Showing results for 
Search instead for 
Did you mean: 
Showing results for 
Search instead for 
Did you mean: 

Community Tip - Have a PTC product question you need answered fast? Chances are someone has asked it before. Learn about the community search. X

Tips for text

5-Regular Member

Tips for text

Here's an open discussion for text and notes in Creo and Pro-engineer.

Add tips and tricks that you know and ask questions that would be a good addition to this topic.

If you know of any previous threads that will compliment this topic please provide us the link.

131 REPLIES 131

To see the result of a note change without closing the note window, simply click on your drawing's background when the changes are done.

It will act like a "Preview" button.

What was the trick for putting in your own dimension?

It has something to do with @D0 or something and then you type in your own dimension.

@OmyOwnDimension - @O overwrites the default content

Thanks. That is what I was looking for. Just remember it's an "O" (oh) and not a zero.

Hi Dale...

In Wildfire 5 and beyond there's also a radio button for "Override" on the Dimension Properties window that does the same thing.



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.

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.

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.

If you don't want to mess with pen tables and you export PDF drawings, try assigning "thickness" to your text.

I use .012 in in/lb (SAE) drawings providing nice crisp text in the PDF export.

Also, a nice font for distinguishing 1 (one) from I (upper case i) and l (lower case L) is ISO30985FONT. It is the closest thing I found to the Creo Direct Modeling default HP font.

Anyone know how to create the Feature Control Frame B below?

Hi Antonius...

That's called a Composite Tolerance. from the Datum Refs tab, select the radio button for Composite Tolerance. See below. If you need help with the other stuff (diameter symbols, etc) just let me know.




Sorry, I meant with the text editor.

Hi Antonius...

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.

Take care..


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.

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:

Note 1

@[ <Datum Target Symbol> @]

Note 2

@[ <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.

Take care...


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.

Datum_tags_display.JPG 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.

Hi Antonius...

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!


Oh... and I meant to add the next best thing I can suggest is a custom symbol. That should get you around the problem.



Egad... even the custom symbol idea is a harrowing nightmare. I was able to create a gorgeous symbol that does everything you want except for one very silly limitation. You cannot use a construction circle as the basis for a radial attachment point in a symbol. You also cannot use an arc (portion of a circle). It MUST be a full, solid circle... not a partial... not a construction.

WHY?! Geez do we really care if the symbol attachment point is based on the center of a construction circle (which does not show up on the field of the drawing)? Okay then so maybe I'll just use a teeny, tiny arc... solid... but so small it's not detectable. Nope. Doesn't work. What about a really big arc... 359 degrees? Nope. Doesn't work either.

I've just joined the Detailing Technical Committee (took about a month to get on it). I can promise I will bring these issues up and see if I can get them resolved. These have to be very easy fixes.

Thanks... and sorry this is such a pain!

How do you get onto this committee?

When I last used Pro/E for extensive detailing, we were still using the old style datum tags ( [-A-] ). These were easy to fake in.

In the drawing that caused the system to crash, I needed to tie the datum tag to a horizontal line representing a contiguous surface that the datum tag represents. It simply couldn't be done since the line was a drafting sketch feature.

I have a second problem with model generated datum tags in drawings. The axial datum comes out bold (line thickness) while the tagged plane datum came out thin. This is really a very lousy implementation. Why am I the 1st to comment on this?

You can sign up for the Technical Committees (abbreviated as just the "TC's") by going to and clicking on PTC/User Technical Committees in the center of the homepage under "Get Involved". Here's a direct link to the Technical Committee homepage (Direct Link)

Once you're on the homepage, click "Find a TC" from the left hand pane. If you're not yet a member of PTC/User, you'll have to sign up before you can go any further. Once you're signed up (totally free), you can see the various committees and select which one(s) you'd like to join.

Participation in the TCs requires a bit of a commitment. Users are expected to participate in meetings and contribute to the group. Two face-to-face meetings occur each year- one in January at PTC Headquarters and a second one at the Planet PTC Live Event. Next years' Planet PTC Live event will be held in Anaheim (June 9-12). During these meetings, the entire committee has the opportunity to sit down with PTC developers and Product Line Managers. We discuss the software, enhancement requests, bugs, and ask questions to get answers "directly from the horse's mouth" so to speak.

It took me quite a bit of effort to get onto the Detail TC (the committee concerned with drawing & detailing issues). Now that I'm on it, I'm anxious to start logging my feedback. I'm tempering this enthusiasm though because historically I know PTC hasn't put much into the drawing package. I also know this is intentional. As a long time user, I have felt (and continue to feel) that this is a critical mistake. If I had the ear of the developers, CEO, CFO, or anyone else who would listen, I'd try to steer them from this path. PTC has always believe that model-based engineering is the way forward and that paper is antique and archaic. While I agree, I can tell you from experience that most industries and most companies are not ready for this yet. It's just starting to get traction and adoption will continue to be painfully slow. In the meantime, people WANT and need drawing tools that work. In my opinion, PTC makes a tremendous blunder by allowing their competitors to service this space while they ignore it waiting for a day when their vision meets with reality.

So... I joined the Detailing TC and I plan to do my best to push for enhancements. If not earth-splitting enhancements that create the drawing package we want, then at the very least fixing the bugs, closing the loopholes, and making the drawing package we already have work to it's optimum.

Sweet, Brian. I can think of no better voice in the committee than yours. If it wasn't for the commitment for the face-time, I would be happy to participate. I simply don't have funds to go flying all over the country on my dime.

If what you say is true, and if it continues, I will save my maintenance pennies and invest my $ and hours in SolidWorks or possibly Elements Direct. At this point, I simply cannot make certified documents with the incomplete detailing tools in Creo/Pro. This is certainly not acceptable on my end as this is how I make my living. I will continue to submit support requests to achieve the minimal requirements to do my job.

Is it part of the committee's function to review SPR's submitted by users in relation to limitations and problems with making proper drawings?

I also submitted the recreation of the crash with datum tags in drawings. very sad!

Can I send PTC a bill for my lost hours to do what their QC failed to do?

Sorry Kevin, for hijacking your wonderful post. I was hoping for answers, not more problems.

The TC's don't normally review SPRs as far as I know. But we do review enhancements and ideas submitted from committee members. I'd love to see the ideas from Planet PTC Community find their way to the TC's for voting, too. I've mentioned this to several people but I don't think we know what will "officially" become of the ideas from this site yet.

There was a time I didn't hold out much hope to see meaningful improvements in the software owing to a sort of "tone deafness" from PTC. And, it's certainly fair to say maybe I am the only one who perceived that tone deafness. However, in the last couple of years I've seen real improvements in the way PTC has addressed some long-standing problems. For awhile I was cautiously optimistic. The first signs of progress were almost like seeing a mirage. I wasn't sure if I was really seeing what I thought I was seeing. But over the past 1-2 years I have to say, there's definitely something positive going on. Now, there are still problems... but it feels like PTC is really starting to listen. It feels like they're really starting to try to hear voices from the user community. This is real progress. They may have gone through the motions of listening and responding to criticism before... but now it feels like their heart is in it.

I think that makes all the difference in the world. So now, I do have hope that we can improve the drawing package. I'll do whatever I can to pursue that goal. I'd encourage anyone else who'd like to join to visit and learn more about the TC's.

Take care...

Yes, I'd seen this before in days long past but it was only a fizzle in the pan.

Back on subject;

YOU TOO CAN CREATE YOUR OWN FONT! ( maybe I should define a "DATUM" symbol font set )

Technically, the .fnt fonts, as compared to true type fonts, are simple micro-plotter files.

They have a small definable grid in which you can define "move to" and "draw" commands between grid points.

There are source files, index files, and compiled files. Don't trust the source files, however since I have already decompiled a few fonts where the source and the decompiled versions did not match. Another QC glitch!

All the tools are there and the getting started manual has pretty much everything you need.

I do have one SPR into tech support. The manual clearly states that the max text box height is 63, and there are fonts with heights up to 76. Which one is in error? That SPR has been submitted over a month ago and they assure me that they are still working on it.

Brian Martin wrote:

...Now, there are still problems... but it feels like PTC is really starting to listen. It feels like they're really starting to try to hear voices from the user community...

Do you still hold this opinion after the recent PTClive? With respect to drawings in Creo?

I found this that might help this category:

Use a $ in relations to use negative values -


All relations valid in a Creo Parametric model can be entered in a Pro/PROGRAM design.

If an expression you want to include in the RELATIONS statement contains more than 80 characters, use a backslash (\) to interrupt the current line and continue the expression on the next line.

The format can be as follows:


Changing the material density in a part causes the system to update the mp_density value in relations and vice versa.


  • When using negative dimensions, a dollar sign ($) must precede the dimension symbol in both the input statement and the external input files. For example, use $d20 instead of d20. The dimensions will not be updated if a dollar sign does not precede the symbols.
  • If the program assigns a value to a dimension variable that is already driven by a part or subassembly relation, two error messages appear. Edit or remove the program relation and regenerate.

Also found this:

If you have a string of variables like in hole callouts, you noticed that you require spaces between the end of the variable and new text characters. This is why you see...


UNF - 2B
...a text string which is obviously not to any standard that we as engineers accept.

But there is a little known method to remove the requirement for the space:

{0:&THREAD_SERIES}-{1:&THREAD_CLASS} ...which returns


Old school editor but this is what makes it work.

Why didn't PTC do this for the hole CALLOUT_FORMAT?

PTC, are you listening? This is what "we" call fit and finish

The extraneous spaces have always been an issue. I've been removing them for years... or else just skipping the automatic cosmetic thread notes altogether.

23-Emerald III

I have seen before where the font size was changed within a text box (i.e. not separate text boxes).

Top Tags