By Scott Hendren
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 Parametric 3.0 and earlier, Set Datum Tags could be created in one of two ways:
- Using the (Set Datum Tag annotation) option in the Datum dialog box, as shown below, or the (Set Datum Tag annotation element) option from inside an annotation feature.
- 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 model geometry. This means that when you open a model that was created in Creo Parametric 3.0 or earlier, you have to update any existing Set Datums to Datum Feature Symbols if you need to make any changes to dimensions, Geometric Tolerances, and so on. It is important to note that the Set Datums might also be connected to geometric tolerances, so you must manage that circumstance as well.
As of Creo Parametric 4.0 M060, a Legacy Datum Annotations Conversion tool is available to help convert legacy datums to datum feature symbol annotations.
The following steps should be followed:
- Set the configuration option combined_state_type to mbd or semi_mbd. Note that Creo Parametric 5.0 uses semi_mbd by default.
- Use the Model Tree Items dialog box to ensure Annotations display are enabled in the Model Tree, as shown below.
Note the following:
- If you are working in Drawing mode, you must open the model and access the Legacy Datum Annotations Conversion dialog box from there.
- If you are working in Assembly mode, you must access the Legacy Datum Annotations Conversion dialog box from the top model.
- For annotations assigned from an inheritance feature, the Legacy Datum Annotations Conversion dialog box must be accessed from the source model.
5. All legacy Set Datums must be converted to Set Datum Tag annotations. Click Convert All Set Datums to complete that conversion. The results of the conversion appear in the Set Datums and Datum Annotations Table of the Legacy Datum Annotations Conversion dialog box, as shown below.
- If the conversion is successful, the datum is moved from the Set Datums column to the Annotations column and the Status column is empty.
- When a conflict is encountered, the datum is moved from the Set Datums column to the Annotations column, and displays in the Status column.
Change Reference appears in the Required Actions column.
- When a failure is encountered, the datum stays in the Set Datums column and displays in the Status column. Create DFS displays in the Required Actions column.
- You can hover over to see additional information related to a conflict or failure, as shown below.
6. Resolve the conversion conflicts by clicking Change Reference and selecting a reference on the model. The legacy Set Datum Tag annotation converts to a Datum Feature Symbol annotation. This must be repeated for all conflicts. Once corrected, the Annotations turn green, as shown below.
7. When Creo Parametric cannot convert a legacy Set Datum, Create DFS displays in the Required Action column, indicating a failure. Several scenarios exist that could cause the failure, each requiring a you to edit the datum references:
- Scenario 1: A Set Datum is placed on a datum axis and the axis is normal to the current orientation plane.
- Scenario 2: A Set Datum is placed on a datum axis and the axis is at an angle to the current orientation plane.
- Scenario 3: A model Set Datum is placed on a Geometric Tolerance that was created in Drawing mode with the As Free Note placement type.
- Scenario 4: A model Set Datum is placed on a model Geometric Tolerance that was placed on a model dimension in Drawing mode. The dimension was created with the Dimension Elbow placement type and an Edge reference.
- Scenario 5: A model Set Datum is placed on a model Geometric Tolerance that was placed on a model leader note in Drawing mode. The note was placed with the Note Elbow placement type.
8. Repeat the previous step for all the failures that have a workaround, and then click Convert All Set Datums to convert the legacy Set Datums to Set Datum Tag annotations.
9. If no workaround (from Step 7) is available for the failure, click Create DFS to create a new Datum Feature Symbol annotation. The datum feature symbol annotation appears in green with the same name as the set datum. Repeat this step for all failures that do not otherwise have a workaround. Once complete, the Annotations display in green as shown below.
10. If any legacy Set Datum Tag annotations remain, click Convert All to DFS to convert all them to Datum Feature Symbol annotations, which will appear in green.
Note that you can use the Save Results option to save the current state of Set Datums and the Datum Annotations Table to an information file.
If you are working in a drawing, you have to open the part to perform the conversion operations. Once you have finished, return to the drawing and update all sheets using the following steps:
- If there are multiple sheets, right-click a sheet and click Select All.
- Select the Review tab and click Update Sheets from the Update This will update all of the drawing sheets.
Select the Annotate tab and click (Show Model Annotations) to display the new Datum Feature Symbols.
Using these 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.
Learn more the creation and usage of Datum Feature Symbols and other model annotations in the Rand 3D Creo Parametric: Working with 3D Annotations and Model Based Definition guide.