Item numbers on Assembly Drawings 1

[pdybeck]

I am throwing this out there for discussion (this is also posted on the SolidWorks forums under EPDM).... This is related to whether you show BOMs on Drawings and how you manage your BOMs with ERP and Drawings (and there could be implications with EPDM). I am interested in hearing what other folks do...


A little history on ourselves - We moved away from showing the BOMs on assembly drawings about 7-8 years ago to reduce the amount of double entry for our designers managing a BOM table on drawings and a BOM in ERP. I was not completely on board with the implementation, because SolidWorks implications were not being fully considered. Most of the struggle that he time was with editing tables in AutoCAD and then re-entering the data in ERP. As a result, on all of our drawings we now just show the item number and do not show a BOM table. The item number shown on the drawing has to match the Item number in ERP. This gets "fun" for larger SolidWorks assembly drawings that go through multiple changes. We have developed methods for keeping the Item numbers the same between ERP and SolidWorks assembly drawings. As a trend, a single source of BOM is where companies are headed and keeping that master BOM in ERP seems like the best place for it to reside when you have CAD and ERP. Frank B. Watts in his book, Engineering Documentation Control Handbook (2nd edition), agrees with an approach like this as a company grows and shows the trend in the future will be toward this method of a single BOM being maintained in ERP (or PLM/PDM linked to ERP if you like). I would agree with that approach, but it still makes item number management in SolidWorks drawings a pain.


This got me thinking about item numbers on drawings in general. What is the point... It seems to be just a pointer to get you to some other controlled table so that you can find a unique identifier (part number)... hmmm seems to be jumping around a little bit and creating an extra step. As part of the work order packet our production folks here print the BOM from ERP and print the drawing for assembly builds on the shop floor. The assembly folks look at the drawing and find the ballooned item number, only to then look on the BOM and find that item number so they can get a part number. The item numbers seem like the extra step... It seems to me that maybe item numbers are a carry over from a bygone era when drawings were hand drawn and BOMs were maintained on drawings. Item numbers allowed easier changes to the BOM table without editing the drawing (when it was tedious to do by hand drawing). Is there really a need for item numbers in a modern world?


I am currently thinking out (with other's help here) why it wouldn't make sense just to show the part number of ballooned items on an assembly drawing and not the item number. This would be much more efficient than having to consult another piece of information just to get what you are looking for. Our assemblers would just see that unique identifier (part number) right on the drawing next to the item they are looking for. I would advocate that the BOM in ERP be sorted to be in numerical order for easy reading and description location once the part number is seen on the drawing... or do show the BOM table on a SolidWorks drawing, but show it without item numbers and sorted by part number numerically. This seems more efficient to me and would make looking at SolidWorks assembly drawing a nice thing. Plus, we wouldn't have to go through the rigmarole of making item numbers match.


Does anyone operate this way? Can they see flaws with this approach? Are item numbers really needed? Let me know if I need to clarify.


Thanks in Advance

 

[CorBlimeyLimey]

You are right in that the item number is a hang over from the past, but it still has a valuable role to play. It is a very simple reference to a complete line of information in the BOM. It's not just a substitute part number. An Item Number is usually just one or two digits. They are easy to fit into the surrounding area of a view.

Many part number systems involve many more digits. My company has a system using 8 digits and I've seen others using about 20 or so digits. Can you imagine the clutter that would add to the drawing? Having to remember that extended number when searching for the part would also be a PITA, especially when BOM's are rarely in alpha-numeric order.

I'm happy with the item number cross-reference.

 

[ctopher]

I agree with CBL.

Test it. Create an assy dwg without balloons, only show the BOM.
Give it to the assy people in the shop to build it, no instructions.
You find some of them confused, depending on the complexity of the dwg.

Chris
SolidWorks 13
ctopher's home
SolidWorks Legion

 

[dsgnr1]

pdybeck,
I think yes you are doubling your work. With no bill of mat'l on the face of the drawing, you are referencing a reference in your erp (item 79).
You already have the data for the part number loaded into your erp somehow, so you could just use that.

I have also seen a practice here that uses a "three letter callout", where M10 might be a machined part and H15 would be a piece of hardware.

For your purpose, you are on the right track.
(twenty years in Systems Engineering)
Jim

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[pdybeck]

CBL,

Our part numbers are also 8 digit.... XX-XXXX-XX. I did a test on a busy assembly drawing of ours. Everything fit nicely. Didn't seem too cluttered to folks here. Font size could also be reduced if needed and still plenty visible. As far as finding the part number in a list.... Both SolidWorks and ERP have capabilities to show the list in an increasing or decreasing numerical order by part number. On large lists, its actually not too bad... no worse than finding an item number, cross referencing to another document and moving over a row or two to find the part number... I wouldn't propose changing all our old drawings, just as a new method of documentation. Just trying to think my way through this with the help of others. I think I have answered your potential downsides. Its a bit subjective the points you raise and some I would agree on a little bit, but worth thinking about since this is somewhat shades of gray territory. Thanks for your input. Greatly appreciated.

 

[pdybeck]

Jim,

Are you saying that showing part numbers in balloons is potentially the right track for us? I was a little confused after reading your posts.

I have fond hints in books and other places that something like what I am proposing seems to be a logical progression towards a more efficient operation and less competition between really a documentation system and ERP system (2 systems).

 

[EEnd]

On our assembly drawings, rather than balloons with item numbers, we have a leadered note with a text description and the part number. There is no BoM table shown on the drawing. The BoM is maintained in the ERP system, although engineering typically generates the initial BoM from the SolidWorks assemblies. The description and part number in the note are pulled from the part's properties, so they are only entered into SW once. The space taken up by the description in the notes can be a bit problematic, but it is partially offset by not showing a BoM table.

Our assemblers requested labeling the parts directly with the part number and a description. It saves them the step of cross referencing an item number to a line in a BoM table. The parts get picked from a list generated by the ERP BoM and put in containers labeled with the part number. The assemblers get the containers and the drawing and put it together. From their end it works well.

It does take a little convincing to get SW to work in this manner. The components need to have their number and description properties entered. Our drawing templates link the title block to these properties so they need to be entered anyway. On the part and assembly configuration properties, we set the BoM options to user specified name with $PRP:"Description"<alt 0010>$PRP:"Number"-$PRP:"Revision". Here <alt 0010> means holding down the alt key while entering 0010 on the number pad. This makes the text two lined. For drawings we set the balloon style to None, the balloon text to Custom Properties, and select the Callout Text custom property. These changes can be set in the part, assembly and drawing templates, but I have a macro for setting them in existing drawings. Finally we saved some dimension styles for notes with text like () $PRP:"Description"<alt 0010>$PRP:"Number"-$PRP:"Revision". There are actually 4 forms created by combining 1 or two lines and with or without the () for the quantity.

This prep work gives lets us create annotations in 2 ways:
To annotate a part, we can just add notes with the appropriate style attached to the part.
To annotate a subassembly, we have to insert a BoM off to the side of the drawing and attach a balloon to one of the parts in the subassembly. If we attach a note to a component of a subassembly, it shows the property of that component, not the subassembly. A quantity can be added to the balloon text by double clicking on it and adding it in the popup text editor.

This method is by no means perfect. The biggest fundamental problem is that the quantities are non-parametric, however the drawing does not drive the BoM, and the quantity in the callout just serves as an indication of how many objects the note applies to. Also for some reason the macro is unable to get the change to "User Specified Name" to stick on some files. This requires toggling the setting manually and rerunning the macro. Finally we create assembly drawings in spurts, so I periodically get asked by other users why the note is not showing the desired text. The solution to these queries are generally one of: run the setup macro on the correct file, fill out the description or part number property in the correct file, or insert an off drawing BoM and use a balloon rather than a note.

But in the end we can create a drawing that has the information that the assemblers (primary customer of the drawing) need in a form that is convenient and easy for them.

Eric

 

[pdybeck]

Eric,

Sounds like you are doing what I was thinking about. Good to know. By the way, you can now call out part number directly in balloons without having a macro needed. It works in SolidWorks 2013 (don't know which release it was added in). I think you may be able to get what you want with a stacked balloon, or a custom note... without the use of macros. Just a thought.

 

[pdybeck]

Eric,

Are you a large company? Small?

 

[EEnd]

The macro is not required for the process, it is just more convenient that taking the steps manually. Now that we have these setting in our templates, the macro should not need to be used very often. We still run into the odd file where it is useful to run it. Some of the extra effort is related to including the description, part number and revision into a two line note like:
Cable Clamp
1199-0020-A

This is currently accomplished by setting Callout Text. It looks like we could use a different custom property name, and today I might chose to create one that is 2 lines and one that is all on 1 line. I think the choice to use Callout Text was a vestige of an earlier iteration where the "balloon" had part number and revision, and we included a BoM table with that as the key plus Description and Quantity. It has been long enough (5 years +) since I set it up that I don't quite remember the rationale.

Eric

 

[pdybeck]

Since you are showing revision in your balloon on the assembly drawing, do you then update your drawings every time a component used in that assembly has a revision done to it? Yikes.

 

[EEnd]

We consider the revision level of an assembly's components as part of the information specified by an assembly at a given revision level. So when a component's revision level changes, the revision level of any assembly containing it changes. This trickles all the way up to the highest level assemblies. So your are correct, Yikes.

This is how we track which combination of component revisions were in use at a given time.

Once the revision level has been updated in the component files, the new revision level shows in the assembly drawing when we go to update the assembly's drawing to show its new revision level. Ideally there is no additional cost in having the component revision levels on the assembly drawings, assuming that we were going to update the assembly drawing to reflect the new revision level of the assembly.

It is enough of a hassle that we try to make those changes in batches.

The only way I see around it is to not consider the revision level of components as part of the information specified by the assembly's revision level. Then the assembly would not need to be revised when a component is revised. However we would then need a different way to track what revisions were in use for a given build, and if the appearance of the parts change then we would need a way to know which of the assembly drawings of a given revision level shows the current appearance.

Eric

 

[pdybeck]

Eric,

Wow, Yikes. Your top level assemblies must have a ton of revisions. Is this a requirement? FDA, DOD? Just curious. Anyhow, I was just kicking around the exercise of having part numbers ballooned and not item numbered as it would side step a lot of this...

 

[snowshoe2]

To comment on the revising of assembly level drawings every time a component is revised, I have been at companies that did it both ways, depending on what that situation required.

But the process of part numbers identifying components rather than item/balloon numbers seems like an easy one. Essentially it's the part number of the component that is the unique piece of info in the system, why not use it in a simple way, especially if your drawings are clear while using it and the staff who live with the documentation like it.

(20+ years in engineering and manufacturing)
have a good wknd
Steve