How can I keep the 'Drawing_units' in drawing options?

[sbang]

Plz let me know.

I'd like to keep the drawing_units from inch to mm.

[TomD.inPDX]

Drawing template files

[sbang]

Your mean is save in drawing template files?

I use CREO2.0,

I can't find it. How can I save my modified drawing options?

[ChristianBADEL]

Hello,

If you use template you should know were they are as Creo don't offer such templates in a fresh install.
In CONFIG.PRO there must be a line giving the path were find templates as this:
  START_MODEL_DIR  C:\creo\start_geom
That means that if there are templates to use they are located at C:\creo\start_geom.

If not then you use formats.
In this case take in account only the PRODETAIL.DTL file.

Keep in mind that if nothing is specified in you CONFIG.PRO then Creo will use inches and pounds
But be careful : be sure your drawing and its model share the same unit !

If not, changing the drawing unit will only affect the scale and the 2D detail you may add to your drawing.

[ChristianBADEL · Accepted solution]

Hello,
There are, depending of what you want, different ways to manage units in a drawing.

A- For new drawings:
1) If you don’t use templates:
  You should complete two files:
  In CONFIG.PRO:
  Set DRAWING_SETUP_FILE to the location of PRODETAIL.DTL
        (eg: drawing_setup_file c:\proeconfig\prodetail.dtl)
  Then complete PRODETAIL.DTL with:
  DRAWING_UNITS   mm

2) If you use Templates:
  Edit each Template, go to FILE/PREPARE/DRAWING PROPERTIES, click CHANGE on line "Detail options" and set the line DRAWING UNITS to: "DRAWING_UNITS mm" then save your Template.

B- For existing drawings:
  Do the same as for Template files, for each ones.

(Creo reads PRODETAIL.DTL once when creating a drawing, then copy all options in the drawing. Hence none of PRODETAIL modification will affect already created drawings)

[sbang]

Thank you for your clear answer.

It has been a great help.