drawing decimal places for metric dimensions?

Hi to all,

Noticed something weird with showing metric dimensions in drawings,
and was wondering if there is a fix for it, or some config setting.

If I want to show a dimension of 21.00mm, Pro/E seems to want to
shorten this to 21mm, chopping off the two decimal places. This seems
to only happen with metric dimensions, and only if the numbers after
the decimal point are zeroes. This happens no matter how many decimal
places I set within the Properties box.

Obviously, if the numbers are anything other than zero, they are
displayed correctly. But when they are zero, they are removed by Pro/
E.

Is there a way to display these zeroes in metric? The same problem
doesn't occur with English units.

Any info or advice is appreciated.

Thanks.

Lee

 

It may be a .DTL file option. Take a look at "lead_trail_zeros" and
"lead_trail_zeros_scope"

Andy

 

Andy, thanks for the quick reply. Your answer was right on, I had to
adjust the "lead_trail_zeros" option from its default setting to
"both" in the .DTL file.

Thanks a lot.

Lee

 

Before you go and change the behavior of the system, look at the standards
that your company uses to define how a drawing is to be interpreted. ASME
Y14.5m-1995 says that metric dimensions do NOT use trail zeros after the
decimal place.
Just because you want it to look one way, doesn't make it correct.

Ben


Agreed! Those dimensioning with US Customary Units got away with a quick and dirty shotcut to tolerancing with the default tolerance based on number of decimal places. Therefore, a half inch, to tolerance .0003 had to be displayed as .5000, a comparable number of trailing zeros (and the plus/minus sign), making the dimesion display incredibly long. Thus the reluctance to use anything but the default tolerances. ISO makes the dimension and tolerance display as simple as possible AND encourages whole number MM dims making it much less odious to EXPLICITLY tolerance every dimension: no decimal place shortcut to tolerancing with ISO. AND no confusion over tolerances when a decimal place is inadvertently dropped because zeros are truncated automatically.

David Janes

 

It is also NOT a CAD company's job to make it difficult to do dimensioning however you want. PROE makes this mistake over and over. If one expects prints to work side by side with legacy prints, then some one who isn't a CAD salesman or a stubborn user who worked somewhere else needs to make the decision to change to updated standards.