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Table of contents
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Creating a digital prototype with complex blends and curves that extend across multiple parts presents unique challenges. Starting with the finished exterior shape and working out individual part details as you go is a more natural workflow to many designers. The technique of designing the finished shape and extracting components is sometimes called a top down design method.
A multi-body part is a top-down workflow which allows you to create and position multiple bodies within a single part document. This technique is especially useful for designing plastic parts. A top down workflow eliminates the need for complex file relationships and projecting edges between parts. You can control visibility, assign a different appearance, and calculate the mass for each solid body. When you complete the design, you can export the individual solid bodies as part files.
The advantages of using a multi-body part in a complex design are:
- Significantly reduces design time.
- The entire design resides in one document.
- All editing takes place in a single file.
- No up-front planning for file structure is required.
- All generated part files are associative with the master design.
How do I create a multi-body part?
The workflow for creating a multi-body part is designed to be minimally disruptive to the user. In other words, you can use common modeling commands to create a new body. Use sketch-based modeling commands like Extrude, Revolve, Loft, Sweep, and Coil to create a new body by selecting the New Solid option in the dialog box.
Use the Split command with the Split Solid option to create separate bodies in a part file. You can use workplanes, 2D sketches, and surfaces to define the split boundary. Use surfaces to define complex split boundaries.
Use the Derive command to import components into a part file as new bodies or to use as toolbodies for a cut, join, or intersect operation.
You can use the Move Bodies command to accurately position a body within the part document. Use the Combine command and select one or more solids to use as toolbodies to perform a join, cut, or intersect operation on a selected body.
What happens if I create a multi-body part by mistake?
If you accidentally create a multi-body part, you can edit a sketch based feature to change the solution to a Join, Cut, or Intersect operation. An undo operation also reverses the step. If it is too late to perform an edit or undo, you can use the Combine command with the Join option to merge the bodies. You can also delete the operation, such as a split, that created the new body, but you may lose features that were created on the body.
What happens if I create a new feature instead of a solid by mistake?
A body is an independent collection of features contained within the part file. All new bodies are added to the appropriate folder in the browser at the time of creation. You can control the visibility and appearance of solid and surface bodies by selecting a body and choosing Properties in the right-click context menu.
Expand a body in the folder to list the features that are applied to each body. Different bodies can share the same feature such as a fillet, chamfer, or hole.
An Application Option in the Modeling tab of Document Settings allows you to specify the default naming scheme prefix for new solid or surface bodies. This provides each new body with a meaningful name when you create it. The default body names are Solid for solid bodies and Srf for surface bodies.
How do I control body visibility?
There are two ways to select bodies to set the visibility status; set the selection filter to Select Bodies and pick one or more bodies in the graphics screen or expand the solid bodies folder and select one or more bodies in the browser. After you select one or more bodies, the context menu contains the following selections:
- Visibility
- Show All
- Hide Others
Use Show All to unhide all solids in a part file.
Use Hide Others to retain the selected solids, and to turn off the visibility for all unselected solids.
How do I document a multi-body part?
You can create a drawing document for a multi-body part as you would for any other part file. All solids are visible in a drawing regardless of the visibility state in the part file.
A multi-body part is a top down workflow which allows you to create and position multiple solid bodies within a single part document. This technique is especially useful for designing plastic parts. A top down workflow eliminates the need for complex file relationships and projecting edges between parts. You can control visibility, assign a different appearance, and calculate the mass for each body. When you complete the design, you can export the individual solid bodies as part files.
- Create a model representing the exterior shape of the finished part or, import a finished industrial design surface set and use stitch to create a solid model.
- Add features, such as fillets and shell, as required to complete the exterior of the part.
- Use work planes, 2D sketch geometry, or surfaces to split the part into separate bodies.
- Use sketch based modeling commands such as Extrude and Revolve to create new bodies in place.
- Use Derive to insert components into the part file as bodies.
- Use Move Bodies to accurately position the bodies in the part file.
- Use Combine to perform a Join, Cut, or Intersect operation between solids.
- Add additional features such as holes, grills, lips, and bosses to each body as required.
- Use the Make Part command to save the individual solids as derived part files linked to the master part design.