Getting swept away in 3-D CAD modeling

Like an extrude or revolve, a sweep is a tool for modeling a 3-D shape. A sweep consists of three basic elements—a profile, a path, and a set of rules for "sweeping" the profile along the path.

Before getting too far into the details of sweeps, I am going to offer up a couple of disclaimers. First, if you're not using the same software as I am, some of the operational details and terminology may be a bit different. Second, we're going to cover only a little bit of what sweeps can do.

Peek at a Peg

Figure 1 shows a cylinder that has a 1-inch diameter and a 1-in. length. Can you tell how it was modeled? Is it an extrude, a revolve, or a sweep? Without having access to the model, you really can't answer that question. The part in Figure 1 could have been modeled in any of several ways to achieve the same dimensional result.

This example, however, was created as a sweep. Figure 2 reveals the two sketches that were required. It doesn't matter in which order the sketches were created. In this case, the sketch with the circle was completed first. This sketch is the profile—the cross section of the sweep. Then a second, separate sketch for the path was made. In this case, the path is just a straight line. The final step was to launch the sweep tool. The sweep tool allows you to select which sketch to use as the profile (the circle) and which sketch to use as the path (the line).

To create the elbow shown in Figure 3, I edited the path sketch by adding a second line and creating a fillet in the sketch. This example begins to reveal the distinctive advantages of sweeps. The path can be made from a variety of lines, curves, and splines. The profile must be a closed loop—or set of loops. Sweeps are powerful tools for modeling tubing, wiring, and other shapes that follow some sort of path.

Twist and Shout

For extra fun and excitement, the twist along path option can create a spiraled rotini noodle as shown in Figure 4. In this example, the path and the sketch are nearly identical to those used in Figure 3. The main difference here is in the option settings that were used when configuring the sweep. The profile is twisted around the path 10,800 degrees, or for 30 revolutions of 360 degrees.

Perhaps a more cogent example for those of us in the manufacturing trade is the boltlike item shown in Figure 5. This model was created using a sketch of a trapezoid to represent the thread profile. This profile was then swept along a path—a straight line—along the axis of the fastener and twisted for 10 revolutions.

To improve the demonstration, a revolve feature is used to represent the body of the bolt. As finishing touches, a sketched hexagon was extruded for the head and a fillet added to deburr the part.

If your model must include details like a twisted pair of wires, sketch the path that the wires will follow. In a separate sketch, draw the profile that represents the cross section of the wires.

Figure 6 was created using a profile that resembles an 8. The final step is to sweep the profile along the path using an appropriate twist value.

Guidance Needed

The hammer handle shown in Figure 7 was created with a sweep with a guide curve. The path for the sweep is a straight line. We could have used something more exotic for our handle, but a straight handle is pretty common on tack hammers.

The profile for the sweep is a simple ellipse. The changes in cross-sectional size along the handle are controlled with the guide curve. In this example, a spline is used to sketch the guide curve to keep the handle smooth and comfortable for the craftsman who would be using it.

Because this sweep uses only a single guide curve, the software uniformly scales the profile (the ellipse) relative to the path. With an additional guide curve, a CAD operator can control the sweep with greater refinement.

In Figure 8a, notice a second guide curve sketched on a plane that is perpendicular to the plane used for the first guide curve. The design intent is to strengthen the narrow section of the handle by making it more round instead of the thin ellipse shown in Figure 7. Figure 8b shows the result in a shaded view.

It is undoubtedly easier to visualize these exotic shapes in a 3-D CAD system as opposed to small, 2-D images in this magazine. If you'd like copies of these models, just let us know.

Next month I'll take a closer look at using lofts as a modeling technique to create 3-D solid bodies. These can be very handy for creating models of ductwork as well as other shapes that just don't lend themselves well to extrudes, revolves, or sweeps.

Gerald would love to have you send him your comments and questions. You are not alone, and the problems you face often are shared by others. Share the grief, and perhaps we will all share in the joy of finding answers. Please send your questions and comments to dand@the fabricator.com.