saving individual solid bodies as new parts

[office6PUWT]

Can someone show me how to remove Solid 3 from the attached ipt part and save it as a new .ipt file. I also need to save the door as a new ipt file so that I can assign separate materials and appearances to them in my assembly. with this single part file in the assembly my drop down list of available mats/apps disappears?

many thanks Luke

[leowarren34 · Accepted solution]

Hi @office6PUWT,

The part you have uploaded has some unresolved references (linked files) however you can bring solids out a part using the Make Components tool in the manage tab - It will create new part files for any solids selected and bring them into an assembly.

[paulmWABYD]

Is there a way to do this without creating an assembly? The original question was asking about saving a body out as a new part; using a new parent assembly is a work-around. This would be similar to the "save bodies" functionality in Solidworks. 

[kacper.suchomski]

Yes; use Make Part tool.

[paulmWABYD]

This mostly addresses the issue, thank you. A crucial missing piece, I feel, is having the option to remove the body from its original part file so that you don't end up with a duplicate (the body now exists in old and new parts). 

EDIT: I see in office6's original post that he actually specifically asks for the body to be removed. So the original question truly hasn't been addressed. The "save bodies" tool in SW gives all of this functionality and more. 

[SBix26]

Can someone explain how the SW tool handles inter-body dependencies?  One of the great benefits of multi-body modeling is sharing sketch geometry and workfeatures between bodies, as well as features which cut through multiple bodies.  What happens to these sketches and features when a body is removed?  How is the removed body defined in its new file without the geometry on which it depends?

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Sam B

Inventor Pro 2024.1 | Windows 10 Home 22H2

[paulmWABYD]

I used SW for 10 years before I went to an Inventor-only employer. 

All parent geometry still exists in the parent part. When bodies are saved out as separate parts, a feature is inserted into the feature tree, much like Inventor's "make part" feature. However to modify parent geometry, you need only roll back the feature tree to before the save feature (the equivalent of moving back the "EOP" marker) and modify your parent part. When you move the EOP forward again, the changes are applied to all child parts. If you make modifications AFTER the save feature in the tree, changes are only made to the parent part. So, the changes are chronological based on their status before or after the save feature. It makes multi-body modeling a breeze, because you can always go back and modify geometry from the parent part, but the geometry doesn't have to exist in the parent part, so you can have both parent and child in an assembly without duplicates. 

Here is a video on it. Fair warning, I didn't watch the video.

https://www.youtube.com/watch?v=A0vLgZUfR4E&ab_channel=AliNasser

[SBix26]

Sounds pretty much like Inventor's derived part workflow (which is what Make Part/Make Components use) with some bells and whistles added.

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Sam B

Inventor Pro 2024.1 | Windows 10 Home 22H2

[paulmWABYD]

I would argue that the differences are massive, and functionally, one offers so much more:

• Ability to remove saved-out parts
  • Can't use parent and child in the same assembly, as the saved body will be a duplicate
• Presence of a feature in the feature tree
  • Allows chronological editing before/after part is saved. This is crucial, as it allows BOTH editing of derived parts or only of the parent part

As of right now, if you have a part with two bodies in it, you're forced to make a new assembly and save them both out separately as new parts. Not only that, but you must retain the original part somewhere, as it's saved as a reference. So if you've been working on one part for a while and decide you'd like to cut off a piece of it, you need to change your assembly structure and/or workflow. Having additional features makes a big difference, and it's very noticeable if you once had access to them and now must use workarounds. 

[SBix26]

Agreed, the feature in the browser which shows where the division occurred is useful. 

One method to achieve this in Inventor is to pattern the original solid body some convenient distance away from the original, making it a New Solid.  Now you have the Pattern feature in the browser to indicate the division, and you can add features before the pattern (common to both) or after (specific to one or the other).

Yes, you will be best served in Inventor by keeping the master file as the driving geometry and deriving out the two solid bodies in separate files for iProperties, material and appearance, annotation.

You are incorrect, though, that somehow this requires an extraneous assembly to be created-- not sure where that comes from.

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Sam B

Inventor Pro 2024.1 | Windows 10 Home 22H2

[paulmWABYD]

I was referring to the fact that you can only save out one part at a time. If you were to use "make components" to save out more than one body, you need to form an assembly, which is what I ran into when trying to save out a multibody imported STP. 

[SBix26]

Don't have to if you don't want to:

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Sam B

Inventor Pro 2024.1 | Windows 10 Home 22H2