Dimension Value PropertyManager

In the Dimension Value PropertyManager, you can specify the display of dimensions. If you select multiple dimensions, only the properties that apply to all the selected dimensions are available.

To open this PropertyManager:

Select one or more dimensions.

If you select multiple dimensions, only the properties that apply to all the selected dimensions are available.

Dimension Assist Tools

Allows you to dimension a drawing with Smart or DimXpert (for drawings) dimensioning. Click DimXpert to access the DimXpert (for drawings) and Autodimension tabs.

Smart dimensioning Lets you create dimensions with the Smart Dimension tool.
Rapid dimensioning Lets you enable or disable the rapid dimension selector. Select to enable; clear to disable. This setting persists across sessions.
DimXpert Lets you apply dimensions to fully define manufacturing features (patterns, slots, pockets, fillets, etc.) and locating dimensions, using DimXpert for drawings.

Style

Style

Tolerance/Precision

  Callout value Choose a value in the selected dimension. This is available for dimensions with multiple values in the callout.
Tolerance Type Select from the list. Selections available depend on the type of dimension. See Examples of Dimension Tolerance and Precision.
Maximum Variation  
Minimum Variation  
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.
  Link precisions with model For imported dimensions, sets changes in unit or tolerance precision to be parametric with the model.
  Configurations (Parts and assemblies only.) Applies the dimension tolerance to specific configurations for driven dimensions only.
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).)

Stacked with line display

Stacked without line display

Linear display

  Show parentheses Parentheses are available for Bilateral, Symmetric, and Fit with tolerance tolerance types. Parentheses are available for Fit with tolerance if you specify Hole Fit or Shaft Fit, but not both.

2nd Tolerance/Precision

Available for chamfer dimensions. See Inserting Chamfer Dimensions into Drawings.

Primary Value

Primary Value is displayed for driving dimensions and can be changed to alter the model. You can override the dimension value. For dimensions that are not referenced, you can change the dimension name. Driven (reference) dimensions list a value and name, but you cannot change them.

  Name The name of the selected dimension.
  Dimension value The value of the selected dimension.
  Override value Select to override the primary value, and type a new value. If you clear Override value, the dimension returns to its original value but retains the tolerance. Override values do not automatically update when geometry changes.
Original value
Overridden value
Reverse Direction Change the dimension direction between positive and negative sense.
  Configurations (Parts and assemblies only.) Applies the Primary Value data to specific configurations.

Dimension Text

  Text The dimension appears automatically in the box, represented by <DIM>. Place the pointer anywhere in the box to insert text. If you delete <DIM>, you can reinsert the value by clicking Add Value (XX.XX).

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.

For ISO Drafting Standard dimensions with solid leader and aligned text, you can use the Dimension Text field to place text above and below dimension lines, or split dual-dimension text above and below dimension lines for linear, diameter, and radius dimensions. You can split text only if the Text Position is set to Solid Leader, Aligned Text in Tools > Options > Document Properties > Dimensions for the dimension. Use the second box to place text under the solid dimension line. Parenthesis and inspection outline may be applied to the top and bottom independently from each other.

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 to the center of the extension lines.

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

  Reverse callout order

Reverses the callout order for holes created with the Advanced Hole tool.

Reverse Callout Order selected


Reverse Callout Order cleared
You can define the callout in the feature by including additional text. Type the text to include in Text Above and Text Below.

  Switch near and far side messages Select to switch the near and far side text strings.
  Justify You can justify text horizontally and, for some standards, you can justify the leader vertically.
  • Left Justify , Center Justify , Right Justify
Left Justify
 
 
Right Justify
  • Top Justify , , Bottom Justify
Top Justify
Middle Justify
Bottom Justify
  Symbols Click to place the pointer where you want a standard symbol. Click a symbol icon or click More to access the Symbol Library. See Using the Symbol Library.

  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.
  Chamfer Dimension Display

Distance X Distance

Distance X Angle

Angle X Distance

C Distance

Available only for chamfers with 45° angles.

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 Document Properties - Units . You set where the alternate units are displayed in Document Properties - Dimensions . Dual dimensions are displayed in brackets.

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.
  Link precisions with model For imported dimensions, sets changes in unit or tolerance precision for the secondary units to be parametric with the model.
  Inward rounding Controls the inward rounding for each individual dimension.
  Split Select to set new dimensions with dual dimensions to display split above and below the unbroken dimension line. You can split text only if the Text Position is set to Solid Leader, Aligned Text in Tools > Options > Document Properties > Dimensions for the dimension.