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Dimensions Overview

Dimensions in a SolidWorks drawing are associated with the model, and changes in the model are reflected in the drawing.

Model Dimensions. Typically, you create dimensions as you create each part feature, then insert those dimensions into the various drawing views. Changing a dimension in the model updates the drawing, and changing an inserted dimension in a drawing changes the model.

Mark for Drawings. When creating dimensions, you can specify whether the dimension should be included when inserting model dimensions into drawings. Right-click the dimension and select Mark For Drawing. You can also specify that dimensions marked for drawings be inserted automatically into new drawing views. Select Dimensions marked for drawing under Auto insert on view creation in Document Properties - Detailing.

Reference Dimensions. You can also add dimensions in the drawing document, but these are reference dimensions, and are driven; you cannot edit the value of reference dimensions to change the model. However, the values of reference dimensions change when the model dimensions change.

Standard Dimensions. You can create standard dimensions in drawings, such as dimensions created in a sketch. This includes Smart, Horizontal, and Vertical dimensions.

Rapid Dimension. Use rapid dimensioning to place evenly spaced dimensions.

Color. By default, model dimensions are black. This includes dimensions that are blue in the part or assembly document (such as the extrusion depth). Reference dimensions are gray and appear with parentheses by default. You can specify colors for various types of dimensions in Tools, Options, System Options, Colors and specify Add parentheses by default in  Document Properties - Dimensions.

Arrows. Circular handles appear on dimension arrows when dimensions are selected. When you click on an arrowhead handle (on either handle if there are two for the dimension), the arrows flip outside or inside. When you right-click on a handle, a list of arrowhead styles appears. You can change the style of any dimension arrowhead individually by this method.

Flipping the arrows

Changing the arrowhead style

Selection. You can select dimensions by clicking anywhere on the dimension, including dimension and extension lines and arrows.

Hide and Show Dimensions. You can hide and show dimensions with Hide/Show Annotations on the Annotation toolbar or View menu. You can also right-click a dimension and select Hide to hide the dimension. You can also hide and show dimensions in annotation views. To show dimension names, click View > Dimension Names or Hide/Show Items > View Dimension Names (Heads-Up View toolbar).

Formatting. The dimension palette appears when you insert or select a dimension so you can easily change the dimension's properties and formatting. You can change the tolerance, precision, style, text, and other formatting options in the palette without going to the PropertyManager.

Hide and Show Lines. To hide a dimension line or extension line, right-click the line and select Hide Dimension Line or Hide Extension Line. To show hidden lines, right-click the dimension or a visible line and select Show Dimension Lines or Show Extension Lines.

Radius and Diameter Displays. You can change a dimension to diameter, radius, or linear display. On screen, right-click a radius or diameter dimension and select:

Display As Diameter. This example is shown without the second arrow. Click Use document second arrow to display both arrows.

Display As Radius

Display As Linear. Sets the dimension to linear style (for diameter dimensions only.)

You can right-click and select the above options only when you first create the dimension. If you edit the dimension later on, right-click the dimension and select Display Options, then select an option above.

Slant. When you insert or select dimensions, handles appear so you can drag the dimension to slant the extension lines.

Display Options. Right-click a dimension and select Display Options. The choices available depend on the type of dimension and other factors and can include the following:

  • Remove Slant

  • 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.

  • Change Plane

  • Align Ordinate

  • Jog

  • Re-Jog Ordinate

  • Show Parentheses. You can display driven (reference) dimensions with or without parentheses. They are displayed with parentheses by default.

  • Show as Inspection

  • Display As Diameter

  • Display As Radius

  • Display As Linear

Link external dim text. If you insert text into a dimension in a drawing, this option inserts the text into the dimension in the part or assembly as well. Right-click the top-level icon in the drawing's FeatureManager design tree and select Link external dim text to allow dimension text to propagate back to the part or assembly.

When linking text between an assembly and a drawing, the dimension in the drawing must have been inserted with the Model Items tool.

Related Topics

Baseline dimensions

Ordinate dimensions

Modifying dimensions

Moving and copying dimensions

Dimension Value PropertyManager

Creating jogs in dimension extension lines

Adding multiple jogs to radius, diameter, chamfer, or hole callout dimensions

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