GD&T text boxes in Creo 3

[cmarquardt]

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

[TomD.inPDX]

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!!!

[rcook]

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.

Thanks,

Roger

[James62]

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

[rcook]

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.

[TomD.inPDX]

The GTOL implementation is a lot of work.

You really need to make a case for justifying it.

In Creo 2.0, when I started to use it, Creo would crash at every other datum tag move.

I am also not a fan of rules while I am still working out the assignments.

It is a good option, no doubt.  It is not for everyone.

And the lack of real detailing upgrades just makes upgrading Creo less and less attractive.

[cmarquardt]

Hey Roger, it worked for me as well the first time I tried it, which made the user asking the question to me annoyed that things always work for me.  But then, after editing it again, the separation went away.  And then I tried it again and it didn't work at all.  And then I tried it again, and some of the vertical lines showed up, but others disappeared.  So, maybe it is a bug specific to M080?  But, the vertical separations are undependable at best.

I think your argument that GTOLS should just be stored in the model is valid in most cases.  But, for people dealing with legacy data where those datum's aren't set up, or have the occasional drawings that don't have an associated model, or "what-have-you" case, it isn't always an option.  And often the ROI just isn't there to instruct people to recreate this information every time they revise a drawing.

In the end, PTC needs to keep the needs of all of its customers in mind when making changes.  Flat out removing this capability is not acceptable- which to be fair I don't think was their intention.  I hope this was just a bug...  I will start a support case on the subject, being it appears it is not a common issue.

[StephenW]

Creo 3 M070, If I type the GDT onscreen using the wysiwyg input, I get the code onscreen.

If I then go to the format tab (with the text selected), hit the drop down arrow next to text and then TEXT EDITOR, it take me to notepad, I can just exit and it "converts' the GDT to the good frames.

I know, it's not a good work around but you can get the job done.

You could mostly automate with a mapkey

[fklink]

We just installed Creo 3.0 M100  for that reason.

They brought back the text editor as it was in the past and this allow us to edit easyly that kind of annotation

[TomD.inPDX]

That's the tip I was looking for   Thanks Francois.

[cmarquardt]

Interesting, thanks for taking the time to test and relay the info.  Unfortunately, still no go here.  It imports it looking properly until you edit the note again, then it breaks it.

For example, you open the drawing last saved in Creo 2, and it looks fine.  Then you edit the note and exit from the note, and it's broken.

For eg. I type this:

And then go into the text editor and exit as you suggest, and it highlights the vertical separators like its going to do it.  But, as soon as you de-select the note, it's broken again:

Like I said, it must be a bug if the rest of you aren't experiencing it.

Thanks!

[TomD.inPDX]

If you look at my earlier reply, this is exactly what happens.  It looses the separation location and just puts in a lot of style delimiters ("[3:xxx[").

Not ever seeing the delimiters makes this a mess very quickly.

Also, in the past we could change text styles in the middle of the string by use of these delimiters.

I don't see that capability any more either.

[dgallup]

That worked for me in Creo 4 M020 but what a stupid thing to have to do!!!!  Totally unintuitive and a bunch of extra clicks.  But's that what I think of ALL ribbon interfaces.  Hopefully in a few more years the idiots at MS will move on to something that's way more efficient and PTC will follow along like an obedient dog.

[ewalton]

Sometimes I just want to show the datum in more places or other drawing sheets. Being able to do so with the boxed text is just quicker.

[cmarquardt · Accepted solution]

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.