pic: GT2 Pulleys

25 tooth GT2 5mm Pitch pulleys for 9mm width belt.
For use in a West Coast Drive, pulleys are 3 parts. 2 Plates for flanges and the center with the teeth. Cut on a Tormach CNC Mill with an 1/8 rough cut, then a 3/32 finish cut.

Did you machine the tooth profile or did you use pulley stock?

Nicely done! I bet this saved some serious coin for your team.


You made the entire pulley in house? Or did you buy pulley stock and add your own flanges? Either way, that’s awesome. Pulleys ain’t cheap.

I think you could probably afford to run thinner flanges, but it’s not a ton of weight either way.

The pulleys were completely machined by me, the stock was a 3/8 6061 plate, which fits the 9mm tooth width perfectly.

Each pulley took about 20 mins to do on the machine, this includes the .5 hex profile as the bore.

The CAD model was downloaded from SDP SI’s site.

I could run thinner flanges, they were just the thinnest piece I had and I was setup for that operation on the machine so whatever. :stuck_out_tongue:

Did you just run them on a CNC mill with a small endmill to get the tooth profile? If that’s all you needed to do, we might have to seriously look into machining our own pulleys in 2014.

Its exactly what Mark did. We both use a 3/32 endmill to clean it up.


Neutrino has done the same, we did the profile with a 3/32nd end mill though, and did it in multiple steps (2-3 mm at a time)

We machined them like: https://sphotos-a.xx.fbcdn.net/hphotos-ash3/530424_4304939790338_206600436_n.jpg

Just a plate bolted to the table and a 1/8 endmill to rough cut then a 3/32 end mill to finish it off. Once I got the program finished and speeds/feeds good it was just a set and leave operation.

We usually make our own #25 sprockets. In house we can make then for about $1.20 a piece vs. the $9 average to buy one. At this point we’ve made all “standard” sizes up to 60 teeth, so we have the CAM’s saved, as well as the fixture. So now its just a matter of running the operation to make them, and setting up the tools. Its really nice for prototyping when we want a specific size!

I love the idea of making our own sprockets with a CNC mill, but have a couple questions for the more experienced:

(1) What’s the best way to keep the sprockets from moving around on the last pass? (Especially if you are doing a tool change for finishing…) Are you using a vaccum table or another method?

(2) What’s the easiest way to get the hex-shaped bore for the sprocket? Is the fillet from the CNC mill negligible or do you need to file or broach it after milling?

Thanks for any advice!

For the profile, I’d probably screw them down to a jig you hold in a vise, and then do the profile all in one pass. You already need holes to bolt the flanges on, so you might as well use them to hold the part down during the last op.

[STRIKE]I haven’t milled any timing belt sprockets personally on a CNC mill, but[/STRIKE] I have machined a lot of 25 pitch roller chain sprockets out of 7075 aluminum when I was in college and the process is similar. I would make 25p sprockets in three operations:

  1. Drill the center hole (usually 0.375in or 0.5in and mill out everything except for the teeth profile itself. On small sprockets where there were no additional holes beyond center hole, I would mill a very slight double-D pattern into the hub to align to the fixture plate in step 2. Here’s a photo taken before I milled the double-D:

  2. Take the plate out of the vise and put the pre-made fixture plate into the mill. The fixture plate would have tapped holes for either 0.375in or 0.5in bolts, and would have a double-D pocket in it to keep the sprocket from rotating. I would then bolt down the piece from step 1 and mill out the outer profile of the sprocket. Here’s a photo:

  3. As the final step, I would remove the sprocket from the fixture plate, flip it over, and use three equally-spaced 6/32 screws to bolt the sprocket to the fixture plate so I could face-mill off the double-D pattern and bring the overall width of the sprocket down to 0.405in to match COTS sprockets

After step 3, I would then hex broach the center holes.

Generally since I was making these sprockets at quantities of at least 20 at a time, I would do step one for every sprocket, change to the fixture plate, then do all step 2, then do all step 3. Sometimes if the machine shop was empty I would use three CNC mills, one for each step to speed up the process.

Edit: I almost forgot but I have “made” belt sprockets on a CNC mill and lathe before. To save time, instead of milling the profile myself, we bought timing belt pulley stock from SDP-SI, cut it down into wafers, then did the final machining on the CNC mill and lathe before hex broaching. Generally I never bothered adding flanges if at least one of the two sprockets had them. Here’s two photos:


For those of you machining either roller chain sprockets or timing belt pulleys, what models are you using for the tooth profiles?

For the 25 pitch roller chain, I used the sketch formulas found in (I believe) Machinery Handbook and made a Solidworks equation driven model where you would enter in the chain pitch, roller diameter, and number of teeth and it would generate the CAD model.

After a quick Google search I found this PDF but I haven’t verified the equations: