DimXpert Value PropertyManager

In the DimXpert Value PropertyManager, you specify the display of dimensions and tolerances.

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. See
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.
See

Style

Style for details.

Tolerance/Precision

  Tolerance Modifier Applies ISO 14405-1:2016 standards-based symbols to dimensions and tolerances in DimXpert.

You can add symbols and other text directly to ISO dimensions and their tolerances.
  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.

  Show as half angle Displays a conical angle dimension as a half angle. This lets you convert a full angle of a cone to a half angle.

Dimension Text

  Instance Count For patterns, this shows the number of instances.
  Text The dimension appears automatically in the box, represented by <DIM>. Place the pointer anywhere in the box to insert text.
Holes use the format specified in the txcalloutformat.txt file. See DimXpert Size Dimension, Callout format file, for more information.
For some types of dimensions, additional text appears automatically. For example, a Hole Callout for a counterbore hole displays the diameter and depth of the hole (<MOD-DIAM><DIM><HOLE-DEPTH>xx). Hole Callouts for holes created in the Hole Wizard display information from the Hole Wizard. You can edit the text and insert variables from the Callout Variables dialog box.
Add Parentheses You can display driven (reference) dimensions with or without parentheses. They are displayed with parentheses by default.

Inspection Dimension
Center Dimension When you drag dimension text between the extension lines, the dimension text snaps between the center of the extension lines.

Offset Text Offsets dimension text from the dimension line using a leader.

  Justify You can justify text horizontally and, for some standards, you can justify the leader verticIn descriptally.
  • 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 Symbols 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.
  All uppercase For the selected dimension or hole callout, displays the text in all uppercase in the graphics area. Clear the option to return to mixed case.

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.