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dksix1-Visitor
1-Visitor
February 13, 2019
Solved

Dimensions disappear on a drawing

  • February 13, 2019
  • 3 replies
  • 14415 views

I have a part file and a drawing file. I have extensive dimensions on the drawing but need one with more basic dimensions so I do a save as and rename a copy. I delete the dimensions not needed on the copy, save and print it. The problem is that the original drawing no longer shows the dimensions that were deleted on the copy. Stranger more is that when opening the original drawing the preview shows the missing dimensions. 

 

This has happened in both Creo 3 and 5 on 2 different computers one multiple file sets. 

Best answer by StephenW
https://www.ptc.com/en/support/article?n=CS17143&language=en&posno=2&q=create_drawing_dims_only&source=search
 
Article - CS17143

 

Effect of setting "create_drawing_dims_only yes" in Creo Parametric

Created: 04-Feb-2011   |   Modified: 01-Dec-2017   

 

Applies To

  • Creo Parametric 1.0 to 4.0
  • Pro/ENGINEER and Creo Elements/Pro Wildfire to Wildfire 5.0

Description

  • Effect of setting "create_drawing_dims_only yes"
  • What are the limitations when setting config.pro option "create_drawing_dims_only" to "yes"
  • How to create the dimensions saved within the drawing

Resolution

  • Default: No - Saves driven dimensions created in Drawing mode on solid geometry in the solid.
  • here, set to Yes - Saves all new driven dimensions created in the drawing inside the drawing as associative draft dimensions.
  • Dimensions created in the drawing are saved with the drawing
  • Created dimensions display in the drawing independent of the version of the displayed model
    • However, since they reference model geometry, they appear as broken dimensions (magenta), if the referenced geometry does not exist in the model version
  • Geometry tolerances cannot be related to created dimensions
  • Created dimensions cannot be changed to ordinate dimension referencing a base stored in the model
  • Created dimensions cannot be changed to coordinate dimensions
  • Pro/TOOLKIT function ProDimensionDecimalsSet() returns PRO_TK_GENERAL_ERROR for created dimensions
  • Created Dimensions cannot be used for Verification Step in Pro/CMM
  • The dimension value can not be used as a symbol in a note
    • Example: "All rounds have radius &d5"

3 replies

Dale_Rosema
23-Emerald III
Dale_Rosema23-Emerald III
23-Emerald III
February 13, 2019

You need to "erase" the dimensions (hide them) and not delete them from the "Saved As" copy.

Deleting them will remove them from both the "Save As" version and the "Original" drawing.

D
dksix1-VisitorAuthor
1-Visitor
February 13, 2019

I understand what you're saying but why does the dimensions that was deleted from the new drawing (created through save a copy with a different drawing name) still appear in the preview of the original drawing? 

 

These are manual added dimensions on the drawing (drw) not dimensions driven from the model. 

S
23-Emerald III
StephenW23-Emerald IIIAnswer
23-Emerald III
February 13, 2019
https://www.ptc.com/en/support/article?n=CS17143&language=en&posno=2&q=create_drawing_dims_only&source=search
 
Article - CS17143

 

Effect of setting "create_drawing_dims_only yes" in Creo Parametric

Created: 04-Feb-2011   |   Modified: 01-Dec-2017   

 

Applies To

  • Creo Parametric 1.0 to 4.0
  • Pro/ENGINEER and Creo Elements/Pro Wildfire to Wildfire 5.0

Description

  • Effect of setting "create_drawing_dims_only yes"
  • What are the limitations when setting config.pro option "create_drawing_dims_only" to "yes"
  • How to create the dimensions saved within the drawing

Resolution

  • Default: No - Saves driven dimensions created in Drawing mode on solid geometry in the solid.
  • here, set to Yes - Saves all new driven dimensions created in the drawing inside the drawing as associative draft dimensions.
  • Dimensions created in the drawing are saved with the drawing
  • Created dimensions display in the drawing independent of the version of the displayed model
    • However, since they reference model geometry, they appear as broken dimensions (magenta), if the referenced geometry does not exist in the model version
  • Geometry tolerances cannot be related to created dimensions
  • Created dimensions cannot be changed to ordinate dimension referencing a base stored in the model
  • Created dimensions cannot be changed to coordinate dimensions
  • Pro/TOOLKIT function ProDimensionDecimalsSet() returns PRO_TK_GENERAL_ERROR for created dimensions
  • Created Dimensions cannot be used for Verification Step in Pro/CMM
  • The dimension value can not be used as a symbol in a note
    • Example: "All rounds have radius &d5"
    Dale_Rosema
    23-Emerald III
    Dale_Rosema23-Emerald III
    23-Emerald III
    February 13, 2019

    For non-windchill environments, if you have your extensions turned on in your files  (12345.drw.23 - where .23 is the 23 iteration of the drawing 12345.drw). You might be able to delete the latest iterations before when you deleted the dimensions from original drawing so that you do not have to recreate them.

     

    So if you did this at 12:30 this afternoon, remove, quarantine, or delete the iterations before then to get back to where you were.

    D
    dksix1-VisitorAuthor
    1-Visitor
    February 13, 2019

    I tried that first. I deleted the newly created drawing which had the dimensions deleted as well as new versions of the original drawing. That took it back to the version that's dated from 2018 and I also emptied the programs memory. I also shut down and restarted CREO 3, tried it another set of files in CREO 5. Both my versions use the same config pro file as well as the other machine this occurred on. 

    E
    estgeorge1-Visitor
    1-Visitor
    February 15, 2021

    I had this happen to me a few times before with no luck restoring them back.

    Problem and Solution:

    I believe this happened when I hit "Save a Copy" of the drawing into a new directory with a new name. This, for some stupid reason, resaved my open .prt files in my working directory as the next version (ie, from example.prt.1 to example.prt.2), and deleted the dimensions associated. Therefore, when I opened my drawing after closing and erasing, from the working directory, the dimensions were missing. I simply deleted the .prt file versions that were created at the same time stamp that I "Saved a Copy". Cleared and erased, and then reopened the drawing, and BAM dimensions were back!

     

     

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