Gear CNC machining essentials for engineers

• 1
  Why gear CNC machining is a different problem
• 2
  Which tooth forms can be cut on a machining center
• 3
  Blank preparation, fixturing and cut strategy
• 4
  Heat treatment changes the gear, not just the hardness
• 5
  How to check a milled gear without a gear tester
• 6
  Milled gear or ground gear: pick by the numbers

A gear is a cam that repeats. Every tooth has to sit at the same angular pitch, carry the same load, and roll against its mate without shock. A milling machine cuts one tooth at a time, so the pitch error comes from the rotary axis and from how the blank was held, not from a hob that indexes itself. That is the whole difference.

Gear CNC machining earns its place when the batch is small, the geometry is not a standard catalog shape, or the gear is one feature on a larger part. A housing with an internal ring gear, a sector with three teeth, a timing wheel with lightening pockets: these are milled, not hobbed, because the setup survives the mix.

The trade is speed for flexibility. A gear shaper or hobber removes a tooth in seconds. A ball end mill takes minutes and leaves scallops that must be blended. You pay for that in cycle time and in the skill of the programmer. You get back a part that can be finished in the same setup as its mounting bores.

So the first question is never which machine. It is whether the tolerance on pitch, profile and runout can survive a milled surface at all, and at what cost per part.

• 1
  Milled gears win on low volumeOne to a few hundred pieces, or any part where the gear shares a setup with other features.
• 2
  Hobbed and shaped gears win on volumeThousands of identical teeth justify a dedicated machine and a dedicated fixture.
• 3
  Gear CNC machining wins on integrationWhen bore, face, keyway and teeth must share one datum, milling keeps them concentric.

Spur and helical gears in module 1 to 6 are routine. The tool is a ball or bull nose mill, smaller than the tooth gap, swept along a path generated from the involute. Tool diameter sets the minimum root radius, so a module 2 gear with a 16 mm bore cannot use a 12 mm cutter in the gap. Programmers check that before quoting.

Internal gears and ring gears are the strongest case for gear CNC machining. A shaped internal gear needs a special cutter and a relief groove. A milled internal gear needs only a tool that reaches past the bore, and the same fixture can face, bore and cut the teeth.

Bevel and hypoid gears are a different animal. Spiral bevel geometry is generated by a cradle motion that a three-axis mill cannot reproduce, and a five-axis approximation only holds for light loads. If the application is a real bevel pair carrying torque, buy the pair ground. If it is a display model or a low-load index, milling is fine.

Non-involute profiles are where milling has no competition. Cycloidal discs, Novikov arcs, asymmetric teeth, ratchet sectors, and clock escapements are all just curves. A CAM system cuts them as easily as a circle, while a gear machine would need a form tool that does not exist.

• 1
  Good fitSpur, helical, internal, racks, sectors, non-involute profiles, timing wheels.
• 2
  Possible with careStraight bevel at low load, worm wheels in soft material, splines that double as gear teeth.
• 3
  Wrong fitGround spiral bevel pairs, high-volume automotive transmission gears, any gear above about module 8.

The blank decides the outcome. Saw cut bar with 1.5 mm to 3 mm of stock, then turn both faces and the bore in one operation so the bore is square to the face. Any runout here becomes tooth runout later, and it cannot be corrected by the cutter path. For a gear that will be hardened, leave 0.3 mm to 0.5 mm on the flanks for finish grinding after heat treatment.

Fixturing is where most milled gears go wrong. A three-jaw chuck does not repeat well enough for a rotary table index. Use a collet or a dedicated arbor with a shoulder that seats the gear face, and indicate the bore to within 0.01 mm before cutting. On a five-axis machine, the trunnion plus a Ø400 mm rotary table holds the gear at any angle, so a helical tooth can be cut without re-clamping.

Cut strategy for a soft steel gear: rough the gap with a smaller end mill at 0.5 mm to 1 mm radial step, then semi-finish leaving 0.15 mm on the flanks, then finish with a single pass per flank. Climb milling on both flanks keeps the load even and avoids a burr on one side. A 6 mm carbide ball mill in 4140 at 38 HRC runs around 180 m/min surface speed and 0.05 mm per tooth feed.

Cooling matters more than on a plain pocket. The tool spends time in a narrow slot, so through-spindle air blast or high-pressure coolant is needed to clear chips. Recutting a chip in a tooth gap will chip the edge and mark the flank, and that mark becomes a stress riser after hardening.

• 1
  Turn the bore firstBore and face in one operation, then use them as the datum for every gear feature.
• 2
  Leave stock for grind0.3–0.5 mm on flanks if the gear is case hardened or through hardened.
• 3
  Clear the chipsAir blast or high-pressure coolant; a recut chip ruins the flank finish.

Case carburizing at 1,650 °F to 1,700 °F distorts the part. A 100 mm diameter gear can move 0.05 mm to 0.15 mm on the bore and a similar amount on the pitch diameter. If the drawing calls for ±0.02 mm on the flanks and the gear is carburized, the teeth must be cut undersize by the expected growth and ground after. That is a two-stage process, and it has to be planned before the first cut.

Through hardening behaves differently. Quench and temper to 28 to 32 HRC on 4140 gives a tough core with modest movement, and a milled gear can often be used as cut if the tolerance is loose. Above about 45 HRC the flank cannot be cut with a carbide mill at a sane cost, so plan on finish grinding.

Nitriding adds almost no distortion because the temperature stays near 1,000 °F. It is the right choice for a milled gear that needs a hard skin but cannot be ground afterwards, such as an internal ring gear with a closed shoulder. Depth is thin, 0.1 mm to 0.3 mm, so it resists wear and not shock.

We coordinate heat treatment and finish grinding as one sequence. The blank is cut with grinding stock, the lot goes out to the furnace, and the flanks come back for a light pass. Sending a finished gear to the furnace usually means scrapping it.

• 1
  Carburized gears need grind stockExpect 0.05–0.15 mm of movement on a 100 mm diameter part.
• 2
  Nitride when you cannot grindLow temperature, low distortion, thin case.
• 3
  Never heat treat to final sizePlan the sequence before the first cut, not after.

Most shops do not own a dedicated gear measuring machine, so inspection is built from what is available. A coordinate measuring machine with a scanning probe can trace a flank and report profile error and lead error against the nominal involute. That is the closest thing to a gear tester and it produces a number you can compare to the drawing.

Pitch error is easier. Index the part on a rotary table, touch the flank of each tooth with a dial indicator or a probe, and record the readings. Total index variation of 0.02 mm over 24 teeth is a normal result for a milled gear. If it is 0.08 mm, look at the fixture before blaming the machine.

Runout is the check that catches the most problems. Mount the gear on a mandrel that matches its bore and measure the pitch circle with a dial indicator. Bore-to-pitch runout of 0.03 mm will make a gear noisy at speed even if every flank is perfect. This is exactly the error that gear CNC machining is good at controlling, because the teeth were cut on the same datum as the bore.

For surface, a simple comparison works. Ra 1.6–3.2 μm is the as-machined range; a finish pass with a smaller stepover gets to Ra 0.8–1.6 μm. A flank that looks polished but measures rough usually means the tool was rubbing instead of cutting, so check the feed per tooth.

We inspect 100% of parts before shipment, with raw material check, in-process monitoring and final inspection, and reports are available on request.