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Creating Driven Dimensions

You can create additional dimensions within a drawing, as
needed, if a dimension is not available to be shown or as
company standards dictate.
• Driven dimension types include:
– Linear
– Angular
– Radial/Diameter
– Point-Point
• Add additional text:
– Prefix
– Suffix

Creating Driven Dimensions 2
Figure 2 – Viewing Created
Dimension Types
Creating Driven Dimensions

Creating Driven Dimensions 1
Figure 1 – Created Dimensions
versus Shown Dimensions
A driven dimension is created by the user. This type of dimension reports a
value based upon the references selected when the dimension is created.
The dimension value is driven by the geometry selected, and therefore it is
not possible to modify the value of a driven dimension. A driven dimension
does not pass back to the model; it appears only within the drawing. A
created dimension displays in the drawing tree differently than that of a
shown dimension. In Figure 1, the dimensions in the front view are created
dimensions, while the dimensions in the top view are shown dimensions.
You can create a Standard driven dimension by selecting Dimension – New
References
from the Dimension types drop-down menu in the Annotate
tab, or by right-clicking and selecting Dimension – New References. The
system creates a dimension based upon one or two selected references,
similar to how you create dimensions in Sketcher. The dimension’s witness
lines automatically clip to their selected references.
Standard driven dimension types include linear, angular, radial, diameter, or
point-point dimensions.
When creating a driven dimension, you can select an edge, edge and point,
two points, or a vertex. You can further filter which entities the dimension
attaches to using the following attach type menu commands in the menu
manager:
• On Entity – Attaches the dimension to the entity at the pick point, according
to the rules of creating regular dimensions.
• On Surface – Attaches the dimension to the location selected on a surface.
• Midpoint – Attaches the dimension to the midpoint of the selected entity.
• Center – Attaches the dimension to the center of a circular edge. Circular
edges include circular geometry, such as holes, rounds, curves, and
surfaces, and circular draft entities.
• Intersect – Attaches the dimension to the closest intersection point of two
selected entities.
• Make Line – References the current X and Y-axes in the orientation of
the model view.
Depending upon the selected references, you may have to further specify the
type of dimension to be created. For example, you may be asked to specify
whether the dimension you create is to be Horizontal, Vertical, Slanted,
Parallel, or Normal to the selected references. If your selected references
are arcs or circles, you must specify whether the dimension is to be created
between the arc Centers, Tangent, or Concentric.
Adding Prefix and Suffix Text
You can add additional text to a dimension. Text can be added as a prefix or
a suffix to the dimension value. For example, if a radius dimension is typical
of all radii on the part, you can add the suffix TYP to the dimension.

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