If I make a multi-body part can each and every body be saved as a separate body with it's own file name?
How do I save each body separately?
right click on the bodies in the Solid Bodies folder of the Feature Manager Tree and you can insert them in to new parts.
That worked Dan, but, it looks like a dumb solid. I can't edit the tapped hole.
You'll want to edit the original multi-body part. Any changes you make there will transfer over. Changes to the derived part will not transfer backward, however.
I don't get that option...
Rick Becker wrote: I don't get that option...
Rick Becker wrote:
That's because there's only one body.
There are 3 bodies in the screen capture... (I just didn't capture the tree in that screen snippet)
Can you post the Part file?
Thanks for taking a look at the Glenn.
I'm not getting that option when right-clicking on a body in the graphics area either. I suspect it's because they were all created with one feature. However, when I expanded the Solid Bodies folder and tried again it's there.
This probably falls into the inconsistent UI.
Select in graphic doesn't select the body. So different commands came up.
Do a "Save as" on your multi-body part. Call it Body 1. Delete bodies 2 and 3.
Do a "Save as" on your multi-body part. Call it Body 2. Delete bodies 1 and 3.
Do a "Save as" on your multi-body part. Call it Body 3. Delete bodies 1 and 2.
Edit: Or do you want to keep the relations to the original multi-body part?
That worked Scott. Thank you.
I just wish it was "clean" By that I mean I wish any and all remnants from the 2 deleted bodies were gone. I do fundamentally understand that a history based system needs to retain everything.
If you don't need the relations, you could export as a parasolid / iges / step and the re-import. You would also lose the rest of the features in the history tree.
Rick Becker, I enjoy building assemblies this way, especially when the geometry is likely to change during the design process. By creating new parts from bodies, you're linking the new parts back to the original. Any time you edit the multi-body part, your new parts will update as well. I comes in particularly handy when creating welded assemblies.
If you want to keep the relations, then create the new part. Use "Insert Part" and pick the multi-body part. Use "Delete Body" to get rid of the bodies you don't want.
Assembly from Part – No mates required | Boxer's CAD CAM Blog
You can also use configurations to manage these things and reduce the number of part files knocking around. Also when you come to do the drawings just change the configuration on a sheet to get the other "parts". Of course that approach really only works if the bodies are similar - but it is really handy for doing manufacturing plans:
Config 1 - stock
Config 2 - initial cuts
Config 3 - holes
On a multi sheet drawing you just duplicate the initial sheet, then change the configuration. This is one of SolidWorks USPs as far as we are concerned - things like this are generally considerably harder to do and manage in other systems.
meant to add, the single part configuration approach is also great for parts and tooling. We've done many cavity inserts this way:
Config 1 - part design
Config 2 - shrinkage added and shut offs
Config 3 - Cavity insert "assembly"
Config 4 - cavity insert
should be able to save bodies out to parts.
Yes you can.
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