When I go to the save bodies as a part it doesn't carry with it the features used to create it. As shown in the picture. I don't want the Stock- <part name>. I want a complete independent body with all the features used to created listed.
the simplest way is to do a save as of the original file, and then delete out the other features (or maybe just the other bodies, if there are dependencies you don't want to re-map) from the new file.
Yes that would work but my original file has some many bodies and features. What I'm trying to do is to make an assembly with all the many bodies I have so I would have to do your method for every body
First question has to be why you need the features?
Many people use the multibody method to create their assemblies. All the features are parametrically linked & accessible from the original multibody part.
That sounds like a good way to save a little time early and waste a lot of time later on.
There are different schools of thought on Multibody (Master Model) vs normal Assembly (Separate Parts) techniques. I use both without problems, but am old school enough to prefer the separate parts in an an assy method, but usually controlled with a Master Sketch/Skeleton.
Some pros' & con's...
SolidWorks Featured Author Blog: Multibody vs. Assembly
Me too. That is why when I took over the multi-body part/design, I wanted to convert it to assembly. Then I ran into the "save Body" -"Stock" thing and could not believe there wasn't away to save the body into an independent (no "Stock" thing) part.
A coworker built a multi-body part consisting of 16 bodies. It should have been done using assemblies with mating. This assembly needs a lot of modifications from time to time. I used the "Save Bodies" command with the "Create Assembly". So now I have the assembly....no problem......BUT....every time I need to modify one of the part features in the assembly, I must open the part in its own file, then right click, select "Edit in Context", then another window opens up, (I now have 3 windows open), then make my changes to the feature. Then say yes to saving the part on the next 2 screens. Pain in the butt. So yes the features are parametrically linked and yes I can modify the features....However considering the scope of this software and power behind it, I assumed there would be an easier way than having several screens and menu selections to wade through to simply edit a feature of a part that was saved from a multibody.
why not make seperate configurations where you can suppress the parts of the tree you don't need for each part and when you goto assemble just pick each part by it's configuration?
Mike, seperating a model into individual bodies is not particularly difficult for a CAD package to do. Updating those bodies down stream is more challenging because editing the model can easily change the number of bodies generated and assigning them to a particular file is an exercise in predicting the intent of the user.
What you're describing is even more difficult. There is no way to systematically correlate features to geometry without knowing what the geometry looked like before the feature.
In this model, there is one feature which generates the two discs (cut extrude1). I can insert the thin disc into a new file, but beyond that the software has a dilemma: Without the base feature (Boss-Extrude1), the cut that defines the thin lid doesn't exist and with the base feature, the model has excess geometry. Now, you could argue that this could be resolved by simply adding a Delete Body feature and removing the thick disc. But that doesn't do anything to simplify your feature tree and may be impossible with features that are linked by equations or are driven by assembly-context references.
You could try exporting it then import it back in and use recognize features. But that has it's own issues.
Retrieving data ...