Model w/ Drawings as Template

[ptc-4482052]

Hello PTC Community,

I am currently trying to set up a completed project as a template project that includes all assemblies, sub-assemblies, parts and associated drawings. What I need to accomplish is to be able to make a copy of an existing finished project (including drawings) to a seperate unlinked file, then modify that copy as a seperate (stand alone -no links back to original) project.

I am able to 'Save As' a copy by using the main pull-down, which allows me to assign a new project number to each related item name by checking the 'Use a Template' box and assigning the new number. (Copies seem to be unlinkes as required) The issue is that even with the 'Copy Associated Items' , Copy Drawings box checked, the file only copies the assembly and parts. (No copied Drawings). This causes me to have to repeatedly create new drawings from scratch instead of having the copied file modify a full set of drawings as the model is changed.

My questions are as follows:

Is there something I can do to copy over the entire file, including drawings so that they would be related (linked) only to the renamed (copied) assembly?

Do I need to save my original project as a template first?

Why are the drawing files not being copied even with the 'Copy Drawings' box checked?

Also, is there a way to re-assign what model a specific view on a drawing is looking at?

Thanks,

Ted Fulton

This thread is inactive and closed by the PTC Community Management Team. If you would like to provide a reply and re-open this thread, please notify the moderator and reference the thread. You may also use "Start a topic" button to ask a new question. Please be sure to include what version of the PTC product you are using so another community member knowledgeable about your version may be able to assist.

[TomD.inPDX]

It is not quite as easy as you like but it is doable.

This is a long time challenge that any seasoned PTC parametric user has run across at one time or another.

The biggest problem is that drawings are orphans when not in memory, and even if they are, they are in a sense a higher level file that branch out from the part, not the master assembly. Its logical, yet silly.

But no worries, SaveAs/Backup is your friend.

Open all your files... change your working directory... and SaveAs\Save a Backup your top-level assembly. Now activate each drawing and do the same.

Close all files and erase not displayed.

Reopen you top-level assembly in this backup folder (make sure you are in the right folder).

Reopen all the drawings.

Now go through the process of Renaming (file/manage file/rename) all the applicable files (drawings, assemblies, and parts). You have to consciously save each affected level so the new model is used in their next level assembly and drawings. There is logic behind this but you have to remain aware or you will miss something. I'm sure you know, but just for completeness, when you rename a part (on disk and in session), any open file that uses that renamed file (in session) will also change its reference to the new filename. But you have to save that using file to keep that new "relation". <= there's got to be a better way to say this

I am confident that there are other methods but this has been my failsafe way to accomplish what you are asking.

[BrianMartin]

Hi Ted...

What version of Pro/ENGINEER or Creo are you working in?

If you're working in Wildfire 5 (Creo Elements/Pro 5) or less, try setting the config.pro option rename_drawings_with_object to both. This should do what you want. When you save that top level assembly with drawings, all subassemblies, parts, and drawings thereof should rename and become completely independent of the originals.

If you're in Creo 1 or 2, go to File->Options->Configuration Editor and add the same option (rename_drawings_with_object and set it to both). This should solve your problem.

Let me know if that works for you!

Thanks!

-Brian

PS: Antonius' method will work... but if you can avoid it you don't want to have to go through that kind of emotional torture.

[ptc-4482052]

Hi Brian,

I am currently using CREO Parameteric 1.0 and have changed the configuration as you suggested. Unfortunatly, the only difference is that the 'copy drawings' box is automatically checked when I use 'Save As' "Save a Copy'. The drawing files are still not copied.

[BrianMartin]

Ah excellent, Ted! Glad I could be of assistance.

No need to thank me, really.

Heheh just kidding... hmm. Let me take a closer look and get back to you.

[BrianMartin · Accepted solution]

Hi again Ted...

I've opened up a mid-sized project of about 200 parts, subassemblies, and drawings. From the top level I issued the Save A Copy ("Save As") command. I selected the button to include drawings. I gave new names for all parts and assemblies except for common hardware and off-the-shelf parts. I executed the command and got copies of all parts, subassemblies, and drawings as expected.

I've tried this in both Creo Elements/Pro 5 and Creo 1.0 with identical results. Therefore, I am unable to recreate the problem you're seeing. This leads me to a few questions:

1. Are all drawings for your assembly located in the same directory as your models?
2. Are all drawings for your parts and assemblies named exactly the same as your models?
3. Are you performing the Save A Copy command from the very top level assembly model?

If I had to take a shot completely in the dark, I would havwe to guess that your models and drawings are somehow not exactly the same. For example, some companies append the drawing size to their filenames. So a model called 123456.prt would have a drawing called D123456.drw (the "D" being for "D-Sized Drawing"). This will prevent Creo from copying your drawings. The copy function only works when your drawing is precisely named the same as your models.

Of course this may not be the problem. I'm merely taking a blind guess based on the most likely scenario.It could always be something else. Perhaps your build code of Creo 1.0 is has a legitimate bug preventing the drawings from copying.

If it's not a naming issue, the only other thing I could think of would be if the drawings were not in the same directory. This shouldn't present a problem if the drawings are within Creo's search paths... but perhaps that's the issue?

Write back and I'll try to help troubleshoot further.

Thanks!

-Brian

[ptc-4482052]

Thank you Sir! What a time saver!

I didn't notice that I had used an underscore between my project type designation letter on my model while I had used a dash on the drawing. Re-named the drawing file to be the same and everything copies without issues.

[BrianMartin]

Great news Ted! I'm happy to have been able to help.

(Okay so that's the official response. But just between us, whenever I blindly pull the correct diagnosis out of thin air like that I celebrate a little in my cubicle. My co-workers think I'm a nut.)

[TomD.inPDX]

Looks like you have yet another tutorial subject, Brian.

I've never liked the Save-As dialog. Good to hear PTC has at least thought about this longstanding shortcoming.