Reference Dimensions
Reference dimensions show measurements of the model, but they do not
drive the model and you cannot change their values. However, when you
change the model, the reference dimensions update accordingly.
Reference dimensions are enclosed in parentheses by default (except
ordinate dimensions). To prevent parentheses around reference dimensions,
clear the Add parentheses by default
check box in Tools, Options,
Document Properties, Dimensions.
You can control the color of reference dimensions in Tools,
Options, System
Options, Colors.
Select Dimensions, Non Imported (Driven)
and click Edit.
You can use the same methods to add parallel, horizontal, and vertical
reference dimensions to a drawing as you use to dimension sketches. For
more information, see Dimensioning
in Sketches.
Ordinate
Dimensions and Baseline Dimensions
are both types of reference dimensions in drawings. Ordinate and baseline
dimensions in sketches are driving dimensions.
Reference dimensions are automatically hidden when a feature is suppressed.
The dimensions are shown again when the feature is unsuppressed.
To add a reference dimension:
Click Smart
Dimension 
(Dimensions/Relations
toolbar) or click Tools, Dimensions, Smart.
-
In a drawing view, click the items you want to dimension.
You can dimension to a silhouette edge.
Point to the silhouette edge, and when the 
pointer appears,
click to dimension.
Use rapid
dimensioning to place evenly spaced dimensions. Alternatively, move
the pointer outside of the rapid dimension manipulator to place the dimension.
To change the alignment of a reference dimension:
You can change the alignment of a reference
dimension if its references are vertices or hole centers.
Right-click the dimension and select Set
Horizontal, Set Vertical,
or Align to edge.
If you selected
Align to edge, select an edge.