Dimensions disappear on a drawing

[dksix]

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. 

[Dale_Rosema]

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.

[dksix]

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. 

[Dale_Rosema]

I do not understand the programming logic behind it, but somehow when you create a driven dimension on a drawing, it still relates it to the model (12345.prt dimension abc) so that when you do a "Save As", that dimension description in the software is still related to the model and then when you delete it in the "Save As" version, you are deleting dimension "abc" and now "abc" cannot be for on the original drawing because it was deleted from the model.

Sorry if I am not clear, but I know how it works, but not the code behind it.

[StephenW]

Preview is a snapshot of how the drawing looked when you last saved it. I no way is it Creo looking at what the current geometry is, only what a snapshot of it was at the time of the last save. It's actually an embedded JPEG (maybe different file type) in the creo file.

The drawing dimension is a little more complicated, kind of. By default, created drawing dimension are actually saved within the model. This makes them available for model GD&T to be applied even on created dimensions (there may be other benefits/reasons, but the GD&T one always is a gotcha).

There is an option in the config.pro (create_drawing_dims_only) that you can use to make your dimensions save within the drawing only and you won't have the disappearing dimension issue (on newly created dimensions) but, at the very least, you won't be able to use model GD&T with respect to those dimensions (again, there may be other advantages/disadadvantages I am not aware of).

[StephenW · Accepted solution]

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   

• Available in: English 

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"

[dksix]

To Dale and Stephen,

Thanks to both of you. In the future I'll try hiding or erasing instead of deleting in these cases. I'll experiment some with changing the config pro sometime when I have extra time.

One thing Stephen. The post you made lists that it applies to Creo 1.0 - 4.0. We are still using a Wildfire .scl file and our config pro definitely predates Creo 5. Would Creo 5 be different by default but since we are using existing config pro settings we just aren't allowing Creo 5's default or was the article just before Creo 5 and Creo is the same?

[StephenW]

The option has been around for many, many revisions of pro/e so any version of Wildfire would use it and I am 99% sure it was always defaulting the same. Oh, and looking back at the article, it specifically includes 

• "Pro/ENGINEER and Creo Elements/Pro Wildfire to Wildfire 5.0" (Wildfire 5 and Creo Elements/Pro are the same release, just re-branded)

I am on Creo 4.0 so I can't test  Creo 5.0 but a quick search tells me the option and functionality is the same in Creo 5.0 also.

[Dale_Rosema]

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.

[dksix]

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. 

[estgeorge]

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!