"Copy As" an assembly with new article numbers also copies the drawings.

[CAD_Monkey]

If an article has a drawing, and I save it with a new name, I have the option to also automatically duplicate the drawing with the new name, and references are redirected accordingly.

ABC.PRT has drawing ABC.DRW

ABC.PRT is Saved As DEF.PRT - it automatically gets a DEF.DRW using DEF.PRT.

This does not work on subcomponents of assemblies.

I can in one operation Save As GHI.ASM (containing X1.PRT and X2.PRT) to JKL.ASM (containing Y1.PRT and Y2.PRT that are Save As copies of X1 & X2) and the drawing GHI.DRW will also be duplicated into JKL.DRW.

But there will be no Y1.DRW and Y2.DRW. The option to also Save As the drawing files is not there.

This is a major pain, because if I want to fork an assembly to test some new design and wish to preserve the painstakingly detailed drawings, I can only Save As the assembly, then I have to individually open each part and Save As them, and then replace them one by one in the assembly.

And the assembly drawing will b0rk, because all components got new identities. BOM balloons fail, dimensioning fails, et cetera.

Please add the "copy drawing" function for assemblies, because this is a scourge of my work. I know the problem can be solved by acquiring a PDM system, but it is not quite my position to demand such wherever I go as a consultant. Procuring Windchill is no small operation for minor companies, and not done for the convenience of a single contractor.

[KenFarley]

Parts and assemblies have no data in them that associates them with a particular drawing. The drawing references the part(s)/assembly(ies), but not the other way around. Logical, since one could have a model that is referenced in a number of drawings, i.e. a part that has stages in its development (casting->pre-machined->final machined).

The method I use to develop a new design with an existing one as the start point is:

(1) Copy the files to another directory, using Windows Explorer. I don't use the "Save a Copy" in Creo because it saves *everything* - hardware, springs, whatever - as new files. This leaves all sorts of orphaned copies of "standard" parts all over the place.

(2) Start up Creo and navigate to the new directory.

(3) Load the assembly.

(4) For each part/subassembly I want to rename, bring up its drawing file, rename the part, rename the drawing. Save them as you go, though renaming is kind of a sneaky save operation.

(5) Once done be sure to save the assembly and any subassemblies you might not have saved yet.

It's kind of tedious, but sometimes that's part of the job. The key thing is to absolutely make sure I don't forget to save anything that I have in memory that might refer to a part/assembly I have renamed.

[CAD_Monkey]

Yes, that is what I do as well, and just because it is tedious I would like a better method.

PRT(&ASM) do not have references to DRW, but this does not stop Creo from offering to copy the DRW when you copy a PRT to a new name.

It only works if the PRT & DRW have the same file names, but this is my normal case - and what I ask for is that this existing functionality is extended to also work for subcomponents when saving and ASM to a new name.

There is another method that I sometimes use, and that is to Replace a component in an ASM using "By copy". This works like Save As minus a few steps.

[StephenW]

I *think* this is the same request as https://community.ptc.com/t5/Creo-Parametric-Ideas/save-assembly-parts-and-drawings/idi-p/467863

[CAD_Monkey]

Ah, yes, it is.

With the only difference that cmartin-3 thinks of the Save a Backup whereas I think of Save a Copy.

[CAD_Monkey]

Oh, hey - wait a minute!

I just did a Copy As of an assembly in Creo 8, and it did have the Include Drawings, and it did copy the newly minted subparts with drawings...?!?

So, is this something new for Creo 8, or has it been there for a long time, or am I only dreaming?

[KenFarley]

We don't name the drawing files the same as the part/assembly, because when you're looking at a directory of 100s of files, it is very difficult to find the part of interest if everything is named things like prt-0001-000010-01. Particularly if you're looking for something involved with a design that you didn't do.

And again, the assumption that a particular part or assembly is used in only one drawing is dangerous. Often we will use multiple parts/assemblies in a drawing to show different assembly states, indicate the proper configuration of a specialized locking washer, etc.

When addressing all the use cases of models and drawings, what seems simple becomes a real difficult problem. And, again, the part or assembly itself doesn't have any data stored in it to indicated what drawing(s) it is being used in. Creo would have to parse the drawings looking for references, etc. A very complicated bit of detective work - especially if drawings referencing a part might be in another directory.

[CAD_Monkey]

I generally name things NNNNNN_DESCRIPTION, then I use a Relation that strips the file name from character seven on, and populate the Parameter ARTICLE_NO with it.

Then my drawing head writes the article number in the corner automatically. So for this reason, using the same names for PRT/ASM and DRW is practical. But I don't often use multiple drawings on the same parts.

It seems that this query is moot anyway, because I found that Creo 8 does exactly what I wished for. I could have sworn that this was not the case in Creo 7.

[StephenW]

I don't have easy access to Creo 8 but this would be a really good enhancement. We have PDMLink and between copying files w/drawings, renames and save-a-copy with replace, those are the most useful things that save tons of hours.  In the past, there had been talk of moving to a different storage system based on other corporate needs/wants/desires so these kind of enhancements would make that more realistic.