Dimension Value PropertyManager

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 currently 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.

Dimension Text

	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 to 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. 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 text 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.
	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 Center Justify Right Justify Top Justify , Middle 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.
	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.