Well, last week was so hectic that at times I wished I could be the one splitting myself into multi-bodies. Hmm, perhaps, what I really need, is a few good buddies (like Molly Maid and Supper Nanny) that can come over and give me a hand every now and then. Anyway, not so long ago, I was telling you about my little exercise in creating new parts using the Split command. But that isn’t the only way to create new parts out of a multi-body part in SolidWorks. Because multi-bodies can be the result of something as simple as creating an extrusion that doesn’t merge with the rest of the part, and aren’t always the result of slicing the part by means of the Split command, there are also other ways to save those bodies as parts or to insert the bodies into a new part. I know, both options sound the same, but the results are slightly different.
As part of my exercise, I created a copy of my original part and named it “Buggy Two”. This time, I cut the part in half by means of an extruded cut, instead of the Split command. The cut removes a thin layer of material, right across the middle of the part, and creates two bodies. SolidWorks then prompts the user to choose whether to keep all bodies or only one of them. I chose to keep both bodies and ended up with a multi-body part, just as I wanted. Now, to create new parts out of these two bodies.
First, I tried Save Bodies. You can find this option by RMB clicking on the bodies folder from the feature manager. You will then see the following dialog box, which looks and works very similar to the Split command, but without the Trim tool.
In the parent part, Buggy Two.sldprt, a new Save Bodies feature has been added to the feature manager. The references and dependencies between the parent file and the two new files that were created this way are very similar to those of files created by using the Split command. Any change done to the parent part BEFORE the Save Bodies command, will spread to the new parts. Changes done AFTER the Save Bodies command won’t. Also, if the Save Bodies feature (or the extruded cut) is suppressed in the parent file, the new parts won’t be able to load at all, unless the parent file is closed or can’t be located, in which case, the new part will open with an out of context reference to the parent file.
Inserting a body into a part, however, works a bit different. To test this option, I saved a copy of Buggy Two.sldprt as it was just before saving the bodies, and renamed it “Buggy Three.sldprt”. I opened the bodies folder in the feature manager and RMB clicked on each body, selected Insert into Part from the menu, and gave each of my new parts a name.
The two new parts have references to the parent file Buggy Three.sldprt, but there is no trace in the history of Buggy Three.sldprt, that may provide a clue about the two new parts that were just created this way or when in the history of the parent file were the other two created. There is no way to access those files from the parent part, either. Also, any changes made to the parent file, at any time, will spread to the other two files, unless the reference to the parent part is broken or out of context (file can’t be located or was renamed).
Out of curiosity, I suppressed the extrude-cut feature that created the two solid bodies in Buggy Three.sldprt, just to see what would happen to the other two parts. Unlike with the Split command, both parts were able to load, but can you guess how they looked like? Yes, they looked exactly like the parent part before the cut!
So far, I think I like what can be done by using multi-bodies in SolidWorks, specially when creating objects that contain many pieces that must fit together like a puzzle, following a shape in particular, but I’m a bit concerned about all those references. It seems to me that in order to avoid potential trouble for ourselves or others that may have to work with our models, we must try to be a bit organized: document what we’re doing, keep the files and their parent together, etc. Now, that’s a bit of a challenge!
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