Sub-Assembly and BOMs

New Corporate Standard.

Actually maybe you could do an indented bill and uncheck the sub-assemblys you don't want in there. I think you may end up with gaps in your numbering scheme though. I have heard 2004 handles BOMs a bit better but will it solve your problem someone else may know.

Sounds like your MRP people, do not understand drawings.

Isn't the Bal Ref just a field in the MRP system under the Assembly number? Also, how do you handle the same part used on a different Assembly where the Bal Ref would be different?

-- Tony O'Hara Melbourne, Australia.

Rob,

You've stumbled across the age old problem of engineering BOM vs. manufacturing BOM. Engineering BOM's are geometric specific while manufacturing are item master specific.

As a designer I am concerned with correctly representing the geometry in a model. As a purchaser, all I'm concerned with is how many parts I have to buy and when in order to meet my MRP requirements for production builds. Hence your current problem.

The easiest solutions is to look at the various workgroup PDM systems that are relatively inexpensive and very powerful.

For example, I am using DBWorks (Solidwork's Gold Partner)to generate an engineering BOM. DBWorks allows you to designate sub-assemblies as a single part (As it would be if you were given a supplier model but purchased the assembly as a single line item on your purchase order).

Advantages of DBWorks (as applied to BOM's) include:

- Can designate parts as make, buy, or no BOM (the latter is what you want to designate all the sub-components that make up the purchased assembly).

- Can add phantom parts with quantities (including A/R)without needing any SW models (i.e. Blue Loctite - 6 drops, part number XXXXXX).

- Can format the engineering BOM (Excel template) to create a format specific file that your MRP system can batch input (rid yourself of the dual entry dilema when converting engineering BOM to manufacturing BOM.

- I havent' tested this but you may be able to assign a balloon (item or find number) to each part which would match your MRP find number. You may be able to have a script file modified which checks the type of BOM in DBWorks and assigns that data field to your drawing balloon callout. This would be a project specific value which would allow you to have different numbers for your various projects.DBWorks, like SW has a open API that allows you to create just about any solution you may require.

Additional benefits of using these workgroup PDM's include automatic filling out of drawing titleblock values (batch mode); Revision control of model and drawing files (including configurations); Approval control; Product definitions, elimination of the "he/she who saves last wins" game in a multi-seat environement, etc.. etc.. etc.... Powerful stuff for an 800.00 USD program. I need to confirm this but I was just told it allows multiple materials in a single part model. How about a single Toolbox part file that contains a carbon steel, 18-8 SST, or nylon (.250-20 X 1.00 long

3A UNC) bolt that correctly configures itself (density, cross section, material call-out) in drawings and models?

Hope this has helped.

Len K. Mar, P.Eng. President E-data Solutions

G'Day Tony!

Yes, I don't believe that our MRP people understand drawings.

To answer your questions, yes the balloon ref is a field in the MRP system. You look at the balloon number on the drawing, find the corresponding ref on the MRP bom and that gives you the part number. A part used on two assemblies can have different balloon numbers, but the part number will be the same.

Rob

We could do that. Its just much more labour intensive. Besides I'm sure that I'd screw up the numbering.

I was hoping that SW would allow me to expand the BOM the way I could with MDT and Inventor. With those programs, you open the bom dialoge box and a plus sign would be beside each sub-assy in the bom (much like a folder with sub-folders in Windows Explorer). Just click on the plus sign, the bom expands showing the sub-assy's components, and item numbers (balloon #) are assigned to the components. The sub-assy is then greyed out. To collapse, just click the minus sign.

One of the very few things I miss about MDT.

Rob

I guess I should have used a smiley face or something I meant it more as a joke. I understand that in many companies this would be an imposibility.

Corey

One way you may be able to separate your subs that are Weldments and Subs that are not is to save your Weldments as Part files this way you would have

2 models of your weldments one as an assembly one as a part. Then you insert the part one into your top level assembl as a single part. The only problem you may experience is when changes are made to the weldment it will not be associative and to update the part file you will have to save over it. I don't know what this will do to your top level. Your mates may go hay-wire but I haven't tested it. The only other thing I could suggest is get someone to build an API that would do what you want.

Regards Corey

No use crying over spilled milk. :^)

Rob,

PDM/Works will not do what you want unless you spend considerable money creating a custom program. In order to gain access to the PDM\Works API you will have to shell out $5K to get the advanced server plus x dollars for the customization (which will need to include a DB in order to be able to tag the different balloon numbers in different assemblies).

I've tried to make PDM/Works do what I want for the last 4 years without success. DBWorks is $200.00 cheaper and 10x more powerful. You'll want them to show you exactly how it will do what you've asked in previous posts. I've beta tested PDM/Works 2004 and cannot see any new functionality that would allow you to do this. I'd skip the VAR and go directly to SW customer support or product manager.

I'm going to go out on a limb here and guess your VAR will try and steer you to Smarteam in order to get this "functionality".

Email me if you want any more detailed information. We can take it off-line.

Cheers,

Len K. Mar, P.Eng. President E-data Solutions

Have you tried using the option to not show child components in BOM when used as a sub assembly. It is in the configuration properties. You can turn it on for any subassemblies that you want to be numbered as a single component and off for the subs that you need to see the parts of. Then you can still use the BOM option to Show Parts Only.

Todd

Thank you Todd!

I was carefully watching this thread since this is also a problem I had. I'd never seen this little option before. I don't know if it will help Rob but it will definetely help me with those sub-assemblies I wish to treat as a single item in the BOM.

You made my day, have a nice one!

Pascal

"tbryant" a écrit dans le message de news: snipped-for-privacy@posting.google.com...

Weldments aren't really assemblies, a finished weldment is really a part. The way we handle that is creating an assembly showing all the pieces of plate etc. then use "Join" to turn that into one part which represents the finished weldment. That part is what's inserted in the next level assembly. Perhaps you could apply this same idea to purchased assemblies too? At any rate this suggestion might solve part of your problem. The only real downside to it is changes to the weldment assembly don't update automatically, you need to open the join.sldprt to propogate the changes.

Your product structure should match your feature manager. I don't agree with creating subassemblies for ease of modelling an assembly when that means your feature manager items don't jive with your MRP BOM. Maybe you should keep everything as individual parts and try to use folders instead to organize things.

It's not just an organizational matter either. You end up with assemblies that don't have associated part numbers or drawings. Just a bunch of orphan assemblies created out of short term convenience.

Devlin quipped:

while i agree with you, this is exactly counter to what SW and my VAR have said: With large assy's, use sub-assy's to make the large assy easier to work with.

The big problem is that your SW BOM will NEVER match your MRP BOM.

What I really want is an option something along the lines of: Make all components of this sub-assy appear as top level in the big assy.

ie: I have a forming slide assembly, and a wire puller slide as sub-assys in my main assembly. Neither one is an assy as far as MRP is conerned tho. Now, I have a plate that is used in both sub-assy's #P-6495-3. My MRP BOM shows a quantity of (2) #P-6495-3. There is no way to see (2) of those parts in a SW BOM. The option above would remove the two slide assembiles as far as the BOM is concerned, and it would show (2) of those plates.

you can't tell SW to show parts only, since it will "dissove" all the sub-assy's WITHIN the slide assy's. Since I have MRP-assy's within each slide SW-assembly.

I'm sure the folders help (well, i know they do) as far as organization goes, but they don't help as much as far as performance goes, since the point of creating sub-assys for SW is to help performance. And keep mategroup1 to a reasonable level. The fewer mates to solve in the main assy, the better off you are. SW doesn't need to resolve the mates within the two slide assemblies each rebuild, but would need to if all components are inserted to jive with the MRP BOM.

--nick e.

Setting the BOM to "Show parts only" has always been the setting I've used for every BOM I make. I just makes it easier that way. "One setting does it all". Sub assemblies show up as a single part if needed and child components can be shown as well. You have total control.

To avoid that problem, I use the "Don't show child components" setting, and use another configuration if I need to show child components.

I know this isn't the answer for some rare cases, but with the new

2004 BOM system, you should get SW to show parts just about any way you want.

Mike Wilson

GREAT!!!!

Thanks Todd, that is exactly what I was looking for! :)

It's going to be a bit of a pain in the butt going back and turning this on for all of the sub-assemblies I don't want expanded in the bom. SW should have option turned on by default.

Thanks again!

Rob