Solidworks Part Numbering

[LSPSCAT]

I realize there are numerous discussions regarding this and I have read most of the threads. The thread below is close to what I am looking for.

http://www.eng-tips.com/viewthread.cfm?qid=147500&page=3

I am in a similiar situation, currently working mainly in AutoCAD creating 2-D drawings of welded assemblies with a BOM which includes the sections and lengths and weights. There is a push to use more Solidworks and I have done some preliminary testing with assemblies and my only hangup is the large number of part files that need to be created for various components of the assembly. It is hard to see that going from a single 2-D drawing to an assembly with 40 parts makes things easier.

The assemblies are fairly robust and I can quickly change the the lengths of various components to generate various new complete assemblies and arrangements with minimal user interaction to update mates. This is useful especially for the drawing creation.

The assemblies are for frames for skid mounted units and contain various structural shapes of various lengths. Most of the assembly is welded construction however it often includes various fasteners and accesssories. Sizes are non-standard and can range anywhere from 2' x 2' to 12' x 18', with an infinite number of options....no two are ever the same; total yearly quantity is around 1800 individual assemblies * 40 parts each ...72,000 part files.

Part numbering to date has been based on drawing numbers..which i have maintained for the assemblies..configurations have been handled the same as the old tabulated drawings by adding the suffix (-02,-03,-04) Is it a bad idea to name the parts using the drawing number for the part file with the configuration as a suffix and then the item number from the BOM as a suffix...

A5673-03-05

Drawing Number: A5673
Configuration: 03
BOM Item Number: 05

This does not really need to tie into the MRP system as each cut section is not assigned an individual part number, so this is really just to manage the SW part files that are going into the assemblies.

Any thoughts?

 

[JMirisola]

Naming the parts with the drawing number isn't a bad idea at all. That's how I do it, though the description is usually more, um, descriptive.
FWIW - You might want to look into DriveWorks, TactonWorks, or another KBE system. It could end up making your job a lot easier.

Jeff Mirisola, CSWP, Certified DriveWorks AE
CAD Administrator, Ultimate Survival Technologies
My Blog

 

[LSPSCAT]

To clarify - each part of the assembly does not and will not have a separate drawing for it. The main assembly will have a drawing number, now in Solidworks I will have 40 different parts...90% of these are just cut plate/structural sections that need nothing more than a line in the BOM. However, they will be in a separate SW part file. It is just keeping track of all these additional files that I am struggling with or looking for the best way to handle.

 

[LSPSCAT]

I suppose part of this is just getting Solidworks to work in a production environment with many drafters/engineers all on the same page. I have always mainly used Pro/E and SW in an R&D or "special project" environment where all the details of making a consistent BOM and drawings did not matter as much as we were making a single-one of a kind rather large machine. Mistakes could propagate, however, I was judge, jury, and executioner so I could silently fix all mistakes in the middle of the night!!

 

[gwubs]

Although I am a HUGE fan of 3D modelling, you may be better off staying with 2D. That said, I am certain that a very effective configurator style system could be designed. This leads to the next point - a really good system does not just happen, it takes a LOT of hard work. The question that needs to be answered is WHY you are considering 3D as a company. It has to be understood that to use a 3D system, you have to do more work up front. You are no longer drawing lines, so you need to do more work to produce all the lines later. Kind of like 2D = x^2 and 3D = x^3. This is very hard for managers to grasp, because they want to see quick results. The payback on a properly planned 3D implementation is enourmous, but ONLY if it is well thought out, and rigouroulsy executed. Quick and dirty is very possible in software like SW, but in my opinion is nothing but a waste of time. That said, I can tell you that we have used SW for 10 years and none of us, managers included would ever consider going back to 2D.

 

[ShaggyPE]

I like your naming convention. At first I was hesiatant to accept having the BOM item number in the file name. I was more in favor of having another dash number indicating it is a sub component of a primary dash number... but that is basically what your BOM item number is.

A potential challenge I see is that one of your piece parts might want to be configured itself (or common amongst all of your weldment configruations). So having a configruation parameter in the part number wouldn't make sense. i.e. this part file works with multiple configurations of the main weldment. In that case, the file name could be: A5673-XX-05. Indicating that it is the 05 BOM item number for all of the configurations of A5673.

-Dustin
Professional Engineer
Certified SolidWorks Professional
Certified COSMOSWorks Designer Specialist
Certified SolidWorks Advanced Sheet Metal Specialist

 

[LSPSCAT]

Good call ShaggyPE I started using this a couple of months ago and it seems to be working..It is a good idea to go with the XX-05 for parts that are consistent across configurations.

I have some time this week so I am rexamining some of my original ideas. Putting it out to ENG-TIPS to air out some concerns. Since engineering departments have been shrunk so much it is the best resource we have for getting feedback.

Gwubs,

You are absolutely correct about the upfront planning. The sad part or fact of life is that we as engineers basically have been left to complete these "side" tasks on our own time and dime, otherwise they will not get done. Our management is completely out of date and touch with much of the new technology so explanations or details are lost after the first sentence. The only thing we can do is develop solutions like this on our own time if we want to progress forward.

I am pushing because I can see the end result of a great configuration type system based simply on user input from outside the SW interface. (When finished the product line will be outsourced or the software will change so my system will be obsolete!!!)

As I mentioned, I typically work on more R&D and larger single installation type projects where I do not have to think of every detail of creating an efficient system for a future product line...in this case I have been sucked in and would like to turn around a nice little system.

 

[sldwkmin]

Investigate the weldment tool. One part file just as you are now. All items listed on a cutlist. Could be an option.

One thing I have noticed through several implementations of SolidWorks is we often get hung on trying to make the new tool work in a procedure that was developed for the old tool. So try keep an open mind and maybe massage your processes a little and you may see great gains. An analogy I often us is "We don't buy an air nailer then flip it over and use it to pound in a nail". All too often though when implementing software that is what we try to do.

Cole M
CSWP, CSWST, CSWI, CPDM
Certified DriveWorks AE
HP XW4300, 3.4g proc, 2.5g RAM, ATI Fire GL 3100
Dell M90, Core 2 Duo, 4g RAM, Nvidia Quadra FX2500M
Equus (custom), P4, 3.4g proc, 3g RAM, Nvidia Quadro FX3400

 

[ShaggyPE]

both great points sldwkmin

-Dustin
Professional Engineer
Certified SolidWorks Professional
Certified COSMOSWorks Designer Specialist
Certified SolidWorks Advanced Sheet Metal Specialist

 

[Gurjjeet]

I do a lot of weldment I do it in one file. that way you do not need a big assy & part files. Try doing a skeleton sketch & weldment. It will surely be fast & efficeient to use.You might not need all the fuss of configuration as a skeleton sketch is lot easier to make & edit.

Only good thing about the Assy Idea is that you can use same part no. & drawing of a part in 2 or more assemblies.
If you have too many common parts then it will save you time & money in design & in production as well.

It will be a great idea to do a demo project on the side of an existing project in both ways(Assy & part) & then decide about the way to go which is most suitable to your needs.

 

[MechEng2005]

ShaggyPE and LSPSCAT:

I like your thinking, but... What happens if one part is used in configurations 1-4, and a different part is used in place in configs 5-8? You would have two parts, both used in multiple configurations. Would you then need another few digits on the part number, A5673-XX-05-01 and A5673-XX-05-02? In that case, I'd be tempted to use a part with number A5673-01-05 for configs 1-4, and A5673-05-05 for configs 5-8. However, that means you will have a part number for configs 2-4 and 6-8 that does not match the actual configuration you are trying to build. Defeats the purpose of having the middle digit be anything besides a "dumb" number.

Little off the original topic, but issues like this seem to consume WAY too much of my time...

-- MechEng2005

 

[ShaggyPE]

The XX simply indicated that it was a variable. It would be possible (don't know how much I like it) to have your 1-4 file be called A5673-XX-05.SLDPRT and your 5-8 file be called A5673-YY-05.SLDPRT

Your solidworks configurations would then be named A5673-01-05, A5673-02-05... in the A5673-XX-05.SLDPRT and A5673-05-05, A5673-06-05... in the A5673-YY-05.SLDPRT.

Kind of convoluted naming, but it really isn't the name that matters, it is the part number that appears in the bom. This methodology would achieve the desired result.

Alternatively, the XX and YY could be replaced with "var_1" and "var_2" etc. Simply indicating variable 1 and variable 2. This will ensure that your parts have unique names.

-Dustin
Professional Engineer
Certified SolidWorks Professional
Certified COSMOSWorks Designer Specialist
Certified SolidWorks Advanced Sheet Metal Specialist

 

[tph216]

Not sure if this has been covered, but there are various things you could do to reduce the complexity of your models:

a) Use multibody parts where appropriate. I typically use these where there is a fixed connection (e.g. weld or adhesive) between parts.

b) Use weldments feature. It in effect creates multibody parts, but is tailored for structural sections.

c) Use configurations, and make use of their names as suffix parts of part numbers for drawings. Seems you are already doing this.

d) Use relative views in drawings. Insert > Drawing View > Relative to Model. This enables you to pick out specific bodies in a part file to display in drawings.

e) Rename solid bodies where appropriate, and use their names as parts of part numbers.

f) Use custom properties of files to control / manipulate data used for cutting lists or BOM's. You can, for instance insert 'Part No' and 'Description' as a custom property (File > Properties), and then configure your BOM table to reference these properties. So you could, say, control the display of part numbers different to the file name if necessary (e.g. with bought out parts - supplier p/n etc, but retaining an internal part number as file name).

Hope some of those ideas help.