When non-native part models contain solid bodies, their import, insertion in existing parts, and inclusion in assemblies as part components create multiple solid bodies in the imported part models in Creo. New bodies are created in Creo for each of the bodies in the source model. The Bodies folder contains the solid bodies of the imported part or part component of an assembly model and is the first node of the imported part model on the Model Tree.

There is an individual Bodies folder on the Model Tree for each part component of an assembly model. Each Bodies folder contains the solid bodies of the part component to which the folder belongs. The number that appears in parenthesis next to the Bodies folder of the part model or a part component of an assembly model is the number of solid bodies contained in the part model or part component. The number of solid bodies contained in the imported parts or part components of assemblies is the same as the number of solid bodies in the source models. Having the same number of solid bodies maintained in the source and the imported models, ensures the preservation of the body structure of the source models in the imported models.

When you expand the Bodies folder on the Model Tree, the solid bodies are listed according to the order of their creation and you cannot reorder them. The first body in the folder is the default solid body of the part model. Each of the remaining solid bodies in the Bodies folder contains an import feature that corresponds with a child feature of the part model or part component. The import feature of each solid body has the same ID as the import feature of the part model or component.

A body consists of solid geometry and can have its own material assignment. You can assign a different material to each body of an imported part and the part can have more than one material. When more than one material type constitutes the solid geometry of an imported part or part component, the part or the part component contains as many geometric solid bodies as the different material type of the solid geometry of the part or part component.

When you right-click a body in the Bodies folder, the shortcut menu includes the following options:

The mini toolbar for the solid body of a part model contains body-specific, Boolean, and geometric operations commands. The body-specific commands include setting a body as the default body of the part, splitting a body, removing a body and its geometry from the Bodies folder, and view commands. The geometric operations commands include moving, patterning, and mirroring of bodies. The commands to create, split, or remove bodies, and the Boolean operations command to merge, intersect, and subtract bodies are also included on the Body tab (Model > Body) of Creo.

You can use the view-related commands on the mini toolbar to zoom a body to the bounding box of a selected object, hide and unhide a selected body, only show a selected object and hide all other objects of the same type, or show all objects of a specific type except the selected object of the same type.