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cadbart1-Visitor
1-Visitor
November 2, 2020
Solved

Why copy of drawing influence on origin?

  • November 2, 2020
  • 2 replies
  • 3019 views

Hi,

I'm working with Creo Parametric 6.0 and I'm making drawing of simple part. When I've done this drawing I've created a copy of this origin drawing (File->Save As->Save a Copy). Then I made some changes inside the copy (mainly deleting some dimenssions) and i I saved it. When I opened the origin drawing I realized that dimenssions which I remove in copy have been also removed in origin drawing. 

It looks like the changes made in copy influence on origin file. Is there some way to turn off this influence?

Thank you in advance for all answers!

Best answer by StephenW

There is a config.pro option you need to add to keep created dimension in the drawing only.

create_drawing_dims_only YES

 

This will keep your created dimension from actually belonging to the model even though you created them in the drawing (sounds strange but it's the way it works).

 

Be careful and do testing with this option before putting it in to widespread use. It will potentially cause issues with your GD&T with respect to created dimensions and model GD&T. PTC may have fixed this, but it used to be difficult to get everything to works together like you expect.

2 replies

B
23-Emerald III
BenLoosli23-Emerald III
23-Emerald III
November 2, 2020

Are both drawings using the same model?

Sounds like you are using model dimensions shown on your drawing.

If that is the case, a deleted dimension in one drawing will remove it from the model and also the other drawing.

C
cadbart1-VisitorAuthor
1-Visitor
November 2, 2020

Yes, both drawings use the same model (just the other drawing has been created as a copy of this first). Actually 99% of dimenssions was created via Annotate->Dimenssion feature. One of stuff that was added by Annotate->Show Model Annotations is geometric tolerance symbol however it wasn't deleted in origin drawing (although it was manually removed in copy)... So the case is really strange. 

S
23-Emerald III
StephenW23-Emerald IIIAnswer
23-Emerald III
November 2, 2020

There is a config.pro option you need to add to keep created dimension in the drawing only.

create_drawing_dims_only YES

 

This will keep your created dimension from actually belonging to the model even though you created them in the drawing (sounds strange but it's the way it works).

 

Be careful and do testing with this option before putting it in to widespread use. It will potentially cause issues with your GD&T with respect to created dimensions and model GD&T. PTC may have fixed this, but it used to be difficult to get everything to works together like you expect.

    C
    cadbart1-VisitorAuthor
    1-Visitor
    November 2, 2020

    To be honest I'd not like to have problems with GD&T 😄 Seriously there's no another way to indepent a copy from origin? This is strange for me because Creo deleted usual dimenssions which are not directly realated to the model...

    KenFarley
    KenFarley21-Topaz II
    21-Topaz II
    November 2, 2020

    When you create a dimension in a drawing, by default, Creo stores that dimension information in the model. The options pointed out will prevent that, and require Creo to instead save the dimensions you create in a drawing in the actual drawing itself. Hopefully this will prevent the problem you were having.

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