DimXpert Size Dimension
Use the DimXpert Size Dimension tool 
to place tolerance size dimensions on DimXpert features. In the following procedure you dimension a simple hole.
To use the DimXpert Size Dimension tool:
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Click Size Dimension (DimXpert toolbar) or Tools, DimXpert, Size Dimension.
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Select the face of the feature to dimension.
To define a width feature, you can also select a linear edge bounded by two parallel planes that are perpendicular to the edge. Edge selection is only supported for width features. 
The Feature Selector appears in the graphics area with a default feature type selected. If necessary, select a different type of feature in the feature selector.
Use the appropriate feature selector option when defining a new width or compound hole from multiple faces.
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Click to place the dimension. 
The DimXpert PropertyManager appears. The selected feature is listed as Tolerance Feature 
under Reference Features.
In general, you can attach dimensions to any edge of the feature or to any pattern instance. Select the dimension and use its drag handle to reposition the dimension.
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Set the PropertyManager options and click 
.
The DimXpertManager updates to include the feature and dimension type.
Notes
Default Tolerance values. Set the tolerance values in Tools, Options, Document Properties, DimXpert, Size Dimension.
Pattern features. DimXpert recognizes many patterns and defines instance counts automatically. The format is defined in the DimXpert callout format file. If DimXpert does not automatically recognize pattern features, you can define them using the DimXpert Pattern Feature tool.
Callout format file. Some dimensions are displayed using a callout format. A template file (
txcalloutformat.txt
) that defines this format is found under Tools, Options, System Options, File Locations, DimXpert Callout Format File. The template lets you define individual formats for each dimensioning standard.
Grouping. When the selected feature is defined as a datum or is controlled by a geometric tolerance, the size dimension, datum feature symbol, and geometric tolerance are automatically combined into an annotation group.
Depth Dimensions. Depth dimensions are applied to blind features only. Other criteria, such as the geometry bounding the top of the feature and the geometry of the blind end condition, can affect whether a depth dimension is created.
Threaded holes. When a hole is threaded, the thread designation is used instead of the hole diameter and tolerance. This is true for hole types defined with the Hole Wizard or linked to a cosmetic thread.
Supported Features
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Feature
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Example and Dimension Type
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Notes
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Boss
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Diameter
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Chamfer
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Angle-distance
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Distance-distance
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DimXpert dimensions SolidWorks chamfers with the method used to define them.
Chamfers recognized by their topology are dimensioned Distance-Distance.
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Cone
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A set of external or internal cones must have the same included angle and lie on a common plane.
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Cylinder
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Radius
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Feature
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Example and Dimension Type
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Notes
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Fillet
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Radius
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Intersect Circle
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A circle derived at the intersection of a cone and plane. The cone must be perpendicular to the plane, and it cannot be created from an ellipse. The cone and plane can be interrupted by a fillet or chamfer.
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Counterbore Hole
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Countersink Hole
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Feature
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Example and Dimension Type
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Notes
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Simple Hole
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Diameter and depth (when blind), or thread designation and depth (when blind)
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Notch
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Length, width, and depth (when blind)
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Slot
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Length, width, and depth (when blind)
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Specify the dimension type in the DimXpert options dialog box.
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Width
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Width
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Feature
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Example and Dimension Type
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Notes
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Sphere
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