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Why copy of drawing influence on origin?

cadbart
10-Marble

Why copy of drawing influence on origin?

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!

1 ACCEPTED SOLUTION

Accepted Solutions
StephenW
23-Emerald II
(To:cadbart)

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.

View solution in original post

7 REPLIES 7
BenLoosli
23-Emerald I
(To:cadbart)

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.

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. 

StephenW
23-Emerald II
(To:cadbart)

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.

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
21-Topaz I
(To:cadbart)

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.

Well, I didn't know that dimenssions infomrations are stored inside model. Thank y'all, I'll try this option in my case 

StephenW
23-Emerald II
(To:cadbart)

I haven't used the create drawing dimensions setting in years. It may have changed. A lot has changed with respect to GD&T in creo over the last few years so there may not be any problems with that anymore.

You should do some testing with the setting to see if it does what you need.

Another option is to NOT delete created dimensions in your original drawing. Use the hide command to not show the drawing. The dimension is still available for use in the other drawing.

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