CNC Gear Processing Guide for Machined Gears
Gears rarely fail because the material was wrong. They fail because the tooth flank, the bore and the mounting face were not held to each other. This guide explains how CNC gear processing works, where it beats hobbing and shaping, and which gear geometries should never be quoted as a machined part.
In this article
- 1
- 2
- 3
- 4
- 5
- 6
How CNC gear processing actually cuts a tooth
Two families of machines make gears. Generating machines roll a hob or push a shaping cutter through the blank, and the tooth form comes out of the cutter profile plus the rolling motion. CNC gear processing works the other way: the tooth space is a pocket, and a rotating tool removes it along a programmed path.
That difference decides everything downstream. A hob cuts every tooth in one continuous pass on a dedicated machine. A machining center cuts one flank at a time, or one tooth space at a time, and the flank position comes from the machine axes and the tool radius. There is no cutter that already knows your profile.
The practical result is a lead-time and batch-size trade. Generating machines pay off above roughly 10,000 identical gears, where the setup cost of a dedicated hob or shaper cutter is spread thin. Below that volume, and anywhere the part has a bore, a keyway, a flange or a threaded hub, CNC gear processing wins because the same setup produces the tooth and the mounting features.
Cycle time is the honest cost. Milling a 24-tooth module 2 spur gear with a Ø3 mm end mill takes far longer than hobbing it. For a one-off fixture gear that is irrelevant. For a 50,000-piece automotive pump gear it is fatal to the business case, and we say so at the quote stage.
Involute profiles, modules and what the tool can reach
An involute flank is a curve, and a small ball or bull nose tool can only approximate it. Two settings control the approximation: chord tolerance and scallop height. Chord tolerance in the CAM toolpath keeps the programmed points close to the true involute; scallop height controls the ripple left between adjacent passes.
For a module 2 gear running at moderate speed, a scallop height of 5–10 μm is usually smooth enough after a light finishing pass. For a ground-equivalent gear running at high pitch line velocity, that ripple becomes noise and a wear point. If the drawing calls for AGMA 10 or better, the flank normally needs grinding after milling, and we treat it as a two-process job.
Root fillet radius is the other hard limit. A full radius root is the single biggest driver of bending fatigue life, and it is exactly the feature a small end mill struggles to leave clean. Tool shank clearance and reach determine the smallest internal gear you can cut. Below module 1, the tool simply does not fit between the teeth.
Internal gears and racks are tighter still. An internal spur gear with a small bore and a large tooth count leaves no room for the tool holder to swing inside the ring. Those parts go to shaping or to wire EDM for prototype quantities. We will tell you which route is realistic rather than quote a machined part that cannot be cut.
Material choice for machined gears
Alloy steel is the default for loaded gears. 4140 and 4340 in the pre-hardened or quenched-and-tempered condition give a strong core with enough toughness to survive shock loads. 1045 is cheaper and machines cleanly, and it is a reasonable choice for moderate-duty gears that will be case hardened later.
Stainless covers corrosion and clean-room work. 303 is the easiest to machine but the sulfur addition costs fatigue strength. 304 and 316L hold up in food and medical environments. 17-4PH (SUS630) is the one to reach for when you need both corrosion resistance and real strength; it machines well in the H1025 or H1150 condition and can be finish-machined after heat treat with modest distortion.
Aluminium and plastics have a clear place. 7075-T6 handles light-loaded timing and encoder gears where inertia matters. POM, PA and PEEK run quiet and need no lubrication, which is why they show up in medical and office equipment drives. Their tooth strength is low, so check the torque before you commit.
Bronze and brass are common for worm wheels and low-speed drives. C93200 bearing bronze is the standard worm wheel material because it tolerates sliding contact. Hardened steel worms running against bronze wheels is a proven pairing. Running a bronze wheel against a bronze worm is not, and it will gall.
Bore, face and tooth in one 5-axis setup
Tooth accuracy is meaningless if the bore is not concentric to the pitch circle. The most reliable rule in gear work is to cut the bore, the mounting face and the teeth in the same setup, or to cut the teeth from the finished bore as the datum. Every extra setup adds runout.
Simultaneous 5-axis machining makes that practical. The rotary table holds the blank, the tool stays perpendicular to the flank as it sweeps the involute, and the same program reaches the bore, the keyway and the hub face. Our shop runs 16 simultaneous 5-axis centers with a Ø400 mm rotary table for exactly this kind of part.
For long shafts and large ring gears the work envelope matters more than the axis count. We machine up to 4,000 mm in the largest travel, so a long gear shaft can be turned, milled and drilled without re-chucking. Re-chucking is where runout is born.
Thermal drift is the quiet error. Aluminium grows about 23 μm per meter per degree Celsius, so a 200 mm gear checked on a warm machine can read 5 μm off by the time it cools. For tight tolerance gears we let the part stabilize before final inspection, and we cut aluminium with coolant volume high enough to keep the blank temperature steady.
What to measure, and when milling is not enough
A gear is a system of features, and inspection has to treat it that way. The bore diameter and roundness set the mounting. The pitch circle runout sets the mesh. The tooth-to-tooth spacing sets the noise. Profile and lead deviation set the load distribution across the face width.
Basic inspection covers bore diameter, face runout and over-pin or span measurement, which is the practical shop-floor way to verify tooth thickness. Over-pin measurement with the right pin diameter gives a number that maps directly to tooth thickness, and it is fast enough to run on every part.
Analytical inspection on a gear measuring center gives profile and lead charts. That is the right call when the drawing specifies an AGMA or DIN quality grade, or when a gearbox is noisy and nobody can say which part is at fault. On a first article we will run the chart and send it with the report.
Quality grade is the dividing line. Machined and lightly finished flanks land around AGMA 8–10 depending on module and tooling. AGMA 12 and above normally requires form grinding after heat treat, and that is a different process chain with a different price. Claiming a higher grade without grinding is where gear quotes go wrong.
Our tolerance floor is ±0.005 mm (±0.0002 in) on the features we control, with finishes from Ra 0.2–0.8 μm on fine-ground work up to Ra 1.6–3.2 μm as-machined. Every part gets a raw material check, in-process monitoring and a final inspection before shipment, with reports on request.
CNC gear processing versus hobbing and shaping
Pick the process from volume, geometry and the quality grade the drawing asks for.
| Factor | CNC machining | Hobbing / shaping | When it decides the job |
|---|---|---|---|
| Typical volume | 1 to a few thousand | Above 10,000 pieces | Small batch goes to CNC |
| Tooth form | Toolpath approximation of involute | True generated involute | Grade above AGMA 10 needs grinding |
| Bore and teeth | Same setup, low runout | Often a second op | Concentricity-critical parts favor CNC |
| Smallest module | About module 1 | Well below module 1 | Fine pitch goes to generating |
| Internal gears | Limited by tool clearance | Standard capability | Small internal rings go to shaping |
| Racks and long parts | Up to 4,000 mm travel | Length limited by machine | Long racks favor CNC |
| Prototype lead time | 3–5 days after DFM | Cutter lead time first | Prototypes favor CNC |
| Hardened flanks | Milled then ground | Hobbed then ground | Both finish with grinding |
Where this lands
If the gear is a prototype, a low-volume run, or a part where the bore, face and teeth must be concentric, machine it on a 5-axis center and grind only if the drawing asks for AGMA 10 or above. If it is a fine-pitch or small internal gear above 10,000 pieces, hobbing or shaping is the honest answer and we will say so.
Gear machining questions we get weekly
Can you cut a gear to AGMA 12 without grinding?
No. Milled flanks land around AGMA 8–10 depending on module and tooling. AGMA 12 and above needs form grinding after heat treatment because the tooth form has to be corrected for distortion, and no milling strategy reaches that band on hardened steel.
If the drawing specifies AGMA 12, quote the job as mill plus grind. A milled-only quote at that grade will fail inspection.
What is the smallest module you can machine?
Around module 1 on a 5-axis center, and the limit is tool clearance rather than machine accuracy. Below that the end mill that fits between the teeth is too small to leave a usable root fillet or to survive the cut.
Fine-pitch gears go to hobbing, shaping or wire EDM for prototypes. Send the tooth count and we will tell you which route is realistic.
Do you machine internal gears and racks?
Yes, within limits. Internal gears are constrained by tool holder clearance inside the ring, so a small bore with a large tooth count is often not machinable. Racks are easier because the travel is open, and we can cut up to 4,000 mm in the largest work envelope.
For long racks, straightness after heat treat is usually the bigger risk than the tooth form.
Which materials do you stock for gears?
Alloy steel 4140, 4340, 1045 and 4130; stainless 303, 304, 316L, 17-4PH and 440C; aluminium 6061-T6 and 7075-T6; bronze and brass including C93200 worm wheel bronze; and plastics POM, PA and PEEK.
For worm wheels we would steer you to C93200 bearing bronze. It tolerates sliding contact far better than a straight brass.
How do you check tooth thickness on the shop floor?
Over-pin or span measurement is the fast method. It gives a number that maps directly to tooth thickness and it is quick enough to run on every part rather than a sample.
Base tangent length on external gears works the same way. Both are cheaper and faster than a full profile chart, and they catch the errors that actually matter at the mesh.
What do you need to quote a gear?
Module or diametral pitch, tooth count, pressure angle, helix angle, profile shift if any, material, heat treatment, quality grade and the mounting features. A 2D drawing with the bore and face tolerances plus a 3D model is ideal.
Send the files and we return a quotation with a free DFM analysis within 12 hours. No minimum order quantity, and uploads stay confidential under NDA on request.
Send the gear drawing and get a manufacturability answer
Module, tooth count, pressure angle, material and quality grade are enough for us to tell you whether it should be machined or generated, and what it will cost.
12-hour quote + free DFM100% inspection before shipment1 pc to 10,000+ parts
More gear and machining notes
We publish setup notes, tooling trials and inspection data from the factory floor.
