Chapter 3: Working with Sketches ...............................................................................................
SolidWorks sketch entities include many types, some of which you will use all the time, and some
of which you may not use, even if you spend years working with the software. Next, I identify each
entity type. This enables you to see it at least once and know that it is available if you need it at
some point.The Sketch toolbar
In the following section, I first identify the default buttons on the Sketch toolbar, followed by the
rest of the entities that you can access by choosing Tools ➪ Customize ➪ Commands ➪ Sketch.Sketch opens and closes sketches. You may notice that the name of the button changes depending
on if the sketch is open or closed. If you preselect a plane or planar face and then click the Sketch
button, SolidWorks opens a new sketch on the plane or face. If you preselect a sketch before click-
ing the Sketch button, SolidWorks opens this sketch. If you preselect an edge or curve feature
before clicking the Sketch button, SolidWorks automatically makes a plane perpendicular to the
nearest end of the curve from the location you picked. If you do not use preselection, and only
click the Sketch tool with nothing selected, SolidWorks prompts you to select a plane or planar
face on which you want to put a new sketch, or an existing sketch to edit.3D Sketch opens and closes 3D sketches with no preselection required. 3D sketch is covered in
more detail in Chapter 31.
Smart Dimension can create all types of dimensions used in SolidWorks, such as horizontal, verti-
cal, aligned, radial, diameter, angle, and arc length. You can create dimensions several ways, as
shown in Figure 3.1:
l By selecting a line and placing the dimensionl (^) By selecting the endpoints of the line and placing the dimension
l By selecting a line and a point and placing the dimension
l (^) By selecting a pair of parallel lines and placing the dimension
Selecting the line is the easiest and fastest method. Selecting parallel lines on the ends is not rec-
ommended because if you delete either of the selected lines, the dimension is also deleted; how-
ever, sometimes this method is necessary.
You can use the first and second techniques for the angled line shown in Figure 3.1 to create any
of the three dimensions shown. To accomplish this task, drag the cursor while placing the dimen-
sion until the witness lines snap to the orientation you want.
Tip
To lock the orientation of a dimension while moving the cursor to place the actual dimension value, click the
RMB. To unlock it, click the RMB again. The RMB cursor appears as a lock when the functionality is unavail-
able and an unlock icon when it is. n