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 Design CheckerDesign Checker
Expand Design Studies in SolidWorksDesign Studies in SolidWorks
Collapse Drawings and DetailingDrawings and Detailing
Expand Detailing OverviewDetailing Overview
Expand AnnotationsAnnotations
Expand TablesTables
Expand Bill of Materials (BOM)Bill of Materials (BOM)
Expand Table Columns and RowsTable Columns and Rows
Adding Symbol Text to BOM or Table Cells
Expanding Tables
Expand Equations in TablesEquations in Tables
Expand Drafting StandardsDrafting Standards
Expand Print SettingsPrint Settings
Collapse DrawingsDrawings
Drawings Overview
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
Expand Drawing View Alignment and DisplayDrawing View Alignment and Display
Expand Drawing ToolsDrawing Tools
Expand Drawing OutputsDrawing Outputs
Expand Title Block ManagementTitle Block Management
Expand Print OptionsPrint Options
Collapse Dimensions in DrawingsDimensions in Drawings
Dimensions Overview
Inserting Dimensions into Drawings
Dimension Type
Dimensions Options
Aligning Dimensions and Notes
Dimension Alignment: Parallel/Concentric
Dimension Alignment: Collinear/Radial
Rapid Dimension
Autodimension
DimXpert
Parallel Dimensions
Reference Dimensions
Baseline Dimensions
Expand Ordinate DimensionsOrdinate Dimensions
Chamfer Dimensions
Expand Tolerance and PrecisionTolerance and Precision
Moving and Copying Dimensions
Modifying Dimensions
Deleting Dimensions
Expand Dimension PaletteDimension Palette
Extension Lines
Attaching Dimension Extension Lines
Hide/Show Dimensions
Dimensioning to Midpoints
Using Snap Options to Move Dimension Extension Lines
Jogging Extension Lines
Creating Jogs in Dimension Extension Lines
Multiple Jogs for Dimensions and Callouts
Expand DFMXpressDFMXpress
Expand DriveWorksXpressDriveWorksXpress
Expand FloXpressFloXpress
Expand Import and ExportImport and Export
Expand Large Scale DesignLarge Scale Design
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 ToolboxToolbox
Expand WeldmentsWeldments
Expand Workgroup PDMWorkgroup PDM
Expand TroubleshootingTroubleshooting
Expand GlossaryGlossary
Hide Table of Contents

Ordinate Dimensions

Ordinate dimensions are a set of dimensions measured from a zero ordinate in a drawing or sketch. In drawings, they are reference dimensions and you cannot change their values or use the values to drive the model.

Ordinate dimensions are measured from the axis you select first. The type of ordinate dimension (horizontal or vertical) is defined by the orientation of the points you select.

You can dimension to edges, vertices, and arcs (centers and minimum and maximum points). You can also dimension to midpoints when you add ordinate dimensions.

Ordinate dimensions are automatically grouped to maintain alignment. When you drag any member of the group, all the members move together. To disconnect a dimension from the alignment group, right-click the dimension, and select Break Alignment.

You can drag the zero dimension to a new position, and all the ordinate dimensions update to match the new zero position.

If adjacent dimensions are very close together, the leaders are automatically jogged as needed to prevent overlapping text. Drag handles are displayed at the bends when you select an ordinate dimension with a bent leader. You can remove the bend, or add a bend to a different ordinate dimension.

You can set ordinate dimension document properties in Document Properties - Ordinate Dimensions. You can specify that the leaders not be automatically jogged by clearing Automatically jog ordinates.

To create ordinate dimensions:

  1. Click Ordinate Dimension on the Dimensions/Relations toolbar, or click Tools, Dimensions, Ordinate.

    You can select Horizontal Ordinate Dimension or Vertical Ordinate Dimension to specify the direction of the dimensions.

  2. Click the first item (edge, vertex, and so on) from which all others will be measured to be the base (the 0.0 dimension), and click again to place the dimension outside the model.

  3. Click the edges, or vertices, or arcs you want to dimension using the same ordinate. As you click each item, the dimension is placed in the view, aligned to the zero ordinate.

  4. Select another mode or another tool or press Esc to exit from the ordinate mode.

To add more dimensions along the same ordinate:

  1. Right-click an ordinate dimension, and select Add To Ordinate.

  2. Click the edges, or vertices, or arcs you want to dimension using the same ordinate. As you click each item, the dimension is placed in the view, aligned to the zero ordinate.

  3. Select another mode or another tool or press Esc to exit from the ordinate mode.

To modify ordinate dimensions:

You can modify ordinate dimensions using commands on the shortcut menu. Right-click an ordinate dimension, select Display Options, then choose from these options:

  • Align Ordinate. Aligns all the dimensions along the ordinate with the 0.0 ordinate.

  • Jog. Bends the leader line of a dimension and allows you to reposition the dimension.

  • Re-Jog Ordinate. Applies the automatic jogging algorithm to the ordinate dimensions.

  • Show Parentheses. Adds parentheses around the selected dimensions.

  • Show as Inspection. Shows the selected dimensions as inspection dimensions.

To display as chain dimensions:

  1. Select an ordinate dimension.

  2. Click the Leader tab and select Ordinate chain.

  3. Click .

Select  Display as chain dimension in Document Properties - Ordinate Dimensions to chain all ordinate dimensions in the drawing.



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

 
*Email:  
Subject:   Feedback on Help Topics
Page:   Ordinate Dimensions
*Comment:  
*   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:




x

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
x

Web Help Content Version: SOLIDWORKS 2011 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.