Coaster Brake Bike: Clutch Cone

Here’s another part with some interesting features. On the brake shoe, we used a revolve and a pattern to create ridges on the brake to create friction. On this part, we have a cut sweep, an extrude, and a thread. I see people on the SW forum asking about relatively simple but possibly not exactly straight forward stuff like this all the time, so let’s go through this part.

The first feature is a revolve, which is simple enough, but the second feature is the straight V groove on the near external bevel of the clutch. How do you make a cut go in some direction other than straight ahead? Here’s how.

First, sketch the V, and close it to make a triangle. Notice the line closing the V is well outside the solid. If you try to make the line right on the edge of the solid, the cut is going to be very close to the actual surface. CAD often uses approximations, or at least exact numbers that may not be what you think they are. When you try to do something “exact” like surface-on-surface cuts, the faces may weave in and out, and you might get thin little slivers left over. Anyway, the game plan should always be to “overbuild”, by which I mean that you shouldn’t try to be exact, let the software figure it out, and give it a wide margin of error. You don’t want a funky in-and-out edge, you want a clean edge.

Notice also that the sketch is fully defined. I’m not one of those religious “thou must fully define thy sketches” kind of guy. I think that if it doesn’t matter, it doesn’t matter. SolidWorks is not going to change something unless you give it a reason to, and if that line were underdefined, it wouldn’t change the outcome at all. In this case, fully defining the horizontal line in the triangle doesn’t matter, but fully defining it comes cheap, and doesn’t cost me anything, so I went ahead and did it. Notice I used a construction line to locate the triangle on the revolved sketch line. A better way than using the 0.071dimension would have been a midpoint relation (the .071 and .025 dimensions appear reversed here for some reason).

Second, in the Direction 1 box, I selected one of the lines used to make the revolve. So the extrude is not just cutting perpendicular to the sketch plane, the way it does by default, it is cutting along the angle of the line. This is like doing a sweep along a straight line. So the cut moves at an angle to the sketch plane, and acts like a sweep along a straight line. Or you could say that a sweep along a straight line is like an extrude at an angle. Just for info, you can’t extrude along anything other than a straight line, that would be a sweep.

Ok, the third feature is a little trickier. I needed the groove to angle in two directions, but I couldn’t use an extrude, because the path had to be curved, in fact, it’s helical. Without doing a helical curve, I approximated this somewhat, so it’s not technically exact. First, I drew a straight line on a plane and projected it onto the conical surface using the Projected Curve feature, which shows in the tree as Curve1.  Then I sketched the V again, and gave it a relationship to the curve. I used the Pierce sketch relation, which is the only sketch relation that has a 3d component to the way it works. It calculates where the selected 3d curve pierces the sketch plane, and places the selected sketch point, end point, or midpoint at that location. So it you move the sketch plane, the pierce point moves. This sketch relation is really built for sweep features.

From there, it was just creating a Cut Sweep feature.

Technically, I should have made the groove twist as it swept, just as a cutter would do on a mill or lathe, but I didn’t. If I had, I would have measured how much angle change was involved in the twist, and used the Specify Twist Value setting in the Cut Sweep Options to drive that.

Some features in SolidWorks have a lot of settings, and the Sweep is one of them. They aren’t always intuitive to understand, so if you’re going to know what they do, you have to experiment a lot, or read reports from people who do. Sometimes the Help can clearly explain what’s going on, but don’t count on it.

The last feature was the multi-lead helix. This is one that I conveniently misused. A couple of blog posts ago, I bragged at how good the Thread feature was. And then immediately came across a significant limitation.

The thread feature is great for making features like… well… threads. It has profiles for V-profile threads, and more complex plastic injection molded threads. We need actual threads on models sometimes because we might have to cut the threads into a mold to mold a plastic part, or maybe to 3d print a part. We can’t always tap/die cut or roll threads.

The “thread” on the inside of this clutch is really a lead screw, and the profiles used in lead screws are different from thread profiles. I used the plastic bottle thread profile to approximate the lead screw profiles, which I know is wrong, but I love this Thread feature, and wanted to use it, especially since it has an option to create multiple lead (or start) threads.  So yes, I cheated. So sue me.

Anyway, if SolidWorks were to add a way to specify your own profile (or provided a set of drive profiles) in this feature without needing to go through the circle-helix- cut sweep-pattern routine manually, then I could have drawn in some sort of appropriate profile, and they could rename this Helical Cut feature to include lead screws and threads.

Oh, and there is also the weirdness of threads that add material rather than remove it. I guess in design we don’t have to be exactly literal about manufacturing methods, but it does reinforce bad habits.

That’s three different ways to create features that look like swept cuts.

If you like little explanations like this, please pass on the link for this blog to coworkers or your user group. Thanks for reading.