Create drawings from models (Creo Elements/Direct Annotation) > Modify drawings > Add and modify dimensions > Projected dimension reference points
Projected dimension reference points
When creating dimensions on a view, it is occasionally necessary to specify a dimension reference point that does not physically lie on the view. For example, a blend in a 3D model will appear as a fillet in the Creo Elements/Direct Annotation view, but you may want to dimension from the original vertex of the pre-blended geometry.
In these cases, it is necessary to project the two lines that define the vertex to their point of intersection. In Creo Elements/Direct Annotation you can create a special projected reference point marker at the projected intersection point of two straight lines. The lines of projection are also shown in the geometrical marker.
Projected reference points and their markers are associated with the base geometry used to define them. When this geometry is modified or deleted, you can update the reference points, manually or automatically, to reflect the changes.
The appearance of the markers is controlled by a set of parameters. The settings are valid for all projected reference points, new or existing, so that they can be easily distinguished.
When you delete reference points and markers, any dimensions attached to them are also deleted.
In this section:
Limitations and restrictions
You can project only linear geometry.
The base geometry must ultimately be owned by a view.
The marker that appears is neither a sketch nor a symbol, and cannot be acted upon with the sketch and symbol commands.
Create projected reference points
1. Click Annotation and then, in the Annotate group, click the arrow next to Proj Ref Pnt.
2. Click Create Ref point.
3. Select the first geometry line to project.
4. Select the second geometry line.
5. Creo Elements/Direct Annotation projects the lines to their point of intersection, and draws a marker to indicate the projection lines and projected reference point. You can now select this point for dimension references.
Update projected reference points
When the geometry associated with a projected dimension reference point is modified, the projected point may no longer be valid. However, you can update the point to correct its positioning. Creo Elements/Direct Annotation briefly highlights all projected points on the sheet, and then corrects those that have changed. Any points that cannot be repaired (for example, if associated geometry has been deleted) remain in the color for lost geometry. It is also possible to have projected reference points updated automatically after a view update. Note that all projected points are updated on the drawing, not just those attached to the views that have been updated. You can switch between manual and automatic update of projected points in the PRP Attributes menu.
An update operation acts on all projected reference points in the drawing.
All dimensions referring to projected reference points are updated when the reference points are updated.
If projected reference points are not set to be updated automatically after view updates, you will need to update the points manually to correct any whose associated geometry has changed. Until such an update, it is possible that some dimensions are incorrect.
To update projected reference points manually:
1. Click Annotation and then, in the Annotate group, click the arrow next to Proj Ref Pnt.
2. Click Update Ref point.
All reference points on the sheet blink briefly, and Creo Elements/Direct Annotation adjusts all points in the drawing that refer to modified associative geometry.
If a projected reference point's associated view geometry is changed, but the PRP Update Behavior is set to Manual, you will still need to use the PRP Update command to correct the reference point. It is therefore possible that directly after a view update, not all dimensions are correct until a PRP update is effected.