Splitting (exploding) a solid consisting of several separate bodies

[Anonymous]

Hi,

Inventor 2017 SP4 user here. Talking about imported geometry, I have a model which in fact consists of several disconnected parts but in the feature tree they all go as one solid body. I would like to split this body so that each part would become a separate body without creating all these split planes / surfaces etc.

Should be possible, right? Or not really (because it is Inventor after all).

Thanks!

[TheCADWhisperer]

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@Anonymous wrote:

.... Or not really (because it is Inventor after all). 

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How much training have you had?

Attach your original file here and someone will create a video demonstrating how to do it.

[WHolzwarth]

Try this (extracted from Help):

On the ribbon, click 3D Model tab Modify panel Copy Object .Choose Body to select one body

Select an output option

Surface creates a Base Surface feature for every body or every set of contiguous faces of a single body selected.
In the graphics window, select the geometry to be copied as a new feature.

Click Apply to complete the specified action without closing the dialog box.

Stitch the new surface to a separate body

Delete the copied faces (Lump option)

Next one

[johnsonshiue]

Hi! I think the part you are working on consists of multiple disjoint lumps. In earlier releases, Split command cannot separate disjoint lumps if the tool does not intersect with all of the lumps. The restriction was lifted in 2017.4 (not exactly sure). You should be able to use a work plane (not intersecting any lump) to split the lumps. If you want, you can post the file here or send it directly to me (johnson.shiue@autodesk.com), I can take a look and show you how to do it.

Many thanks!

[Anonymous]

Thanks guy.

I think I have found the solution for my particular case. I have saved the model as STEP (since it was an imported geometry anyway, albeit modified with a couple of Extrude commands), and then I opened the STEP and got all of them as separate bodies.

[fkellogg]

I had a similar problem, with a single shape that kinda looked like a science fair display board; three intersecting 3/4" thick planes.

I successfully Split the back plane off, and was left with the two side planes as one (disconnected) solid.

To separate the two side planes, I used Split again, using a bisecting work plane, that did not even touch either of the solids.

Wa. La! Three separate solids.

I'm used to AutoCAD's Separate Solids command.

Maybe you did not want all those work planes that now cannot be deleted, but that will have to do for this newb. Next time I'll extrude them separately in the first place.

[johnsonshiue]

Hi! Just to clarify the terminology a bit, those separate entities are disjoint lumps within a solid body. They are not separate solid bodies. Inventor (and AutoCAD) supports an unique concept of disjoint lumps. They belong to one body. They are separated in the space. But, when they intersect each other, they will be merged. This is a big distinction between lumps and bodies.

In the past, it was relatively confusing and painful to separate disjoint lumps into multiple solid bodies. Now it is very simple by using Split command.

Many thanks!

[SBix26]

It might actually be easier to go back and edit your initial extrusion(s) to make separate solid bodies than to create the planes and splits.  If you post your file, someone here can show you how to do that.  Depends on the complexity of the geometry, but editing existing features to change your model is an important skill to develop.

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Sam B
Inventor Pro 2020.2.1 | Windows 10 Home 1903
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