Splitting a solid body

[ToddPig]

I have a sheet metal part where I would like to make a cut thru the part, and have the result be two solid bodies.  I am able to make the cut, and but even though it looks like there are 2 solid bodies, the feature tree only shows 1?

[JDMather · Accepted solution]

You are creating a Disjointed solid body.

Use Split.

Attach your *.ipt file here if you can't figure it out.

[johnsonshiue]

Hi Todd,

Inventor allows disjoint lumps, meaning a body can have separate lumps and they are not joined together. This is a concept not available in Solidworks. I understand that it can be a bit confusing but it has its own strength. It can make some modeling operations more flexible. For example, you can easily mirror a feature with space in between. They are two lumps in the space. Then you add another feature to connect the two.

Like JD mentioned here, you will need to use Split command to split the body into two separate bodies. Extrude command can create a brand new body or operates on the same body. It cannot separate a body into two bodies.

Many thanks!

[ToddPig]

That worked. Thanks JD

[ToddPig]

Johnson,

This concept has been available in Solidworks for a long time. This is what lead me to trying this in Inventor.

To make sure I'm using the correct term in future posts.... A solid split into more than one body, is a "lump"? I see the Solid Bodies folder in the feature tree, and I see the number increase when I use the split command (this is the same as Solidworks), but I don't see anything referencing "lumps". The term "lump" is more entertaining, but I want to make sure I'm using it correctly.

[JDMather]

Imagine this shows in the browser as one solid body.

Futher, imagine that the "box" is hollow on the inside with some wall thickness.

If you wanted to delete the disjointed lump you can use the Delete Face command with the Lump option.

If you wanted to delete the hollow inside of the box you could use the Delete Face command with the Void option.

These techniques can be important when you can't simply go back and edit earlier features as that might interfere with downstream features or particularly when working with imported base (dumb) solids.

[Curtis_Waguespack]

Hi everyone,

Just to add to the general knowledge of the Split tool and disjointed bodies, see the attached 2017 file for an example where split creates 2 solid bodies where we would expect 6.

This is simply a limitation of Inventor's at the moment. I think there is an Idea Forum idea for this, but I don't have the time to look right now.

Ideally though we'd have some control in in the results of the split tool, to tell it to make disjointed bodies separate solids, or maybe some other tool that would be run on a solid body that has disjointed bodies and make them separate.

I asked about this when multi-bodies were released approx. 8 years ago, but have not seen any attention devoted to this. I have in the past done work that required a great deal of extra effort to make a part like my example into separate solids.

The current behavior of creating disjointed bodies that can then be joined with other features that johnsonshiue describes does have merit, and provides convenience for an entire other set of workflows, but it would be nice to have the ability to create new solids from disjointed bodies as well. 

I hope this helps.
Best of luck to you in all of your Inventor pursuits,
Curtis
http://inventortrenches.blogspot.com