Quick answer: To cut a spur gear on a milling machine, turn a blank to (Z + 2) × module diameter, mount it on a mandrel between a dividing head and tailstock, center a gear form cutter over the blank, and cut each tooth space to a whole depth of 2.25 × module (metric) or 2.157 ÷ DP (imperial), indexing 40 ÷ Z turns of the crank between cuts on a standard 40:1 dividing head.
That is the whole process in one paragraph. The rest of this guide covers each step in the detail you actually need at the machine: the calculations, the setup checks that determine whether your gear meshes or gets scrapped, cutting speeds for HSS form cutters, and the mistakes we most often see when customers send us photos of failed teeth.
This method, called gear milling or form milling, is how machine shops have produced one-off gears, replacement gears, and small batches since long before hobbing machines became common. It remains the most practical way to make a gear when you have a milling machine and a dividing head but no dedicated gear cutting equipment. Maxwell Tools has manufactured the form cutters used in this process since 1976, and this guide reflects what works on the shop floor, not just in a textbook.
What You Need Before You Start
Gear milling needs surprisingly little equipment:
A milling machine: A horizontal mill is the traditional choice because the arbor-mounted cutter setup is more rigid, which matters when you are hogging out tooth spaces in steel. A vertical mill works too, with the cutter mounted on a stub arbor in the spindle. Rigidity is the deciding factor, not orientation.
A dividing head (indexing head) with tailstock: The dividing head rotates the blank by an exact angle between cuts so that every tooth space is equally spaced. Most dividing heads use a 40:1 worm ratio, which is what the indexing formula below assumes.
A gear form cutter matched to your gear: The cutter must match your gear’s module (or diametral pitch), pressure angle, and tooth count range. Cutter profiles change with tooth count, which is why cutters come numbered 1 through 8, each covering a range of teeth. Selecting the right number, pressure angle, and material is a topic of its own, and we cover it fully in our guide on how to choose an involute gear cutter. For the cutting process itself, just verify the three markings on the cutter face: module or DP, pressure angle, and tooth range.
A mandrel, arbor, and a machinist’s square or dial indicator for alignment.
A gear blank: Usually turned on a lathe from the same material as the mating gear or per the drawing. Blank accuracy decides gear accuracy, as you will see in Step 1.
Step 1: Calculate the Gear Dimensions
Three numbers control the entire job. For a metric gear with module m and Z teeth:
Blank outside diameter = (Z + 2) × m
Whole depth of cut = 2.25 × m
Indexing = 40 ÷ Z crank turns per tooth
For imperial (diametral pitch) gears, blank OD = (Z + 2) ÷ DP and whole depth = 2.157 ÷ DP. One practical note: most quality form cutters have the whole depth stamped or etched on the cutter body. When the marked depth differs slightly from the formula, follow the cutter marking, because it reflects the exact profile ground into that tool.
Worked example. Say you need a module 2 spur gear with 35 teeth, 20° pressure angle:
- Blank OD = (35 + 2) × 2 = 74.00 mm
- Whole depth = 2.25 × 2 = 4.50 mm
- Indexing = 40 ÷ 35 = 1 and 5/35 = 1 and 1/7 turns per tooth
For the fractional part, pick an index plate circle divisible by 7. On a 21-hole circle, 1/7 of a turn equals 3 holes. So after each tooth: one full crank turn plus 3 holes on the 21-hole circle. Set the sector arms to span 3 holes so you never count wrong at tooth number 23 of 35.
If you want to skip the arithmetic, our spur gear calculator outputs blank diameter, tooth depth, and all standard dimensions from module and tooth count in both metric and imperial.
Why blank diameter accuracy matters more than it looks. The gear’s outside diameter never touches the mating gear, so machinists sometimes turn the blank casually. This is a mistake. The blank OD is your only reference surface for setting depth of cut. If the blank is 0.2 mm oversize and you cut to nominal depth from its surface, every tooth ends up 0.1 mm too thick per flank and the gear binds. Turn the blank to within 0.02 to 0.05 mm of calculated OD, and make sure the bore is concentric with the OD, ideally by finishing both in one lathe setup.
Step 2: Set Up the Dividing Head and Blank
- Clean the mill table thoroughly and bolt down the dividing head and tailstock. Chips under the base translate directly into runout at the gear.
- Align the dividing head spindle parallel to the table travel using a test bar and dial indicator. Misalignment here produces tapered or bevel-shaped teeth.
- Press or clamp the blank on a mandrel and mount the mandrel between the dividing head and tailstock centers, driven by a carrier and catch plate. The blank must be absolutely tight on the mandrel. A blank that slips mid-cut produces a spiraled, scrapped gear.
- Check blank runout with a dial indicator. Anything beyond about 0.02 to 0.03 mm will show up as pitch variation in the finished gear.
Step 3: Center the Cutter on the Blank
The cutter’s centerline must pass exactly through the blank’s axis. An off-center cutter produces teeth with asymmetric flanks: one side of every tooth has the wrong profile, and the gear runs noisy or fails under load even though it looks fine to the eye.
The classic method: raise the table until the blank nearly touches the cutter, hold a steel rule or use a centering gauge to bring the cutter tip to the exact top dead center of the blank, then lock the saddle. On a vertical mill, indicate off both sides of the blank and split the difference. Take five extra minutes here. Centering error is the single most common cause of gears that “measure right but run wrong.”
Step 4: Touch Off and Set the Depth of Cut
Start the spindle, and carefully raise the table (or feed the cutter) until the rotating cutter just grazes the blank surface. A cigarette paper or feeler gauge between cutter and blank makes this precise. Zero the vertical dial or DRO at contact.
Now feed in the whole depth. For our example gear, that is 4.50 mm total. Whether you take it in one pass or two depends on the gear size:
- Fine pitches (module 1.5 and below, roughly 16 DP and finer): a single pass to full depth is normal and avoids the errors introduced by re-referencing.
- Module 2 to 4: rough at 80 to 90 percent of depth, then take a finishing pass to full depth around the complete gear. The finishing pass cleans up cutter deflection and gives every tooth an identical final cut.
- Coarse pitches (module 5 and up): two or three roughing passes, then finish. Forcing a coarse tooth in one pass overloads the cutter corners and shortens tool life dramatically.
Important: complete each pass around all teeth before increasing depth. Never cut some teeth to full depth and then return, because cutter wear across the job would make early and late teeth measurably different.
Step 5: Cut, Index, Repeat
- Lock the dividing head spindle. Cutting with the spindle unlocked lets the blank rock against worm backlash and ruins tooth spacing.
- Engage the table feed and cut the first tooth space clear through the blank width.
- Return the table to the start position with the cutter withdrawn or stopped; dragging a form cutter backward through the slot scores the flanks.
- Unlock the spindle, index the crank (one turn plus 3 holes in our example), always approaching the final hole in the same rotation direction to take up worm backlash. If you overshoot, go back half a turn and come in again.
- Re-lock the spindle and cut the next space. Repeat until the gear is complete.
Count your teeth as you go and mark tooth one. The oldest gear cutting mistake in the book is index confusion at tooth 30 of 35.
Cutting Speeds and Feeds for HSS Gear Cutters
Form cutters are HSS form-relieved tools with fine cutting geometry, so run them slower than you would run a plain milling cutter of the same diameter. Practical starting values for HSS involute gear cutters:
| Workpiece material | Cutting speed | Feed |
| Free-cutting mild steel | 20 to 25 m/min | 0.04 to 0.08 mm per tooth |
| Medium carbon steel (C45, EN8) | 15 to 20 m/min | 0.03 to 0.06 mm per tooth |
| Alloy steel (EN19, 4140, pre-hardened) | 10 to 15 m/min | 0.02 to 0.05 mm per tooth |
| Cast iron | 15 to 20 m/min | 0.05 to 0.10 mm per tooth |
| Brass and bronze | 30 to 45 m/min | 0.05 to 0.10 mm per tooth |
| Aluminium alloys | 60 to 90 m/min | 0.05 to 0.12 mm per tooth |
Convert to spindle RPM with: RPM = (1000 × cutting speed) ÷ (π × cutter diameter in mm). A typical 75 mm diameter module 2 cutter in mild steel at 22 m/min runs at roughly 90 to 95 RPM. That will feel slow if you are used to carbide end mills. Resist the urge to speed it up: overheated flank corners are the number one killer of form cutters.
Use cutting fluid generously on steel. On cast iron, cut dry or with air blast.
Six Mistakes That Scrap Gears (and How to Avoid Them)
- Cutter off center. Asymmetric tooth flanks, noisy mesh. Fix: center carefully in Step 3 and verify by measuring the first tooth space symmetry before cutting the rest.
- Depth referenced from a wrong-size blank. Teeth too thick or too thin across the whole gear. Fix: turn the blank to tolerance and verify OD with a micrometer before touching off.
- Blank slipping on the mandrel. Spiral witness marks, ruined spacing. Fix: proper press fit or expanding mandrel, and check tightness after the first two teeth.
- Indexing against backlash. Cumulative spacing error, one visibly wide or narrow tooth space. Fix: always approach index holes from the same direction, and lock the spindle before every cut.
- Wrong cutter number for the tooth count. The gear cuts cleanly but the profile is subtly wrong and meshes poorly, because each cutter number is profiled for a specific tooth range. Fix: verify the tooth range marked on the cutter against your gear before mounting it. Our cutter selection guide explains the numbering system in full.
- Skipping the finishing pass on coarse teeth. Visible tool marks, tooth-to-tooth size drift from cutter deflection. Fix: rough to 80 to 90 percent, finish all teeth in one continuous final pass.
How Accurate Is a Milled Gear, and When Should You Hob Instead?
A well-executed milled spur gear on a sound dividing head typically achieves commercial quality in the range of DIN 9 to 10 (roughly AGMA Q7 to Q8). That is entirely adequate for machine tool change gears, replacement gears in gearboxes running at moderate speeds, agricultural and material handling equipment, and prototypes.
Form milling has two inherent accuracy limits. First, one cutter profile serves a range of tooth counts, so the profile is theoretically exact only at one count within that range. Second, spacing accuracy depends on the dividing head’s worm and your indexing discipline. For high-speed, high-load, or noise-critical gears (automotive transmissions, for example) generated processes are the right tool. Continuous generation with gear hobs produces a theoretically correct involute at every tooth count and is far faster in volume. If you are weighing the two methods for a production decision, see our detailed comparison of gear hobbing vs gear milling.
The practical rule: one to twenty gears, or any gear too large for your hobbing capacity, mill it. Hundreds of gears, hob it.
Frequently Asked Questions
Can you cut gears on a milling machine without special equipment?
Yes. A milling machine, a dividing head with tailstock, and a gear form cutter matched to the gear’s module and pressure angle are all you need. This form milling method produces gears accurate enough for most industrial replacement and low-volume applications, without any dedicated gear cutting machine.
What is the depth of cut formula for gear cutting?
For metric gears, whole depth = 2.25 × module. For imperial gears, whole depth = 2.157 ÷ diametral pitch. A module 2 gear therefore needs 4.50 mm total depth. Always check the cutter body first: quality form cutters have the exact cutting depth marked on them, and the marked value takes priority.
How do you calculate indexing for gear cutting?
On a standard 40:1 dividing head, crank turns per tooth = 40 ÷ number of teeth. For 35 teeth: 40 ÷ 35 = 1 and 1/7 turns, which is one full turn plus 3 holes on a 21-hole index plate circle. Choose any plate circle divisible by the fraction’s denominator.
Can I cut a spur gear on a vertical milling machine?
Yes. Mount the cutter on a stub arbor in the vertical spindle and the dividing head on the table with its axis horizontal. A horizontal mill is more rigid and preferred for coarse pitches and steel, but a vertical mill handles small and medium gears in most materials without trouble.
Do I need coolant when milling gears?
For steel, yes: flood the cut with soluble oil or cutting oil to protect the HSS cutter’s fine profile edges and improve flank finish. Cast iron and brass are normally cut dry. Because form milling is interrupted cutting, each tooth cools between engagements, but coolant still meaningfully extends cutter life in steel.
How accurate is gear cutting on a milling machine?
With a sound dividing head, an accurate blank, and careful centering, form milling typically achieves DIN quality 9 to 10, sufficient for replacement gears, change gears, and general industrial transmissions at moderate speeds. For precision or high-speed gearing, generated methods like hobbing or shaping followed by finishing are the better choice.
What cutter do I need to mill a spur gear?
You need a form cutter matching three parameters of your gear exactly: module or diametral pitch, pressure angle (14.5° or 20°), and a cutter number whose tooth range includes your gear’s tooth count. Cutters are numbered 1 to 8 across the tooth range. See our involute gear cutter selection guide for the full numbering chart.
Can you cut helical gears on a milling machine?
Yes, but it requires a universal milling machine with a swiveling table and a dividing head geared to the table’s leadscrew so the blank rotates as it feeds. The table is swiveled to the helix angle. It is significantly more involved than spur gear milling and deserves its own setup guide.
Get the Right Cutter for the Job
The process above is only as good as the tool profile doing the cutting. Maxwell Tools has manufactured HSS gear form cutters in Rajpura, India since 1976, in module and DP sizes, 14.5° and 20° pressure angles, standard and half-number sets, exported to workshops in over 50 countries. Every cutter is form-relieved so the profile stays correct through its full resharpening life.
Tell us your module, tooth count, and material, and we will confirm the exact cutter you need, usually within one working day. Call or WhatsApp +91 82646 21011, or send your gear drawing through the contact form.