topic Re: Delete (derived) Solid Bodies from Part in Inventor Forum

Delete (derived) Solid Bodies from Part

SEC_MECH — Fri, 01 Mar 2024 03:48:08 GMT

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.

Re: Delete (derived) Solid Bodies from Part

A.Acheson — Fri, 01 Mar 2024 04:44:11 GMT

Hi @SEC_MECH

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.

Re: Delete (derived) Solid Bodies from Part

Gabriel_Watson — Fri, 01 Mar 2024 05:53:27 GMT

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.

Re: Delete (derived) Solid Bodies from Part

Biju.Veedu — Fri, 01 Mar 2024 06:07:09 GMT

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?

Re: Delete (derived) Solid Bodies from Part

James_Willo — Fri, 01 Mar 2024 06:41:07 GMT

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.

Re: Delete (derived) Solid Bodies from Part

johnsonshiue — Fri, 01 Mar 2024 22:00:46 GMT

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!

Re: Delete (derived) Solid Bodies from Part

SBix26 — Sat, 02 Mar 2024 19:41:33 GMT

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

Re: Delete (derived) Solid Bodies from Part

A.Acheson — Sat, 02 Mar 2024 20:49:54 GMT

Hi @SEC_MECH

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.

Re: Delete (derived) Solid Bodies from Part

kacper.suchomski — Sun, 03 Mar 2024 03:17:41 GMT

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.

Re: Delete (derived) Solid Bodies from Part

SEC_MECH — Sun, 03 Mar 2024 21:32:49 GMT

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.

Re: Delete (derived) Solid Bodies from Part

metal — Fri, 18 Oct 2024 11:17:47 GMT

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.

Re: Delete (derived) Solid Bodies from Part

Bjornar_Andre_Vik — Thu, 15 May 2025 07:55:51 GMT

Hi Gabriel. This is not working with me (the option 2). Solids that is invisible will join the new simplified part and merged into a solid representing the part it belonged to. And it is ignoring the fact that I have saved and chosen the correct view representations for this. Maybe it is something about the model state I am missing...