Revisited: Multi-User File Issues

[MadMango]

Our company has ~6 SW users that work in designing new components for our products. Some users are in Product Development, some are in Applications. We do not have a PDM system, and are waiting to install SW05 when SP1.0 is available (currently using SW03, SP 3.1). I know those warning bells are already going off in your heads.

I have for my settings:

System Options> External References
Enabled- Open referenced documents with read-only access
Enabled- Don’t prompt to save read-only referenced documents (discard changes)
Enabled- Allow multiple contexts for parts when editing in assembly
Enabled- Search file locations for external references
Enabled- Update component names when documents are replaced

This allows me to pull existing released components from one network location (S-drive) to use in new designs that are saved in a different network location (L-drive) for R&D work. When the final design is ready for Production we have a person in Document Control that saves our designs to the released components folders on the network (S-drive). These settings prevent me from creating copies of our standard components in the R&D network location (L-drive).

I know not all users have the same settings, even after repeated attempts to get all SW users to standardize their settings. The main complaint is that they do not like the Read Only files, and prefer to make local copies of components. This creates a lot of extra files that don’t need to exist.

There are times when some components (usually hardware) have mate errors. This is puzzling to me as when I am finished with a design I ensure there are no errors of any sort. When I open the components on my machine, I get no errors. But I can go use another machine and see that there are indeed errors.

I have checked the SW settings of the Document Control computer and everything is set the same as my machine. Does anyone have an idea why these errors occur?

Also, I am wondering if I have the correct settings in System Options>External References? If any one has a better method for working in this manner, I would love to hear them.

[green]"I think there is a world market for maybe five computers."[/green]
Thomas Watson, chairman of IBM, 1943.
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[macPT]

I have the same options enabled you have, except the 3rd (don't know exactly how this afects the work). The way of working is almost the same except:
- the definitive files on the server are write protected (I don't remember why, but when I first installed and "production" tested SW, I've figured out that would improve file integrity)
- we never make copies from data base, except in those cases that we want to create a new part/assemblie based in the work already done. But in that case, the first task is to change file names so we are not confused.

You must consider one thing (I think that is why the files are write protected). Don't know why, but some times, during the design process, even with the 2nd option enabled, SW tries to save the reference document, asking you to give a different name. In this situation you can discard the saving but you can also force the saving with the same name and location! Obviously this can change something in your "standard" file (the one in the local drive) that make your assembly no recognize the STANDARD file (the one in the server) properly. If you or someone of your team do that, that will be OK during design, but problems will arrive when the Doc guy saves the design, except the standard parts.

Right now, I can't figure out another reason for your error and I hope that this will help you.

Regards

 

[CorBlimeyLimey]

It sounds like the other machine(s) have a differently oriented version of the offending hardware parts.



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[MadMango]

I should clarify that no files are stored on local-to-computer hard drives. All files are stored on the corporate network.

Files in our network location for our standard parts are write protected. Only only one person (in Document Control) has access to write, all users have access to read.

We've created an internal program that we call "The Locator" that allows a user to plug in a file number and the program will search 2 locations on the network where the released files are kept and the project network location. If the file is a SW file or DWG you'll see a preview of it, and have the options to open it or view-only open it.

I would agree that different oriented hardware models would give the error I am describing. But only one version of the model exists according to our Locator. Is that program perfect? I couldn't tell you, but we have been using it for the past 2 years, and it works as expected.

[green]"I think there is a world market for maybe five computers."[/green]
Thomas Watson, chairman of IBM, 1943.
Have you read faq731-376 to make the best use of Eng-Tips Forums?

 

[CorBlimeyLimey]

I should clarify that no files are stored on local-to-computer hard drives.

Are you abso-posi-lutely sure?

The main complaint is that they do not like the Read Only files, and prefer to make local copies of components.

I would double check the other machines. Have you tried "Find references" on the assy file, to see what is actually being called up?

If not the above, then it sounds like a network or SW glitch.





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[TheTick]

One thing might help...

under "Options --> System options --> External references"
Make sure "Automatically generate names for referenced geometry" is OFF (unchecked). This way read only files don't get tagged as dirty just for being used in assemblies.

 

[macPT]

MadMango
The expression "local folder" should be understood as "any place other than the data base folder". The relevant issue is the copy of the data base to other folders (duplicated documents = big mess).

CBL
Good point. A few days ago I was getting mad because SW was ignoring my changes on a model. Why? I was realy changing a backup copy somewhere on the network (that was not a normal procedure)! So we must be shure that there are no duplications.

TheTick
I have that unchecked. What about you MadMango?

Regards

 

[MadMango]

It's unchecked.

[green]"I think there is a world market for maybe five computers."[/green]
Thomas Watson, chairman of IBM, 1943.
Have you read faq731-376 to make the best use of Eng-Tips Forums?

 

[SBaugh]

Enabled- Allow multiple contexts for parts when editing in assembly

I'm sure you know, but do you understand what this option does?

This option allows all user of that machine to in-context a single part to multiple assemblies. You cannot in-context the same feature, but you can in-context that one file to multiple assy. And the recommendation from SW Support is either not use it, or if you do your kind of on your own, because would be no way for SW to track a file like that.

Just want you to be aware.

This option maybe off on other users and that's why your seeing errors on other peoples machines.

My settings are:

System Options> External References
Disabled - Open referenced documents with read-only access
Disabled- Don’t prompt to save read-only referenced documents (discard changes)
Disabled- Allow multiple contexts for parts when editing in assembly
Enabled- Search file locations for external references
Enabled- Update component names when documents are replaced

I have very few problems with these settings, even when opening my customers files.

Regards,

Scott Baugh, CSWP
3DVision Technologies

http://www.3dvisiontech.com

http://www.scottjbaugh.com

faq731-376
faq559-716 - SW Fora Users

 

[macPT]

Thanks for the clarification SB. Maybe Madmango's problem is in the "Allow multiple contexts for parts when editing in assembly" option. I have it unchecked and I also have no problems.

Regards

 

[SBaugh]

That is what I was thinking, but it's something that you will need to test MM.

Regards,

Scott Baugh, CSWP
3DVision Technologies

http://www.3dvisiontech.com

http://www.scottjbaugh.com

faq731-376
faq559-716 - SW Fora Users