Revision control

[wisker]

I just started a new gig where I'm the only SW user. We're a 'fast pace' job shop. Whenever I release .... this is taking too long. Here's what I need =
I need to be able to have access to past revisions of components even if they are created in and tied to assemblies that aren't on the same revision.
The assem is on Rev D. All components are on D. However I need to be able to replace a component with Rev B of the same part to see what effects it might have. (ie whether it will fit with the Rev D components)

wisker

 

[SnowCrash]

Responding quickly, perhaps too quickly ;-) my approach is the current version of all models and drawings is always unchanged file name with rev level noted in properties and displayed on the dwg. The old versions are "saved as copy" with the rev level as prefix to the filename. Old version drawings are "saved as pdf" files with the rev as part of the file name. *.dxf or dwg works, too.

--
Hardie "Crashj" Johnson
SW 2005 SP 4.0 (reluctant to change)
Matrox Millenium G550
AMD Athalon 1.8 GHz 512 Meg RAM

 

[ctopher]

I suggest you use PDMWorks. You can do what you want in a heart beat. Otherwise, you will have to do a replace and hope the mates work.

Chris
Systems Analyst
SolidWorks/PDMWorks 05
AutoCAD 05
ctopher's home site (updated 06-21-05)
FAQ559-1100
FAQ559-716

 

[wisker]

I've been looking at PDMworks, I've just never used it before. Here's a question though. Part 001 is on revB and part 002 has features tied to it (ie holes constrained to the temporary axis of part 001). Using PDMworks if I roll Part 001 back to revA and the holes move - will they update in Part 002 to the revA location? Or will I see that they no longer align?
I guess a little more into the project. ~50 sheetmetal components w/ 600+ holes that need to align so that the assm can be pop riveted together. We cut parts, changes were made, the shop floor wants to utilize everything they cut (including past revs). They want to know specifically what holes relocated so that they can adjust the components to fit with the latest rev parts. It's not how I would prefer to work, but I'm outvoted.
I created all the components in one assembly file (top down) so I could be sure that everything aligned. Now, I change some compoents and it effects other ones (like it should). In smaler assems I have no problem keeping track of whether Part A needed something from part B, but this ones a little much.
This is a new method of working to me, so any suggestions are welcome. I may be hosed on this one, but I can see this happening again.

wisker

 

[ctopher]

In PDMW you can open an assembly "as built" to a certain rev (if all of the previous revs have been checked in) and all of the parts that were used at their specified rev in the assy will show up. Without some type of PDM software, it is a heachache tracking files the way you want. You would have to control them how it make sense to you.

Chris
Systems Analyst
SolidWorks/PDMWorks 05
AutoCAD 05
ctopher's home site (updated 06-21-05)
FAQ559-1100
FAQ559-716

 

[wgchere]

Chris,

In this case I think what Wisker wants, would be to open the latest rev of the assy "as built," then open the part he wants to explore in the earlier rev and click "yes" for "Do you want to write over the earlier file in you directory?" This would give the current assembly using an earlier rev part.

 

[wisker]

What wisker wants is to work from all the same Rev....but I don't see that happening. After talking to some other SW guys I think that I'll save off a part that I intend to modify as a copy and break/lock all of the references, creating a dummy part with a similar, but different name. This will allow me to have a CAD analog to what they've got on the floor. A part that's already made and isn't going to change. This isn't a solution that I'm thrilled with, but it will keep me burning parts.
Here's a thought. What if SW had a "Save as Revision" command. It would take a snapshot of that part in it's current state then track all modifications from that point on. You could then roll back to an earlier revision and it would suppress any features added after that save and modify any parameters back to that revsion state. Much like the configuration manager.
Maybe it's already there and I don't know about it, or maybe that's in PDMW, but I think that's a pretty simple request that could come in handy.

wisker

 

[ctopher]

wisker,
It's in PDMW.

Chris
Systems Analyst
SolidWorks/PDMWorks 05
AutoCAD 05
ctopher's home site (updated 06-21-05)
FAQ559-1100
FAQ559-716

 

[EEnd]

Because the parts still have in context definitions, even with PDMWorks, SolidWorks will not behave like he wants. For instance, lets say:

Part X has in context references to part Y.
Part X rev A was designed in context with rev B of part Y
Part X rev B was designed in context with rev C of part Y

If he uses PDMWorks to load an assembly of part X rev A and part Y rev C, part X gets rebuilt using the features of part Y rev C, which can easily make it different than the true part X rev A, which was rebuilt using the features of part Y rev B.

<begin thread hijack>
For this reason I think that it is a bad idea to have in context definitions left in the models once they get under revision control. The in context definitions can cause SolidWorks to modify your models without you realizing that they have been modified. Then you think you are looking at part X rev A, when in reality you are looking at a modified part X which may not correspond to any defined revision.

For integrity of your revision scheme, features should be redefined to eliminate the in context references. Painful as it is to do, I cannot see how to ensure that part X rev A is always the same if in context references remain. I prefer to use equations to achieve design flexibility as they can be toggled on and off.
<end thread hijack>

One possible workaround for wisker is to use PDMWorks to open the part in question at the desired revision level using as built references and save it out as a parasolid. Then the parasolid could be inserted into the current assembly to check fit and function. This is similar in spirit to saving drawings as PDFs to have an unchanging record of a particular revision.

 

[wisker]

EEnd sounds like he feels my pain. And I considered the parasolid format, however I'm working in sheetmetal and really need access to both the formed and flat parts.
So let me pick some brains out there. How would you guys go about modeling something like this? ~50 sheetmetal parts that must fit together. Things are still fluid, but we're making product.
EEnd, would you do it top down, like I have, then break all the external references? If so how would you make changes to the assembly later?
My personal experience has been to work in the current state, old revs be damned. They were changed for a reason. I can guarantee that if you're building a RevC assem and using all RevC parts it will go together. If you try and put a RevB widget in there - you're on your own.

wisker

 

[rgrayclamps]

Hi, wisker:

It is a good idea to use top down approach during initial development stage. When you release documents for production, it is better to break external references for revision control purpose. It seems that you do not completely understand assembly revision process. When you make changes to component parts or component sub-assemblies, your assembly may not need a revision. You have to identify whether a change is a component revision or an assembly revision, or sometime both. Also, you do not need to worry your old revision of your components/assemblies. You need to aware revision process is always one-way. If you have a part, which is currently rev. C, and you want to change it to something identical to Rev. B, it will become rev. D. Your assembly may not necessarily go through revision process.

Alex

 

[wisker]

Alex,
I completely agree and have worked that way in the past. However my new job, operates completely different than I'm used too. It's a welcome change (multinational corporation with me all over Asia for half the year to a job shop w/ 30 people total), but it's got me a little scattered. There is very little as far as document control goes. We're also very much a quick turn shop.
With the above assem I did one entire shot and sent it to the floor. They cut 5 part As and 20 part Bs, meanwhile the customer came back with changes to parts E, F, & G. Some of which affected part B. So I've got my assembly, which is current to the latest requests. And various old variations on the shop floor. The shop forman doesn't want to scrap anything.
This shop deals in tens, and one offs. We're just starting to get into larger higher number jobs. I came from a place with a document control dept. and I filled out ECOs and all the BS that goes along with it.
The "Rev the Assem" at every component change is how they do things here. Somehow it helps on the floor.
We've started to get off subject here I guess. More than anything I just wanted access to the CAD analog to parts I've already released.

Thanks for all the help everyone,
wisker

 

[BSMECAD]

Hi Wisker,

I agree with the previous comments that top down design is best suited for layout purposes only. Personally I always try to use bottom up assembly methods.

Here is possible suggestions that might help now:
1. Maybe you can always add accurate construction holes to your sheet metal parts. You could then develop a mechanical assembly fixture with dowel pins that align with the contruction holes on the parts. The fixture could be used to quickly assemble your parts or
troubleshoot/repair existing old revisons. You would need to add constructions holes after the fact based on some logic such as part centerline since parts are already made.

2. The best revisioning solution without PDMWorks was already suggested by Snowcrash. Instead you might try to use configurations in the Solidworks part file to keep track of all revisions instead of saving off. However, this method has many negative drawbacks but may help you align your parts.