Part I: SolidWorks Basics
FIGURE 3.11
The Offset Entities interfaceThe options available in the Offset Entities interface are as follows:l (^) Add dimensions. Constrains offset sketch entities. Instead of the On Edge relations,
Offset Entities creates an Offset sketch relation that cannot be re-created manually.
l (^) Reverse. Changes the direction of the offset.
l Select chain. Selects continuous end-to-end sketch entities.
l (^) Bi-directional. Offsets to both sides simultaneously.
l Make base construction. If you are offsetting sketch entities within the active sketch, this
option converts the original sketch entities to construction sketch geometry.
l Cap ends. Is available only when you have selected the Bi-directional option. Capping the
ends with arcs is an easy way to create a slot from a sketch of the centerline. This function
works with all sketch entities; it is not limited to straight slots. Figure 3.12 shows exam-
ples of the Cap ends option.
Caution
The Offset Entities command may fail if the offset distance is greater than the smallest radius of curvature, and
you are attempting to offset to the inside of the arc. n
In addition to the bi-directional offset with capped ends, SolidWorks also has slot sketch entities
for straight and curved slots, which are covered later in this chapter. Composite slots (made of a
combination of straight and curved sections) still require the offset method.
Trim is actually several functions rolled into one, and it is an extremely powerful tool for editing
sketches. Trim Entities allows several methods for trimming, as well as extending and deleting
sketch entities. Figure 3.13 shows the PropertyManager interface for this function.