Problem
This article goes over how to use the Save Bodies feature in a multi-body part file to save each body to a separate Part file and create an Assembly.
Solution
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Open up a part file with multiple bodies in it. Note: The example below has four bodies.
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Go to Insert > Features > Save Bodies
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This will bring up the Save Bodies Property Manager showing all the available bodies and some options for the feature
- Check the box near each body in the list to enable it and have the name auto-assigned. The "Auto-assign Titles" button can also be used to have this done for all listed bodies.
- To use a custom name, double-click the body in the list under Title or the flag in the graphics area.
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Under Template Settings, use the default templates set in Tool > Options > System Options > Default Templates, or override this by selecting the 3 dots next to each template file path
- Select "Consume cut bodies", which removes the body from being listed in the FeatureManager design tree under Solid Bodies.
- Select "Propagate visual properties" to transfer the visual properties
- Use the "Origin location" selection box to change the origin
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To create an assembly, select "Browse" under the "Create Assembly" section to choose a name and location for the assembly
- Accept the feature by clicking the green check mark, and a new feature at the bottom of the tree for this command will appear
- If any new bodies are added or changes are made, they will need to be added before this Save Bodies feature in order to show up when editing the Save Bodies feature
The separate Part files can now be opened, which will have a feature referencing the Save Bodies feature, and the Assembly file can be opened as well.
In the assembly, all parts will be fixed and have an external reference back to the original part file.
For additional support, existing customers can submit a ticket or new customers can contact Hawk Ridge Systems.
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