview of groups, see Create Groups for Simulation.

A mesh group can contain only one type of mesh entity. A variety of tools are available for creating mesh groups:

Geometric and Proximity Groups

You can select geometry from your model (points, lines, or faces) and create a mesh group containing the mesh entities (nodes, element edges, element faces, or elements) that either underlie your selection or are within a specified distance from your selection.

Spatial Groups

You can select a point on your model and define the dimensions of a box or a sphere centered on that point. The box or sphere contains all the mesh entities of the selected type (nodes, element edges, element faces, or elements) in the group.

Boundary Groups

You can select geometry from your model (lines or faces) and a boundary (points on a line or curves on a face) and create a mesh group containing all of the mesh entities (nodes on a line or element edges on a face) that fall on the selected geometry within the selected boundary.

Manual Groups

You can select the type of entity in the mesh group (nodes, element edges, element faces, or elements) and do either of the following:

Select the entities directly from the finite element mesh representation.
Create a polygon that contains all the selected entities.

Boolean Groups

You can create three types of Boolean groups by operating on existing mesh groups:

Union
Intersection
Difference

The selected groups must contain the same type of entities.

If the mesh is not linked with the underlying geometry, you can select only spatial, proximity, and manual groups as the support for a feature. In addition, if you are working with an imported mesh that has no underlying geometry, you can select only spatial and manual groups as the support for a feature.

Note: You cannot use groups of native hex-dominant mesh items as supports for other features. For example, you cannot create a hex-dominant mesh of a fluid domain, then create groups from that mesh and use them as supports for other features.

Important: If you deactivate a mesh, any entities from that mesh are not used for solving the simulation. Missing entities can change or effectively remove supports for model features and invalidate your simulation. Verify that all groups have the correct content before running a simulation.

If the mesh is regenerated or edited, you can right-click a group in the tree and select Update to update the contents of the group. In addition, you can right-click a group in the tree and select Show Content to view the number of mesh entities in the group. The number of implicit nodes is also displayed, where:

For a group of element edges, the implicit nodes are the nodes at the vertices of the selected element edges.
For a group of element faces, the implicit nodes are the nodes at the vertices of the selected faces.
For a group of elements, the implicit nodes are the nodes at the vertices of the selected elements.

When you are reviewing the results of your simulation with Physics Results Explorer, you can use the display group tools to remove portions of the model from the display. This allows you to focus on areas of interest. Mesh groups are used by the finite element analysis, and they appear as display groups in Physics Results Explorer. However, the converse is not true: display groups are not available as supports when you are defining the features of your scenario.

Similarly, you use user sets only to organize entities in the tree. User sets do not have the functionality of groups; they cannot be selected as supports.