Page 258 - Mastering SolidWorks

|
230 CHAPTER 7 Modeling with PriMary Features

On the Website
the part shown in Figure 7.13 is in the download material from the wiley website for this chapter
under the filename Chapter 7 3D Sweep.sldprt.

This part is created by making a pair of tapered helices, with the profile sketch plane perpen-
dicular to the end of one of the curves. The taper on the outer helix is greater than on the inner
one, which causes the twist to become larger in diameter as it goes up.
To make the circle follow both helices, you must create two Pierce relations, one between
the center of the circle and a helix, and the other between a sketch point that is placed on the
circumference of the circle and the other helix. This means that the difference in taper angles
between the two helices is what drives the change in diameter of the sweep.

Using a Cut Sweep with a Solid Profile
The Cut Sweep feature has an option to use a solid sweep profile. This kind of functionality has
many uses, but it’s primarily intended for simulating complex cuts made by a mill or lathe.
Figure 7.14 shows a couple of examples of cuts you can make with this feature. The part used
for this screen shot, called Chapter 7 - cut sweep solid profile.sldprt, is also in the
website download material.
Figure 7.14
cuts you can make with
the cut sweep feature
using a solid profile

The solid profile cut sweep has a few limitations that I need to mention:

◆ It requires two bodies: the target and a cutting tool.
◆ The path must start at a point where it intersects the solid cutting tool body (path starts
inside or on the surface of the cutting tool).

◆ The path must be tangent within itself (no sharp corners).