two drw file for same assembly?

[otman73]

Hi all,
Is it possible to have two drw file for the same assembly? I use my assembly to create a Assembly drawing and Approval drawing. When I go to Save As, I want it to copy both of the drawings with it. The work around is to have multiple sheet but I would rather not do that if this can be done instead. Your thoughts are appreciated.

 

[ankarl]

If you use Save as, dont you get a copy of the drw associated with the same assy?


Or, do you want to copy all three files, assy + 2 drw's?

The last is easily made in intralink with the duplicate object function

 

[zpaolo]

Or, do you want to copy all three files, assy + 2 drw's?

The last is easily made in intralink with the duplicate object function

Or you can open drawing and assembly and use the rename function (only in session), then save the renamed parts, assy and drawing

Paolo

 

[audctrl]

We do the same thing with some of our assembly drawings. But we do not copy the drawing. Most of the time in our case we have to use a different format and the views are set up differently, like first angle for some customers.


Another option might be multiple sheets depending on your situation. Then you can still have just one drawing file.

 

[otman73]

When you use "Save as" You only get the one drw file which is the same name as the assembly file. I want both of the drw file to go with it not just one.
for example:
AHS_assembly.asm
AHS_asssembly.drw (drawn from AHS_assembly.asm)
approval.drw (drawn from AHS_assembly.asm)

"Save as" CS-9000
CS-9000.asm
CS-9000.drw (this one automatically get rename)
approval.drw does not get copy

hopefully that clear things up

 

[SRINIVASANIYER1]

I didnt get the difference between Approval drawing and
Assembly drawing. If approval drawing is not showing the
details, you can create a representation and a drawing or
sheet for that representation.
Personally I would prefer a single drawing with multiple
sheets, with PDF outputs for submission to clients for
approval.
I hope I have got it right.

 

[zpaolo]

I do a lot of multiple drawings from a single assembly, one is a drawing for customers, the other for internal reference, another for the guys at the assembly line... the internal one usually shares the name of the assembly, all the others have different numbers. I don't understand the problem otman is having, I can "save a copy" of the drawing and give it a different name, and still maintain relation with the assembly, or simply start with a blank drawing and add the assembly once it's open...

Paolo

 

[liwinter_9]

do you use PDMlink?


if yes, it is very simple to realize your idea.


open the PDMlink website use IE, search AHS_assembly.asm and then save as.

 

[otman73]

Thank you all for your input. Sorry for the delay in reply. It was the long weekend

Response to SRINIVASANIYER1
Our Approval drawing shows detail dimensional clearance which is submitted to the customer
Our Assembly drawing shows explode view of the assembly, no dimension and include the BOM

Response to zpaolo
I'm still new at PROE (less than a year) so forgive me

Assembly and drw file must have the same name in order to do a "Save as" on the assembly and it will automaticlly rename the DRW file correct? or am I wrong in this.

Response to liwinter_9
I don't even know what PDMlink is

guess I'll have to look that up later. Another one of those module you have to buy?

I'll explain what I'm doing and maybe that will shed some light on things. I'm trying to automate the work we have here and most of it is custom work. I'm making a generic assembly, drawings and BOM. All of this will be driven by Pro/Program. The user just answer bunch of question and do a "Save as" and Print it all off and send it off to manufacturing. I've already done all this in AUTOCAD but somebody thought it was a good idea we move to PROE

Sounds like I will just have to use multiple sheets

 

[zpaolo]

I'm still new at PROE (less than a year) so forgive me

Assembly and drw file must have the same name in order to do a "Save as" on the assembly and it will automaticlly rename the DRW file correct? or am I wrong in this.

Hmm I only have "Save" and "Save a copy" in my Pro|E menu, maybe I'm wrong but I've never done something like you said. My experience (though limited) is as follows:

if you have a part and a related drawing (a drawing you created when the part was open) and you save a copy of the part, that copy is no longer related to the drawing. Vice versa you can "save a copy" of the drawing, and the copy will maintain the relation with the original part.

Also notice that if you have a part and related drawing IN SESSION and rename the part, the linked model in the drawing will be updated, but not the drawing name. Example: 001.prt is linked to 001.drw. If you open both and "rename" (on disk and in session) 001.prt to, say, 002.prt you'll have a drawing still named 001.drw but linking to the part named 002.prt.

I hope I've written all correctly, maybe there are ways to have better relationship, anyway this is our company configuration

Paolo

 

[PRStockhausen]

If the config option "let_proe_rename_pdm_objects" is set to yes, then doing a save as in a pro/e part or assembly will copy a drawing of the same name. Doing what the OP wants should be possible with some programing.

 

[liwinter_9]

hello, otman73:


PDMlink is main modular of pro/e. i think it may be not cheap.


you have another way to your question: open the assembly and two drw file, rename these three files. because those original three files already checked in, these three new files will be created.

 

[otman73]

Thanks for the idea. It is "Save a Copy"

I was trying to minimize the work for the Operator by just opening the main assembly, run Pro/Program, "Save a Copy" and Print. I'm making it work with having multiple sheet. Thank you to all for your assistance.

Now if I can only figure out how to automatically print a PDF of all the DRW file that would be the BOMB!