Solidworks Part Numbering
Solidworks Part Numbering
(OP)
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/viewth read.cfm?q id=147500& amp;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?
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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?






RE: Solidworks Part Numbering
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
RE: Solidworks Part Numbering
RE: Solidworks Part Numbering
RE: Solidworks Part Numbering
RE: Solidworks Part Numbering
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
RE: Solidworks Part Numbering
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.
RE: Solidworks Part Numbering
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
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Equus (custom), P4, 3.4g proc, 3g RAM, Nvidia Quadro FX3400
RE: Solidworks Part Numbering
-Dustin
Professional Engineer
Certified SolidWorks Professional
Certified COSMOSWorks Designer Specialist
Certified SolidWorks Advanced Sheet Metal Specialist
RE: Solidworks Part Numbering
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.
RE: Solidworks Part Numbering
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
RE: Solidworks Part Numbering
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
RE: Solidworks Part Numbering
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.