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Mfridman
Mfridman16-Pearl
16-Pearl
November 21, 2021
Question

How are you using the "create_drawing_dims_only" config.pro option?

  • November 21, 2021
  • 14 replies
  • 7511 views

Hello all,

I would like to gather feedback from this community about how of the long existing "create_drawing_dims_only" config.pro option is being used in your organizations.

 

First let me provide a short summary for the values of this option

If set to NO  - when creating a driven dimension in the drawing, the dimension is stored with the model (however not visible there). this dimension can be essentially leveraged to another drawing of the same model (but is not really going with the model based approach)

 

If set to YES - when creating a driven dimension in the drawing, the dimension is stored with the drawing only

 

My impression is that many Creo users (and their CAD Admins) have set this option to be set to YES, in order to avoid pushing drawing information to the model 

 

Currently the default value of this option is set to a value of NO. we (PTC) are considering to change the default value of this option to be YES (which seems to be more suitable for many Creo users who are already using this value in their organizations)

 

So here are my questions to this community, hopefully you can help:

1. Which value are you currently using for the "create_drawing_dims_only" config.pro option, in your organization and why you prefer this value over the other?

 

2. Do you have any concerns from us changing the default value of this option to be YES (please note that we are not removing this option, we are just considering to change its default value to match to what seems to be used by many.

Also a change of this option will not impact any existing dimensions in your drawings, it applies ONLY to newly created dimensions

 

I would appreciate any feedback on the above

 

Thanks and regards

Michael Fridman

Creo Product Manager

    14 replies

    Show previous replies
    M
    MichaelToledano14-Alexandrite
    14-Alexandrite
    December 6, 2022

    Hi Michael,

    We use this 'create_drawing_dims_only' config.pro option with the value of 'YES'.

    As each model is drawn in a single drawing (in the vast majority of cases), we do not have the need to utilize driven dimensions elsewhere outside the scope of that single drawing.

     

    Best Regards, 

    Michael

    Mfridman
    Mfridman16-PearlAuthor
    16-Pearl
    December 6, 2022

    Thanks a lot for your feedback Michael

    L
    LawrenceS18-Opal
    18-Opal
    May 26, 2026

    We recently switched from Creo7 to Creo11 and immediately noticed that we were no longer able to place additional ordinate dims on existing baselines due to the change talked about in this forum: create_drawing_dims_only YES.  Creo11 wants us to delete the ordinate baseline in order to add additional dims. Switching to NO allows us to reuse existing baselines.  

     

    At some point I realized that we actually did try in our company config.pro years ago (I think wf4/Creo2) but then commented it out.  We Use GD&T a lot and many find it easier to add this to the model while in drawing mode because all the dims are already displayed.  It is a pretty big pain to ask people to recreate all their dims (ordinate) in order to swtich this to yes. This is an immediate turn off for us but if there was a method to convert existing dims then we could reconsider it.

    S
    Srinivasan-Iyer14-Alexandrite
    14-Alexandrite
    May 27, 2026

    kept it yes as we had the issue of dimensions disappearing after a check in. not every time but some time. We have changed it recently to study the effect it would have on the model. However, we have temporarily excluded it from config.sup.

    Good to see that PTC is moving away from the current default. Our aim is to go for full MBD.

    L
    LawrenceS18-Opal
    18-Opal
    May 27, 2026

    Interesting. I am curious what else affects whether dims disappear after check-in as that is not anything I have ever seen at our company and we have had it set to the default of NO at least since 2014.  Not only have I not experienced this, but I don’t recall any of our ~200 Creo users mentioning it either.

    S
    Srinivasan-Iyer14-Alexandrite
    14-Alexandrite
    May 28, 2026

    It doesn’t happen all the time. We had a few designers report it occasionally with all of them following the identical config file. Then we came across a PTC Article - CS17143 and Article - CS41916. We also came to know that the setting create_drawing_dims_only to yes is the Default Creo 11.0.

    We emphasise on having the Model Driving dimensions as the Drawing Dimension to have a bi-directional associativity to the extent possible. Any Setting that helps in achieving Classification Code 5 (Full MBD) as detailed in ISO 16792: 2021 - Digital Product Definition is welcome as we see that as the way forward.

    Regards

    D
    dgarcia12-Amethyst
    12-Amethyst
    May 28, 2026

    We have always used YES.

    Intuitively, if you create a dimension in the drawing then it is stored in the drawing.

    As a bonus, when something fails in the 3D model shown dimensions can dissapear, created dimension turn to red. Then you know somehting has happened.

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