Page 103 - Mastering SolidWorks

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72 CHAPTER 3 Working With SketcheS and reference geometry

The Quick Snaps flyout enables you to quickly filter types of entities that sketch elements will
snap to when you move or create them. To access the tools, click the drop-down arrow to the
right of the toolbar button.
The Mirror Entities tool mirrors selected sketch entities about a single selected centerline and
applies a Symmetric sketch relation. In addition, a Dynamic Mirror function is described later in
this chapter.
The Convert Entities tool converts edges, curves, and sketch elements from other sketches into
entities in the current sketch. When edges are not parallel to the sketch plane, the Convert
Entities feature projects them into the sketch plane. Some elements may be impossible to
convert—for example, a helix, which would produce a projection that overlaps itself. Sketch
entities created using Convert Entities get an On-Edge sketch relation.
The Offset Entities command works like the Convert Entities feature, except that it offsets the
sketch to one side or the other of the projection of the original edge, sketch, or curve, and Offset
Entities doesn’t have a selection box. Figure 3.10 shows the PropertyManager interface for
this command.

Figure 3.10
The offset
entities interface

The options available in the Offset Entities interface are as follows:
Add Dimensions: This option constrains offset sketch entities. Instead of the On-Edge
relations, Offset Entities creates an Offset sketch relation that cannot be re-created manually.
Reverse: This option changes the direction of the offset.

Select Chain: This option selects continuous end-to-end sketch entities.
Bi-directional: This option offsets to both sides simultaneously.
Cap Ends: This 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 3.11 shows examples of
the Cap ends option.
Construction Geometry: This option enables you to select which geometry (if any) you
would like to make into construction geometry—the original selection, or the entities that
are offset.