Is there a way to control Assembly expansion in Inventor drawing?

[Anonymous]

Hello members,

I am running into an issue, for which I am not sure what is the right way of doing it.

So here it is, 

1. I have created an assembly drawing with having a few subassemblies. On my first sheet I am putting main assembly, and BOM of that assembly only. Until now I haven't expanded the childrens in BOM (see picture attached).

2. Now I am creating Second sheet, to show no.2 subassembly, with its children of course to show what it is made from. (see pic attached below)

However, by doing this, the BOM on first sheet also expands for Item.2, which I don't want.

So is there a way to come up from this issue?

FYI,

1. I am using Inventor 2021

2. For second sheet I am using same model but with only It.2 subassembly Level of detail.

3. For second sheet I am filter out BOM to show items for the Level of detail only. (In our case It.2)

Any thought on this would be highly appreciated.

Thank you all

Be safe!!

[andrewiv]

The only way that I know of to do this is to expand the assembly on sheet 2, like you've done, and then go back to sheet 1 and turn the visibility off on the extra lines that you don't want to show on sheet 1.

[admaiora]

try doubleclick on the table in the drawing, then collpase the items clicking the -

[Anonymous]

@andrewiv  Thank you for your valuable feedback.

As an alternative, I found that I can create separate drawing of sheet-2, so It is not linked as it would be on same drawing. 

[Anonymous]

@admaiora  no that doesn't work. Tried that.

[cadman777]

One thing I do when I want to use the same assembly but have different BOMs is create a new assembly and Insert your original assembly into it. Save it under a different name so you know it's for that 2nd BOM. Then bring that new assembly into your 2nd Sheet and make a BOM for it, and adjust your BOM accordingly. That's how I SEPARATE the BOMs of the same assembly on the same drawing. Maybe that'll work for you?

[Anonymous]

@cadman777  I'd try it.

However, I would consider it as a last option as don' t want to create many assembly, just extra work. There sholuld be an easy way to get it done quickly with less hassle. 

Btw Thanks for valuable suggestion. 

[cadman777]

You're welcome!

Yes, I agree. But this defect in the software has existed for over a decade. So for me, the quickest way to deal with it is the usual: WORK-AROUNDS. Too bad it's like that, but that's what I do, b/c it saves me the aggravation and cussing that an unresponsive Autodesk causes when they refuse to add simple functions to their software that everybody would use, or that should be there as part of the basic functionality.

Incidentally, my method isn're really a lotta extra work. The only time it becomes a 'burden' is when the GA assembly is HUGE. That causes 'wait times', which is undesirable for those of us who are under time constraints.

[johnsonshiue]

Hi! Basically, you want to be able to show PartsLists of different BOM structures from the same assembly, right? To keep item number persistent, Inventor only allow one BOM structure type per assembly (PartsLists and Balloons) in a drawing. You can trick it by creating a PartsList of a different BOM structure in a different idw file. Then copy and paste it back to the old idw file.

Another option is to simply save the assembly as a different iam file. There you can place PartsList in different BOM structure, since the new iam file is considered a different model reference.

Many thanks!

[cadman777]

Johnson,

In the past I tried what you said about copying the assembly to a different filename, but that complicates the process. If you change one assembly AND FORGET to change the other assembly, you're SCREWED.

The way I BYPASS the Inventor ITEM NO convention is to number the parts MANUALLY. The fact is, Numbering is CRITICAL in all CAD applications. So the little extra time it takes me to make my own number using a Custom iProperty, makes the whole process work much better than out-of-the-box Inventor. Like I've said in other forum threads, I use the PartNumber for sorting the list for the RollUp function, and don't show that in the BOM, but instead I make my own PartNumber and call is Description. So, between my own PartNumber and ItemNumber, there's a lotta flexibility with the BOM. That's why I can Insert the SAME assembly in a different assembly file, and it will update when changes are made to the original assembly, PLUS I can use it in the same drawing with a different presentation of ItemNumbers.