Revision management
Revision management
(OP)
Hi,
I'm part of a startup company, and we're having some questions concerning the management of our drawings.
I have some experience with Solidworks during through college (I'm a recent grad) but am not an expert. So, I can make pretty nice models, but I've never had to do much organization
Our biggest question is about the organization and creation of revisions. What kind of features does SW2003 have that can help us automate the process? Is there a way to automatically generate a revision block? Can you then reference the Rev number in the title block to the last revision in the revision block?
Once a new revision of a part is made, a subsequent revision of the assembly must also be made. Once the new part is inserted, is there a way to automatically update the parts list in the drawing to reflect this? I may be asking for a little much here, but if there isn't a way to do it now maybe these discussions will spur them into adding it to future versions!
I'm part of a startup company, and we're having some questions concerning the management of our drawings.
I have some experience with Solidworks during through college (I'm a recent grad) but am not an expert. So, I can make pretty nice models, but I've never had to do much organization
Our biggest question is about the organization and creation of revisions. What kind of features does SW2003 have that can help us automate the process? Is there a way to automatically generate a revision block? Can you then reference the Rev number in the title block to the last revision in the revision block?
Once a new revision of a part is made, a subsequent revision of the assembly must also be made. Once the new part is inserted, is there a way to automatically update the parts list in the drawing to reflect this? I may be asking for a little much here, but if there isn't a way to do it now maybe these discussions will spur them into adding it to future versions!






RE: Revision management
I wouldnt doubt if you'd see it soon.
RE: Revision management
1.) Make sure that when you save parts, assemblies, and drawings you don't add a rev to the part number. For instance don't save a part as widget-1. Just save it at widget. The reason is that if you have rev levels in your part names the assemblies and drawings that reference them won't know which one to pull in when you update a rev. You don't want to have to manually update and keep track of which assembly calls which version of what part. This way they just pull in the most current version. The downside of this is lack of history. I'd recommend either saving off pdfs of drawings and/or creating edrawings. Or more aggresivly look into PDMworks.
2.) Yes you can automate the rev block in your templates. What you have to do first is decide what properties you want to use for each of your drawings and parts. Common props. are Number, Description, Revision, Author, Created Date, Material, Finish, ect.... After many years of doing this I would recommend you use the default property names used by Solidworks. You find these defaults in the part properties. The reason I suggest using the solidworks defaults is that if later on you need to update part properties it can save you time by not having to type everything. Also it does matter if the names are capitolized or not. Solidworks doesn't care but PDM systems might. Once you define all the properties you want to use in a part, open an appropriate drawing and drop a view of the part into it. Edit the template. If you right click the rev letter and click properties a screen will pop up (sorry, I'm locked out of SW right now so I can't check the names). On the right hand side of the box you will see an icon file folder with some links. I belive it is called link to properties. Once inside chose the external references box and open the scroll down menu. You should see the custom properties you created in the part. For rev choose Revision or whatever you made the property. Then repeat the process for each of the properties you created. Then save the drawing template off and use it as your default. You will also have to save a part template that contains all of the property into as well. You should do the same for assembies too. This allows you to set the rev level in the part and not the drawing. It makes creating drawings and keeping your information much easier.
3.) As far as the rev box area (mine is in the upper right corner) goes I would recommend adding three rev boxes to be used for your first three rev changes. That way you don't have to create new boxes and insert text for each one every time you update a rev. Most of the time parts don't get reved above 3 anyway (at least at some companies) so it will be all set up for you. I'd also recommend going ahead and adding text to these boxes ahead of time (make sure your alignment is correct to). It can be very time consuming to have to add text over and over to rev boxes. Just make the text -- to be edited as needed. I'd also recommend making the revs in the boxes dumb (or not linked to the part). It is a hassle to update them as you go.
4.) As far as adding parts to assembies. Be aware that usually if you just update the rev of a part you don't update the rev of an assembly. Usually you only update the assy rev if you add or remove a component. If this is the case SW has a built in BOM display for your drawings. With an assembly inserted into your drawing. Click somewhere in the drawing and go to Insert/Bill of Materials. This Bill will be smart and will update as you add or remove components. The default BOMtemp includes Number, Quantity, and Description. I'm not sure of the spelling or capitalization of the properties called into the BOM but you can easily look at the spreadsheet to tell what it is looking for. This is powerful as you can add whatever you want to the BOM excel file if you wanted to include custom properties to the BOM.
Sorry that this was so long winded. I would be very curious if most of you do this same sort of organization for there parts/dwgs. Most good places do. And if I haven't explained something very well and you have questions please ask. I just put this down off the top of my head.
Good luck with the Job Andy!
Boggs
RE: Revision management
Suggestion #2. The warm weather is here, so take the SW manuals home (print stuff out if you need to or even take a laptop). Pull out a lawn chair, makeup batch of your favorite beverage and settle in to read them cover to cover. You will be grateful you did and will have a good idea of the features available in SW and what to go test out to get your stuff working the way you want. BTW: this applies to any CAD system or complex softwar application.
3/4 of all the Spam produced goes to Hawaii - shame that's not true of SPAM also.......
RE: Revision management
RE: Revision management
There is no universal one size fits all answer. Differing work environments need different revision management practices.
That said, I am a big proponent of component re-use. Different projects can and do use lots of common parts first developed for something else. Thus, we really do not have project folders in which all parts and assemblies and drawings can be neatly isolated to one folder. Under this sort of work environment, here are a couple of my suggestions:
1.) Forget about any sort of intelligence in your part numbers. Just use a simple sequntial numerical system. In my experience, using an intelligent part number always ends up causing more grief than it is worth. Eventually, you run out of part numbers and you get more exceptions than rules.
2.) Always use a static drawing format like PDFs, DXF, or eDrawing for drawing/design communication to shop floor or outside vendors. SWX drawings are only used to create these static drawings. (You can even write protect the *.slddrw and use the SWX viewer as a static format)
3.) Revision control is accomplished by archiving your static drawing files (PDFs or whatever you are using). Thus, if I make a change to part# 3849-2934, I would find 3849-2934.PDF, rename that "old" file to 3849-2934_REV_1.PDF and then save the "new" 3849-2934.PDF.
4.) For us, the rev block in the drawing is a totally manual process. We just edit the sheet format, copy the previous rev block line, and then edit the text in the drawing. I think it works very well and quick. I can elaborate more on how we do this if you need me to.
The only downside to my method is that you really do not have the model of previous revisions available. IMO, this is really not necessary IF the you follow good revision rules. Namely, if Form, Fit, or Function change, you should create a new part number instead of a new revision. Any revised part number should be fully backwards compatible. If it is not, then a new part number should be created instead of a revision. (Granted, this can be a very difficult philosophy to implement and adhere to, but it is what I believe in.)
RE: Revision management
This makes sense for a production part, which has entered into your company's Engineering Change Control process, since you can switch configurations easily enough to demonstrate how a part can have different Revizions, yet work with different projects.
RE: Revision management
Wanna Tip? FAQ731-376
"Probable impossibilities are to be preferred to improbable possibilities."
RE: Revision management
RE: Revision management
RE: Revision management
But ultimately the responsibility to insure your supliers have the latest revisions is yours.
Sure, an intelligent supplier may have a question - but that is cleared up quite nicely with a phone call.
Just make sure your PO references the correct revision; bada-bing bada-boom.
Our drawing numbers, file names, and rev numbers are not related at all, and we've had no problems - but we're crazy that way!
Read my profile & make me an offer... now!
tatejATusfilter.com
RE: Revision management
Are you going to be using PDM/Works? I would if I was a startup company using SolidWorks.
Try putting the following on the sheet format of your current drawing.
$PRPSHEET:"SW-File Name" $PRP:"Revision" DRAWING
$PRPSHEET:"Revision" MODEL
Create a model, put something in the revision property. Put that model onto the drawing. See what happens.
Bradley
RE: Revision management
1. I concur with the vast majority of people who've told you NOT to put the revision for a particular part number in the SolidWorks filename. If the people you're working with come from planet AutoCAD (where I once lived for about 10 years) then I can understand the reason for the reaction of disbelief to this concept. The bottom line is that SW functions much differently and "smart" filenames are of little use and create a good deal of additional work (and headaches as well).
2. For a short answer to the revision management question I strongly suggest (if you're not in the market for PDM just yet) reading up on the SolidWorks Explorer utility which I found very helpful in one of my former lives where we didn't use PDM. It helps automate the management of part, assembly, and drawing file references.
It's a kind of complex topic to cover but you'll find lots of ideas for different approaches here. Good luck.
Chris Gervais
Sr. Mechanical Designer
Lytron, Inc.
RE: Revision management
The bigger problem I think that you will have is when you have multiple users working on the same project. Especially when people start saving the same part on their local machines and the same rev of the part starts to have divergent properties. This has been the biggest headache I have had in my professional life.
The cost of a PDM system is well worth it. Now if I could only convince my management here of the benefits...
RE: Revision management
(couldn't resist...)
3/4 of all the Spam produced goes to Hawaii - shame that's not true of SPAM also.......
RE: Revision management
RE: Revision management
Enough frivolity - back to serious newsgroup business...
3/4 of all the Spam produced goes to Hawaii - shame that's not true of SPAM also.......
RE: Revision management
RE: Revision management
Regards,
Scott Baugh, CSWP

3DVision Technologies
http://www.3dvisiontech.com
http://www.scottjbaugh.com
FAQ731-376
When in doubt, always check the help
RE: Revision management
What do you when a part in a assembly changes? The way I understand it you would just change the part number of the part. Wouldn't that invalidate your assembly drawing if it has a BOM on it?
RE: Revision management
RE: Revision management
Bradley
RE: Revision management
To me its the same end result. Now, a problem occurs if your company issues drawings and doesn't want the problem of a controlled drawing with a given rev number changing and the rev number staying static. To me this is a no-no.
RE: Revision management
Consider how your manufacturing is going to work. Someone is going to take your BOM, walk into the stock room and build a kit of parts to be assembled. Shortly afterwards, someone else will take the kit and your assembly drawing and put everything together. If every single item on your BOM is correct, then all the required parts will have been ordered, stocked and kitted. If your assembly drawing is all correct, then the item numbers will correspond to the BOM. You should have made your drawing clear enough that the assembler can identify stuff sitting in the kit. The system will be assembled and it will work.
Any part numbers in the system must point to a parts bin with the correct parts in it. The part number on the BOM must be the correct part. This all requires discipline on your part.
Suggestions:
1.) Do not apply the revision number to your part numbers.
2.) Do not modify parts.
You may revise drawings to clarify information, or to correct mistakes. In the case of mistakes, it is assumed here that the parts were fabricated correctly, and you have brought the drawings into conformance. CAD drawings routinely have missing dimensions for example.
If you want to change a part, you generate a new model, and new drawing and a new part number. Alternately, you can tabulate the drawing, adding a code to indicate the new part. The original number is still valid, and unmodified.
This is all crucial once you build a library of parts and start using stuff on several assemblies and projects. When you change the form, fit and/or function of an existing part, you are possibly screwing up an existing design.
If effect, if you organize SolidWorks correctly, you should never have to check out the solid model of a part.
At the assembly level, you should not change the form, fit and function. You can modify the assembly, but it must be forwards and backwards compatible to the existing version. You should log the revision number when you build the assembly.
JHG
RE: Revision management
On a related issue: Say I change a part. And, say its p/n was number 1001. The new part is 1002. It is ver similar to 1001, so much so that I would like to reuse the drawing file for 1001 and incorporate the changes. What is the correct renaming/saving sequence to make this happen fluidly. I have messed this up and have had to fool SW by renaming files, moving things around, and basically doing what shouldn't be done (in my opinion) to get the drawing to look at the new part. I just bought Murray's book, I haven't found any info on this yet (in honesty, I'm going cover to cover and haven't even hit the drawing section yet). Thanks
Andy
RE: Revision management
Good luck
RE: Revision management
The easiest (and safest) way to create a new model and drawing is to start from the drawing. Lets say that you do need to create the part 1002 from part 1001. Open the drawing for part 1001 / do a SaveAs to part 1002 / then using the RMB open the model for 1001 and do a SaveAs to 1002 there as well / Changer your Custom Properties for the new part / Save your model / Switch to the drawing and save it as well. The links in the drawing will be updated and you can make any modifications to it as needed.
The only problem with this approach is that if you have an assembly open that uses part number 1001 in it, every instance will be changed to part number 1002. To prevent this – make sure that the assembly is not open when you create your new part.
Lee
Consciousness: That annoying time between naps.
RE: Revision management
L8R Sk8R
RE: Revision management
Currently the old drafter has left many files with different configurations. Lets say the first file, which has a descriptive name "widget.sldprt", has 3 configurations (one casting and two machining) for which I will be assigning 3 distinct part numbers. Is it okay, in your opinion, if I just leave the descriptive name for the part file? So far, we have been talking about purely sequential numeric numbering for everything, but I can't really give the one sldprt file one numeric name because it contains 3 different p/n's within. Should he have made distinct part files for each? And if so, what would be the point of having configurations in the first place?
CAD was so much easier in college when these issues didn't exist!
RE: Revision management
1001
1002
widget
1004
If you can live with that...
I would still assign a nonsignificant part number to your widget with 3 configs. Are the 3 configs reflecting machining operations for the part, or do the configs reflect 3 distinct parts used in different ways?
MadMango
"Probable impossibilities are to be preferred to improbable possibilities."
Have you read FAQ731-376 to make the best use of Eng-Tips Forums?
RE: Revision management
Regards
RE: Revision management
1. Casting
2. Machined
3. Slightly different machining
In each configuration's properties, I WOULD assign part numbers. But which (if any) part number should I choose to rename the file as a whole, and why even bother if I can set up the assembly and drawing files to look at the information in the configuration properties? It's a file naming issue vs property assigning issue.
Rustdog, to clarify, are you suggesting that I take this file and split it into three seperate files, with correct part numbers for names, and eliminate the use of configurations? I was actually thinking of doing that, it has the benefit of being easy to track but the downside is that I would have a LOT of work ahead of me. I'll do whatever is necessary to make things right though
RE: Revision management
At my last company, we had similar models like the one you are describing. We gave it a base part number 10000-xxx and the seperate configs would be 10000-1 (config name casting), 10000-2(config name machined), etc. They shared the same drawing. Manufacturing would control the process and which sheet drawing to issue depending on the machinig process. It worked well. If a part could no longer share the base part number because form, fit and function change, then it was assigned a new number.
Your other related note: SolidWorks Explorer works well for using the drawing of similar parts.
Good luck!
RE: Revision management
I have not had a really good chance to play with castings. I had a preliminary design going at one point, but we wound up doing it differently. Consider the following scenario.
1. I design a casting, part number 1005.
2. I machine the casting to create part number 1006.
3. I now want a modified version of the machined casting, so I create part number 1175.
Part numbers 1006 and 1175 are fabricated from part number 1005. I can implement this in SolidWorks such that the model of the casting does not get modified.
First, I create a drawing and a part model for the casting.
Second, I create a drawing and an assembly model for the machined part. I insert the casting into the assembly model. Within the assembly model, I carry out my intended machining operations. I do NOT edit the part. SolidWorks lets you remove material at the assembly level. I document all of this on the machining drawing.
Since my fabrication drawing is an assembly, I have the option of adding thread inserts and dowel pins, and using SolidWorks' BOM features to document these. Most of my fabrication drawings are attached to assembly models rather than to part models for this very reason.
Now, consider what you have done in real life. You have designed a casting for which the company has paid something like $10K in tooling. You have designed a machined part out of the casting, which may have cost a couple hundred bucks in CNC programming.
You want to modify the part. The casting is very expensive to modify, and the machining is very cheap to modify. You create a new drawing and a new assembly model. You attach the old casting part model, and generate and document your new machining procedure. The part model for the casting remains locked up in your PDM system if you have it, or else the part file remains read-only.
JHG
RE: Revision management
I noticed your earlier post about changing file names. You do not need to open all related files to change a file name. Have you fully investigated the SW Explorer? It allows one to rename files and updated all its references within a search path.
RE: Revision management
We never have looked at the SolidWorks Explorer. It sounds like it would save a lot of time and renaming issues. When time permits I will look into it.
Thanks for the advice.
Bradley
RE: Revision management
I have to agree with Drawoh
In my last company we did something very similar with electrical control boxes that we purchased and then modified to fit our needs. The only difference was that we had a dash number filing system. There are a lot of reasons why this kind of system is desirable, but in this case, the biggest one is the ability to keep similar files together making locating a file easy.
With a control box, since it is actually an assembly, we created the box components with the same filename but a different modifying descriptor like:
123456-001 Control Box 34x48.SLDPRT
123456-001 Control Box Door 34x48.SLDPRT
The assembly that used them was
123456-001 Control Box 34x48.SLDASM
This allowed the assembly to function (door open/closed) properly. This worked because the assembly was the purchased part and the 2 internal parts would never be purchased separately.
In the modified control box assembly, we placed any cuts or holes needed and gave the part a dash numbered like
123456-002 Project 1 Control Box.SLDASM
The drawing had the same name and was normally a multi-page full-scale drawing that the machine shop used as a template.
One advantage to this was that when we needed to use the control box on another project – most of the work was already accomplished. In fact – most of the time we would simply open the drawing for the original project / save it to the next dash number (–003) / open the assembly & save it to -003 / modify the custom properties / and then make the necessary modifications.
Dash numbers are very beneficial in other ways as well. The best reason for using them that I can think of is the tabulated drawings (a design table driven parts). The problem with their usage is that there is only 1 model and drawing for a lot of parts.
Since most of us used Windows Explorer to open parts and drawings rather than SolidWorks, we needed something to differentiate these files. What we did was to change the dash numbers in the filename to x’s. We used this as a flag to state - There is something special or unusual about this file.
123456-xxx The title of the drawing was added here.SLDPRT
Please note that this still allow the sorting routine in Windows Explorer to order the files properly.
Lee
Consciousness: That annoying time between naps.
RE: Revision management
Unigraphics had a built-in system for recognizing file revisions based on actual file names. It was flexible enough to accomodate nearly every conceivable naming convention. Very difficult to set up in some cases, though.
RE: Revision management
What is the difference between what you did and creating a derived part? In fact, wouldn't it be (marginally) better to create a derived part, so that it is in fact saved as a part and not as an assembly? I don't know if actually is any minute benefit in terms of the way solidworks treats the different file types...
RE: Revision management
RE: Revision management
I have not used the derived parts at all, so I am no judge of them.
My objectives are as follows...
1.] Model what really happens in production.
2.] Preserve expensive tooling such as casting dies.
3.] Preserve CAD drawings and models that control the expensive tooling that I don't want changed.
4.] Design and document new parts are quickly and accurately as possible.
My process above is based on the assumption of expensive tooling. Your problem may be different.
Consider this. When I model a machined part in SolidWorks, I try very hard not to add material. I start modeling from a block, and I remove material. If it is not obvious to me how to remove the material, I assume it is not obvious to a machinist either. This is how you avoid problems in the machine shop.
I'll have to read up on base and derived parts.
JHG
RE: Revision management
During the last 20 years, the majority of my time has been spent in contract positions. In fact – most of my permanent positions - started with a temporary contract. In most of these positions, an intelligent numbering system was used. Personally, I don’t like intelligent numbering systems, but that might be because I have had to work on too many that were poorly planned, overly complex, or just plain stupid.
However – I do have to admit that even a poorly designed intelligent numbering system is good at one thing. They allow the people who use the system on an everyday basis to find what they are looking for quickly without having to resort to a computer or a catalog. With a completely random numbering system – a part search is required for every part accessed. Further, even though a database search is very fast, in large companies you invariably get a listing of several dozen parts that MIGHT be what your looking for – which often requires you to manually pull each part to examine it. All of this adds up to a lot of wasted time when you include accounting, engineering, manufacturing, product support, sales, stock storage, and shipping. As far as the end user is concerned – the only companies that I have seen that didn’t hold the users hand and guide him to what he needed were very small or only had a few products. That is what after market sales is all about isn’t it?
Personally, if I was starting from scratch and the decision was mine, I would implement 2 numbering systems. The first would be for purchased parts and it would have some intelligence. The second would be for manufactured parts and it would be a semi-random list. The reason for the difference is that purchased parts lend themselves to being categorized while manufactured parts (for the most part) do not. Using a double numbering system is good for almost everyone in the company.
The number of significant digits depends primarily on the size and complexity of the companies products. A very large OEM could easily require a 10 digit system, but most smaller companies can normally get buy with only 6 or less. For parts, I would use the format xx-xxxx - which means that there would only be a maximum of 10 basic categories with 10 sub-categories (100 in total). I believe that having any more then that is a waste of effort. For manufactured parts the format would be xxxxxx-xxx. Sorry – but I prefer a 6-3 numbering system. I realize that this is a personal preference but I am a very organized individual and I like to be able to find things quickly. I also like the ability of keeping a group of often used parts together.
You should understand that 90% (guesstimate) of the numbers created would only have a single dash number (-001). For that 90% the dash number is unnecessary but it is included for consistency. The average employee quickly learns to disregard the –001 dash numbers but any other dash number is noticed almost immediately – and they rarely make the mistake of completely ignoring it more than once.
The other 10% is why dash numbers are created and maintained. There are a lot of reasons for using a dash number system. Some of the best reasons are:
· Products with multiple sales configurations or options
· Products sold in countries that have a different language and require different manuals or instruction sheets
· Product Redesign – this is NOT simple revision control – it allows a redesigned product (or several variations of a product) to be sold in specific markets for testing and evaluation before the original product is discontinued – I have seen several products marketed this way before a final design was selected – Normally, this technique is reserved for the top level assembly and major sub-assemblies
· Customized variations of standard products for specific customers (OEM)
· Tabulated Parts
· Cut-To-Length parts like extrusions / pipes / or wires
· Parts with color variations
· Parts that naturally belong together
Yes – All of those things can be handled without using dash numbers – If you are forced to, you can find a way to accomplish almost anything. A dash number is simply a convenient method that WORKS and when implemented it can make life a little easier.
Just my $0.02 worth.
Lee
Consciousness: That annoying time between naps.
RE: Revision management
Having worked for a start-up company once and having survived the issue you're facing with Rivision History woes, my reccomendation to you would be to invest in a simple PDM software. If you purchase SolidWorks Office, I believe they include PDM-Works. It may not be the BEST out on the market, however I feel that's it pretty darn good at what it does do ... KEEPING TRACK OF MODEL, ASSEMBLY & DRAWING histories.
Why bother with trying to re-invent the wheel, it's already been done and redesigned to many times. And if you try to create "smart" part numbers (i.e. part numbers that incorporate the revision) ... well lets just say that can become a huge nightmare.
But that's just my opinion ... Good Luck.
Brian Mazejka
Project Engineer
L-com, Inc.
RE: Revision management
Bradley