Community
Inventor Forum
Welcome to Autodesk’s Inventor Forums. Share your knowledge, ask questions, and explore popular Inventor topics.
cancel
Showing results for 
Show  only  | Search instead for 
Did you mean: 

Multi body and identical parts

5 REPLIES 5
Reply
Message 1 of 6
Anonymous
1622 Views, 5 Replies

Multi body and identical parts

Is there away to treat solid bodies that are identical as as the same part? Since I work a lot with cabinets I end up quite a lot of identical parts (ribs, gables, etc) and in multibody I end up with sepreate solids.
So far, best I came up with is to exclude identical parts when I make my components and then reinsert (and mate) them in the assembly to get the proper bom with right quantities.
Another way is to export it all then merge identical parts in BOM (.haven't tried that yet), I just end up with extra ipts

I'm wondering if there's a different/easier way?

Side question - drawings I produce are usually for wood cabinets that are finished in Laminte, so having seams between panels is not ideal. I used to hide lines but now I shrikrawp my model and reinsert it back into my assembly. This way i control my "pretty picture" isomerics and elevations so it looks seamless, and then in details I use the full assembly. Again, any other way of doing this?

Thanks !
5 REPLIES 5
Message 2 of 6
johnsonshiue
in reply to: Anonymous

Hi! Currently, there is no way to make body occurrences (multiple solids point to the same body definition like parts in an assembly). What you could try is to avoid pushing same solids as different parts into the assembly via Make Components command. Then in the assembly, copy the unique part and paste it multiple times as occurrences in the assembly. It is a bit messy but it should be doable.

Many thanks!



Johnson Shiue (johnson.shiue@autodesk.com)
Software Test Engineer
Message 3 of 6
Anonymous
in reply to: Anonymous

I wouldn't say messy:) just a bit time consuming.
My other solution, is to export it all and just merge identical parts in bom
Message 4 of 6
rhasell
in reply to: Anonymous

Hi

 

One other method that I use quite a lot.

 

I use all the solids, but then make the unneeded solids as reference components in the assembly. I then constrain the common part on top of the "Unused" solid.

 

Once I am done, I switch off the visibility of the reference components. (I also disable the part, the green icon gives me a quick reference of the "Dummy parts" Note you have the re-enable the part to make any changes)

 

Additional Notes:

The extra solids are used where required, especially when I mirror some tricky geometry. The solids are named as a mirror, or extra component.

The assembly build is therefore a lot quicker, because I don't have to worry about tricky constraints. (Grounded insertion of dumb solid, and part constrained on top of it, really easy)

This allows for the healthy BOM.

 

Small example of a solid model, the Mirrors have an 'x' suffix

 

solid model.JPG

 

Reg
2024.2
Please Accept as a solution / Kudos
Message 5 of 6
jtylerbc
in reply to: Anonymous

I use your first method, but constrain the duplicate instances directly to the equivalent faces on the multisolid layout part. That way everything is still being controlled by the multisolid, even if some of that control is being done indirectly through the constraints.

Message 6 of 6
LukeDavenport
in reply to: jtylerbc

Hi all,

For anyone who prefers a more automated process - there's now a dedicated solution for this (a long time in the making) called the Duplicate Replacer. You can scan for duplicates at the end of the design process, and just swap out all the duplicates OR swap out their Part Number iProperties if you prefer.

 

https://youtu.be/sbFZaeBHehY

Luke

Can't find what you're looking for? Ask the community or share your knowledge.

Post to forums  

Technology Administrators


Autodesk Design & Make Report