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Datum Feature Symbols in Creo 4.0

In Creo 4.0 we made some significant changes to the Datum Feature Symbol annotations (otherwise known as "set datum" or "set datum tag" in earlier releases).

I've already gotten a number of questions from users who have started using Creo 4.0 and I think best way to answer the questions, while making that information accessible to the broader user community, would be to write up the answers and post them here to the community site. As this topic is intimately related to MBD, this Model Based Enterprise group seems like the best home for this content.

There are several questions that I'd like to address and I think it would be too much information for a single blog post, so I'll write a series of blog posts and link them all to this one as a sort of top-level post for the whole topic. So, you can bookmark this post and be able to get to all the other posts on the topic from here.

Overview of Creo 4.0 enhancements

I think it makes sense to first provide an overview of all of the enhanced capabilities of the Datum Feature Symbol so we're all on the same page with what's new. Each of the sub-sections below will cover an individual enhancement and also provide a link to the page in the Creo Help system that describes the enhancement and also provides a short video that shows it in action.

Creation and Editing

The workflows for creating and editing Datum Feature Symbols have been streamlined and made more intuitive. When you click the Datum Feature Symbol icon in the ribbon you immediately get a preview of the annotation attached to the pointer. You can drag this to place it on the model. There are a number of different standards-compliant placement options. For example, you can place the symbol directly on a model surface, or attach it to a GTOL, or to a dimension, or to a dimension witness line. Some of the attachment types also offer alternative placements available from the Right-Click menu.

You can edit the properties of the Datum Feature Symbol from a dedicated ribbon tab that will appear whenever a Datum Feature Symbol is selected. When you select a Datum Feature Symbol, the ribbon will appear and if you select something else or clear selection by clicking in open space, the tab will go away. There is no need to select the annotation, and then choose a command to open the UI for editing the properties and there is no need to click OK or Cancel to close the UI.

Check out the video in the Creo Help Center: More Intuitive Workflows for Creating and Editing Datum Feature Symbols

Automatic Naming

When you create a Datum Feature Symbol, it automatically takes the next available name in the standard sequence of valid names. For example, the first Datum Feature Symbol will be named "A", and the next one you create will be named "B" and so on. If there is a gap in the sequence of names of existing Datum Feature Symbols, the next one to be created will take the missing name. For example, the model contains Datum Feature Symbols A, B, D, then the next one to be created will automatically be named C.

You can still change the name as needed from the Label field in ribbon. Creo will check the entered name to make sure that it complies with the standards, and in the MBD environment it will check that there are no duplicate names. In drawings there is no check for duplicate names because it is common practice to have a Datum Feature Symbol shown in multiple views, although the standards compliance checks are still available in drawings.

Check out the video in the Creo Help Center: Automatic Naming of Datum Feature Symbols

Semantic References

Datum Feature Symbols support full semantic references to model geometry. You can click the References button from the ribbon to open the References dialog where you can select additional geometry references. Model surfaces, planes and axes are the supported reference types. If the Datum Feature Symbol is placed on a model surface, this placement reference is automatically added to the References, but if the Datum Feature Symbol is placed on another annotation (dimension or GTOL, for instance) then there will be no semantic references automatically assigned, but you can still add any references that you want.

Check out the video in the Creo Help Center: Specifying Fully Semantic References for Datum Feature Symbols

Additional Text

You can now include additional text as part of a Datum Feature Symbol annotation. There is a text input field in the ribbon where this text can be added and a button to control on which side of the annotation the text will appear.

Check out the video in the Creo Help Center: Specifying Additional Text Near Datum Feature Symbols

Elbow Option

You can now add an elbow to the stem of the Datum Feature Symbol annotation. This allows additional flexibility in managing the cosmetic positioning of the annotation. To adjust the length of the elbow, hold the SHIFT key while dragging the label.

Check out the video in the Creo Help Center: Adding Elbows to Datum Feature Symbols

Standalone Annotation

Datum Feature Symbols are now available as a regular annotation and are not a property of a plane or axis feature of the model. You can create a Datum Feature Symbol either as a standalone annotation, in which case it will appear at the top of the model tree under the Annotations node, or you can create a Datum Feature Symbol inside of an annotation feature.

When created as a standalone annotation, the Datum Feature Symbol possesses the same advanced capabilities as if it were owned by an annotation feature. Those advanced capabilities are: 1) The ability to have parameters, 2) The ability to be Designated as Control Characteristic, 3) The ability to have multiple semantic references, and 4) Errors and Warnings reported through the Notification Center.

Check out the video in the Creo Help Center: Datum Feature Symbols as Standalone Annotations

Links to other blog posts related to Datum Feature Symbols

The links below take you to the other blog posts targeted at specific questions regarding Datum Feature Symbols

  • Updating Legacy Set Datum Tags to New Datum Feature Symbols **Coming Soon**
  • Why can't I attach a Datum Feature Symbol to a plane or axis? **Coming Soon**

If you have any additional questions or comments about the enhanced Datum Feature Symbols, add a comment to this post and I'll answer it as soon as I can.


Hi @RaphaelCNascime

Do you know when the links to other blog posts will be added?

Links to other blog posts related to Datum Feature Symbols

The links below take you to the other blog posts targeted at specific questions regarding Datum Feature Symbols

  • Updating Legacy Set Datum Tags to New Datum Feature Symbols **Coming Soon**
  • Why can't I attach a Datum Feature Symbol to a plane or axis? **Coming Soon**

Hi @DavidBrand

I'm not working for PTC anymore, which is why my response comes from a different user account.

Before I left (in July) I did actually write up a comprehensive blog post covering the first topic of "Updating Legacy Set Datum Tags to New Datum Feature Symbols" and I posted it to the MBE Group page. Unfortunately that was shortly before the Community was transitioned to Lithium from Jive and it seems that blog post (and some other valuable things that I had written) were completely lost. I've asked the Community administration if they could be restored, but since nothing has come of that, my guess is that that content is gone for good. As I'm not with PTC anymore I'm not in a position to attempt to re-write that post from scratch.

It's really unfortunate that so much good content was lost in the Community transition. The whole situation with the Community site is disappointing, in my opinion...


Hey guys,

where did you put the Model Datum feature in Creo 4.0? This is so frustrating. Removing the feature that was there before.

Regular Member

PTC has really missed the target on this "enhancement." 
I can't select a plane as a datum to be parallel to another datum. 

If I select a surface, the target connection isn't dynamic, so in a drawing, I can't simple drag it up or down in a view to adjust it for better viewing. 

It's the simple things that absolutely have to work well.
You haven't made it more intuitive. It's more of a pain.

I was excited to move to Creo 4.0, but this drawing stuff that effects the handling of GTOL's is just the worst.  I've got many operational sketches to get to my shop floor and now I'm screwed. Fumbling around trying to figure out how all this works. Not intuitive at all, just a huge waste of my time, and I still can't get the results I want. My co-workers were right. Instead of renewing our PTC licensing, we should have switched to Solidworks. Been drawing with Pro-E since Wildfire 2.0

Regular Member

Raphael said: "... you can place the symbol directly on ... a dimension witness line". I can't figure out how to get dimension witness lines visible to be able to pick them.  Only way I can find the place a datum feature symbol is on a surface.  I can't find a way to move it "in dim" like the old set datum features.

no doubt, the worst PTC move yet!

Regular Member

I cannot for the life of me figure out why the "references" button is greyed-out when I place datum tags.

This needs to be reset to the wasy it was in Creo 3.0 and earlier. It was driven by the CAD, and when we use the CAD as master (which is very common) having this disconnect is sketchy, to put it nicely.


"Why can't I attach a Datum Feature Symbol to a plane or axis? **Coming Soon**


This!  Someone please answer this.


Axes and planes are not valid attachments per ASME and ISO standards.

Creo was enhanced to support correct semantic definition of annotations, which is why those invalid attachment types were removed.


In Creo 4 I add a datum feature symbol, it selects C, but it should have been B. It says B already exists. This is a small drawing and part. I have tried using the find tool to locate this missing datum feature symbol with no luck. How can I find this? I have tried expanding all views, annotations and datums in the drawing tree and it does not show.


I have been using ProE / Creo since Dec '91. I have seen some good enhancements and I have seen some crappy ones as well. I have recently started using Creo 4 and I must say that they flexibility of adding GTols to features in the models and then getting them to show in the drawing is not intuitive at all. I would highly recommend taking a step back and allowing GTols to be added in the model and just show them in the drawing.



Hi @od_bower 

I'm a little confused by this comment. Maybe I'm missing what you're asking, but it's really simple to create GTOL in the part and show them in the drawing. From the drawing, you can either select the GTOL from the model tree of the part and Right-Click > Show, or just select the Show Model Annotations icon from the ribbon and then hit the GTOL tab and then select the view or feature from the model where you want to show the GTOL. It works just like dimensions, so it's at least as intuitive as showing a dimension from the model in the drawing...




I'm unable to use "X" as a datum feature symbol.  I receive a error / notice that "X" is an invalid datum feature label.  I understand that I, O, and Q are not used, but why X.  Is this a mistake.  All of our casting and machining models use X.  Is there a work around.


@swaney001  This boils down to a difference between ASME and ISO standards. ASME Y14.5 does not allow I, O, and Q as you mentioned. ISO 5459 also includes X in the list of prohibited letters.

Creo will follow either the ASME or ISO rules for the syntax checker based on the Tolerance setting under File > Prepare > Model Properties. If you have the tolerance setting set to ANSI, then X would be allowed. If it is set to ISO/DIN, then Creo will show X as an  invalid datum symbol name.

I hope this helps.

I am a Staff Engineer for a large-ish design department.  We have been using Set Datums with GTOLs from the beginning with Pro/Engineer.  Creo4 has fundamentally changed the game here.  It used to be that GTOLs on Drawings could ONLY refer to Set Datums.  It used to be that there could be only one instance of a Datum name in a part and on a drawing.  It used to be that if you changed the name of a Datum, then that name would also change in all GTOLs that reference that datum.


None of that is true anymore.  Now it's possible to add any number of instances of a Datum Name to any feature on a model or a drawing, with no limitations and no associativity.  We may as well be using Symbols only for both Datums and GTOLs.  Now our Drawing Checkers have more to worry about, making sure that the Datum References for every GTOL are correct.


This is by far the worst update to drafting methodology that I have ever seen in any CAD software, EVER.


PTC needs to keep in mind how their customers actually do things, when thinking about how to move forward into the future.  My company has NO INTENTION of moving to MBD, the whole module adds minimal value.  It seems that PTC have sacrificed significant robustness and methodology legacy in the name of eliminating 2D drawings.  And why?!


All we want is the reliability and associativity of the old Set Datums and GTOLs methodology.  This should be rolled out as an option ASAP.


Where is the PTC feedback here?  You're alienating your customers by ignoring this issue!  Just watch them walk away.



ASME Y14.5 2018 and 2009 are saying in paragraph and 3.3.2 respectively that a dashed line must be used if the datum feature is hidden. By watching fig 6-3 on the 2018 version I understand that "hidden" means behind the projected view.


My question is: Why is CREO 4.0 changing the extension line of a Datum Symbol from a solid one to a dashed one when I drag the Datum Symbol away from the contour line in a projected view where that contour is visible in solid line? That wasn't happening before CREO 4.0 and it is actually not what ASME is showing in multiple examples across the pictures of Y14.5 2018 Standard (Fig 7-52 Datum A, Fig 9-2 Datum A, Fig 9-11 Datum A, Fig 10-2 Datum A, etc.)


This is creating confusion between the R&D and Metrology department in my organization. I appreciate your support to clarify this topic.



Dashed extension lines.JPG