Hello, trying to see if I can make these with my new Nomad. From the research I’ve done most folks use a dedicated gear hobber machine it seems or some guys have done it on CNC lathes. I was hoping to see if it someone has done it using their Nomad.
It is a small gear and it 64 pitch. Diameter is less than 22 mm
The challenge is finding tooling which will reach into the gear teeth and which has flutes long enough to cut them out — if you have the 3D CAD model though, should be otherwise simple enough to load them into MeshCAM and cut them out.
Have also pondered this question (though have not tried it on a scale that small) Agree with Will. Rough out around the gear with a large end mill first, then go in with a very small one to cut the teeth. Probably relatively soft material. Could try doing a two-sided job if the end mill is not long enough, but it will have to be very precise.
I know Eddie Kramer has done production runs of Delrin gears that are one inch across on a Bantam desktop machine that is a Nomad equivalent. Might be worth a troll through his @ekramer3 Instagram.
64 diametral pitch? That’s gonna be tough. To get into the root area, you will need a tool that is about 0.3mm (0.012") diameter (20 degree or 14.5 degree pressure angle doesn’t make much difference at this fine a pitch) for the root, and likely cut the root a little overdepth to get the correct dedendum (depth at the root to clear the tip of the mating teeth). This is going to be tough, and the tools a tad fragile.
My suppliers list depth of cut at 0.036" (0.9mm) (0.060 from Mcmaster, but I don’t know if I would use a tool this small with that much flute), so, working from both sides, a gear about 2mm thick is manageable, maybe.
I milled a couple 16DP change gears using a 1mm diameter tool a while back. Delrin (generic acetyl, actually) was the material. That was kind of dicey for the volume of material the small tool had to remove. Roughed with a 3.2mm (1/8"), second roughed (rest machining) with a 1.6mm (1/16") tool, then real easy rough (rest machining) with the 1mm, followed by a finish pass with same. The thickness at the teeth was about 6.5mm (mating with 3/8" – 9.5mm-- nominal thick gears with actual tooth width of about 7.5mm) to limit deflection on the finish pass. The gears were 37 and 47T for metric threading with an imperial leadscrew. Insignificant error and much smaller than the 50/127T exact match. One day, I might run a 74T for when I need a little more space for a large pitch-setting gear.
I would think you could machine it flat to get the overall shape, then flip it vertically to “hob” your teeth with something like a V bit. You’d have to figure out a way of indexing it on an axle, and you’d have to index it for each tooth and repeat the same toolpath for each tooth. 4th axis would work, but it could fairly easily be done manually, albeit it may be a little tedious. I seem to remember @RichCournoyer doing something like this?
Dan
I’m no expert here but I think it would be best if you to machine both sides with a flat endmill then use a 4th axis to cut the gears using a tapered ballnose endmill.
I’m sure @RichCournoyer would be the best to reply here, he’s the watchmaker of this forum Maybe this thread could be used for inspiration.
That sort of thinking shows the potential of having a 4th axis or a CNC lathe — I really suspect the next big thing in desktop CNC is going to be an affordable/accessible CNC lathe, or well implemented 4th axis.
Take a look at this guide, which was created by a guy solving Pretty much exactly the same problems as you’re trying to. He makes molds to cast tiny robot parts out of high strength resins, gears included, on his CNC machine.
Harvey Tool has tiny cutters with long reach:
http://www.harveytool.com/
I can vouch for the quality, and have received excellent help from them when I’ve needed advice on what to use, etc.
Here’s what I can share from my experience machining several hundred delrin gears on Bantam desktop CNC machines for a commercial client.
Here’s a link to one of my IG posts from that job: @ekramer3 IG Gears
The gear was 27mm diameter, 32 pitch with a tooth height (parallel to the axle bore) of 4.76mm.
The part required two-sided machining but the critical features (gear teeth and center axle bore) were machined in the same setup to avoid introducing inaccuracies in the geometric relationship between these two features when the part was flipped over. I designed a custom fixture to help with alignment for the two-sided job.
I used a 1/8” end mill to machine the part to the specified OD, then switched to a Harvey long reach stub (Harvey part 76225, .025” diameter, .075” flute length, .213” reach ) for the gear teeth machining. This tool was much stiffer than the equivalent long flute length tool of the same diameter, with the tradeoff being time. Several .075” stepdowns needed to machine the full depth of the geometry.
Small diameter tools like the above like high spindle RPM. I ran the tiny tool at 26k rpm 2600mm/min feedrate. At 10k rpm on the Nomad this tool might be a bit more of a challenge.
–cheers,
Ed K.
Thanks so much everyone! I am still busy researching. If anything else, please post- cheers.
This topic was automatically closed 30 days after the last reply. New replies are no longer allowed.
