topic Re: Multi body ipt file in Inventor Forum

Multi body ipt file

Dhegderx — Tue, 28 Jun 2022 05:16:01 GMT

Hi Guys,

I have been using inventor at my work place from past one year. I started learning Inventor on my own and never had any assistance or mentorship from anyone. I usually create individual parts and assemble those parts in assembly file (iam) file.

My question is the guy who was working before me used to assemble all the parts in single ipt file, I am really keen on knowing how this can be done. I tried to reverse engineer his design tree but could not figure out the process.

Can anyone please help me with this???

Thanks

Re: Multi body ipt file

Lucas.dolinarVFXZU — Tue, 28 Jun 2022 05:33:24 GMT

Can you attach his files here?

Re: Multi body ipt file

Dhegderx — Tue, 28 Jun 2022 06:05:00 GMT

here you go

Re: Multi body ipt file

CCarreiras — Tue, 28 Jun 2022 09:26:56 GMT

HI!

Every time you use a feature, which adds material, you can select it as a new solid, creating a multisolid. (also "split" one solid "in solid mode" also create a new solid by separation, etc, etc)

Later, you can transform that multisolid into an assembly based in that multisolid (each solid->one part) staying linked to the source multisolid file: any change in the multisolid, will be reflected in the assembly and assembly parts.

Use manage-> Make components .

Re: Multi body ipt file

JDMather — Tue, 28 Jun 2022 10:22:13 GMT

@Dhegderx wrote:

here you go

No file Attached?

You must Reply via the web forum to Attach files, not by email.

Re: Multi body ipt file

Dhegderx — Wed, 29 Jun 2022 01:51:06 GMT

sorry could not attach the file properly.

Re: Multi body ipt file

CCarreiras — Wed, 29 Jun 2022 08:49:35 GMT

This multisolid is based in onother 3 multisolid files.

These 3 multisolids were loaded to this file with "DERIVE" tool.

So... The file you shared is also a multisolid, but is kind of an "assembly" based in 3 parts(which are multisolids).

Tip: For us to be able to open this file correctly, you must share the other 3 files as well.

You have to study the DERIVE mechanism, besides the multisolid (which I already (slightly) explained above)

Re: Multi body ipt file

Dhegderx — Thu, 30 Jun 2022 06:24:22 GMT

Thanks for the explanation, I just have one more question

I tried deriving the parts and then moving it using move bodies but the problem is when I change the view to half section view, the cross section colour of every body is same as the original base component.

I tried all the different configs and options but still cant change it.

Re: Multi body ipt file

Lucas.dolinarVFXZU — Thu, 30 Jun 2022 08:35:53 GMT

The Derive has a appearance override option, this colors the BODY, but doesnt set the color for the Part itself.

If possible, i wouldnt use the derive to make multibody parts... just make a multibody part and use derive to make a assembly from your master part...

(it does of course have a it's use cases, like importing complex geometry)

Re: Multi body ipt file

CCarreiras — Thu, 30 Jun 2022 09:51:54 GMT

Tip: At some point, people used to turn the multisolid (When is finally ready) into an assembly.

You could do that using Manage->Make Components
As an assembly, it will easy to move (constrain) the parts as you need.

Re: Multi body ipt file

johnsonshiue — Thu, 30 Jun 2022 19:56:30 GMT

Hi! One comment I would like to make is that the Multi-Solid Body workflows in Inventor are intended to define shapes, not worrying about assembly structure or component instances. If you are hoping to create an assembly within a part (without pushing bodies to individual parts in an assembly), you will be disappointed. There isn't much assembly-level documentation workflows for such part. You cannot create a partslist or a balloon describing each body. You cannot reuse the bodies within the part. It is strictly for shape defining purpose. Once the shape is done, you need to push the solid bodies into individual parts in an assembly by using Make Components command.

This is just how Inventor works.

If these workflows are too restrictive for you, I suggest you look at Fusion 360, which offers a more flexible design environment. You can define the shape and turn it into a component or not. All shape and component definitions are all wrapped within one design. It also has dedicated mesh modeling environment and generative design environment.

Many thanks!