3/6/2020 note: There is an easier set of instructions on how to do this here





In my high school CAD II class we are 3D modeling radio controlled cars, 3D printing the parts, and racing them. Everybody is super pumped and things are going well, but our drivetrain options are somewhat limited. We currently use pulleys press fit to the output shaft of our motors and rubber bands to transfer power to the rear wheels, but rubber bands slip badly, break often, and are very inefficient, wasting a lot of power in the form of friction. Some students discovered Inventor’s ability to make spur gears with a true involute tooth profile, and their results were noticeably superior to rubber bands. We assumed that we could use that knowledge to make involute bevel gears as well, but Inventor lacked the “export tooth shape” feature on the bevel gear generator that made accurate spur gears possible. Inventor can generate several types of gears, but they are all simplified for visualization purposes only, and are nearly worthless for 3D printing or CNC machining. Only on the spur gear generator does it have the option to export a true involute tooth shape, which can be used to make a rapid prototyped, functional gear. How to transfer the involute shape of a spur gear into a bevel gear design was a problem that seemed simple at first, but turned out to be extremely difficult to figure out. With the help of one of my students who was also taking trigonometry, we were able to come up with a process that generates working bevel gears using the exported tooth shape from the spur gear generator.

Here is how we did it.





My 3D printer is an Afinia H480, which I recommend heartily to all teachers, and I use ABS filament for strength. I have found that the finest functional teeth that I can reliably print have a module of 1mm. This means that if the gear has a diameter of 24mm, it will have 24 teeth. Lego gears have a module of 1mm.





Open a new assembly file and save it. Open the Design tab, and click Spur Gear. Expand all expanders, to the right, down, and then the” <

Now you should have a couple of gears on your screen. These gears are not ready to be used. If you zoom in you can see that they overlap with interference. We need to right-click on one of them and choose “Export Tooth Shape”. We will have to do the rest of this procedure twice unless your gears have the same tooth count as each other. Once for the pinion (the smaller of the two gears) and once for the gear (the larger of the two gears). Use “Normal” backlash, and choose the largest value it will let you enter. For 1mm module gears, it seems to be about .006”. This backlash will keep the gears from interfering with each other with an imprecise 3D print. Click “OK”.





Now Inventor will take you to an .ipt part, which will be a cylinder with one of the spaces between the teeth on a sketch on the end surface. If you were making a spur gear you would make a cutting extrusion of that space, then do a 3D circular array of it in the amount of teeth you entered in the gear calculator. We, though, are going to delete the extrusion, but leave the pinned Sketch1. Edit that sketch, and delete all of the construction circles. Next do a 2D circular array of the tooth cut, then trim the outer circle so that the sketch shows the actual gear profile all the way around. Click “Finish Sketch”. Now make a new sketch on a plane perpendicular to that gear sketch. I use the YZ plane. Draw a centerline to the right, from the origin, which should be the center of the gear. Make it pretty long. Now draw a construction line straight down, from the origin, at least as long as the gear radius and then a little bit more. Now draw a solid line from the origin, down and to the right, a little bit longer than the gear radius. The angle between this line and the “down-from-the-origin” construction line will be 90 minus the inverse tangent (aka arctan) of the gear ratio divided by two. If I have 32 teeth on my gear, and 8 teeth on my pinion, my gear ratio is 4. The inverse tangent of 4 is about 76. 90-76=14. Half of 14 is 7. My angle from vertical for that line will be 7.





On the Windows calculator, use the “Inv” button to make tan into inverse tan (tan^-1).

Next, draw a line from the end of that line to the other end of the centerline. Then, from that end (end opposite of the origin) draw another line to the angled line sort of close to the end further from the origin. Make that line a construction line. It should look like this:



