CNC gear machining

How CNC cuts a perfect semicircular gear, cut by cut

A practical walkthrough for engineers and buyers who need half-round gear teeth that mesh on the first try. We cover stock prep, workholding, tool paths, cutting parameters, and inspection limits. Read it and you can judge whether your part belongs on a 3-axis mill or a 5-axis center.

Get Instant Quote Talk to an Engineer

±0.005 mm toleranceRa 0.8–1.6 μm finishNo minimum order quantityDFM feedback in 12 hours

5-axis CNC machining of a perfect semicircular gear and engine parts

On this page

Key takeaways

Half-round teeth are a fixturing problemThe geometry is simple; holding the blank so it cannot lift is what decides the result.

Rough then finish, never one passLeave 0.3–0.5 mm radial stock, then take a light finishing pass for tooth form.

Check the root, not the tipRoot radius and fillet carry the load on a half gear; measure there first.

5-axis pays off above 30° helixBelow that angle a 3-axis setup with a form tool usually costs less.

Inspect before you break the setupPitch and runout readings taken on the machine catch errors while you can still fix them.

Basics

What a perfect semicircular gear actually demands

A semicircular gear is a gear segment cut on a radius instead of a full circle. It usually swings through 90° to 180° of arc and carries teeth on the outside or inside of that arc. Because it does not rotate a full turn, nobody balances it. Instead, the tooth form at both ends of the arc has to be right, and the mounting face has to sit square to the pitch line.

Three numbers decide whether the part works. The first is pitch accuracy: the distance from one tooth flank to the next along the arc. The second is runout against the bore or mounting face. The third is tooth profile, which sets how smoothly the segment hands off load to its mate. On a full gear, errors average out around the circle. On a segment, they do not. Every tooth is a boundary case.

That is why a perfect semicircular gear is mostly a setup problem, not a tool path problem. The CAM side is well understood; any competent programmer can generate a trochoidal or form-milled path along an arc. The hard part is keeping a half-round blank from moving, springing, or lifting while the cutter pushes on it.

We machine these on 3-axis, 4-axis, and 5-axis equipment, depending on helix angle and tooth count. For a straight-tooth segment under 80 mm across, a 3-axis mill with a dividing head and a form cutter is often the cheapest route. Add helix, undercut, or a tight root radius and the 5-axis centers earn their keep.

1
Arc length sets the work envelopeA 180° segment of a Ø300 mm pitch circle needs 471 mm of travel.
2
Tooth count drives the indexing methodFewer than 20 teeth usually means single-index milling, not hobbing.
3
Material hardness limits form toolsAbove 40 HRC, plan for ground inserts instead of a shaped cutter.

Setup

Workholding choices for a half-round blank

The blank has no full circle to grip, so a standard 3-jaw chuck will not hold it. Three approaches work, and each has a failure mode. Soft jaws bored to the outside diameter of the arc are the default for short segments. They spread clamping force over a wide area, which matters on aluminium and thin-walled steel. The failure mode is jaw lift: if the jaws are bored on a taper, the part climbs as the cutter passes.

A fixture plate with dowel pins and a strap clamp suits segments with a flat back face. Locate on two pins for position, clamp over the thickest section, and keep the clamp away from the tooth path. The failure mode here is chatter. A strap clamp pressed on one point lets the free end of the arc ring like a bell. Add a jack screw under the unsupported end.

For high-volume runs, a dedicated fixture with a matching radius pocket is the right answer. The pocket supports the whole arc, and a side-acting clamp locks the part against a shoulder. Cost is higher up front, but cycle time drops because the operator loads against hard stops instead of dialing in each blank.

One rule applies to all three. Support the arc under the cut. If the cutter can push the segment into open air, it will, and the tooth flanks will come out tapered.

1
Soft jawsBest for Ø20–120 mm arcs; watch for jaw lift on tapered bores.
2
Fixture plate with pinsBest for segments with a flat mounting face; add support under the free end.
3
Radius pocket fixtureBest above 500 parts; needs a shoulder for repeatable location.

Cutting

Tool paths and parameters that hold tooth form

Roughing removes the bulk between teeth. Use a 3-flute carbide end mill at 60–70% of the tooth depth, and leave 0.3–0.5 mm of radial stock on every flank. A common mistake is leaving too little. On a segment, the finishing tool has to enter and exit at the arc ends, and a 0.1 mm stock allowance leaves nothing to blend the entry marks.

Finishing decides profile. For straight-tooth segments, a form cutter or a ground single-angle cutter cuts the full flank in one pass. Speeds sit lower than normal milling: 40–60 m/min for 4140, 120–180 m/min for 6061-T6. Feed per tooth stays at 0.03–0.06 mm. Push it harder and the flank tears at the root, where chip evacuation is worst.

For helical or crowned teeth, use a 5-axis path with a ball or barrel cutter and a constant lead. Keep the stepover at 0.05–0.1 mm on the flank and let the tool tilt follow the helix. A barrel cutter cuts a wider swath than a ball nose, so you get the same finish with fewer passes and less heat in the part.

Coolant matters more than most people expect. Through-spindle coolant clears chips from the root, where recutting ruins surface finish. On stainless and titanium, use high-pressure coolant and reduce the finishing pass depth to 0.15–0.25 mm.

1
Roughing stockLeave 0.3–0.5 mm radial; never less than 0.2 mm.
2
Straight teethSingle-index with a form cutter; 40–60 m/min in 4140.
3
Helical teeth5-axis constant-lead path; 0.05–0.1 mm stepover on the flank.

Inspection

Measuring a segment without a gear checker

Most job shops do not own a dedicated gear measuring center, and a segment is awkward to mount on one anyway. Three measurements cover the critical geometry. First, pitch: use pin measurement over two or three teeth with gauge pins in the tooth spaces, and compare to the theoretical chord. Second, runout: indicate the mounting face and the bore, then the tooth tips, and hold tip runout inside the drawing limit.

Third, profile: a profile projector or an optical comparator with a tooth overlay gives a fast pass or fail on the flank shape. For load-carrying segments, a coordinate measuring machine with a small stylus can trace the flank and report deviation from the nominal involute. This is slower, but it catches root fillet errors that a projector misses.

Do the first check while the part is still clamped. If pitch drifts at one end of the arc, you can often correct it with a fixture adjustment instead of scrapping the blank. We inspect every part before shipment, with reports available on request, and the same discipline applies to prototype quantities of one.

Surface finish is the last gate. On a gear flank, Ra 0.8–1.6 μm is a normal machined target, and Ra 0.2–0.8 μm is achievable on the 5-axis centers when the drawing calls for it. Below Ra 0.2 μm you are into grinding or lapping territory.

1
PitchGauge pins over two or three teeth; compare chord to nominal.
2
RunoutIndicate bore and mounting face first, then tooth tips.
3
ProfileOptical comparator for speed, CMM stylus for root fillet detail.

Process

Step-by-step: cutting the segment

1
1. Check the drawing and run DFMConfirm module, pressure angle, tooth count, helix angle, and root radius. Flag any root radius under 0.3 × module, because it will need a smaller cutter and a slower pass. Send the model out for DFM review before buying stock.
2
2. Prepare the blankSaw or waterjet the arc profile to within 0.5–1.0 mm of finished size. Stress-relieve steel above 200 mm arc length, then face both sides so the mounting face is flat within 0.02 mm.
3
3. Set the datumEstablish the pitch circle center from the bore and the flat face. On a dividing head, indicate the bore to 0.01 mm TIR. This single step controls pitch accuracy more than any cutting parameter.
4
4. Rough the tooth spacesUse a 3-flute carbide end mill, 60–70% of tooth depth, and leave 0.3–0.5 mm radial stock. Keep the radial depth of cut under 0.5 × tool diameter to control deflection.
5
5. Semi-finish the flanksStep down to a 0.3–0.5 mm radial cut with a smaller cutter. This removes the roughing stair-steps and gives the finishing tool a uniform allowance to follow.
6
6. Finish the flanksSingle-index with a form cutter, or run a 5-axis constant-lead path. For 4140, run 40–60 m/min at 0.03–0.06 mm per tooth with high-pressure coolant. Do not stop mid-flank.
7
7. Deburr and blend the endsBreak the tooth edges at 0.1–0.2 mm × 45°, and blend where the tooth runout meets the arc ends. A sharp corner at the segment end becomes a crack starter under load.
8
8. Inspect before unclampingMeasure pitch with gauge pins and tip runout with a dial indicator while the part is still located. Correct fixture offset if one end of the arc drifts.

Selection

Which setup fits your segment

Match the method to tooth geometry and quantity

Method	Best for	Typical tolerance	Watch out for
3-axis + dividing head	Straight teeth, under 80 mm arc	±0.01 mm pitch	Jaw lift on thin arcs
4-axis mill	Straight or slight helix, mid volume	±0.01 mm pitch	Indexing backlash at arc ends
5-axis simultaneous	Helix above 30°, crowned flanks	±0.005 mm profile	Longer cycle, higher rate
Form milling	High volume, fixed tooth form	±0.01 mm profile	Cutter wear drifts the form
Wire EDM	Hardened steel above 50 HRC	±0.005 mm profile	Slow, no root radius blend

Send the model, get a fixturing plan

A perfect semicircular gear comes down to holding the blank and leaving the right finishing stock. Send us the STEP file and we will tell you which setup fits and where the tooth form will fight you.

Get Instant Quote Talk to an Engineer

FAQs

Questions engineers ask before ordering

Can you cut a semicircular gear from a 3D model only?

Yes. Send STEP or IGES with the pitch circle, pressure angle, and tooth count defined. If the model is a solid without tooth data, we can rebuild the tooth form from module and pressure angle.

DFM feedback comes back within 12 hours, and it often catches a root radius that is too small for the cutter you have in mind.

What is the smallest root radius you can machine?

It depends on the cutter. A standard form cutter leaves a root radius of roughly 0.3 × module. Below that we switch to a smaller single-angle cutter and take lighter passes.

Very small roots on hardened steel are better handled by wire EDM, which cuts any radius the wire can reach.

How do you hold a segment that has no full bore?

We locate on the arc itself or on a flat mounting face. Soft jaws bored to the arc diameter cover most short segments, and a radius pocket fixture with a side clamp covers production runs.

If there is no flat and no bore, we machine a temporary tab into the blank and cut it off after the teeth are finished.

Which materials are common for gear segments?

4140 and 4340 for loaded industrial segments, 17-4PH for corrosion resistance, 6061-T6 and 7075 for lightweight prototypes, and 440C where wear resistance matters.

Bronze and brass segments show up in low-load instrument work, and PEEK covers non-magnetic or chemically exposed cases.

Can you harden and finish after machining?

Yes. We machine in the annealed state, then the part goes out for heat treatment and comes back for a finishing pass or grinding where the drawing allows.

Plan the stock allowance for that second operation up front. Leaving 0.2–0.3 mm on the flanks is normal.

What quantity makes sense for a first run?

There is no minimum order quantity, so a single prototype is fine. Most programs start with one or two parts to prove the tooth form, then move to a fixture and a production run.

For runs above 500 parts, a dedicated fixture usually pays for itself in cycle time.