How to make copy of PART & DRAWING

[agaribay]

I am trying to create a copy of an existing drawing giving it a new number.

I have set the option:  rename drawings with object  =  both

Both the Model and the Drawing have the same part number and are open / in session.

I "SAVE AS" - (Save as Copy), and enter the NEW PART NUMBER.

I end up with a New Drawing, but no new part.  The part in the drawing still shows the Old Part Number.

Any ideas as to what I am doing wrong?

CREO 2.0

Thanks.

-Art

[MaheshSh]

Art,

All steps seems good.

Try to create a part as a.prt and drawing of A.prt as A.drw.

Save in same location and close part and drawing.

Open part A and Save as to B

Check for B.drw.

There are only three conditions for this:

1. Name of part and drawings should be same.

2. Saved in same location.

3. Config options should be set.

[Chris3]

Are you doing save as on the part or the drawing? You need to do the save as on the part.

[Dale_Rosema]

Do you have Windchill? If so, I am not sure.

If you do not have windchill, I save a copy of both the part and the drawing in the file folder where they are located with a naming convention of:

zzzzold_file_name.prt

zzzzold_file_name.drw

I then open both the part and the drawing (the name without the zzzzz prefix) and do a rename of both the drawing and the part. Rename old_file_name.prt/drw to new_file_name.prt/drw. After saving both, I then go back into the folder and rename the zzzz files and remove the zzzzz.

Then the old part still opens and it should and the new part with it's drawing opens as it should.

Thanks, Dale

[Chris3]

If you have Windchill then another technique is to just open both in session and do a rename on both and save. That's it. Renaming both items through the Creo interface in a Windchill environment is the same as a save as.

Make sure to have any next higher assemblies you want updated in session or make sure to erase everything if you don't want next higher assemblies updated.

[Clipper_captain · Accepted solution]

Open the drawing and the part in Creo; make sure the part window is active. At this point, do file / save as / save a copy. In the message portion of your Creo window, you should see the rename of the part and drawing being complete. In case you miss it, you can check the message log and find it there.

Have a good one.

[agaribay]

Thanks guys.  I ended up making a copy of the Drawing and Part in another directory.  I then opened both and renamed in session.  done.

I will have to try SAVEAS with the Part Window Active as I had the Drawing Active.

We do not use Windchill.  We're using Agile Engineering Collaboration.

[MaheshSh]

Art,

As you manage to get it working, you may mark the appropriate answer as correct in the post.

[yyang-4]

that is to say the prt and drawing must be in the same folder, and our company seperate the prt folder and drawing folder ,i think it is not correct .do you think ?

[MartinHanak]

Art,

the description of rename_drawings_with_object option tells us ... options controls whether the system copies associated drawings automatically with parts and assemblies. This means you have to copy the part, not the drawing !!!

MH