Delete (derived) Solid Bodies from Part

[SEC_CAD]

I have created a sheet metal enclosure for a third-party power supply. The enclosure needs to reference features on the power supply so I derived the power supply part into my enclosure part.

I have finished my enclosure design. I cannot create a flat pattern because my part is multi-bodied. I want to delete the 110 solid bodies of the power supply but I can't.

I have tried using Delete Face with Void ON. This removes the item from the display but keeps the solid body in the model tree. It only 'removes' one solid at a time. I would need to do this 110 times to delete the whole power supply but it would be pointless because I would still be left with all of the solid bodies.

I have tried to creating a new solid that surrounds the power supply and then use Combine to subtract the many solids of the power supply but I get the error "problems trimming and discarding faces".

What is a simple and reliable way of deleting solids?

Thanks.

[A.Acheson]

Hi @SEC_CAD 

Is delete solid bodies the only path forwards? Can you suppress the part where it was derived to or beak link or indeed delete? Can you show an image of the browser where your having issue mass deleting solid bodies? 

You could delete solid  by code if time is just the factor. You will likely have to delete the features that made the solid body also. 

[Gabriel_Watson]

Two options here depending on how you prefer it, would be to either:
1- Derive again, this time the whole enclosure part and select to omit the objects/solids coming from the power supply.
2- In your enclosure part, open the "Solid Bodies" folder in your model browser to right-click and remove visibility of the solids from the power supply, then (save and) insert the enclosure part into an assembly, and finally use "Create Simplified Assembly" which can make a new part that ignores what is not visible.

Of course, this all cancels out your ability to re-edit the same file from the newly derived ones. But if you're struggling with a workaround, those are the best ones if you can keep one more file or two around.

[Biju.Veedu]

I don't think there is an option to delete the body of the inventor. Not sure if it works for your situation, but have you tried using "make part" to save the enclosure part and work on it?

[James_Willo]

Hi, you could try these as well. 
Right click and edit the derive and deselect the ones you don't want, you can shift select nodes in the derive tree and deselect all at once.   
Another option is 'make components' on the manage tab and only select the one you want. You're creating a bit of a chain doing it this way so option 1 is better. 

[johnsonshiue]

Hi! Inventor does not have a dedicated Delete Body (solid or surface) command. You may use Delete Face -> Lump selection instead. After the lumps are deleted, the body will become empty. But it is still shown in the Solid Bodies folder in the browser.

Many thanks!

[SBix26 · Accepted solution]

Better in hindsight to derive the power supply as surfaces rather than solids, and to carefully select which bodies to include in the derive.

As others have pointed out, it is not too difficult to derive this into a new sheet metal part and do the flat pattern and suitable iProperties there.  This is the normal procedure for multi-body sheet metal modeling in any case.

---

Sam B

Inventor Pro 2024.2 | Windows 11 Home 22H2

[A.Acheson]

Hi @SEC_CAD 

Just editing the derived part to be surfaces as @SBix26  points out doesn't affect the sheetmetal body in my simple example. So eliminate the solid bodies entirely. 

But maybe if you have edited the solid bodies in some way and the surfaces approach does not work then

 like others have said make components and choose the single solid body you want to be the sheetmetal part.

[kacper.suchomski]

HI

Is there anything stopping you from creating a new part and outputting the housing body to it?

As previous speakers have noted - if something is to be a reference in the target file; it is better to use a derived surface rather than solids.

[SEC_CAD]

Thanks all for your replies. The derive surface work around from @SBix26 worked for my case and was very quick and simple to do. I can now see the flat pattern of my metalwork.

Thanks all.

[metal]

Thank you this answer. It helps also when the derived part has broken, and does not need to re-wrap the whole model just to leave out a few bodies.