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Modeling Strategies

To Copy Drawing Files With Object Rename in Pro/e 2001 by Heckler
Posted: 4 Jun 05

The question to to Copy Drawing Files With Object Rename has surfaced about once a month so I decided to put together this FAQ.  This a definite procedure for Pro/E 2001 and I believe it will work for WF2.  I would like to thank Steve (aka 3dlogix) at http://www.3dlogix.com for his detailed illustration this week on a thread, which prompted me to put this together.

Using the configuration file option rename_drawings_with_object, you can copy a drawing and a part simultaneously with its associated part or assembly file (using File > Save As) and then rename the drawing. The drawing adopts the same new name as the name of the copied part or assembly file.

1. Click Utilities > Options. The Options dialog box opens.

2. Type the configuration option rename_drawings_with_object in the Option box.

3. Select a value for the option from the Value drop-down list. When you specify the value as both, part, or assembly, and then choose Save a Copy from the Pro/ENGINEER File menu for a part, the system also renames the drawing file associated with the renamed part, as long as it has the same name as the part. To disable this option, set this configuration option to none (the default setting). The following diagram illustrates the renaming process when you use Save As to save a part or assembly file that has an associated drawing.

Drawings of parts and assemblies must have the same name for this to work. Example:, you have the following parts, assemblies and drawings.

FLANGE.asm     ------> FLANGE.drw
PIPE.prt       ------> PIPE.drw
PIPE_1.prt     ------> PIPE_1.drw
GASKET.prt     ------> GASKET.drw
VALVE_BODY.prt ------> VALVE_BODY.drw

You want to make a new assembly and rename them as follows. Select FILE > SAVE AS and enter the new part and assembly names as needed.

(new names)      (drw's automatically saved under new names)
FLANGE_NEW.asm      ------> FLANGE_NEW.drw
PIPE_NEW.prt        ------> PIPE_NEW.drw
PIPE_1_NEW.prt      ------> PIPE_1_NEW.drw
GASKET_NEW.prt      ------> GASKET_NEW.drw

For this to be successful, the files should be in one folder. Make a new folder and copy all the parts, assemblies and draiwng over. Do the SAVE AS and renaming here, that way, if you mess up, it doesn't affect the "good" copies. The drawings do not need to be open or in session for this to work.

If your drawings don't have the same names as the parts or assemblies, then this exercise will not work for the drawings.


The following website is a great resource for config file options for both Pro/e 2001 and Wildfire.  Please use caution when trying out new config options - always have a backup of your production config files.


Back to PTC: Creo Parametric (Pro/ENGINEER) FAQ Index
Back to PTC: Creo Parametric (Pro/ENGINEER) Forum

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