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:
To add a dimension to a sketch or drawing:
-
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.
-
Select the items to dimension, as shown in the table below.
As you move the pointer, the dimension snaps to the closest orientation.
Click to place the dimension.
To
dimension the... |
Click... |
Note: |
|
The line. |
|
|
Two lines, or a line and a model edge. |
Placement of the dimension affects the way the angle
is measured.
|
|
Two parallel lines or a line and a parallel
model edge. |
|
|
The point and the line or model edge. |
|
|
Two points. |
One of the points can be a model vertex.
|
|
The arc. |
|
|
The arc, then the two end points. |
|
|
The circumference. |
Displayed as linear or diameter, depending on placement.
|
|
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. |
|
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 dimension shortcut menu provides Display
Options. The choices available depend on the type of dimension
and other factors and may include the following:
Parentheses
Dual dimension
Inspection dimension
Related Topics
Arc Dimensions
Angular
Dimensions
Circular
Dimensions
Dimensions Between
Arcs or Circles