Subtracting the volume of one part from another

[badkuki]

Hello,

I've been googling and looking through the forums, but can't seem to find a solution to my problem. I've tried various methods I've found on the forum and on youtube, but nothing works properly.

I have a part called blazinica_v002.ipt which is the outer part of the bearing, and a part called lezajniMaterijal.ipt which is positioned inside it. Inside lezajniMaterijal there will be a shaft of 155 mm in diameter.

Blazinica has these truncated pyramid-like shapes from the inside. In practice, lezajniMaterijal is in liquid form and is poured inside blazinica, and then cooled. lezajniMaterijal is a cylinder with a thickness of 2.5 mm (not including the truncated pyramids), and then a 155 mm shaft goes on the inside. Since lezajniMaterijal is poured inside blazinica, the truccated pyramids are completely filled with the material.

Since I've already managed to model blazinica including the pyramids, I would now like to create a cylinder and then expand it outwards to fill the pyramids.

From my googling, I found that I should probably create the cylinder for lezajniMaterijal, and then import blazinica as a derived part and as a work surface, and then use Sculpt to subtract it. Unfortunately this doesn't work for me (if needed, I can provide a screenshot of what it looks like when I use the Sculpt tool).

Does anyone have any recommendations on how to go around doing this?

I can always model the pyramids manually on the outside of lezajniMaterijal, but I would like to save myself some hassle. Also, I'd like to learn how to do something like this, in case I have to change up blazinica for some reason, so that I don't have to model the pyramids on lezajniMaterijal yet again!

Thank you in advance!

Inventor 2020 Professional

[Anonymous · Accepted solution]

Take a look at the combine command.

See attached part I made

Edit:
Note you'll have to use "Make components" afterwards, which is basically a new part -> Derive -> Choose a solid to derive.

[NigelHay]

I had a similar problem recently & followed this YouTube method which worked for me.

https://www.youtube.com/watch?v=16-8g4igLDs

[johnsonshiue]

Hi! You need to use "Copy Object" command (3D Model -> Modify -> expand the panel). Edit the part in place and then use Copy Object to link the geometry from another part to this part.

Merry Christmas and Happy New Year!
Many thanks!

[badkuki]

Hi, Combine tool works! Everything is as it is supposed to be! I couldn't open your attached part because it says it is saved in a newer version, but it's okay!

What should I do with Make Components? Could you link some Inventor Knowledgebase article or explain a bit about what it does? I never used that.

From what I gather, it saves this part I got as an assembly and "bakes in" the combine command?

The only problem is that I can't dimension some parts of the drawing when I make a drawing out of lezajniMaterijal. Some are dimensioned fine, some simply can't receive a dimension. I haven't done the Make Components thing yet, is this the reason why?

[johnsonshiue]

Hi! Make Components command facilitates the process of pushing out individual solid bodies within a multi-solid body part to individual parts in an assembly. The multi-body part serves as the master part driving changes to the derive parts.

For documentation, most of the model dimensions (except holes and threads) in the master part will not carry forward to the derive parts. You will need to create the 2D dimensions instead of retrieving model dimensions in the drawing.

A workflow you may consider is to create design views in the master part. Each design view shows one visible body. You can simply create drawing views of the master part (associated with the design views). And, retrieve model dimensions from the master part accordingly.

Many thanks!

[Anonymous]

As JohnsonShiue says, using the combine tool, you can't pull dimensions from the part creation, as there are no dimensions tied to the part.

In regards to the "Make Components" command, it allows you to create separate single body parts from a multi-body part.

Combine only works in a multibody part, so that's why you have to separate them afterwards