Dimension tolerances can't be shown in a new drawing Creo 10. But visible in part dimension.

[Nico_Naas]

Working with Creo 10 Rev: 10020:
I created a new drawing and with "show annotations" I can show dimensions of my part features in all the views.
But when I click on a shown dimension the tolerances tab is grey and I'm not able to show tolerances of the activated dimension in the drawing. I can add/see/edit this tolerance of dimensions in the part itself.
Even More strange is, that in old drawings this works without a flaw!

Can you tell me what I do wrong?

[StephenW · Accepted solution]

In the part, can you see the tolerance on the dimension. If not, search your config.pro options for TOL_display and set it to yes. This is an overall option that controls all model and drawing tolerances.

If it is already set to yes, then go to the drawing

In the drawing setup file under File - Prepare - drawing properties - detail options change look for the option TOL_Display. It should be set to yes.

If it is a new drawing, most likely either your drawing template or your drawing setup file has the option tol_display set to no for all new drawings. If you are in a company that has someone who controls those file, contact them to have them change the option in the template or drawing setup file. If it just you, you will need to find your drawing setup file and change it or adjust your drawing template options.

[KenFarley]

I don't know what your setup is, but there are settings that can be set up that will be applied to any new drawings. I have a file called drwsetup.dtl which consists of a long list of settings that I want as default for any drawing I'm creating. The setting that allows one to change the tolerances, and seems to default to NO in Creo is:

tol_display YES

This is probably set to YES in the old drawings you are opening, which is why they are behaving the way you want.

In order to have my preferred drawing setup be the default, I have to tell Creo to read the file when I start it up. That is done by putting a line in my config.pro file, telling Creo where to find the drwsetup.dtl file. Here's the line from my config.pro:

drawing_setup_file c:\ptc\DefaultFiles\drwsetup.dtl

If you have old drawings that have behave the way you like, it would probably be easiest to open one of those drawings, navigate to the settings via:

File -> Prepare -> Drawing Properties

then next to Detail Options, click on the "change" link.

Save the list of options and their settings to a file with the save button, and you can use that as your initial go at the settings.