Model-Based Definition > Model-Based Definition > Annotation Features > Annotation Feature Basics > About Annotation Orientation
  
About Annotation Orientation
An annotation orientation refers to the plane or the parallel plane in which the annotation lies, the viewing direction, and the right direction or text rotation. An active annotation orientation refers to the annotation orientation that will be used for creating the next annotation or annotation element. A current annotation orientation refers to the annotation orientation of an annotation or Annotation Element that is placed.
The gallery on the Annotate tab in the Annotation Orientations group displays the annotation orientations in a model. When you move the pointer over the annotation orientations in the gallery, the annotation grid plane turns green in the graphics area. To define an active annotation orientation, you can select an annotation orientation from the gallery.
Alternatively, using the ANNOTATION PLANE MANAGER dialog box or the ANNOTATION PLANE dialog boxes, you can define an annotation orientation using a datum plane, flat surface, or named view. You can also define annotation orientations such that they are placed flat to screen and also switch between these different types of annotation orientations.
The ANNOTATION PLANE MANAGER dialog box opens when on the Annotate tab, in the Annotation Orientations group you click the dialog box launcher .
The ANNOTATION PLANE dialog box opens when you right-click an annotation and click Current Orientation on the shortcut menu.
Note the following points about annotation orientations:
• Define the active annotation orientation, if required, before creating the first annotation in any session. This annotation orientation is retained per session per model. Thus, when you define the active annotation orientation and create a new annotation or Annotation Element, Creo Parametric retains that annotation orientation and uses it to create the next annotation. All subsequently created annotations retain the same orientation unless the Annotation plane information is changed. This holds true for new Annotation Elements created in new Annotation Features as well.
• The default annotation orientation is a frozen orientation in the Z-direction of the default coordinate system. This default annotation orientation corresponds to the FRONT datum plane or FRONT orientation in the PTC template for parts. However, this default orientation does not reference the FRONT datum or FRONT view. In the ANNOTATION PLANE MANAGER dialog box, the default orientation is defined by the view. However, view name is not specified.
• When redefining an existing annotation, if you change its annotation orientation, the changed definition of the annotation orientation is not retained for the next created annotation.
• If you delete or suppress a datum plane or named orientation that defines the annotation plane in an annotation, the next annotation orientation is frozen.
• If an annotation cannot be placed on the current annotation orientation, then Creo Parametric displays a message stating that the annotation plane is invalid and that a new annotation plane must be defined.
• If the last created Annotation Element created a datum plane for its annotation plane, thus creating an embedded datum, then the next created Annotation Element in the same Annotation Feature uses the same orientation as the Annotation Element with the embedded datum plane. If the next created Annotation Element is in another Annotation feature, then the Annotation Element does not directly reference the embedded datum plane.
• When you open the ANNOTATION PLANE MANAGER or ANNOTATION PLANE dialog box, the current or active annotation plane is visible as a grid plane. The active annotation grid plane is displayed in green, that is, the Highlight-Edge system color while the annotation orientation of an existing annotation is displayed in orange, that is, Secondary Selected system color. Both grid planes show viewing direction and text direction.