Cycloidal gears in Fusion 360

Fusion 360 has tools for creating involute gears, including its own spur gear add-in and GfGearGenerator, and they work well. However, if you want cycloidal gears, it's not so easy to find something that works. Here's one approach, in case this turns out to be helpful to anyone else.

Start by generating the gear in DXF form using Rainer Hessmer's Cycloidal Gear Builder. Make sure to use the highest quality level. It's useful to include a hole in the middle so you can identify the center. Download the DXF file. If you load this DXF into Fusion 360 (Design > Insert > Insert DXF) you will get an unhelpful error message. The DXF file isn't in a form that Fusion 360 can handle and we need to fix it.

You can fix the DXF by importing into FreeCad and then exporting it again. Another option is to import it to Inkscape and save it with "Save As". The DXF should then import into Fusion 360. However, if the gear is large, Fusion 360 may sit for hours processing it. It might never finish. Selecting "One sketch per layer" when inserting it sometimes helps, but generally does not. So another option is save it as a SVG from Inkscape and insert that instead. It's still slow, but does work. If you are lucky, you might be able to extrude the result and create the gear from it. Or sometime Fusion 360 will just abruptly exit.

The Cycloidal Gear Generator is supposed to have an option to output to SVG but it was missing when I looked for it. However, instead you can download a desktop version of the app from here. This will give you a SVG with much better segments. Note that you have to specify that you want a pinion. In the web version you can omit it. The desktop version raises an exception if you try. The result will load into Fusion 360, but it won't work as the segments don't join into a closed curve. However, we can use the sketch as a starting point.

First note that the imported SVG won't have the right size. We need to scale it. To find the scale factor measure an element of known size. For example, if you created a 6mm hole in the middle of the gear, measure its actual diameter and scale by 6 divided by this. Measuring the radius is usually easiest, and so then you would scale by 3 divided by the measurement. To scale the whole sketch, exit sketch mode, go to Modify>Scale, select the sketch from the browse list, and enter this factor.

Now we want to go into edit sketch and delete everything except for the center hole and one tooth. The tooth will consist of two lines and two arcs. You ought to be able to create a circular pattern with these and the arc joining them to the base of the next tooth, but you don't get a closed path if you do. The problem is that the exact end points of the lines aren't right. So change everything to a construction line (with x), then change the two lines and two arcs back. Create a center circle with circumference on the ends of the lines. Now create a circular pattern with the two lines and the two arcs about the center of the gear, with a number of elements equal to the number of teeth you want. You should now be able to exit sketch mode, select all the teeth and the circle you just created, and extrude your gear.