DimXpert Value PropertyManager

To set the default tolerance and precision values:

Click Options > Document Properties > DimXpert.

Reference Features

	Tolerance Feature	The top plane P2. For size dimensions, only Tolerance Feature appears in the PropertyManager.
	Origin Feature	The bottom plane P1. See ASME Y14.5M -1994, Paragraph 2.6.1 or ISO 129 for information regarding origin and toleranced features.
	Swap Features
	Examples Using Different Origin Features: Origin Feature = the bottom plane P1. Origin Feature = the top plane P2. The origin symbol, in place of the arrowhead, denotes the origin feature. Note the different dimension results.

DimXpert Direction

This option appears when you apply a dimension between two axis- or line-type features. The X, Y, and Z options are relative to the part coordinate system and are enabled for each part axis that is perpendicular to the axes of the features.

The axis of the features is along Z, which enables the X and Y options.
The normal option N orients the dimension along the direction defined by the shortest distance between the two features.
The user-defined option U orients the dimension along a direction parallel to an edge or normal to a planar face. In this example, the dimension is oriented parallel to an edge.

Style

See Style for details.

Tolerance/Precision

	Callout value	For hole type callouts with multiple specifications, all dimensions are listed individually. This functionality is valid for simple holes with depth, counterbore holes, countersink holes, combined slot dimensions, and chamfers.
	Tolerance Type	Select from the list. Selections available depend on the type of dimension.
	Maximum Variation
	Minimum Variation
	Show parentheses	Inserts parentheses around the tolerance value.
	Unit Precision	Select the number of digits after the decimal point from the list for the dimension value.
	Tolerance Precision	Select the number of digits after the decimal point for tolerance values.
For Holes and Shafts:
	Classification	(Fit, Fit with tolerance, or Fit (tolerance only)) When you select either Hole Fit or Shaft Fit (below), the list for the other category (Hole Fit or Shaft Fit) is filtered based on the classification.
	Hole Fit and Shaft Fit	(Fit, Fit with tolerance, or Fit (tolerance only)) Select from the lists, or type any text. Bilateral tolerances (Maximum Variation and Minimum Variation) are available in the Fit with tolerance or Fit (tolerance only) type if you specify Hole Fit or Shaft Fit, but not both.
	Fit tolerance display	(Fit, Fit with tolerance, or Fit (tolerance only)) Select one of the following: Stacked with line display Stacked without line display Linear display

Primary Value

This option is read-only. It displays the dimension name and value.

Dimension Text

	Instance Count	For patterns, this shows the number of instances.
	Add Parentheses	You can display driven (reference) dimensions with or without parentheses. They are displayed with parentheses by default.
	Center Dimension	When you drag dimension text between the extension lines, the dimension text snaps between the center of the extension lines.
	Inspection Dimension
	Offset Text	Offsets dimension text from the dimension line using a leader.
	Text	The dimension appears automatically in the center text box, represented by <DIM>. Place the pointer anywhere in the text box to insert text. Holes use the format specified in the txcalloutformat.txt file. See DimXpert Size Dimension, Callout format file, for more information.
	Justify	You can justify text horizontally and, for some standards, you can justify the leader vertically. Left Justify , Center Justify , Right Justify . Top Justify , Middle Justify , Bottom Justify .
	Symbols	Click to place the pointer where you want a symbol. Click a symbol icon or click More to access the Symbol Library. Use caution when adding symbols to DimXpert dimensions because the symbols may change the fundamental definition of the dimensions and tolerances.

Dual Dimension

Specifies that the dimension is displayed in both the document's unit system and the dual dimension units. Both units are specified in Tools > Options > Document Properties > Units.

	Unit Precision	Select the number of digits after the decimal point from the list for the dimension value.
	Tolerance Precision	Select the number of digits after the decimal point for tolerance values.