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,
You can control the color of reference dimensions in Tools, Options, System Options,
. 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.