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.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 in part sketches, 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. Click Tools, Options, Document Properties, Detailing and select Dimensions marked for drawing under Auto insert on view creation.
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.
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 Tools, Options, 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.
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.
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 in the Dimension Properties dialog box or on screen. On screen, right-click a radius or diameter dimension and select:
Display As Diameter
Display As Radius
Display As Linear
You can right-click
and select the above options only when you first create the dimension.
If you edit the sketch 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
Offset Text
Change Plane
Align Ordinate
Jog
Re-Jog Ordinate
Show Parentheses
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.