Updating Set Datums to Datum Feature Symbols in Creo Parametric 4.0

If you are new to Creo Parametric 4.0, and have started working with drawings or the Model Based Definition (MBD) annotation tools, you may be asking, “What is going on with Set Datums?” The simple answer is that Set Datums are replaced by Datum Feature Symbols.

In previous releases of Creo Parametric, a Set Datum was created as a property of a plane or axis feature. Now, a Datum Feature Symbol is created as either a standalone annotation or inside of an annotation feature, and can only be placed on a surface, dimension, witness line, or GTOL.

In Creo 3 and earlier, Set Datum Tags could be created in one of two ways:

1.  Using the  (Set Datum Tag annotation) option in the Datum dialog box (shown) or the  (Set Datum Tag annotation element) option from inside an annotation feature.
   
   
    
2. Using the  (Set) option in the Datum dialog box.

Prior to Creo Parametric 4.0, Set Datums were derived from existing datum planes or axes. Now, Datum Feature Symbols must be associated with solid geometry. So when you open a model created in Creo Parametric 3.0 or earlier, you have to update the existing Set Datums to Datum Feature Symbols. It is important to note that the Set Datums may also be referenced by Geometric Tolerances, so you will have to manage that circumstance as well.

You can  select an annotation in the Detail Tree, right-click and select either the Convert or Convert All option to convert outdated GTOLs and dimensions to the modern annotation types, as shown. 

Unfortunately, simply completing the conversion operation doesn't solve the problem. as the associativity between the legacy datums and GTOLs may be lost in certain scenarios. 

Scenario 1:  (Set Datum Tag annotation) On a Plane or Axis

Note the icon indicating the outdated annotations in the Detail Tree shown.

1. Convert all outdated GTOLs and dimensions by selecting an annotation, right-clicking and selecting Convert All.
2. Right-click and select Change Reference to establish a new reference for each Datum Tag Annotation you have converted. Note that for Datum Tag Annotations, right-clicking and selecting Change Reference will  automatically complete the Convert operation.

Scenario 2:  (Set) Legacy Set Datum Tag

Datum Feature Symbols can not be placed on a datum plane or datum axis, so once you convert the annotations, for any Set Datum, a new Datum Feature Symbol needs to be created and the legacy set datum tag needs to be unset.

1. Convert all outdated GTOLs and dimensions by selecting an annotation, right-clicking and selecting Convert All.
2. Create a new  (Datum Feature Symbol) with the same name as the Set Datum.
3. Select the set datum, right click and select Properties. In the Datum dialog box, click   (Unset) as shown.
   
   
4. Finally, just check any GTOLS that referenced the Set Datum you cleared to ensure it picked up the correct Datum Feature Symbol, as shown.

Using the above steps, you should be able to replace your legacy Datum Tags with Datum Feature Symbols to convert your older models to Creo Parametric 4.0.

In June we will be releasing Creo Parametric 4.0: Working with 3D Annotations and Model Based Definition, where you can learn more about the creation and usage of Datum Feature Symbols and other model annotations. 

About the Author

Learning Content Developer<br><br>Scott Hendren has been a trainer and curriculum developer in the PLM industry for over 20 years, with experience on multiple CAD systems, including Pro/ENGINEER, Creo Parametric, and CATIA. Trained in Instructional Design, Scott uses his skills to develop instructor-led and web-based training products. Scott has held training and development positions with several PLM companies, and has been with the ASCENT team since 2013. Scott holds a Bachelor of Mechanical Engineering Degree as well as a Bachelor of Science in Mathematics from Dalhousie University, Nova Scotia, Canada.

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