How do I convert a part with 2 solid bodies into 2 solid bodies?

[ToddPig]

I have a part were the first extrude is 2 sketches that is  used to create 2 solid bodies.  I continued to finish the design, then (like what I would do in Solidworks), I want to create an STL file for each body.  Is SW I have hide each body, and save as STL.  Is there an Inventor equivalent for this process?  If not, how to I change my part so that each body/solid is shown.  How does Inventor consider 2 volumes that are not touching as one solid?  Why is this the default?

[-niels-]

I know i've saved separate solids from a multisolid as STL's through the 3D print environment by using visibility, you could try that...
Otherwise, you can make each solid into its own part through the make part/make components option on the Manage tab...

Hope that helps.

[SharkDesign]

[JDMather]

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@ToddPig wrote:

I have a part were the first extrude is 2 sketches that is  used to create 2 solid bodies.    How does Inventor consider 2 volumes that are not touching as one solid?  Why is this the default?

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No file Attached???

I will make a wild guess that you created a single Disjointed body rather than 2 bodies.

(It should show in a folder at the top of the browser - just like in SolidWorks).

If that is what you in fact did, and your feature history makes in impractical to Edit the second Extrude to New Solid, then simply do a Split.  Same as in SolidWorks.

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

[ToddPig]

JD,

File attached.  Thanks for the suggestions.

I tried using the split command (the "ExstrusionSrf1" feature was created just for this purpose), but couldn't figure it out.  

Any help would be appreciated.

[JDMather]

I deal with adults.

I saw the name of your first feature and elected to decline participation.

[ToddPig]

I renamed the first feature.    I'm looking forward to your adult solution.

[ferrisb]

When you create a new feature in a part there is a little box you check that "creates new solid"  it's in the extrude, revolve, sweep dialog window ECT...

After the fact you could use the split command.

[mcgyvr · Accepted solution]

Fastest solution I've used before was to just create 2 cut extrusions to remove each piece and suppress one then save my STL.. Then suppress the other and save the second STL.

Just sketch on the side and project the edges (hover over one edge then right click and "select tangencies" to quickly select the perimeter) then extrude (cut) to remove.. Repeat for the bottom

P.S.. Adults swear sometimes.. Its ok.. 

[ToddPig]

That is pretty much what I did, but I used delete faces to see if I can "unbuild" the model. Your idea is much faster. When did Inventor add "select tangencies"?

[mcgyvr]

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@ToddPig wrote:
When did Inventor add "select tangencies"?

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Not sure.. Certainly saves a ton of time for something like this.. 

[ToddPig]

I should've mentioned that I am using Inventor 2020, and it seems like they removed that option. I remember being able to do that in 2018. I tried to go back to my first feature, and change this, but no luck. I also, can't figure out the SPLIT command. I tested the SPLIT command on a part that is one solid body (and also 1 volume), and it worked. But, I can't figure out how to SPLIT a solid body (that is two volumes) into 2 solid bodies.

[johnsonshiue]

Hi Todd,

I think you are talking about the disjoint lumps. This is one of the most frequently complained confusion by SWX users. SWX treats disjoint bodies as bodies. In Inventor, a body can contain disjoint lumps. Spatially separated lumps can still constitute a body. There are advantages of this paradigm. Think about patterning. For example, if you need to pattern 10k rods. In SWX, it will be 10k bodies which will be heavy and slow. In Inventor, you can pattern it 10k and the entire thing is still one body.

To separate the disjoint lumps, here is a workflow you can use. Create a Rect Pattern of the body (with disjoint lumps) -> two instances -> select Create Body option. The two bodies will be overlapped. Hide one. Use Delete Face -> Lump selection -> remove the unwanted lump. Repeat the same step to the other body.

Many thanks!

[DME_Ltd · Accepted solution]

I see that this thread is very old, but it populated at the top of my Google search, and led me to solve the problem programatically.

My issue couldn't be solved with a simple "Split" command, because I had a "Coil" extrude that split my part like a candy-cane (Bevel gear that needed to be 3D printed in two halves).

Here is the VB code that you can create an iLogic rule directly, and it should work in any environment. For some reason using "Select Tangencies" didn't actually work, but this will do the same thing.

Dim p As PartDocument = ThisDoc.Document
Dim ss As SelectSet = p.SelectSet
Dim f As Face = ss.OfType(Of Face).FirstOrDefault

If f Is Nothing Then
	Try
		f = ThisApplication.CommandManager.Pick(SelectionFilterEnum.kPartFaceFilter, "Select a Face")
	Catch
	End Try
End If

If f IsNot Nothing Then
	Dim obj As ObjectCollection = ThisApplication.TransientObjects.CreateObjectCollection()
	For Each c As Face In f.FaceShell.Faces
		obj.Add(c)
	Next 
	Logger.Info("Faces found :: {0}", obj.Count)
	ss.SelectMultiple(obj)
Else 
	Logger.Info("No Face Selected. Pre-select a Face and run again.")
	MessageBox.Show("No Face Selected. Pre-select a Face and run again.")
End If

You will need to pre-select a face, then run the code.

After which, I used the "Direct" feature (under the "3D Model > Modify"  Ribbon Tab). You can "Delete" your selection, or "Move" or "Rotate" to achieve what you need.

I opted to just export as a single STL, but you could then do as '@mcgyver' commented above, make a large extrude and "extrude -cut" out each piece. Gives you options.