Dimensioning a 2D Sketch

You dimension 2D or 3D sketch entities with the Smart Dimension tool. You can drag or delete a dimension while the Smart Dimension tool is active.

Dimension types are determined by the sketch entities you select. For some types of dimensions (point-to-point, angular, circular), the location where you place the dimension also affects the type of dimension that is added.
You can create features without adding dimensions to sketches. However, it is good practice to dimension sketches. Dimension in accordance with the model's design intent; for example, you might want to dimension holes a certain distance from an edge, or else a certain distance from each other.
There are several automated tools associated with dimensions and relations. You can let the SOLIDWORKS application:
  • Fully define sketches
  • Resolve over-defined sketches

To add a dimension to a sketch or drawing:

  1. Click Smart Dimension on the Dimensions/Relations toolbar, or click Tools > Dimensions > Smart. The default dimension type is Parallel.
    Optionally, you can choose a different dimension type from the shortcut menu. Right-click the sketch, and select More Dimensions. Choose from Horizontal, Vertical, Ordinate, Horizontal Ordinate, or Vertical Ordinate. If you are editing a drawing view, you have additional choices of Baseline and Chamfer.
  2. Select the items to dimension, as shown in the table below.
    You can undo previous selections by pressing Esc. For example, when dimensioning multiple entities using the Smart Dimension tool, you can press Esc to undo the last selection. This is helpful if you accidentally select an entity that you did not want to dimension.
    As you move the pointer, the dimension snaps to the closest orientation. The dimension text is semitransperant during placement.
  3. Click to place the dimension.
    To dimension the... Click... Note:
    Length of a line or edge The line.  
    Angle between two lines Two lines, or a line and a model edge. Placement of the dimension affects the way the angle is measured.

    Video: Dimensioning the Angle Between Two Lines
    Distance between two lines Two parallel lines or a line and a parallel model edge.  
    Perpendicular distance from a point to a line The point and the line or model edge.  
    Distance between two points Two points. One of the points can be a model vertex.
    These distance dimensions were all created by selecting the same two points, then selecting a different location for each dimension:

    Video: Dimensioning Point-to-Point
    Radius of an arc The arc.  
    True length of an arc The arc, then the two end points. Video: Dimensioning Arc Length
    Diameter of a circle The circumference. Displayed as linear or diameter, depending on placement.

    Video: Dimensioning a Circle
    Distance when one or both entities is an arc or a circle The centerpoint or the circumference of the arc or circle, and the other entity (line, edge, point, etc.). By default, distance is measured to the centerpoint of the arc or circle, even when you select the circumference.
    Midpoint of a linear edge Right-click the edge whose midpoint you want to dimension and click Select Midpoint. Then select the second entity to dimension. You can also dimension to midpoints when you add baseline or ordinate dimensions.
    The doubled distance between a sketch entity and centerline The sketch entity, then the centerline. Then drag the pointer to the opposite side of the centerline. Doubled distance relations create a value that is twice the distance of the sketch entity to the centerline. These relations help you determine the equal distance to the other side of the centerline. Doubled distance relations are helpful when you create profile sketches for revolved features.

    Video: Dimensioning Doubled Distance

    The dimension shortcut menu provides Display Options. The choices available depend on the type of dimension and other factors and may include the following:
    • Show Parentheses
    • Dual dimension
    • Show as Inspection