Splitting Non-interfering Parts of a Body

[mkrsmanovic]

I have a body that's got two non-interfering parts. It's not possible to create a plane in between them that would avoid them both. How can I split these two parts?

Here is an oversimplified illustration. In reality this geometry are two pipes coiling around each other without touching.

[davebYYPCU]

How did you make that as one body?

Where do you want to split it?

Use origin as source of any required planes.

Might help…

[jhackney1972]

Which way do you want to Split them, across the ends?  Please attach your model.  If you do not know how to attach your Fusion 360 model follow these easy steps. Open the model in Fusion 360, select the File menu, then Export and save as a F3D or F3Z file to your hard drive. Then use the Attachments section, of a forum post, to attach it.

[mkrsmanovic]

@davebYYPCU, I got the model from someone else so I have no idea how they combined two different pipes into a single body. The only thing I can imagine is someone converted a different file type into a fusion file. I'm not sure.

@jhackney1972, I'm unable to attach the file as it is a proprietary information. 

The way I want to split it is to break up the two "sub-bodies" (in lack of better term) that are not in contact. I ran interference check, so I would like to separate as different bodies anything that's not connected. So, from my example above, I would like to end up with two bodies, where each body would be a half-torus.

[davebYYPCU · Accepted solution]

Then show in a pic the expanded Browser, and the Timeline, hide the actual bodies in the window if need be.

From here, create a Boundary Fill for each body. Hide the originals.

Might help….

[Drewpan]

Hi,

Maybe you cannot easily split this "one" body, but you may be able to make an exact copy of it and replace it.

Since the two parts are not touching this might make it easier to do this. Draw a box on a plane that will enclose

the geometry.

Extrude the box and turn off the visibility of the body you want split so they are not joined.

Do a combine cut operation using the interlocked bodies as the cutting tools to create the mold.

Do a split body to cut the mold in half and access the inside.

Switch to surface and create a surface of the mold with the offset tool.

Stitch the four half surfaces together.

Use thicken to replace the surfaces with a body.

Create Components from the bodies.

Now you have two separate bodies of the original single interlocked body.

This is a very crude method but it should work. If the original bodies are two pipes then the mold should create

inside and outside dimensions of the pipes.

Cheers

Andrew

[TrippyLighting]

There are several ways to do this.

You should be able to use the boundary fill feature (surface tab -> Create->boundary fill) and create a duplicate of each object by selecting only that cell. 

If the geometry is simple enough, you could also unstitch the surfaces and re-stitch them for the individual objects.  

[mkrsmanovic]

I'm going with Boundary Fill approach as @davebYYPCU and @TrippyLighting suggested.

@Drewpan, I appreciate the suggestion. That would work for the simplified example I shared. But my case is more complex. Imagine the shape of spaghetti in a bowl, just without touching.