Community Tip - Have a PTC product question you need answered fast? Chances are someone has asked it before. Learn about the community search. X
Hello all,
How can I add a zero before the decimal when dimensioning a part in a drawing? For example, I am getting ".57" for a dimension. How can I make it appear as "0.57"? Is there a setting I need to get to to change this? Also, is there a way to make this a permanent feature, so I wouldn't have to keep changing it for every dimension on every drawing I make?
I am new to Creo, so forgive me if this is a silly question. However, I've been looking all over and can't find an answer. Please help. It is very much appreciated.
Thanks for your help,
Halle
Solved! Go to Solution.
Hi,
You can alter this setting with "lead_trail_zeros" drawing option. When setting it to "both" all default dims should show with both leading and trailing zeros.
This one, and plenty of other drawing file options are stored in *.dtl file. To have a *.dtl file loaded into every new drawing you have to set a config.pro option called "drawing_setup_file" with path to this file.
There is also some sort of iso *.dtl file already predefined in the Creo installdir.
Hope that helps.
Hi,
You can alter this setting with "lead_trail_zeros" drawing option. When setting it to "both" all default dims should show with both leading and trailing zeros.
This one, and plenty of other drawing file options are stored in *.dtl file. To have a *.dtl file loaded into every new drawing you have to set a config.pro option called "drawing_setup_file" with path to this file.
There is also some sort of iso *.dtl file already predefined in the Creo installdir.
Hope that helps.
CORRECT ANSWER!
I went into the iso.dtl file, and it read "YESlead_trail_zeros". Should I switch the "yes" to "both"?
Thanks for your help!
Be careful with that, if it's per ASME, inch dimensions do NOT get a zero left of the decimal, but METRIC does. Also, 3-place inch dim should be shown as: ".050" whereas metric truncates a 3-place to not have a zero at the end, as in: "0.05".
You can change settings in Pro/E, but if it's supposed to be per ASME spec, make sure you have the settings correct.
Thanks, I did not know that. All the companies I've worked for have used a leading zero. Is this a new standard?
Sometime companies have their own standards that started with a prescribe standard like ASME or ANSI, but have modified it to their own likings and preferences. ASME and ANSI have been around for a long time.
I use creo elements/pro 5.0 and in my drawings the dimensions linked to the model would not change to having a leading zero unless I changed lead_trail_zero_scope to all.
I wonder if that was some kind of bug or other anomaly.
Creo 2.0 option... this one is from the model properties. The options are identical in the drawing setup.
As of Creo 1.0 it's possible to set all the drawing options (*.dtl) directly from config.pro.
Also, all of the system color options (*.scl) can be set from config.pro as well, while if the same config option, for instance system_curves_color, is set in both places, the config.pro always wins.
In the drawing detail option file I've got the lead_trail_zero_scope set to dims, and the zeros show correctly.