Splitting components within an assembly

[andre-the-PM]

I have an assembly. One of the components I'd like to split and use those split bodies as starting points for new components. The reason for this is it's impossible to fabricate the component as designed. It would have to come out of multiple pieces of material. How can I do that?

[SBix26]

You didn't give much to go on (images or files, for example), but generally you will need to create another part.  There are several different ways to do that, depending on the complexity of the part and how you foresee it being split.

The simplest method (to describe!) is to simply create two new parts and replace the previous one.  Other methods that come to mind:

• copy the part, then edit the original and the copy until you have the two separate parts defined the way you want
• copy the part, then simply split off the unnecessary part of each one
• use the original part as a master, split the original solid body into two, then derive those two solid bodies into separate parts to be used in the assembly.

Since you haven't told us what sort of assembly this is, we can only guess.  If it's a wooden cabinet, the answer might be different than if it's a structural weldment, and different again if it's a molded plastic whatsit.

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Sam B

Inventor Pro 2024.2 | Windows 10 Home 22H2

[andre-the-PM]

The assembly consists of welded sheet metal and HSS. I figured out that I can split the body and then "create part". Then i can choose to delete the faces in the original part file so that half of the body doesnt show anymore. Before doing that I break the link in the created part. What do you guys think of this approach?

[SBix26]

That will work, but it leaves the derived part an orphan without reference to the features that created it.  I would instead recommend that you split the part into two solids, then derive them both to new parts (Make Part or Make Components), leaving the links intact.  Then you can make edits in the original file where all the features were created in the first place.

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Sam B

Inventor Pro 2024.2 | Windows 10 Home 22H2

[andre-the-PM]

How would I then eliminate the original part from which multiple parts came? I would like to do that so that it doesn't exist in BOM. 

Also what's the problem with orphaned parts? I do like the idea of dumb solids living in my part files. I don't want them accidentally getting screwed up by any outside changes. 

[kacper.suchomski]

Just remove the part from the assembly.

[SBix26]

If you're absolutely certain that you will never need to make any edits to the orphaned part, I guess there is no problem with having a dumb solid in your assembly.  I would never knowingly do such a thing-- I'm never that certain of a design until it's shipped and in service, and even then the customer may request modifications to the design at a some later point.

Having a master model controlling your design (in this case just two parts of it) is not an "outside" change-- it's the defining file.  It doesn't end up as a component in the assembly, but it drives two components (or more if you decide to incorporate more of your design in the master).  Many designers use this technique to drive the entire design of smaller assemblies-- all design changes happen in the master model and the parts follow.  I prefer this method whenever possible.

If you are interested, and are allowed to post a small assembly here, I'd be happy to show you how this might work for you.  I note that you haven't yet told us what version of Inventor you're using.

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Sam B

Inventor Pro 2024.2 | Windows 10 Home 22H2

[andre-the-PM]

I appreciate all the responses. Can't send my assembly. 

I'm using Professional 2023. 

I really like master model modeling. I like to drive the initial major design in a multibody part file, then I like to break up into components and finalize details. I used to do that in NX. In NX there was the ability to send everything into components as dumb solids, then use direct modeling to modify or to add finishing touches to the body inside each component. 

[swalton]

Take a look at the Make Components workflows from a multi-body part file.  You can build a multibody solid, and then derive the individual solids into individual part files and place them into an assembly.

Helpfile link:

https://help.autodesk.com/view/INVNTOR/2022/ENU/?guid=GUID-77C9230C-2C88-4BFD-BECF-0F5B4E1E4F82