6
MODELING WITH COMPLEX CURVES

At this point in the book, you’ve already learned enough to re-create about 75 percent of the mechanical models you can find on a design-sharing site like Thingiverse, even if how to go about it might not always be obvious. Your ability to create complex models depends more on how creatively you can take advantage of basic features than on how many advanced features you know how to use.

That said, you’ll still encounter situations where you need to use unusual tools. In this chapter, we’ll focus on the Sweep and Loft features. You’ll use these to create organic-looking shapes so that you won’t be limited to building blocky models.

Sweeps and Lofts

The Sweep feature shown in Figure 6-1 creates a solid body by extruding a closed-loop profile along a path. Unlike the path of a regular extrude, the path of a sweep can curve and twist in all three dimensions, which makes this feature great for creating wires, tubes, and handles.

Figure 6-1: The Sweep feature moves a profile along a path to create tube-like bodies.

The Loft feature creates a solid body by using two or more closed-loop profiles as cross-sections, which the software then merges into a single solid. Unlike Sweep, the Loft feature doesn’t need to use a path; it simply morphs one cross-section into the next, yielding a single seamless body like the one shown in Figure 6-2.

Figure 6-2: This loft stitches together three cross-sections of different shapes and sizes.

Before we use these features, you’ll need to familiarize yourself with the concepts of tangent lines and planes, along with perpendicular lines and planes. Both are critical to getting the solid you want from sweeps and lofts.

It’s surprisingly difficult to express the concept of tangency. Mathematically, it’s a line with a slope equal to the slope of a curve function at a single point, but you most likely understand it intuitively as a line that continues on from a point in a curve. Imagine swinging a marble at the end of string and then releasing the string. The line that the marble flies along would be tangent to the curve of the marble’s path at the exact moment you released the string.

This is illustrated by the sketch shown in Figure 6-3. On the left, the line is tangent to the circle—just like the path of the marble after it has been released. On the right, the line is not tangent and represents a path the marble therefore couldn’t follow. The good news is that Fusion 360 understands tangents, and all you have to do is add one as a constraint.

Figure 6-3: Only the line on the left is tangent to the corresponding circle.

Perpendicular lines are much simpler—they’re just two lines, a line and plane, or two planes that meet at 90-degree angles.

These concepts are important because both the Sweep and Loft features take relative angles into account. The Sweep feature looks at the angle of the path where it meets the profile, whereas the Loft feature looks at the angles between the cross-sections. In most cases, you’ll want to ensure that the paths and profiles are either tangent, perpendicular, or parallel in order to avoid surprises. In addition to the parts of a single sweep or loft, you’ll also want to pay attention to how they intersect other features. The model in Figure 6-4 shows a gap created because the ends of the sweep weren’t made perpendicular to the block faces.

Figure 6-4: The path for this sweep isn’t perpendicular to the blocks it joins.

This model could easily be fixed in one of two ways. The sweep path could be made perpendicular to the blocks by either decreasing the arc radius or changing the block angle. Alternatively, if those items couldn’t be changed because of some design constraint, the path could be extended further into the blocks to eliminate the gap.

How you choose to handle similar problems will depend on what you’re designing, but it’s always a good idea to pay attention to the geometric relationships among sketches, paths, profiles, and features. Doing so is not only good design practice but will also save you from modeling headaches in the long run.

Organic Shapes and a Teapot

It’s time to learn how to use sweeps and lofts. You’ll be modeling a teapot like the one in Figure 6-5. As you can see, it’s made of curving organic surfaces you could not have created with extrudes and revolves.

The entire model is made up of only four major features. We’ll use a loft for the main body, a sweep for the handle, a second loft for the spout, and a shell to make the whole thing hollow.

Figure 6-5: This teapot is made up of organic shapes modeled with lofts and sweeps.

The Teapot’s Body

We’ll start by creating the teapot’s body using the Loft feature. We’ll make three individual sketches and merge them into a single object, as shown in Figure 6-6.

Figure 6-6: The first loft is made up of three sketches.

Feel free to choose your own dimensions, but you should use an ellipse as the base sketch (Profile 1), a larger ellipse as the middle sketch (Profile 2), and a circle as the top sketch (Profile 3), which will make it easy to model a lid later on. All three sketches share the same centerpoint, which should be centered on the origin point.

You can draw the sketch for Profile 1 on the existing x-y plane. For the other two profiles, you’ll need to create construction planes. To make those, select Offset Plane from the Construct drop-down menu and offset them from Profile 1’s sketch plane. When you have your two construction planes, draw your sketches on them.

To complete the loft, match the dialog in Figure 6-6. This loft doesn’t require guide rails, so you can leave that section empty. Make sure to check the Chain Selection box and set the Operation field to New Body. Select each of the profiles you’ll use in order and then click OK.

The Teapot’s Handle

Next, we’ll create the sweep that will form the handle of the teapot. You’ll create a path for the sweep to follow and then a profile that defines the cross-section of the handle. We’ll create the path sketch first. That will give us a reference point to use for our profile sketch, as well as a line we can use to make the profile perpendicular to the path.

Start the sketch of the path on the x-z plane perpendicular to the teapot’s base. My path, shown in Figure 6-7, is made up of two arcs, but you can make yours whatever shape you like. That said, you should make sure the path extends into the body of the teapot. If you were to draw it so it stopped at the edge of the body, you’d be left with a gap like the one shown back in Figure 6-4. To make that interaction easier to see, you can switch the Visual Style to Wireframe from the Display Settings menu at the bottom of the screen.

Figure 6-7: Draw a path for the sweep to follow.

You probably noticed you didn’t define your dimensions. You should almost always define the dimensions of a sketch explicitly. In this case, though, the actual dimensions aren’t very important, because we’re just going for visual appeal. You should still constrain the path to make sure it doesn’t unexpectedly move. To do that, simply select the lines and then add a fix constraint from the same Constraints menu you use to make lines perpendicular or parallel. That should lock the lines in place where they are and change them to green to signify that they’re fixed.

Now that you’ve made your path, you can create the profile for the sweep. To avoid the issue we saw in Figure 6-4, the profile should be perpendicular to the path at the point where they intersect. That’s difficult to do, though, considering both arcs end at unusual angles that we didn’t specify and wouldn’t be able to measure without additional work. So, we’ll create a construction plane that’s perpendicular to the path.

Fusion 360 actually provides a construction tool specifically for this sort of scenario called Plane Along Path, which can be found under the Construct drop-down menu. Choose it and then select the path you just sketched, as shown in Figure 6-8.

Figure 6-8: Use Plane Along Path to easily create a plane perpendicular to the path at a given point.

Next, set the Distance field, which determines where along the path to put the construction plane. Rather than asking you for a number in millimeters or inches, it asks you for a decimal ratio of the total length of the path. So, “0” would place the plane at one endpoint, “1” would place it at the other endpoint, and “0.5” would place it halfway between the two. In this case, choose either 0 or 1, and the construction plane will automatically appear perpendicular to the tangent at the endpoint of the path.

Now you can be sure that the plane is perpendicular to the path at its endpoint. All you have left to do is draw a profile for the cross-section of the handle on that plane. Unlike the Loft feature, which pieces together multiple profiles, the Sweep feature will simply extend one cross-section along the path. In Figure 6-9, you can see the profile I drew (I hid the body to make it easier to see). Once again, you can make this whatever shape you like.

Figure 6-9: The profile sketch for the sweep

When you create the Sweep feature, which is found in the Create drop-down menu, you’ll need to select the profile and path you just sketched. The purpose of the other options in the dialog you see in Figure 6-10 isn’t quite as obvious. Here’s a breakdown of what they do:

Type This lets you use a guide rail or surface to control the twist of the sweep. It’s possible for the sweep to develop an unintended twist, particularly if your path is drawn in three dimensions. A guide can help eliminate this twist.

Distance Like the Plane Along Path tool, Distance asks you to enter a decimal ratio of the path’s length. If you don’t want the sweep to go the entire length of the path, you can specify that.

Taper Angle By default, the profile will remain constant in size throughout the sweep. If you want it to either grow or shrink as it goes, you can specify a Taper Angle setting.

Twist Angle This spins the profile around the path’s axis as it moves.

Orientation Use this to determine the profile’s orientation in relation to the path. Because we drew the profile perfectly perpendicular to the path, we’ll want it to remain perpendicular.

Figure 6-10: The Sweep dialog options are complicated and will usually remain at the defaults.

To give the handle a smooth transition into the body of the teapot, add a couple of large fillets so your model looks similar to Figure 6-11.

Figure 6-11: Fillets are always great for adding smooth transitions.

To do this, just select the edges where the handle meets the body, and Fusion 360 will take care of adding the fillets to the nonuniform edges.

The Teapot’s Spout

The next feature, the spout, is the most complex part of this model. It’s a loft, but it uses a guide rail that acts similarly to the path of a sweep.

As with the sweep path we used for the handle, start by drawing that guide rail. Mine is shown in Figure 6-12. Once you’ve sketched your own, hold it in place using the fix constraint.

Figure 6-12: The loft’s guide rail acts similarly to a sweep’s path.

You’ll need one profile at each end of the guide rail to form the beginning and end of the spout. Use the Plane Along Path construction plane to sketch those profiles perpendicular to the guide rail. As you can see in Figure 6-13, I made one profile a large ellipse where it meets the teapot body and the second profile a smaller circle at the end of the spout.

Figure 6-13: Adding profiles on either end of the guide rail to form the spout

To create your loft, start by selecting the two profiles you just sketched. The Guide Type field of the dialog gives two options for the guides: Guide Rails and Centerline. You would use the Guide Rail option if you wanted the guide rail to intersect with the edge of the profiles, and you would use Centerline if you wanted the guide rail somewhere inside the profiles. It doesn’t need to be in the exact center of the profiles—that would be very tricky with irregular shapes. It only needs to be located so it’s definitely different from a guide on the edge of the profile. Choose Centerline and then select the guide rail you drew.

Hollowing Out the Teapot

To finish up the model, add a fillet at the base edge of the spout and then add a Shell feature for the entire model to hollow out the teapot. When you create the shell, you’ll want to select both the top face (where the lid goes) and the face at the tip of the spout.

The thickness of the shell may cause some errors for your model. That’s because the handle is fairly narrow, and Fusion 360 gets thrown off when it can’t create a shell with a single open cavity. If, for example, the handle is 10 mm wide at its narrowest point, then a 6 mm wall thickness would cause the two walls to intersect, giving you an error. You may need to tweak the thickness and possibly change it to Outside instead of Inside (or even use both). In the end, the model should look something like Figure 6-14.

Figure 6-14: The teapot, in all its organically shaped glory

Exercise

I’ll end this chapter by leaving you to model the lid of the teapot on your own using the Sweep and Loft features. It should look something like the one in Figure 6-15.

Figure 6-15: Try modeling this lid using the skills you just learned.

Make sure the bottom of the lid is a circle that will fit into the top of the teapot. The lid should then taper up into an ellipse. Add a small handle on top and use fillets to smooth it all out. You should be able to model this by applying the skills you learned in this chapter.

Summary

The Sweep and Loft features that you learned how to use in this chapter can seem complicated at first, but ultimately they allow you to create organic geometry that is inaccessible with the tools you learned in previous chapters. At this point, you can model practically anything you can imagine. But there are still a few tools that may be useful in specific scenarios. Flip to the next chapter to learn all about coils, threads, and solids that require complex construction geometry.