Page 105 - Mastering SolidWorks

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74 CHAPTER 3 Working With SketcheS and reference geometry

Power Trim: This trims by dragging a cursor trail over multiple entities. The entities that you
drag the cursor over are trimmed back to (or extend up to, when using the Shift key) the next
intersecting sketch entity. Each time you trim an entity, a red box remains until you trim the
next entity. If you backtrack with the cursor and touch the red box, this trim is undone. This
option is best used when you need to trim a large number of entities that are easy to hit with a
moving cursor. Figure 3.13 shows the Power Trim feature in action. You can also use Power
Trim to extend sketch entities along their paths by dragging the endpoints. Regular dragging
can also change the position or orientation of the rest of the entity, but by using the Power
Trim feature, you affect only the length.
Figure 3.13
Power trim in action

Corner: This trims or extends two selected entities to their next intersection. When you
use the Corner option to trim, the selected portion of the sketch entities is kept, and anything
on the other side of the corner is discarded. Figure 3.14 shows two ways that the Corner
option can work.

Figure 3.14
Using the corner option

Trim Away Inside: This trims away selected entities inside a selected boundary. The bound-
ary may consist of a pair of sketch entities or a model face (edges of the face are used as the
boundary). Only entities that cross both selected boundaries (or cross the closed loop of the
face boundary twice) can be trimmed. This option does not trim a closed loop such as a circle,
an ellipse, or a closed spline.