# Sprocket Design Tutorial

As a sequel to my pulley and gear design tutorials, I’ll be explaining how to design a sprocket today. Sprockets are special in that their profiles are kind of arbitrary, and there are generally two ways to design sprockets for FRC - standard hob sprockets, and ANSI standard sprockets. Standard hob sprockets are easier to design, but to my knowledge they are less efficient and wear on the chain faster than ANSI sprockets.

The Math
Much of the math for a sprocket remains roughly the same independent of which sprocket profile you choose. The key thing to keep in mind is that unlike belts, chains are not flexible, and so instead of stretching to wrap around a pulley, a chain will rigidly “fold” around a sprocket. This means that sprockets don’t quite have a pitch circle so much as they have a “pitch polygon”, although we generally call the circle circumscribing it the pitch circle.

Above you can sort of see what I’m talking about. The distance between pins on the sprocket is along a chord, rather than along the arc length of the pitch circle. An unfortunate consequence of this is chordal action, in which the rotation of the sprocket causes the apparent width of the sprocket to roll in and out. ThIs is one of the reasons why you can tension a chain really hard, and then rotate it a little and find it’s loose again. The way you mitigate this issue is by using larger sprockets, since their pitch polygons are closer to their pitch circles.

As mentioned above, the pitch circle is the circumscribing circle of the pitch polygon. I’ll handwave a bit of geometry, but this means that the diameter of the pitch circle, PD, is not the same as on pulleys or gears. We typically describe sprockets using the pitch p, which is the distance between pins on the chain, and the number of teeth n. p, n, and PD are related by this equation:

PD = p \csc(\frac{180^{\circ}}{n})

Remember that this equation is not the same as for a pulley!

We also have another two values which we should be aware of, called D_r and D_s. These two values are the diameters of the roller pin on the chain, and the diameter of the “seating curve” on which the roller sits in the sprocket. D_r is simply a standard value; for #25 chain, D_r is 0.13 and for #35 it’s 0.2. $D_s$is defined as below:

D_s = 1.005 D_r + 0.003 \text{in}

Those two numbers are arbitrary, but they ensure that the seat is always a larger diameter than the roller, preventing binding.

Standard Hob Sprockets

We start as always in the equations tab. I add the equations I wrote above and get started. As you can see, I’m making a 24T #25 sprocket.

I draw a construction circle here with a diameter of PD, then add a chord. I dimensioned the length of this chord to be equal to p. This is representative of one link in the chain. The angular position of this chord is arbitrary, so I put one point of it directly above the origin.

On each endpoint of this chord I add a circle. I dimension one of the circles to have a diameter of D_r, and mark the other circle as tangent to the first. The larger circle is a simulation of the travel of one pin as it rotates around another. If you imagined dragging the circle with diameter D_s around the other circle, the result is what we traced out.

To finish up this half-profile, I draw a radial line outward from the midpoint of the chord, and a radial line inward from the center of the circle with diameter Ds. I trim the cricles down so that only the arcs connecting the two circles remain. I also added some construction circles to help show you where the circles were trimmed from, but you don’t need these. We’re done with this sketch now, so you can go fire off another sketch.

After starting a new sketch, I draw a new circle, and set it so that it is coincident to the outermost point of the half-tooth we drew earlier. This circle is the outer diameter of our sprocket.

I now extrude the outer diameter into a blank. The width of this extrusion is based on the standard of the chain. For #25 chain, the width is 0.11", and for #35, the width is 0.169".

I then fire off another sketch. I converted over the geometry from my first sketch, then mirrored that half-tooth profile about a radial line from the center of the sprocket to the center of my D_s circle.

After closing off the sketch with the outer diameter, I cut out a single tooth profile from the blank.

I pattern the tooth profile n times around the sprocket, and with that, the sprocket is done!

ANSI Sprockets

ANSI standard sprockets are a lot like standard hob sprockets, but they’re a little wider to improve life and efficiency. The math of the pitch polygon, pitch circle, and D_s are all the same as on a standard hob sprocket.

This picture, while a bit busy, illustrates roughly how an ANSI sprocket works. Here are the equations which define some of the dimensions you see here in the picture:

A = 35^{\circ} + \frac{60^{\circ}}{n}
B = 18^{\circ} - \frac{56^{\circ}}{n}
R = \frac{D_s}{2}
ac = 0.8 * D_r
ab = 1.4 * D_r

The other dimensions in the picture are handy when making hand drawings, but since we have parametric CAD tools, we don’t need them. Note that the value of ac is the distance between points a and c, and likewise for ab. The magic constants in the equations above are frankly rather arbitrary, but they’re part of the ANSI standard, so we abide by them.

Lastly, although the above picture has sharp pictures, I prefer to have flat tips to the teeth on my sprockets. Therefore, I specify a value for OD.

OD = PD + \frac{p}{2}

Like before, we start with our pitch circle and one chord. I then dimension the pitch circle’s diameter to PD and the chord length to p. Lastly, I draw a circle with diameter D_s about one end of the chord.

Tangent to the D_s circle, I add one more circle. To the new circle, I add a tangent line, and to that line I add another tangent circle.

Now, I add a few construction lines. Note that the one from the center of the chord is coincident to the center of the sprocket, and there is a horizontal line from the center of the D_s circle.

Now I add the dimensions for A, B, ac, and ab. I also make sure to locate the center of the leftmost arc (whose center is b) on the chord.

To finish out the half-tooth, I trim down the D_s circle to only the part that I need.

Since the half tooth is done, I fire off a new sketch on a plane perpendicular to my half-tooth sketch. This is the profile for the blank of my sprocket. The radius of the blank is OD/2, and since I’m using #25 chain, the thickness of the blank is 0.11". I also chamfer the end such that the width of the chamfer is \frac{p}{8} and the height is \frac{p}{2}.

I revolve out the sketch about the origin to make the blank for the sprocket.

After firing off a new sketch, I convert the half-tooth profile from before and then mirror it, as well as closing the sketch to make a cut.

To finish things off, I cut out the full tooth profile and pattern the cutout n times around the sprocket. Now the sprocket is ready for whatever other features I want to add.

*Wrapping Up

For comparison, here is a side-on view of both profiles on top of each other. It’s pretty clear to see here why the ANSI sprocket would be preferable - it has more room for a chain to slide in and out.

I hope you found this tutorial helpful. As always, if you have any questions, don’t be afraid to let me know. Additionally, if there are any other things you’d like me to explain, not just about sprockets but about gears, pulleys, or other mechanical design aspects, ask away. I’ve attached the solid models of both the parts I created below:

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Can you confirm the diameter of the smallest construction circle in the Hob Sprocket? It is measured as Dr in the creation step, and in the diagram, but then referred to as the Ds circle. I’m pretty new to CAD so forgive me if I’m misunderstanding. Thanks!

Either value will work. I personally would recommend using D_s, as that allows for clearance for the roller, but a “true” standard hob sprocket would use D_r.

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Awesome, thanks!

The link to the gear tutorial leads to the timing pulley, I believe you meant to use this link. Involute Gear Design Tutorial - CAD - Chief Delphi
Also thanks for making these, they are great!

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