Configuration Files

[Speedy]

Hi Folks!

I have been asked to set up drawing and part / assembly templates for the company. Pro-E is relatively new to the company so no in-hse depth of experience.

From what I can figure, I have to set up a configuration file which will load in my templates, formats etc from there.

My question; how do I set this configuration file to effectively default at start-up so that it doesn’t have to be re-loaded each time.

(Using Wildfire 2.0)

Thanks,
Speedy

 

[Guest0527211403]

Right click on the desktop Icon for Pro/Engineer, and select Properties.

Then, specify the "Start In" location as the location where you want the Working Directory to be set to every time Pro/E starts up.

In this folder should be a config.pro, with (at least) these settings pointing to the FULL directory location:

pro_dtl_setup_dir (DTLs are drawing setup file)
pro_format_dir
pro_font_dir
pro_group_dir
pro_symbol_dir

(under Tools-->Options, hit find and search for "pro_" for a ful listing)

also:
template_solidpart
template_sheetmetalpart
template_designasm

These allow you to manually specify a default part/assembly template.

 

[looslib]

You can aslo set up a company-wide config.pro by putting the file in your Pro/E loadpoint text directory; c:\ptc\wilfire2\text.


"Wildfires are dangerous, hard to control, and economically catastrophic."
"Fixed in the next release" should replace "Product First" as the PTC slogan.

Ben Loosli
CAD/CAM System Analyst
Ingersoll-Rand

 

[Guest0527211403]

Ben, do you know the correct location of a config.sup file?

The config.sup can be used to set option that cannot be overridden (overriding company presets is the bane of any CAD admin's existence), but I never really figured out where they go.

Generally, we use config.pro's in the startup working directory because we often use customer-specific settings. Creating a new icon on the desktop brings you right into the settings for that particular client.

I remember reading that if you have one in your login directory (e.g. c:\Documents and Settings\USER1\), Pro/E will load it as well.

 

[3dlogix]

Try our free Config.Pro Mentor on

http://www.3dlogix.com.

It is for Pro/E2001, but the basics are the same. It explains the config.pro settings, what they do and how to set up Pro/E to work with them.

Regards, Steve

http://www.sprdesign.com

http://www.3dlogix.com

 

[looslib]

I would put a config.sup in the <loapoint>/text directory. That is the first location Pro/E looks in for the config.* files.


"Wildfires are dangerous, hard to control, and economically catastrophic."
"Fixed in the next release" should replace "Product First" as the PTC slogan.

Ben Loosli
CAD/CAM System Analyst
Ingersoll-Rand

 

[Speedy]

Guys,

Thanks a lot. I got it to work. Slightly different to what you said.

Basically I saved a new configuration file 'config.pro' in to the folder directed from 'start in' in the start-up icon for PRO-E.
I did this through /Tools/Options/ within Pro-E.

i.e. there were no config files in this folder prior to this.

Speedy

 

[edleit]

Speedy,

You didn't mention if your solution worked for a single user or your entire workgroup. I'd suggest that you have the settings that you DON'T want altered at all in a config.sup file at the loadpoint directory on your server, then allow individual users to have their personalized settings defined locally.

This put you in control of the most important configuation options, especially the template files, yet allows individual customization (with the big plus of preventing the items within config.sup from being changed).

Ed Leitkowski