Gear Broaching Machine: How One Linear Pass Cuts a Full Tooth Form

• 1
  What Happens Inside a Gear Broaching Machine
• 2
  Tooth Forms a Gear Broaching Machine Handles Well
• 3
  When Gear Broaching Beats Hobbing and Shaping
• 4
  Broach Design Details That Decide Part Quality
• 5
  Inspecting Broached Gears and Holding Size
• 6
  What to Send When You Ask for a Broached Gear Quote
• 7
  Internal Gear Process Comparison

A gear broaching machine works on a simple principle: one tool carries the whole tooth form, and the machine only has to move it in a straight line. The broach is a bar of hardened tool steel with hundreds of cutting teeth ground along its length. Each tooth sits slightly taller than the one before it. As the bar is pulled or pushed through a bore, tooth number one removes a few micrometers, tooth fifty removes a few more, and the last few teeth are ground to full size and act as sizing teeth.

The tooth rise per cutting edge is the number that controls everything. Roughing sections typically rise 0.05–0.10 mm per tooth, semi-finish 0.02–0.04 mm, and finishing/sizing teeth 0.00–0.005 mm. A typical internal gear broach for a 40 mm bore runs 600–1,200 mm long and may carry 200 to 400 teeth. Because the rise is fixed in the tool, the machine contributes no feed axis in Z. It only supplies stroke force, stroke speed and guidance.

That is why broaching is called a generating-free process. There is no hob rotation, no dividing head, no electronic gear train. The tooth profile exists in the tool steel before the cut starts. The machine's job is to keep the broach straight, lubricated and at the right speed, and to hold the workpiece so the bore axis matches the broach axis within a few micrometers.

The consequence is speed and repeatability. A single stroke of 1–3 seconds produces a complete internal tooth form. Between parts, the operator swaps the workpiece, and the next stroke repeats the same geometry from the same tool. Spacing error from part to part comes almost entirely from workpiece location, not from the cutting action.

• 1
  Rise per tooth sets chip load0.05–0.10 mm roughing, 0.02–0.04 mm semi-finish, near zero for sizing teeth.
• 2
  No feed axis in the cutStroke force and speed are the machine's variables; profile comes from the tool.
• 3
  Sizing teeth do the accuracyThe last 4–8 teeth remove almost nothing and correct size and finish.

Internal spur gears are the classic application. A straight-sided bore with a straight tooth profile lets the broach be ground as a simple prismatic bar. Module 1 to module 4 internal gears with 12 to 60 teeth are routine. The limiting factor is usually broach length: a small module with many teeth needs a long bar, and a long bar needs a long stroke, a longer machine and a bigger investment.

Helical internal gears are possible but expensive. The broach must be rotated as it passes through the workpiece, so the machine needs a rotary broach drive synchronized to the stroke. The helix angle must match exactly, or the teeth will smear instead of cut. Helix angles up to about 15° are common; steeper angles push tool cost up sharply because the broach is ground on a helical path and cannot be resharpened as many times.

Splines, serrations and keyways share the same mechanics and are often cut on the same machine family. An involute spline is essentially an internal gear with a shallow tooth. A keyway is a single-tooth broach with a simple rise. If your part has a bore with any repeating internal profile, broaching is worth a look, because the cost per part falls fast once the tool exists.

Blind bores are the hard limit. A broach has to enter and exit, so the tooth form must run through the part or into a clearance groove. A blind internal gear with a shoulder at the bottom cannot be broached without a special relieved tool, and even then chip evacuation becomes a problem. If the drawing shows a blind toothed pocket, expect to mill or shape it instead.

• 1
  Great fitThrough-bore internal spur gears, module 1–4, 12–60 teeth.
• 2
  Possible, costlyHelical internal gears up to roughly 15°, needs rotary broach drive.
• 3
  Poor fitBlind bores without a clearance groove, interrupted profiles, very large modules.

Hobbing is the default for external gears and for large internal gears where the bore is big enough to admit a hob head. It is flexible: change the hob and the program and you cut a different gear. Broaching is the opposite. The tool is dedicated to one profile, so it only pays off when the same tooth form repeats. For an internal gear with a small bore, hobbing often cannot reach inside at all, which is where broaching becomes the only practical option.

Gear shaping sits between them. A shaping cutter strokes axially while the work rotates, generating the profile. It handles blind shoulders and large internal gears, and the tool is cheaper than a broach. The trade-off is cycle time. Shaping an internal gear can take minutes per part, while broaching takes seconds. If your annual volume is in the thousands and the profile is stable, broaching usually wins on cost per part.

The break-even is not a single number, but the logic is consistent. Broach tooling is a fixed cost, and the machine stroke is a fixed cycle. Higher volume spreads the tool cost and exploits the short cycle. Low volume with many variants favors hobbing or shaping, where the tool is cheaper and changeover is a program edit rather than a new broach.

There is also a bore-size rule of thumb. Internal hobbing needs radial clearance for the hob head and arbor, so it suits bores above roughly 80–100 mm. Below that, shaping or broaching takes over. At 20–60 mm bores with a through profile, broaching is usually the fastest route to a finished internal gear.

• 1
  Pick broachingStable profile, through bore, thousands of parts per year, bore under ~60 mm.
• 2
  Pick hobbingExternal gears, large internal bores, frequent design changes.
• 3
  Pick shapingBlind shoulders, large internal gears, low to medium volume.

Broach length is the first constraint. Total length equals the sum of roughing, semi-finish, finishing and sizing sections plus a pull end and a follower end. If the calculated length exceeds the machine stroke, the tool must be split into two or three passes, which adds handling and hurts concentricity. Designers often reduce the number of teeth or increase the rise per tooth to shorten the broach, but a bigger rise means a bigger chip and more risk of tearing in soft steel.

Chip load per tooth depends on the material. Free-machining steel such as 1045 and 4140 broaches cleanly at 0.06–0.10 mm rise per roughing tooth. Stainless 304 and 316 work-harden at the cutting edge, so the rise should stay above about 0.04 mm per tooth to keep the edge biting under the hardened layer rather than rubbing. Aluminium 6061 and 7075 broach very fast but tend to build up on the tooth face, so a polished rake face and a generous cutting fluid flow matter more than the rise value.

Concentricity between the bore and the tooth form is set by the fixture, not by the broach. A typical setup locates on a pilot diameter or a face and clamps axially so the part cannot shift during the stroke. If the drawing calls for the tooth form concentric to an outer diameter within 0.02 mm, that relationship has to be established in the fixture before the first cut.

Tool life is measured in meters of stroke, not parts. A well-ground broach in 1045 might run 300–800 meters between resharpenings. Each resharpen removes 0.05–0.15 mm from the tooth face and reduces tooth height slightly, so the sizing section is usually built with extra stock to allow 8–15 regrinds. Once the sizing teeth can no longer hold size, the broach is scrapped. That is why the tool drawing, not the part drawing, often decides the real cost per piece.

• 1
  Length drives machine sizeSplit broaches are possible but cost concentricity and handling time.
• 2
  Stainless needs a minimum riseKeep above ~0.04 mm per tooth to avoid work-hardening rub.
• 3
  Plan regrinds into the toolExtra sizing stock supports 8–15 resharpenings.

Broached internal gears are inspected on the same equipment as hobbed gears: involute profile checkers, lead checkers, span or pin measurement, and runout fixtures. The difference is what tends to drift. In broaching, size drift comes from tool wear on the sizing teeth, and it moves slowly and predictably. Operators track the last few teeth and pull the broach for resharpening when the pin measurement approaches the upper limit, rather than waiting for a reject.

Profile error is usually a tool grinding issue, not a machine issue. If the involute form is out but size is good, the broach needs regrinding or the tool was ground to the wrong pressure angle. If size drifts while profile stays good, wear is the cause. Separating those two symptoms early saves a lot of machine downtime that would otherwise be spent chasing a fixture problem that does not exist.

Surface finish on a broached tooth is normally Ra 0.8–1.6 μm, which is often good enough to skip a finishing operation. Tearing or chatter marks point to a chip load that is too high, insufficient cutting fluid, or a workpiece that is not rigidly clamped. In soft low-carbon steel, a small rise per tooth with a sharp edge gives a better finish than a heavy cut.

For production runs, we inspect 100% of parts before shipment, with raw material checks, in-process monitoring and final inspection. Reports are available on request. Where a customer needs traceability for automotive or medical programs, the inspection plan is written into the process sheet before the first article is cut. GreatLight holds ISO 9001:2015, IATF 16949:2016, ISO 13485:2016 and ISO 27001:2022.

• 1
  Size drift = tool wearTrack pin measurement and resharpen before the limit.
• 2
  Profile error = tool grindCheck pressure angle and regrind history first.
• 3
  Finish marks = cutting conditionsReduce rise, increase fluid, stiffen the fixture.

A broaching quote needs more than a 3D model. Send the part drawing with module, number of teeth, pressure angle, helix angle if any, bore diameter, tooth width, and the tolerance on each of those. State whether the tooth form runs through the part or stops at a shoulder. Confirm the material grade and heat treatment sequence, because hardening after broaching changes size and may require a grinding allowance.

Also state the annual volume and the expected number of years in production. Broach tooling is a fixed cost, and it only makes sense if the profile is stable across that volume. If the design may change, say so. In that case, a shaped or milled internal gear may be the better first step, with broaching introduced once the design freezes.

For prototypes and small batches, we can mill internal profiles on 4-axis and 5-axis machining centers instead of cutting a dedicated broach. This gets a functional part in days without tooling investment, and the same CAD data can later drive a broach if the design holds. GreatLight runs 127 high-precision CNC machines, including 16 simultaneous 5-axis machining centers, with a maximum processing size of 4,000 mm and a Ø400 mm rotary table for larger work.

Quotation and free DFM analysis come back within 12 hours, and production can start within 24 hours of approval. Parts ship in 3–5 days for standard work. There is no minimum order quantity, so a single prototype and a 10,000-part run go through the same process planning. Uploads are handled as confidential, and an NDA is available on request.

• 1
  Include in the RFQModule, tooth count, pressure angle, helix, bore, width, tolerances, material.
• 2
  State the volumeAnnual quantity and design stability decide whether tooling pays off.
• 3
  Prototype firstMilled internal profiles avoid tooling cost before the design freezes.