NX How to display point (such as Center of Mass) within the model on its drawing view?

When a point is created on a model data in Modeling application, such as Datum Point or Center of Mass point, and drafting view is created in Drawing file for this model. How to have drafting view display/show the point?

By adding the point object into the Model reference set of the model data, then update the drafting view will show the point in it:

Below are the detail steps to perform:

1. In Assembly Navigator, highlight the model data and Right Mouse Button -> Open in Window

2. With model data as the active display part, go to "menu -> Format -> Reference Set" command.

3. Highlight the existing reference set named Model, now select the point object, notice the count for Selected Object will increase from selecting to point to include.

4. Hit Close button on the Reference Set dialog to complete the operation.

5. Switch the display part back to the drawing file and update the view.

In addition to Datum Points, this article also applies to Datum Axis.