What Is Broaching CNC Machining?

• 1
  Key takeaways
• 2
  How broaching CNC machining removes material
• 3
  What a broach can cut, and what it cannot
• 4
  Finish, accuracy and the sizing teeth
• 5
  Broaching vs milling, EDM and shaping
• 6
  Materials, fixtures and coolant on the shop floor
• 7
  Signals that broaching is the right process
• 8
  Choosing between broaching and other internal-profile methods

A broach is a bar of tool steel carrying hundreds of cutting teeth in a row. Each tooth stands slightly taller than the one before it, and the rise between neighbours sets the chip load. The tool moves along a single straight axis, so every tooth takes its own slice as it passes. The last few teeth are often identical, acting as sizing teeth that finish the profile without changing depth.

That arrangement makes broaching different from milling or turning, where a rotating edge sweeps the surface many times. Here the cut is linear and one-directional. Cutting speed is typically 3–15 m/min in steel and 15–45 m/min in aluminium, and the whole cycle can finish in a few seconds for a short stroke. There is no tool-path programming for the profile itself.

The finished dimension is built into the broach, not into the motion. Once the tool is set and the stroke length is correct, every part that follows gets the same form. That repeatability is the main reason broaching cnc machining holds ground in high-volume spline and internal-gear work, where a mill would need a form cutter or a slow orbiting routine per part.

• 1
  Rise per toothCommonly 0.02–0.08 mm for steel, larger for softer aluminium and brass.
• 2
  Tooth countA long broach can carry 300+ teeth when the profile and stroke length allow.
• 3
  Chip spaceEach tooth's gullet must hold one complete chip without clogging the row.

Internal broaching needs a starting hole slightly larger than the broach's first tooth and a clear path through the part. Round bores, square bores, hexagons, keyways, internal involute splines and internal helical gears all fall inside that envelope on a helical broaching machine. External broaching covers flat faces, dovetails and slots on the outside of the part.

The limits come from the tool and the chip. A profile with a narrow, deep slot gives the chip nowhere to go, so the tooth loads up and breaks. A blind bore stops the tool before the sizing teeth reach the bottom, leaving an incomplete form. A thin wall can distort under the radial force of a wide broach, especially in aluminium or thin-walled stainless.

Sharp internal corners are another stop sign. The broach tooth needs a radius to survive the cutting load, so a true 90° internal corner is not realistic. If the drawing calls for a square internal corner, the usual fix is to leave a relief groove or split the feature into two operations. Engineers who catch this at the design stage avoid a redesign later.

• 1
  Good fitThrough holes, uniform wall thickness, generous chip room, one dedicated profile.
• 2
  Poor fitBlind bores, thin walls, sharp internal corners, one-off quantities.

Because the sizing teeth burnish the wall as they pass, broached surfaces usually come off the machine between Ra 0.8 and 1.6 μm, and a well-ground tool with good coolant can reach Ra 0.2–0.8 μm on the flank. That is often good enough to skip a secondary finishing step, which is one reason the process stays competitive against milling plus grinding.

Dimensional control depends on tool wear, not on machine motion. A new broach cuts on size; as the teeth wear, the profile drifts. Shops track this with periodic re-grinding and gauge checks. On a stable tool, profile tolerance of ±0.005 mm is realistic on a spline minor diameter. Positional tolerance of the feature relative to an outside datum depends on the fixture, so the fixture design matters as much as the broach.

Helical splines add a rotation axis. The tool or the work rotates in step with the linear stroke, and the lead must stay consistent across the full length. When the lead drifts, the spline mates poorly and shows as noise or backlash in the assembled shaft. That is a measurement job, not a visual one.

CNC milling can cut an internal spline with a small end mill and an orbiting path, but the cycle time climbs and the corner radii come from the cutter, not the drawing. For one prototype, that is fine. For 10,000 hubs, it is not. Broaching wins on cycle time once the profile repeats, because the cut is one stroke instead of thousands of interpolated moves.

Wire EDM cuts almost any internal profile and holds tight tolerance, but it is slow and limited to conductive materials with a through path. It suits hardened tool steel, thin sections and odd geometries that a broach cannot reach. Broaching cannot cut a hardened part; the teeth would fail. So the sequence matters: broach first, then heat treat, then grind if needed.

Shaping and slotting sit in between. A shaper cuts a keyway with a single-point tool in many strokes, which is cheap for low volume but slow and less consistent on a long run. For a keyed hub in quantities under a few hundred, shaping is often the practical answer; above that, the broach pays back.

• 1
  Prototype countMilling or EDM avoids the broach tooling cost; broaching is not economical for a single part.
• 2
  Hardened partsBroach before hardening, or use EDM/grinding after.

Broaching behaves well in 4140, 4340, 1045 and 4130 steel, in 303, 304 and 17-4PH stainless, and in brass and aluminium bronze. It also cuts ductile iron and some titanium grades, though tool life drops and cutting speed must come down. Very soft, gummy aluminium can smear instead of shear, so tooth geometry and coolant need attention. Hardened steel above roughly 35 HRC is generally off the table for a broach.

The fixture has to hold the part rigidly against the stroke force and locate the starting bore accurately. A loose fixture lets the broach wander, which shows up as an off-centre spline or a tapered bore. For a spline hub, a pilot bushing that guides the front of the broach into the bore is common practice. It costs a little setup time and saves a lot of scrap.

Coolant does two jobs: it flushes chips out of the gullets and carries heat away from the teeth. Straight cutting oil is typical for steel, while soluble coolant works for aluminium and brass. On a horizontal broaching machine, the tool is pulled through the part; on a vertical machine, it is pushed or pulled depending on the design. Both need a chip path that does not recirculate debris into the cut.

• 1
  Good materials4140, 4340, 1045, 303/304 stainless, 17-4PH, brass, ductile iron.
• 2
  Difficult materialsHardened steel above 35 HRC, gummy pure aluminium, some titanium alloys.
• 3
  Fixture checkPilot bushing, rigid support, clear chip exit path.

The clearest signal is a repeating internal profile in a through bore, with a wall thick enough to take the radial force. If the drawing shows an involute spline, a keyway, a hexagonal bore or an internal gear across a run of parts, broaching usually beats milling on both cycle time and consistency. The tool cost amortises quickly once the order reaches four figures.

A second signal is a surface finish requirement that would otherwise need a separate finishing operation. When the sizing teeth leave Ra 0.8–1.6 μm on the flank, the part may go straight to assembly after inspection. That removes a grinding step, a setup, and the risk of a handling mark between operations.

The opposite signals matter just as much. One-off parts, blind holes, thin walls, sharp internal corners and profiles that change from part to part all point away from broaching. In those cases, milling, EDM or shaping will be cheaper and faster. We review drawings against these signals before quoting, and we will say when broaching is not the answer.