I have been given the job of setting up Wildfire 4 for the office after very limited training.
My first task is to set dimensioning styles and text styles. Where do I find the settings for these styles? My experience is mostly Inventor, Solidworks & AutoCAD where I can just go to dim styles and text styles and work through the options, WF4 doesn't seem to have this in any of the menu's.
I have been told that I need to edit a text file, I have found three copies of this file installed on my computer so I'm not sure which one it is and I can't work out where the text style for dimensions is in the text file. I checked the file location in the config.pro file and that doesn't seem to relate to any location I can find.
Having done proe admin for many years, I should be able to help. Two things you'll note in dealing with Proe admin:
I assume that you are talking about drawings? If so, that's controlled by the *.DTL text file. I'd store it in a server location accessible to all and set the config.pro option 'drawing_setup_file' to point to it (use the full path). I'd also put your company config.pro file on the server and have it copied to your installationn 'text' folder when Pro/E is launched by a simple batch file.
The easiest way to create a *.dtl file is to create a new drawing and then right click in an empty area and select 'properties'. In the menu that pops up in the upper right, select 'drawing Options'. This will get you to all the possible drawing settings. Set as you please and save to a *.dtl file in your server location.
Also note that DTL settings are only applied automatically when a drawing is created. If you change the remote file, you have to manually reload it. This is to prevent a DTL change from making a change to your entire database of drawings without you realizing it.
There are a lot more things to learn, but that should answer this immediate question.
Doug hit the nail on the head. Make a common .dtl file for the company and have every config.pro file point to it.
People will still be able to change the default, but it is a great starting point. If you have multiple standards to manage, like metric/ISO and SAE/ASME, make two versions and default to one in config.pro. Show people how to read the "alternate" when they need it.
There is nothing worse then everyone changing a handful of options on every drawing you touch. Nothing remains consistent for sustainability without putting in the required effort to make a stable detail config file.
And yes, oddly enough there is only a "built-in" version of the file which is not a file at all. It is also best to move custom files out of the WF install folder as software updates will wipe out the modified files.