SolidWorks 2010 Bible

Chapter 7: Selecting Features

Tip
You may have to adjust the length of one of the spline tangency length arrows to keep the spline from remain-
ing inside the cylinder of the helix.

9. Open a sketch on the Right plane, and draw an arc that is centered on the Origin
   and coincident with the end of the 3D sketch helix. The 185-degree angle is created
   by activating the dimension tool and clicking first the center of the arc, and then the two
   endpoints of the arc. Now place the dimension. This type of dimensioning allows you to
   get an angle dimension without dimensioning to angled lines. Exit the sketch.


10. Create a Composite Curve (Insert ➪ Curve ➪ Composite) consisting of the 3D
    sketch and the new 2D sketch.


11. Create a new plane using the Normal to Curve option, selecting one end of the com-
    posite curve.


12. On the new plane, draw a circle that is centered on the end of the curve with a
    diameter of .120 inches. You need to create a Pierce relation between the center of the
    circle and the composite curve.


13. Create a sweep feature using the circle as the profile and the composite curve as the
    path. To create the sweep, you must first exit the sketch.


14. Hide any curves that still display.


15. Choose Insert ➪ Cut ➪ With Surface. From the Flyout FeatureManager, select the Right
    plane. Make sure that the arrow is pointing to the side of the plane with the least amount
    of material. Click OK to accept the cut. The finished part is shown in Figure 7.73.

FIGURE 7.73

The finished part