Lost Dimensions on Part Change

[JONGPC]

I am loosing dimensions in dwt files I create from customer part files when customer sends new version of files.


1. Customer sends files, I create dimensioneddwt files for shop and inspection, all is well...


2.Customer sends same (name)files with minor changes, I place new files in a new folder, copy existing dwt files from old folder to new folder, open up dwt files and all the dimensions I created aregone butthe views I createdare there.

Seems to me that this method had worked in the past but now is not working.


I know the customer rolled the revision from A to B this last time and that the files are backed up from Interlink and sent to me.


ANY IDEAS ARE APPRECIATED !!!

 

[donha]

The dimension information is actually stored with the part. If you created the dimensions on an older part, those created dimensions are stored with that part. When you overwrite the part with a newer part, Pro/E does not know those dimensions exist. There is a setting to store created dimensions in the drawing only. In config.pro: "create_drawing_dims_only yes". This is not a very good option because it saves the dimensions as associative draft dimensions. Perhaps someone has a better solution to your problem. I am in 2001, so I cannot speak for Wildfire.

 

[dr_gallup]

For what JONGPC is doing, "create_drawing_dims_only yes" is the right way to go because his dims get saved in his drawing, not in the part file. When the part gets revised by the customer, JONGPC's dimensions will still show up in his drawing. If the dimension references in the part are no longer valid, Pro/E will change their color and give a warning message.

 

[JONGPC]

Thanks to both of you for your help!


The "create_drawing_dims_only yes" setting is what I need to change


to fix the problem!


Must have changed it a while back and forgot.....