Expand IntroductionIntroduction
Expand AdministrationAdministration
Expand User InterfaceUser Interface
Expand SolidWorks FundamentalsSolidWorks Fundamentals
Expand Moving from 2D to 3DMoving from 2D to 3D
Expand AssembliesAssemblies
Expand CircuitWorksCircuitWorks
Expand ConfigurationsConfigurations
Expand SolidWorks CostingSolidWorks Costing
Expand Design CheckerDesign Checker
Expand Design Studies in SolidWorksDesign Studies in SolidWorks
Collapse Detailing and DrawingsDetailing and Drawings
Detailing Overview
Setting Detailing Options
Model Items
Model Items PropertyManager
Expand SolidWorks eDrawings MarkupsSolidWorks eDrawings Markups
Expand StyleStyle
Add or Update a Style
Expand AnnotationsAnnotations
Expand TablesTables
Expand Bill of Materials (BOM)Bill of Materials (BOM)
Expand Drafting StandardsDrafting Standards
Expand Print SettingsPrint Settings
Collapse DrawingsDrawings
Expand Getting Started in DrawingsGetting Started in Drawings
Expand Types of Drawing DocumentsTypes of Drawing Documents
Expand Standard Drawing ViewsStandard Drawing Views
Expand Derived Drawing ViewsDerived Drawing Views
Multiple Views PropertyManager
Convert View to Sketch PropertyManager
Expand Drawing View Alignment and DisplayDrawing View Alignment and Display
Drawing Statistics
Printing Drawings
Send Mail
Expand Title Block ManagementTitle Block Management
Collapse Dimensions in DrawingsDimensions in Drawings
Formatting Dimensions in Drawings
Dimensions Display Options
Hide/Show Annotations
Expand Highlighting Changed DimensionsHighlighting Changed Dimensions
Inserting Dimensions into Drawings
Dimension Type
Document Properties - Dimensions
Dimension Other PropertyManager
Dimension Value PropertyManager
Dimension Precision
Expand Aligning Dimensions and NotesAligning Dimensions and Notes
Scan Equal
Rapid Dimension
Expand Autodimension a DrawingAutodimension a Drawing
Dimension PropertyManager
Adding Parallel Dimensions to Drawings
Reference Dimensions
Reference Center of Mass in Drawings
Using Parentheses on Particular Dimensions
Baseline Dimensions
Expand Ordinate DimensionsOrdinate Dimensions
Chamfer Dimensions
Expand Tolerance and PrecisionTolerance and Precision
Moving and Copying Dimensions
Modify Dimension
Deleting Dimensions
Expand Dimension PaletteDimension Palette
Expand Dimension Extension LinesDimension Extension Lines
Expand Dimension Leaders/TextDimension Leaders/Text
Example: Dimension Scheme Types
Dimensioning to Midpoints
Expand DFMXpressDFMXpress
Expand DriveWorksXpressDriveWorksXpress
Expand FloXpressFloXpress
Expand Import and ExportImport and Export
Expand Model DisplayModel Display
Expand Mold DesignMold Design
Expand Motion StudiesMotion Studies
Expand Parts and FeaturesParts and Features
Expand RoutingRouting
Expand Sheet MetalSheet Metal
Expand SimulationSimulation
Expand SimulationXpressSimulationXpress
Expand SketchingSketching
Expand Sustainability ProductsSustainability Products
Expand SolidWorks UtilitiesSolidWorks Utilities
Expand TolerancingTolerancing
Expand TolAnalystTolAnalyst
Expand ToolboxToolbox
Expand WeldmentsWeldments
Expand Workgroup PDMWorkgroup PDM
Expand TroubleshootingTroubleshooting
Hide Table of Contents

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.

Dimension Assist Tools

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

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




  Callout value Choose a value in the currently selected dimension. This is available for dimensions with multiple values in the callout.
PM_tolerance_type_dim.gif Tolerance Type Select from the list. Selections available depend on the type of dimension. Examples of Dimension Tolerance and Precision
PM_max_variation_dim.gif Maximum Variation  
PM_min_variation_dim.gif Minimum Variation  
PM_precision_dim.gif Unit Precision Select the number of digits after the decimal point from the list for the dimension value.
PM_dim_precision_tol.gif 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.
PM_dim_tol_fit_class.gif 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.
PM_dim_tol_hole.gif PM_dim_tol_shaft.gif 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 PM_dim_tol_fit_withline.gif

Stacked without line display PM_dim_tol_fit_stacked.gif

Linear display PM_dim_tol_fit_linear.gif

  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.

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
PM_reverse_direction.gif Reverse Direction Change the dimension direction between positive and negative sense.

Dimension Text

PM_AddParenthesis.gif Add Parentheses You can display driven (reference) dimensions with or without parentheses. They are displayed with parentheses by default.
PM_CenterDim.gif Center Dimension When you drag dimension text between the extension lines, the dimension text snaps to the center of the extension lines.
PM_InspectionDim.gif Inspection Dimension Dimension_Inspection.gif
PM_OffsetText.gif 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 PM_add_value.gif.
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.
  Justify You can justify text horizontally and, for some standards, you can justify the leader vertically.
  • Left Justify PM_Text_Justify_Left.gif, Center Justify PM_Text_Justify_Center.gif, Right Justify PM_Text_Justify_Right.gif
Left Justify
Center Justify
Right Justify
  • Top Justify PM_dim_Justify_Top.gif, Middle Justify PM_dim_Justify_Middle.gif, Bottom Justify PM_dim_Justify_Bottom.gif
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.
  Chamfer Dimension Display

Distance X Distance PM_dim_chamfer_DXD.gif

Distance X Angle PM_dim_chamfer_DXA.gif

Angle X Distance PM_dim_chamfer_AXD.gif

C Distance PM_dim_chamfer_C.gif

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.

PM_precision_dim.gif Unit Precision Select the number of digits after the decimal point from the list for the dimension value.
PM_Tol_Precision_DualDim.gif 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.

Provide feedback on this topic

SOLIDWORKS welcomes your feedback concerning the presentation, accuracy, and thoroughness of the documentation. Use the form below to send your comments and suggestions about this topic directly to our documentation team. The documentation team cannot answer technical support questions. Click here for information about technical support.

* Required

Subject:   Feedback on Help Topics
Page:   Dimension Value PropertyManager
*   I acknowledge I have read and I hereby accept the privacy policy under which my Personal Data will be used by Dassault Systèmes

Print Topic

Select the scope of content to print:


We have detected you are using a browser version older than Internet Explorer 7. For optimized display, we suggest upgrading your browser to Internet Explorer 7 or newer.

 Never show this message again

Web Help Content Version: SOLIDWORKS 2013 SP05

To disable Web help from within SOLIDWORKS and use local help instead, click Help > Use SOLIDWORKS Web Help.

To report problems encountered with the Web help interface and search, contact your local support representative. To provide feedback on individual help topics, use the “Feedback on this topic” link on the individual topic page.