Create a multi bodies from divided-separated solid

[chachaman]

Hello,

Is there another way to efficiently recognize obvious separated bodies of a same solid without using the split tool. This is an example of the solid.

This is just an example, the real solid has many more entities....

Thank you all in advance for your contributions.

[hosford]

I'm not sure if I understand your question.

if you have a multi body solid, you can export the solids as an assembly, that will make the individual files for each solid. 

[89198826955]

Press the button create a new body

[Bill_Bogan1]

Hi chachaman,

It would help to understand a little more...

• What version of Inventor do you use, so that someone could attach an example?
• Can it be a pattern of blocks? All the same block, just lots of iterations?
• Do you want it to be "adjustable"? Patterns would allow for that easily.

If you use 2023, here's an example of a pattern looking similar to yours, but each an individual iteration of the extrude.

For example, attached is a 2023 model, it has a 1"x1" cube. In the model are model states. In each model state there is a different material used and a different pattern or two (differentiated by name).

Hopefully, you can view it. Patterning also allows for occurrence suppression (removing an occurrence but keeping the pattern arrangement.

-Bill

[89198826955]

A multi-body sign will appear

[chachaman]

Hello 89,

Are you telling me when you perform an EXTRUDE-CUT, you can select the multi-body feature ?....I am not able to recreate this on INV 2022.  This solution would be ideal if it worked. Please confirm !

Thx

[89198826955]

I have IV 2023.2

[chachaman]

I too have INV 2023....I still can't select both Cut and New Solid at the same time. They are mutually exclusive. Are you able to press the OK button ? see image ..... and thanks for your insights.

[89198826955]

Everything works out great

3 bodies created in multi-part

[3D4Play]

I think I understand this question. Use the pattern to do it. Like this:

Which will create 3 additional bodies. Done!

[johnsonshiue]

Hi! I believe you would like to separate disjoint lumps as individual bodies. Inventor does allow separate lumps to exist in one body. If you have a body with disjoint lumps, there is a not-so-intuitive workflow to convert it into multiple solid bodies. Here is what you need to do.

1) Use Rectangular Pattern command -> select Whole Body -> select the body -> set the number of instance to the number of disjoint lumps -> distance = 0. You will get multiple solid bodies on top of one another.

2) Now, go to Solid Bodies folder -> right-click on a solid body -> Hide others.

3) Delete Face -> Lump Select -> select the unwanted lumps -> Ok.

4) Repeat step 2 and step 3 for each solid body.

Another option is to use Fusion 360. It does have the ability to create individual solid bodies from cuts.

Many thanks!

[chachaman]

Hello John,

User 891...6955 proposed the solution I am looking for, but for some reason I cannot reporduce it. Can you try it on your end?  The idea is to create new parts out of the newly created disjoionted bodies resulting from the cut.

Thank you.

[chachaman]

...still not working for me. Can you upload your ipt file ?

Thx

[89198826955]

ok

[89198826955]

I understand why it didn't work for you

You do it with the first extrusion

And to get a multi-body, put the sign for creating a multi-body for the second and next extrusions