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cmarquardt12-Amethyst
12-Amethyst
November 15, 2016
Solved

GD&T text boxes in Creo 3

  • November 15, 2016
  • 3 replies
  • 15659 views

In past versions of Creo/ProE, you have been able to somewhat easily create GD&T datum reference frames in situations where you don't want to use the annotation.  For example, if you are calling out GD&T in the notes of the drawing.

 

In Creo 3, it seems that the old syntax of @["text"@] no longer will box around your "text", and this function has been replaced with a button in the ribbon bar, called "Box".

 

While Creo 3 imports the @[text@] syntax, if you have two right next to eachother, it removes the separation.  Causing a Creo 2 note that was created as described, to lose all the vertical separations between the different areas of the datum reference frame.

 

(Looks like this)

 

The only temporary solution I have found is to add vertical bar characters | for the separators.  Like this:

 

 

Apologies if this has already been covered, I did some searching and could not find anything specifically referencing this problem.  What is everyone else doing to workaround this problem?

 

Creo 3 M080

Best answer by cmarquardt

Okay everyone, hold onto your chairs:

The answer is that there is something going on in the background, which must be tied to certain DTL options, mixed with the version of Creo the drawing was originally created in.  So, while this may not affect many people, if it does you, see below.

Run the following hidden options in the drawing options:

update_drawing = 2202279

update_drawing = 2211176

Or, alternatively, if you are not concerned about the other changes it make make, do as I did and run this option instead of the other two:

update_drawing = all

Once you run that, the "box" text button works exactly how you would want it to, and the old syntax imports it just fine when you edit the note.

3 replies

T
TomD.inPDX17-Peridot
17-Peridot
November 16, 2016

Just one more reason I cannot use Creo 3 for drawings.

They completely blew the annotation editor.

Creo 3 needs a toggle in Config.pro for legacy annotation.

If they don't do something about this, I will have no reason to continue maintenance.

I have Creo 3 M020 loaded.  It does not do the short line and the lines do not disappear.

What I do see is a VERY messy formatting after many attempts at editing a particular piece of text.

For instance, ".010" was parsed into @[{2:.0}{3:10}@]@[@{...

This is JUNK!, plain and simple.

Once you have the text selected, you can open the editor.  Problem is, it is now Notepad.exe!!!  BLUNDER #2

Where is the original text editor and how can I make that the editor for Creo?  Creo has options for many other text editors, why not text!

Every time I look at Creo 3, like I just did, I have to shake my head at the complete utter ... Meh!!!

R
rcook1-Visitor
1-Visitor
November 17, 2016

Works for me in Creo 3 M100, but I always shiver when I see manually created GTOLs. Why not create an actual GTOL??? You can call it out wherever you want in the drawing and it is much easier to create and manage.

BOXES.jpg

Thanks,

Roger

J
James621-Visitor
1-Visitor
November 17, 2016

Productivity-wise, nothing beats typed out text. Surely not a model polluted with bunch of GTOL reference planes.

R
rcook1-Visitor
1-Visitor
November 17, 2016

I suppose that may be true if all you care about is the pdf/publish of the drawing, but it makes the GTOLs completely useless for any downstream applications. Once you have to recreate a GTOL in many places, the supposed productivity gain of using dumb text goes out the window (as well as increasing the chance for error when recreating the GTOL).

I'm not sure how you are creating GTOLs that your model gets "polluted with a bunch of GTOL reference planes". There are normally a handful of datums at most and they are easily managed through combined states and annotation features.

C
cmarquardt12-AmethystAuthorAnswer
12-Amethyst
November 22, 2016

Okay everyone, hold onto your chairs:

The answer is that there is something going on in the background, which must be tied to certain DTL options, mixed with the version of Creo the drawing was originally created in.  So, while this may not affect many people, if it does you, see below.

Run the following hidden options in the drawing options:

update_drawing = 2202279

update_drawing = 2211176

Or, alternatively, if you are not concerned about the other changes it make make, do as I did and run this option instead of the other two:

update_drawing = all

Once you run that, the "box" text button works exactly how you would want it to, and the old syntax imports it just fine when you edit the note.

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