Scale missmatch when exporting from *.DRW to *.DWG.

Greetings:
I export a simple line 250mm height (SCALE 1:1) from Pro/E (WF2 build M040) to *.DWG. When I open it in AutoCAD the dimension seem to be in
inches (9.8425") even though my AutoCAD drawing units is set to mm and the *.dtl file is set to Std_Ansi and mm. Am I missing something?
Thank you for your time and help.
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drawing_units mm?
Drw File / Page Setup: Millimeters checked?
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Thank you, Jeff, for your help.
I check the page setup. It's in inches. I click on C cell under format column, change to mm. However, when I go back to double check, it's in inches again. Am I missing something?
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: Thank you, Jeff, for your help. : : I check the page setup. It's in inches. I click on C cell under : format column, change to mm. However, when I go back to double check, : it's in inches again. Am I missing something?
"...it's in inches again"? The drawing dimensions? The export/import to AutoCAD? Anyway, this discussion is a little confusing. I know when people get stuck, they try a bunch of things. And, in this case, there are several things which seem to apply to 'units': the units setting in 'Edit>Setup>Units'; a .dtl option called 'drawing_units'; and the radio button selection of inch/metric when setting up a drawing or format. Only the setup of units in the part is absolute ~ it applies everywhere: drawings, formats, exports.
The 'drawing_units' option in the .dtl file is a little confusing. It is one of those misnamed, misleading Pro/e options, leading me (at one time, anyway) to believe that you could specify dimensioning units with it. Not so, as it nicely lets users 'speak' in any system of units to the .dtl file. It tells the drawing setup file how it should interpret measurements, such as, of arrows, leaders, dimension text height, section note height, etc. So, dimension text with a value of "3" will be interpreted as 3mm if drawing units are set to milimeters. If, however, drawing_units is set to inches, you better have a value like .125 or .156 for that same text.
On the last point, of the significance of setting millimeters or inches for the drawing, I'm pretty sure that all this does it tell you, in one system or another, what the size of the sheet is. You can pick a US Customary size like A or B but get it tranlated into mms. Likewise, pick A4 and click the Inches radio button and get this standard ISO sheet size translated into inches. This should not have any effect on drawing dimensions (though it would be nice if were some kind of automatic units conversion) or of the units that get transmitted through an export.
This leads me to believe that the problem is in your AutoCAD setup, perhaps some built in scaling factor. Check your .drw scale factor (sorry, can't telll you where to find it.)
David Janes
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David:
Thank you for your detail explanation and most importantly Drawing_units meaning. I use to believe that this control the drawing export units and set the drawing_units to metric mm while my model is in inches.
"...it's in inches again"? The drawing dimensions? The export/import to AutoCAD?"
I apologize for being so vague and so confused. What I mean was the Page setup properties units. I chose the C size and click on the mm "radio button"; however, when I go back to page setup click on the C size again, the inch radio button is selected instead of mm. For some reason, page size setup to mm doesn't stay in effect.
After reading all comments and suggestion from you and Jeff, I restart from a clean *.dtl, try Jeff's suggestion. Everything is working now as per your advice and as I expected.
In recap:
- model units is absolute and the one I should focus on. - drawing_units is for *.dtl variable (arrow size, text size, leader length, etc) and convert sheet size from inch to mm & vice versa. - pase setup doesn't do anything.
Thank you all for your valuable help
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Oops, sorry. David's probably right about the page setup (it's unimportant).
I do inch stuff so am not familiar with all this, but Drawing Option drawing_units appears to be the guy you are after. A short trial and error to see what happens:
Create a model of a 25.4 mm cube.
Create a drawing of it using the standard A size template.
Save a copy as dwg. This will open as an inch Acad dwg. Units = inch, Distance on a side = 1.
Set Drawing Option drawing_units mm.
Save a copy as dwg. This will open as a millimeter Acad dwg. Units = mm, Distance on a side = 25.4.
How to clean up the annotation mess made by changing drawing_units? Don't know. Maybe open a mm drw template, write out the .dtl and read that in?
Scaling the Acad dwg (* 25.4) will leave you with a similar annotation mess to clean up.
I don't think there is any setting in Acad that will affect all this as the drw is written out to Acad model space (a "unitless" environment).
Sorry, don't know any more and don't have time to experiment with it right now.
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