BOM and inseparable parts

[JorisSteurs1246]

In my main assembly some of the sub assemblies are made inseparable.

They are welded constructions so it makes sense. These welded constructions have stock material in them ( beams, tubes,etc)  how do I generate a corerct cutlist from the main assembly BOM so that also the parts that are welded in the inseparable subassemblies are also presented? 

Thanks for helping me out  

Joris

[jtylerbc]

Unless there's some kind of workaround I'm unaware of, you don't.  The fact that you can't access the parts in the subassembly is essentially the definition of the Inseperable BOM status.

You'll either need to change those subassemblies from Inseperable to Normal, or generate cut lists from them individually.

[JorisSteurs1246]

I'm afraid to put everything to normal, because its a big project, everything is nicely documented, things could get messed up like this. The essence of inseparable welded assemblies is also that they start of as individual parts before production.

Having  these parts uncountable in any way, is in my eyes a flow in the BOM tool. I think it could be easy done by ADSK  that you have  a checkbox  similar to grouping according to partnumber, this can be switched on and of depending on what info you need from the BOM.

[jtylerbc]

It could be viewed as a flaw in the logic, but it is the way the Inseperable BOM setting is intended to be used.  The idea behind Inseperable is that you have access to that assembly's parts, but ONLY through the assembly's own BOM and parts list.  If that's not the way you need it to behave, then Inseperable is probably not the setting you should be using.

Higher level assemblies then essentially treat the subassembly as though it were a single part.  This holds true even to the extent of showing up as a single piece when using a Parts-Only parts list.

You can work around it by setting the subassemblies to Normal, then just not expanding them in the main assembly's parts list (so they still show as a single item).  We have occasionally done that to generate a combined material list.  As you mentioned though, this enters in the possibility that they could be expanded out by mistake, so you must proceed with caution.  Despite that possibility, it's probably your best bet for achieving what you want.

Another possibility is exporting the parts lists to Excel and generating your combined one that way.  However, that could be a lot of manual work as well, in order to get all your total quantities right.

[Mark_Wigan]

i aggree it should be something that autodesk could implement, & there have been several requests put forward on the ideas station that you could vote for if you have time.

also, (sorry if it was said already) if i recall correctly you can successfully export "everything" out to excel using the bom setting in inventor- "structured" with "all levels". but like John said, you will have some manual work to do afterwards.

unfortunately with the options available in the BOM, usually i find that there is always a real need for a person to go away using a couple of these exported boms's and then generate a nice new list of parts and assemblies manually.

one option i have used is to export a "parts only" bom along with a "structured" "all levels" bom and then put them on different sheets in the excel workbook, but you still need to educate the people downstream if you are not going to do any manual editing of the data yourself. usually i think that it is quicker just to do it yourself anyway if you want to get it right.

[JorisSteurs1246]

Yes that is what I'm doing now copying it all to excel, there filter the BOM’s on different iproperties and then paste them together accordingly.  But that is that is my problem also. In the  BOM I'm  playing with the iproperties , copying things over etc. This is very difficult if dealing with more than 10 smaller BOM's and everything has to be correct if moving over to excel otherwise your filters there don't catch certain parts. So to much room for error, and Murphy is al around as we all know.

[mikejones]

This may not be a practical solution but I'll throw it in anyway. How about having a partslist for your top assembly which itemises the components as you parts and sub assemblies/weldments and then show on the same drawing a separate partslist purely for the weldment, the title of this parts list could be changed to specify what assembly it is referring to.

The other option would be to show all levels when inserting the parts list, you would then have the ability to expand the weldment line in the parts list editor and show the components that make it up. You will need to change the view options, View Properties in the BOM first from First Level to All Levels

Mike

[JorisSteurs1246]

Thanks Mike,

That " other option" you talk about, I don't really understand, because I can't find a way to expand the welded assemblies in any way, unless you are in the BOM of the welded assembly itself of course.

Your first option as I understand still works with different BOM's so still preventing me from grouping structural beams to make my cutlist.

For copying Iproperties etc , I found only the following solution:  Make a new assembly and throw in just all the parts you have in the  project ( I always make a new project file per project) then you can do the property changes via the BOM . This assembly  has just 1 part of every thing in you project,   so the quantities are not correct, therefore this system cannot be used for generating cut lists.

[mikejones · Accepted solution]

Follow these steps

1. in assembly file, go to BOM and and structured tab set View Option > View Properties to All Levels
2. in your drawing select parts list from ribbon. Choose your assembly file or select a view on your drawing which is based on the assembly. The BOM Settings and Properties should read

• BOM View - Structured
• Level - All Levels

3.  Place your parts list

4.  RMB your parts list and choose Edit Parts List

5.  Next to each assembly in the parts list table will be a '+' icon which when clicked will expand to show the components used within it including inseperable assemblies

I have created a pdf screen shot but I don't seem to be able to attach it at the moment but I will try again later from a different machine.

Mike

[JorisSteurs1246]

Hey Mike that is an interesting approach, I basically always work “parts only”  when I need to get info for fabrication or adding Iproperties.

I have to investigate if I can do things this way also, thank you for your valuable input 🙂

[johnsonshiue]

Mike's approach is the right workflow to use here. Another way is to simply select the weldment subassembly .iam file when creating a partslist.

Thanks!

[JorisSteurs1246]

Yes just a few annoyances I discovered so far. Since I want only parts in
the part list , I've to make the assemblies invisible. I don't use item
numbers for ballooning but partnumbers. In the part list the sorting
of the partnumbers doesn't work accurate anymore when there are rows
made invisible. Making is very difficult on the work floor
finding the right part number out of a list of 142 items.



Joris Steurs


Design & Fabrication
www.distep.ee

[JorisSteurs1246]

Looked like this could work .... but AAAGH.. now after export to excel and after moving and tweaking I noticed that the quantities in the BOM are not correct.  The quantities seem to be counted only from the the assembly they are directly under .

Basically when the assy_Total has assy_A two times and part_1 is in assy_A  also 2 times then in the BOM I get QTY for part_1 only 2 times  and not 4 although the BOM is derived from assy_Total. Conclusion, using the BOM in the structured way is useless for me and the tab” parts only” doesn't allow me to view the content of inseparable assy's.

This looks not good for making a complete material and cut list.

[Mark_Wigan]

i have stopped using "inseparable" to minimise the amount of checking and manual work for these situations.

the bom export will treat them like a normal part, not what we know is needed in real life to make the welded kit.

so as i mentioned i usually export a "parts only" BOM list, to give to the guys who are cutting, or purchasing steel and commercial items. this gives total qty of every part no matter what. (as long as no "inseparable" weldments reside within. as i said i personally prefer not to use them to simplify this process. if you have to use them then you will need to do some manual work later on to consolidate this information).

and i also export a structured all levels BOM to give to the guys in assembly to accompany the drawings they will be working off.

i put both sheets in a workbook, and clearly write at the top "Structured BOM all levels" & "Parts only Flattened BOM. refer to drawings for assembly information".

if the downstream guys want a consolidated flattened list then it needs to be done manually, so as to show every assembly and every part. until we get the functionality to get this automatically it will be a pain.

[JorisSteurs1246]

Thanks Mark,

I think the way you describe it is the best possible you can do with the
BOM tool as it is today. I also avoided "inseparable" in the past, but with
this project the client needed an IPN with assembly instructions and with a
part list for all the parts needed to assemble the product. So on the
assembly floor a welded construction is 1 part, but on the fabrication
floor and for purchasing it is not. There is LOTS of improvement possible
in the BOM tool.
I also don't understand why you can't have excel doing the work, similar to
iparts where you do your changes in excel and push them back to part.
Excel has tons of functionality. Inventor would just needs to have a
hotlink. Excel tables can be put on the drawings already anyhow.