"Open Drawing" when there's more than one?

[sdb999]

One part model with three configurations. Three drawing files, each references a specific configuration of the part. When in the model the right-click "open drawing" command opens the same drawing every time regardless of which config. is active. Any way around this?

2003 sp4.0

 

[ctopher]

When you first created the part. Did you first create one dwg for all three configs? Then change to 3 dwgs? If so, there could be references in the first dwg that needs to be deleted. Just a thought.
Or it can be opening the last dwg you had opened then saved.

 

[SBaugh]

Why don't you make one drawing file with three sheets each sheet representing a certain config. (You can always edit the sheet if that's an issue for you). Now everytime you open the drawing you have that single drawing that pops up.

I don't think there is away around the issue your having other than this one.

Regards,

Scott Baugh, CSWP

http://www.3dvisiontech.com

http://www.scottjbaugh.com

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[TheTick]

As far as I can tell, all that "Open Drawing" does is find a file in the same directory with the same name and the ".sdldrw" suffix.

 

[CorBlimeyLimey]

If a drawing has the same name as a model, it will automatically be selected & opened. That is probably what is happening.

So if you have to have seperate drawings make sure that none of them have the same file name as the model.

I agree with SBaugh that a single drawing with three sheets is the way to go.


from (the City of) Barrie, Ontario.

What happens if you get scared half to death twice?

 

[sdb999]

Three sheets in one file would be nice but I can't do that. The Tick is correct:"open drawing" will only open a drawing with the same file name in the same directory, failing that it just opens the browser to the last directory used. Rats, foiled again. Thanks for all the help.

 

[SBaugh]

Why can't you?

Regards,

Scott Baugh, CSWP

http://www.3dvisiontech.com

http://www.scottjbaugh.com

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[sdb999]

Long boring story, but the way we rev. control parts within our PDM system requires us to asign unique file names for drawings of parts.

 

[MadMango]

Our system sounds about the same [blue]sdb999[/blue], when we encounter this problem, we just assign the different configurations new part numbers so they stand alone in our PDM system.

Ray Reynolds
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[ctopher]

When using PDM, the only parts/assys that I create configs are cable assys. Each config uses a basic cable and has different wires in different positions for the assy they are used in. Trying to create dwgs for a machined part config in PDMW can be a nightmare. Best to keep them seperate, IMO.

 

[rocheey]

>>(TheTick)
>>As far as I can tell, all that "Open Drawing" does is
>>find a file in the same directory with the same name
>> and the ".sdldrw" suffix.

Just tried, and you're right. Made as "Part1.sldprt" and a "Part2.sldprt" in the same dir. Made a drawing of Part1 and named it "Part2.slddrw". "Open Drawing" from part2 opens the drawing NAMED part2 that is the views of part1

 

[ctopher]

Interesting to see if it changes in '05.

 

[drawoh]

sdb999,

If you think you have problems with PDM now, wait until you want to modify one of those drawings and not the other two. In order to modify any drawing, you must check out the model that controls the other two. Your other two drawings will be linked to an obsolete model, and no one in his right mind will trust them.

Can you do tabulations on your drawing?

Failing that, I would make copies of the models.

It is too bad that, as noted above, this will not solve your "Open Drawing" problem.

JHG

 

[macPT]

I solve this problem at file name level (that is with the part number).

The last 2 digits of the part number refers to "variant" parts (that is, configurations).

If a part as the number (file name) nnnnnnnn00, that means that there's no variants and there's only a drawing nnnnnnnn00.slddrw.

If a part as the number (file name) nnnnnnnnXX (actually the letters XX), that means taht there´s variants. I will have one drawing per variant (configuration) named nnnnnnnn01.slddrw, nnnnnnnn02.slddrw...

The part nnnnnnnnXX.sldprt as configurations named nnnnnnnn01, nnnnnnnn02,.... according to drawings.

This system is working for some years without problems. But Scott's idea seams to worth some attention and I think it can be a good alternative (if not a better way to do it).

Regards

 

[macPT]

Just remember a problem with Scott's idea.

Some of our drawings, having to much detail, can use more than one sheet to have an easier reading.

So it would be difficult to manage multi sheet drawings (are extra sheets caused by detailed drawings or by configs?)

Regards

 

[SBaugh]

The other problem with the idea is that if you have numerous configurations and detail. That can cause a performance issue within the drawing file.

There are Pros and Cons to either way! It's up to the Admin of your company to look at all possible solutions and take the route that he/she thinks is the best, easiest, better performance and most economical way of settings up your system(s).

But I'm not telling guys anything you don't already know.

Regards,

Scott Baugh, CSWP

http://www.3dvisiontech.com

http://www.scottjbaugh.com

If you are in the SW Forum Check out the FAQ section

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[sdb999]

In the case of configurations that are discrete part numbers we apply the rev one rev all approach. That way no drawings are referencing an out of date model. We use configs sparingly when drawings are involved, so usually all the parts are receiving the same revision anyway.