Just in case - remember it'll work only for reference dimensions created in drawing. You can't override value of model dimension, displayed in drawing with Show/Erase or Show Model Annotation.
You can create everything but the initial large target using the text editor.
I haven't tried playing with it. You may be able to come up with something close using text. If you're dead set against trying to use the GTOL features in Pro/E or Creo, your next best option would be to create a really nice custom symbol to do the job. This might take a couple of hours to perfect, but I'm confident it can be done.
This symbol could be made to satisfy all your needs. Actually, I can imagine quite a few people would like to get their hands on such a thing. Maybe you can take a crack at it. If you need help or get stuck, I'll be happy to help out. This might give people a "last resort" type of solution for times when they can't seem to get the internal GTOL functions working properly.
Good luck... and if you decide you need help, just give a shout.
t does work for dimensions created (and associative) in the drawing. I think what Lukasz was saying is that he's calling those "created" dimensions reference dimensions but in fact, this works for any created dimension.
It does not work for "shown" or "driving dimensions" meaning the dimensions used to drive the 3D model. In most cases, though, this is not a big deal. Even for companies who insist upon "shown" dimensions, it's occasionally acceptable to create a dimension for special purposes like this.
Thanks again, Brian. I appreciate both your observations regarding this functionality; re: in GTOL and the text limitation.
I am certainly not against using GTOL as intended but it has to function in the drawings. So far, I am getting nothing but flack from support in my request for getting the tagged datum planes to follow the hide/unhide properly. That, and the system crashing when I move datum tags on the drawing are simply not workable. Since I cannot reproduce the crash reliably, support will not do anything even with the crashlog in hand. Remember that I also have a corrupt drawing file that will no longer allow me to move datum tags representing 2 days hard work. So yes, I'd love to use GTOL... -IF- it worked correctly and reliably in drawings.
The function of composite GTOL is relatively limited in my field. I am sure I can find a way to "bury" the reference data well enough to create the rare occasion I need the composite GTOL within the model.
Yeah, that's right. I just called them "reference dimensions" since it's what they're called in Pro/E / Creo. But you're right, it's about all "hand-made" dimensions in drawing, as opposite to dimensions displayed or "showed" from the model. It was just a note in case someone start wandering why using @O option doesn't work or Override value box is not active.
I completely understand your frustration with the datum tag problem. This type of problem is the reason why many of the larger companies don't jump on the latest revision of the software. We hang back on purpose while the first few production releases are distributed. After 6-8 months, we finally start testing the "new" software. By that time, most of the larger, easy-to-catch bugs have been worked out.
As a side note... using TWO notes, I was able to duplicate the Composite Tolerance format. If you create a single note with the large datum target (at TWICE the text height as usual), you can then create a second note using the @[ and @] nomenclature to create text in a box.
The first note JUST has the large datum target in a box. The second has two lines using the @[ and @] to create the necessary cells. Here's an image of the two notes side by side (click them for a better view, the lines come up faint until you click the images)...
And another of the two notes placed next to each other and grouped so they move together as one unit (again, click for a better view)...
The text for the two notes are as follows. All symbols are from the "Text Symbol" palette:
@[ <Datum Target Symbol> @]
@[ <Diameter Symbol> .004 <MMC Symbol> @]@[A@]@[B@]@[C@]
@[ <Diameter Symbol>.002 <MMC Symbol> @]@[A@]
If you copy/paste those text notes and replace the symbols as noted, you can create a composite tolerance without using the GTOL system at all. Hopefully this gets you around the issue until PTC Customer Support can provide a resolution to your problem.
I am really beginning to appreciate the power of the text editor in UG NX.
Happy to be on the front lines making your job easier at a later date, Brian
Okay, I have another need...
On the left is a valid datum tag and on the right is the best I can do with a note.
Also notice the difference in fonts. I need the iso30985font with .012" thickness. I cannot change the valid datum tag to match this customer requirement.
Anyone have a trick in how to make the note look like the datum?
BTW: crashed again this morning... I could be lighting cigars with $100 bills at this rate.
As far as I can tell, that's the best I can do, too. I never knew you couldn't change the font for a datum tag. If you try to set the tag in the model, there's a Text Style button you can access... but it doesn't let you change font. it only allows you to change a few settings of the default font (and even those settings don't appear to work particularly well). If you try to set the tag in the drawing... you don't get the Text Style button at all! Either way, it doesn't much matter because you can't do anything with it.
I got as sneaky as I could... I even changed the Default Text Font for the drawing without luck. I have to say, it's been awhile since I used any 3D annotations and I was fairly well shocked at how poor they work in Wildfire 5. I still need to go back and respond on the other thread about 3D annotation problems but I think these problems need to be pushed up to the Detailing Technical Committee ASAP so we can get them fixed.
Thanks... and sorry I couldn't figure it out. I really hate when I get stumped!