The purpose of the Bodies view is to provide:
A listing and visualization of bodies defined in the FE model.
A listing of element types present in a given set of bodies, along with corresponding element counts.
An element selection filtered by one or more bodies.
An element selection filtered by one or more element types within a set of bodies.
The ability to group elements into multiple bodies. See Grouping Bodies.

For models based on Mechanical data, each Part corresponds to one body.
For models based on NASTRAN, ABAQUS or Mechanical APDL data, one and only one body, by default, exists. Please see Grouping Bodies below.
For multiple imported mesh files, the process described in the two previous notes is applied by file.
Colors in the graphics display differentiate the bodies.
When importing an archived file from NASTRAN, ABAQUS or Mechanical APDL, FE Modeler allows you to split a finite element model into multiple bodies based on the:
Material assigned to an element.
Or...
Element type assigned to an element.
Or...
Shell Thickness Identifier assigned to an element.
Or...
Element component. This option is not available when importing a NASTRAN file.
By default, the Body Grouping property is defined as: None (only one body is defined). You must select how to group the bodies, either by material, thickness, element type, or element component.
If grouping by materials:
The element grouping is performed even if the actual material definition is not found.
For a Mechanical APDL archived file, the grouping is performed based on the MAT attribute defined with the element in the EBLOCK section.
If an element does not have an assigned material, an additional group is added to contain these elements.
If grouping by element types:
For a Mechanical APDL archived file; the grouping is performed based on the TYPE attribute defined with the element in the EBLOCK section.
For NASTRAN; the grouping is performed based on the element definition (such as CQUAD4).
For ABAQUS; the grouping is performed based on the element name defined with the TYPE parameter on the *ELEMENT keyword.
If grouping by shell thickness:
For NASTRAN, the grouping is performed based on the Property ID used in each element definition (such as CQUAD4). Variable thicknesses and orientation angles are ignored for the grouping.
For a Mechanical APDL archived file, the grouping is performed based on the REAL or SECTION attribute defined with the element in the EBLOCK section.
For ABAQUS, the grouping is performed based on each *MEMBRANE SECTION, *SHELL GENERAL SECTION, or *SHELL SECTION keyword.
If an element is not a shell element, an additional group is added to contain these elements.
If grouping by element components:
The element belongs to the body corresponding to the first element component that refers the element. If an element is referred later in the file to another component, this referral is ignored. Therefore, the order of the components is important.
This option is not available for NASTRAN.
If an element is not referred by an element component, an additional body group is added to contain these elements.
How to Group Bodies
After adding mesh files to the Model cell in the schematic, view the file Properties and change the Body Grouping property as needed for each mesh file.
Body Grouping is only available for NASTRAN, ABAQUS, and Mechanical APDL files.
If you change the body grouping (or any other property) on any imported mesh file after it has been read into the FE Modeler Editor, you will be prompted to destroy all work done to the file in the FE Modeler Editor in order to import the mesh with this new setting. See the mesh import Caution for more information.
Body grouping is done on a per file basis. Only items from the file for which the body grouping was specified will be included in the body that is created.