Detail views of parts referring back to a master part list number

[jyager]

I looked for this but can't seem to figure out what it might be under.

Lets say I have 2 page drawing set of a damper, page 1 contains the main views and all the related part number ballons.

Page 2 contains fabrication details for the parts, brackets, blades etc.

For the parts I just inserted those into the drawing from their respective part file, allowing me to create the necessary amount of views to capture the needed dimensions for the shop.

The problem here is now when I go to apply a balloon to that part it wants to make it part #1 when it may be part # 7 of the assembly.

My workflow on this may be wrong, or maybe there's an easy way around this or something I'm missing entirely.

Thanks for any help.

[blair]

Nope, each time you select a new view, the BOM/Balloon starts over for that view. The easiest is to just use the leader and use the number required.

I am thinking that you might be able to over-ride the number for the Balloon, will have to check.

[dan_inv09]

I'm doing this right now.

This is a smaller assembly (weldment I didn't bother with welds) so I was doing it the cheap way:

Turn off Associativity to the view rep and turn off the Visibility on all the other parts in the assembly.

(Turning off the Associativity is a real pain, you start selecting stuff to turn off and then visibility is grayed out and you have to go back to Edit View because you forgot to do it when you placed the view.)

The right way is to create a View Rep for each part in the assembly.

(For some reason I think there was some sort of plug in or something to do this automatically, but trying to find it always seemed to me to waste more time that just doing it manually.)

Then you place a view of the assembly and select the proper Rep and there you go.

(You can then have the View Rep locked so that when you add a new part it doesn't show up in each and every part detail, and you have to go and turn off the visibility of the new part in all of them, and you think, "I'll just select them all at once." and you miss a click 3/4 of the way through ... twice.)

[dan_inv09]

It seemed clear right up until I hit Post, but now that read it again someone might miss the point.

I'm talking about placing a view of the assembly for each part (just with everything but that part not showing). That way you get the assembly balloon numbers.

[jyager]

This is a smaller assembly so I think I'll just override the ballons (it's only 10 items), this time, but on larger assemblies it seems view reps are probably the best solution. Seems kind of labor intensive...like it would be nice to have a balloon option to always pull from the part assembly, but it's better than having to deal with overridden values when parts start getting added or changed down the road.

thanks!

[dan_inv09]

But what if the part is used in more than one assembly?

They could work on making placing the View Reps a bit less clunky. And I wish I could remember where I saw the thing to automatically generate them.

[blair]

It's always looking at the drawing view you selected. So in one assembly it may be item 12 and in the next assembly it could be item 24.

If you had a variation of a assembly that contained the same parts but the color of the main body may be different, then there is a good chance it could have the same Balloon number.

[jyager]

It seems like the view representations are the way to go for anything with any complexity. We frequently have situations where we may change or add members after seismic analysis...sometimes omitting parts...having to chase down all those part numbers and other human error prone 2D CAD processes was one of the main reasons I pushed to get away from 2D. I don't want to go backwards.

[PaulMunford]

I think that the part number is intended to be the unique reference No. The item No. Just calls the part out so that you can find it in the parts list...

You could try a weldment assembly - this will create your single part reps automatically. Or you could copy the item No.s down to the part level using this technique:

http://cadsetterout.com/inventor-tutorials/autodesk-inventor-creating-coordinated-bom-for-large-asse...