How to keep the detail options in creo parametric/pro e

[GTLuser]

Hello everyone!
I've been trying to set up my creo parametric account for awhile, but I'm having trouble saving some of my settings. I have been going to FILE>PREPARE>DRAWING PROPERTIES>DETAIL OPTIONS, then changing my settings from the default. I then save these settings in the working directory. However, when I restart creo at a later time, these settings do not continue. I have to go back into "detail options" and manually find the saved file and then bring up that file. Is there a way that these options will automatically come up from the start?
Thanks!

 

[dgallup]

Have you set the config option drawing_setup_file?

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The Help for this program was created in Windows Help format, which depends on a feature that isn't included in this version of Windows.

 

[GTLuser]

Where do I do this?

 

[jvian]

How are you starting your Creo session? Are you starting Creo then opening an existing drawing? or creating a new drawing? or something different? It might be a template or format causing your problem.

- J -

 

[dgallup]

Config options go in config files. Thee are multiple locations but they are the same as previous Pro/E releases.

As Jvian said, it makes a difference what you are doing. Every drawing's settings are saved internally. So when you reopen a drawing is should be just the way you last saved it. If you are creating a drawing from a template then the initial settings will come from the template. If you are creating a new drawing either empty or with a format then the drawing_setup_file will be read.

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The Help for this program was created in Windows Help format, which depends on a feature that isn't included in this version of Windows.

 

[GTLuser]

I open the program before I open any existing documents. Then I'll either open a document or start a new one. Is this causing my problem?

In the configuration options there are either lightning bolts and red prohibitory signs beside the options. How can I change these?

 

[GTLuser]

What does the drawing_setup_file do? Or what should I set it to?

 

[looslib]

The drawing_setup_file config option tells Creo where to find the drawing setup file on your computer. It points to the detail.dtl file you created.

In your config.pro file, which is in your home or start-in folder, put this:
(assuming that the detail.dtl file is in my sample folder)

drawing_detail_file c:\ptc_users\common\detail.dtl

That should load the detail.dtl file everytime you start Creo.



"Wildfires are dangerous, hard to control, and economically catastrophic."

Ben Loosli

 

[jvian]

The drawing_setup_file will only tell your system where to look when creating a new format and template. Drawings contain their own detail setup file as part of the format they use within the template. If when you create a new drawing you select either 'use default template' or 'empty with format' then whatever format is used in either option will contain the .dtl file saved within the format/template. My recommendation is to find the format which is used by your default template and set your detail options there and save and close. This was awkward for us at first but works flawlessly now as we rarely change our drawing options anymore except for specific drawings which is easy to manage. Again globally though I think your settings are stored in a format file within a template your drawings use. I should note this will affect all drawings which use that format including all past drawings. We were able to make global setting changes (minor anyway) this way which propagated back through all drawings which use the format and all new drawings have the same settings. Finding the format is easy to do as well if you don't already know where it is.

If you are not using the 'use default template' or 'empty with format' when creating new drawings then ignore this and sorry for rambling.

Hope that helps,

- J -

 

[GTLuser]

Thank you guys so much! I had spent so much time on this and it finally works!