Config.pro won't update

I’m using the “commercial” version, the shortcut to start Creo has a “Start In:” path. I always put my settings files there, that way they are loaded every time when starting Creo.

Hi,

Instead of editing the config.pro file inside the Creo installation folder, create a new config.pro file in your Windows user folder.

For example, create the file in C:\Users\your_username\config.pro.

Inside this file, add the following option:

tol_display yes

Save the file and completely restart Creo Parametric.

As others have stated, in the shortcut you use to start Creo, there is an entry for “Start In” which designates the initial working directory. That is where Creo expects to find a config.pro file, if it is expected to use one. The default Start In is, I believe, something like your Users\username\Documents directory, or something like that.

I think most people have a specific directory they will use for Creo (mine is C:\ptc) as the Start In. That way you can put your config.pro in there, as well as the other many configuration and other files you might be using. You can have directories for start parts/assemblies, materials, etc.

I’m sorry, the tol_display setting needs to be in a different file, one that specifies your desired defaults for drawings. It’s called drwsetup.dtl. The way this stuff is setup for me is:

config.pro has line

drawing_setup_file              c:\ptc\DefaultFiles\drwsetup.dtl

drwsetup.dtl has line

tol_display yes

I really appreciate the advice Ken, so thanks for weighing in again. Unfortunately I still haven’t gotten it working as the tolerances are still greyed out.

I created a second file “drwsetup.dtl” in my startup folder and threw in “tol_display yes”. In addition to that, I added “drawing_setup_file c:\temp\drwsetup.dtl” into the config.pro files in the startup folder (called “temp”) and again into the original location (C:\Program Files\PTC\Creo 13.4.0.0\Common Files\text). 

If you look at the loaded config.pro do you see this.

and 
if you look at the drawing setup of the active drawing do you see this

The DTL file is copied into the drawing on creation and is not updated after that. 

Hi ​@A_Gaillard, 

I think you’re missing one last step from all the previous assistance.

the config.pro tol_display is for 3d models.

the detail option tol_display is for 2d drawings.

If you set tol_display in the .dtl file defined by config.pro drawing_setup_file, this will apply to new, empty drawings.

Changing .dtl options will not retroactively apply to existing drawings as the .dtl options are applied at drawing creation.  You can manually update existing drawings or reapply .dtl files through File > Prepare > Drawing Properties > Detail Options change > open a configuration file.  If you have multiple drawings that need to be updated, you could set up a mapkey to help automate the repeated task.

If you use a template drawing for new drawings, the new drawing inherits the detail options from the template, not from drawing_setup_file.  This means to change the option for new drawings which use that template, you should open the template drawing and update the tol_display option then save the template.  New drawings from this template will use the updated value.

I hope this helps but let us know if there are any further requirements

Mike

Hi,

One other thought.

Its possible that the student license doesn't have pro_detail in it, which may allow for tol’s

can you start Creo and click File > Help > System information > System information.

That shoud list all the modules avalible

Here is a good reference. for tols

https://www.ptc.com/en/support/article/CS20305

for license issues

https://www.ptc.com/en/support/article/CS70897