Revision management 7

[Andy330hp]

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!

 

[rocheey]

Well, my experience with Solidworks is that they must monitor all boards like these and seem to 'read your mind' with new features that either you just asked about, or, if you dabble in the API, a feature that replicates all the code you just wrote <g>

I wouldnt doubt if you'd see it soon.

 

[badboggs]

Let me take a stab at a few of these questions.

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

 

[JNR]

Hopefully your startup will eventually flourish into a prosperous and sizeable company. You will then be looking for a PDM system to keep track of everything. With this in mind, I suggest that you take a peek at how PDM systems tend to limit (or I should say control) file naming and configuration naming. Your VAR should be able to help you on that. I suggest you figure on a system of naming that will (hopefully) be compatible with a future PDM system. Renaming eveything would be very hard.

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.......

 

[Andy330hp]

Are there any good books out on this subject?

 

[Arlin]

Revision management is a complicated and important issue. It has been discussed ALOT both here and ant comp.cad.solidworks.

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 &quot;old&quot; file to 3849-2934_REV_1.PDF and then save the &quot;new&quot; 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.)

 

[relswick]

I am surprised no one has mentioned using various configurations for Revision control.

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.

 

[MadMango]

I would not recommend using Configs for rev control. There are too many things that can go wrong in your configs and assys that might yield the improper final assy.

Wanna Tip? faq731-376
&quot;Probable impossibilities are to be preferred to improbable possibilities.&quot;

 

[rocheey]

While I doubt the SW gods would shine on this one, you can also use a Design table for revision control: if you have Multiple configurations with the same name in a design table, the LAST one of the match will be displayed....

 

[Andy330hp]

I would like to pick up this discussion again. I suggested some of the ideas mentioned here about not having the revision number in the part number, and not changing the assembly number when one of the parts has been revised, and they couldn't believe it. They are solidly under the impression that if we give our suppliers an updated assembly with the same dwg number on it but with ANY different information on it, there will be confusion and possibly errors made by our supplier. Thoughts?

 

[TateJ]

It's real nice to have intellegent suppliers - believe me I've tapped suppliers to help me design new parts.
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[/u]​

 

[Standing]

Andy330hp,
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:&quot;SW-File Name&quot; $PRP:&quot;Revision&quot; DRAWING
$PRPSHEET:&quot;Revision&quot; MODEL
Create a model, put something in the revision property. Put that model onto the drawing. See what happens.


Bradley

 

[RawheadRex]

Chiming in on the topic...

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 &quot;smart&quot; 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.

 

[sirmick]

File naming conventions are one hassle. I prefer putting the rev level in the name and manually updating the links in the assembly and drawings. That way I am cognizant of the ramifications of my changes to a part.

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...

 

[JNR]

Andy330hp: There are a couple of good books on this . Mr Boston's Bartender's Guide - I think that's the name - is a good one for the beverages. You should be able to manage the lawn chair bit on your own..... ;-)

(couldn't resist...)

3/4 of all the Spam produced goes to Hawaii - shame that's not true of SPAM also.......

 

[Andy330hp]

I've already got the playboy bartending book...good enough?

 

[JNR]

Hey..... sounds MUCH better than Mr Boston's!!! Now if we could only find a nice quiet spot for our lawnchairs at the mansion....... but I don't think my wife would approve :-( and there would be that little old man running round in his PJ's....

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.......

 

[EdDanzer]

I would not recommend revision numbers for a startup. If the part is different just give it a new part number. More scrap has been made from reading revision numbers wrong than reading part numbers wrong. We track part numbers in Excel by assigning the numbers sequentially, I haven’t seen a less costly way.

 

[SBaugh]

If you want to use Revisions for management wait for SW04. They have a pretty neat option in there to help with file management using Revisions.

Regards,

Scott Baugh, CSWP
3DVision Technologies

http://www.3dvisiontech.com

http://www.scottjbaugh.com

faq731-376
When in doubt, always check the help

 

[sirmick]

Ed,

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?