About Opening Part Models Containing Multiple Bodies
When non-Creo part models that contain multiple bodies are opened in Creo, each body in the source file opens as an individual solid body within the non-native part. The Bodies folder that appears as the first node of the non-native part or part component on the Model Tree stores the solid bodies of the standalone part or part component. Each part component of an assembly model has a Bodies folder and it contains the solid bodies of the individual part component.
A body consists of solid geometry and its specific material assignment. You can assign a different material to each body of a part and the part or the part component can contain as many bodies as the material assigned to its bodies. The number that appears in parenthesis next to the Bodies folder of the non-native part or part component indicates the number of solid bodies contained in the part model and is the same as the number of bodies contained in the source models. Maintaining the same number of solid bodies in the source models and the models opened in Creo ensures the preservation of the body structure of the source models in the models opened in Creo.
The first body in the folder is the default solid body of the part model and is an empty body. Each remaining body 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 part model or component.
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You cannot insert a part model of a non-native format as an import feature in a part model that you opened as a non-Creo model.
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When you right-click a body in the Bodies folder, the shortcut menu includes the following options:
• Set as Construction—Sets the selected body as a construction body. Construction bodies are not considered for the calculation of mass properties, the analysis of global or volume interference, and the detection of collisions.
The Unset as Construction option is available on the shortcut menu only when you use the Set as Construction option. The Unset as Construction option changes the construction body to a solid body.
• Create Part from Body—Creates a copy of the selected body and then creates a part from the selected body that includes a copy geometry feature.
• Assign Material
—Displays PTC_SYSTEM_MTRL_PROPS as the material that is assigned by default to the solid body. Click Other to open the Materials dialog box and assign a material to the solid body or edit the properties of the material assigned to the solid body.
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 the Boolean operations commands to merge, intersect, and subtract bodies. The geometric operations commands include moving, patterning, and mirroring of bodies.
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You cannot remove a body when it is the only body of a part.
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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 of Creo.
The view-related commands on the mini toolbar enable you 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.
Creo supports multibody models.
Watch a video about multibody support in Data Exchange: