CNC Broaching Applications in Production: Where the Process Fits

• 1
  Key takeaways
• 2
  What CNC broaching actually does in a machining center
• 3
  Keyways and single-slot work
• 4
  Internal splines and multi-tooth profiles
• 5
  Square, hex, and non-round bores
• 6
  Tooling, speeds, and cutting data that hold up
• 7
  Accuracy, finish, and how the feature gets inspected
• 8
  When broaching is the wrong choice
• 9
  Broaching vs milling vs EDM for internal profiles

On a machining center, broaching is a stroked cut, not a spinning one. A broach bar with one tooth or a small cluster of teeth enters the bore and moves along the Z or W axis, taking a shallow radial bite each pass. Between passes the spindle or a rotary table indexes the part, so the next tooth or the next face lines up with the cut.

That is the whole difference from a broaching press. A press pushes one long multi-tooth tool through in a single stroke and finishes the part in seconds. On a machining center the same profile is cut in 15 to 120 strokes, so cycle time is measured in minutes. What you buy in return is flexibility: no dedicated tool, no long tool lead time, and the feature is cut in the same setup as the bore it sits in.

This matters most for internal profiles. A keyway inside a hub, a spline inside a gear blank, a hex inside a coupling: these are features where a milling cutter has to reach around a corner and often cannot. Broaching reaches straight down the axis and leaves walls that are parallel to the bore.

One limit sets the whole process. The tool must have room to enter and exit, and chips must have room to leave. Every application below is really a question of whether the bore is deep enough to justify broaching and open enough at both ends to clear chips.

The most common CNC broaching applications in production are keyways cut after turning. A hub, gear, or pulley comes off the lathe with a finished bore, then a single-point broach bar strokes through and removes the keyway. A 6 mm keyway in a 30 mm bore typically takes 15 to 25 strokes at 0.05 to 0.15 mm radial feed per stroke, depending on the material and how much stock the tool can take without chatter.

Tolerances are comfortable for a machined part: ±0.02 mm on keyway width and about 0.03 mm on depth are routine. The keyway should be cut in the same setup as the bore where possible, because position error between the bore and the slot is what causes assembly problems on a keyed shaft, not the slot width itself.

Tool material follows the workpiece. HSS bars handle aluminum, brass, and mild steel well. Carbide is the better choice for cast iron, alloy steel, and stainless, where abrasive wear shortens HSS life quickly. Coatings help in steel but can hurt in aluminum, where built-up edge is the bigger problem than wear.

A blind keyway or one that stops inside the bore needs a relief at the end for the tool to clear. If the drawing has a square-ended slot with no relief, raise it before quoting. That single detail decides whether the part can be broached or has to be shaped or EDM'd.

Internal splines are where CNC broaching earns its place in low and medium volume. A pull broach for a 20-tooth spline can cost several thousand dollars and take weeks to deliver. A CNC broach bar with a single tooth or a small cluster cuts the same spline in 40 to 120 strokes, and the tool is a fraction of the cost. For a prototype run or a 500-piece order, that difference decides the quote.

The trade-off is time. A press broach might finish a spline in 20 to 40 seconds. CNC broaching may take 3 to 8 minutes per part, sometimes more in tough alloys. At high volume the press wins on cost per piece. At low and medium volume the CNC route wins because there is no dedicated tool to amortize.

Spline accuracy from a stroked cut lands in IT7 to IT8, with 0.02 to 0.05 mm total tolerance on width across the teeth. Inspection is usually go/no-go plug gauges for the tooth form plus a CMM check on the first part and at intervals after that. Position of the spline to the bore and to any external feature is the number that gets checked hardest.

Interrupted bores are the exception. If the spline bore is crossed by cross-holes, ports, or a keyway, the teeth take a hammering at every gap. Sometimes that is acceptable with reduced feed. Often it is not, and the part should be shaped or milled instead.

Square, hex, and other non-round bores are cut two ways. A rotating tool can follow the bore and generate the profile, or a fixed tool can be indexed between strokes to cut one flat at a time. Indexing gives straighter walls and sharper corners because the tool does not sweep an arc into the corner.

A hex bore in a coupling is a typical case. Cutting it with a small end mill on a helical path works, but the corners come out with the cutter radius and the walls can taper in a deep bore. Broaching produces flat walls and a corner radius equal to the tool edge, which is usually much smaller. If the drawing calls for a sharp internal corner, broaching gets closer than milling, though a small radius always remains.

A square bore with an open end is easy to broach. A square bore that must stop blind with square corners cannot be broached without a relief, because the tool has to exit somewhere. Deep non-round bores also push chip clearance to its limit, and that is where cycle time climbs sharply.

For thin plates and shallow hex features, punching or milling is faster and cheaper. Broaching is worth the setup when the bore is deep enough that wall straightness and corner sharpness actually matter to the function.

Surface speeds in broaching are low by milling standards. In steel, run 10 to 30 m/min. In aluminum and brass, 50 to 100 m/min is reasonable. The number that matters more is radial feed per stroke: 0.05 to 0.15 mm is the working range for a single-tooth bar in steel. Push above it and the tooth digs, chatters, and leaves a torn wall.

Chip evacuation is the main process risk, and it drives most of the parameter choices. Ductile materials produce long stringy chips, and a packed bore can break the tool or scrap the part. Through-spindle coolant aimed at the cut, peck-style stroke patterns that retract and clear, and chip-breaking grooves on the teeth are the three fixes that work.

Depth-to-diameter ratio is the practical ceiling. Above about 3:1, chip clearance becomes the limiting factor and cycle time rises sharply. A 20 mm bore 80 mm deep is already in that zone and needs a peck pattern and a coolant strategy agreed before the job runs.

Rigid setup is not optional. The part must be held so the bore axis is aligned with the stroke, and any looseness shows up as taper in the profile. If the part has to be re-fixtured, cut the broached feature in the same setup as the bore or accept the position error.

Typical accuracy from CNC broaching is IT7 to IT8 on the profile, with 0.02 to 0.05 mm total tolerance on width or across-flats depending on the feature. Surface finish lands around Ra 1.6 to 3.2 μm in steel and can reach Ra 0.8 μm with a finishing pass and sharp tooling. Those are ordinary numbers for a controlled process, not a claim of exceptional precision.

Inspection is straightforward but has to be planned. Keyway width is checked with pin gauges or a bore gauge. Splines are checked with go/no-go plug gauges, plus a CMM on the first part for tooth position and lead. Hex and square bores are checked with the mating part or a custom gauge. Taper along the bore is checked separately because it is the error that a simple go gauge will miss.

For a first article, ask for the position of the profile to the bore axis, not just the size. Assembly problems on keyed and splined parts usually come from angular position or taper, and both are invisible to a width measurement.

When a finishing pass is specified, say so on the drawing. It changes the stroke count and the cycle time, and it is the difference between Ra 1.6–3.2 μm and Ra 0.8 μm on the same part.

Broaching is the wrong choice when the feature is shallow and open. A keyway in a shaft end, a slot that breaks out of the side, or a hex in a thin plate is usually faster to mill or punch. The setup cost of a broaching job only pays back when the profile is enclosed and deep enough that the alternative is slow or inaccurate.

It is also wrong for very large profiles, where tool cost and stroke length climb together, and for parts where the bore is interrupted by cross-holes or ports. Interrupted cuts hammer the teeth, and no parameter choice fully removes that.

Heat-treated parts above roughly 45 HRC should be broached before heat treat, or moved to EDM or grinding after. Cutting a hardened spline with a stroked bar is possible in a narrow window, but tool life drops and the risk of a scrapped part rises.

Finally, consider volume honestly. If the annual demand is tens of thousands of identical splines, a pull broach or a dedicated press is the right investment and CNC broaching is only a bridge. If demand is hundreds to a few thousand, and the design may still change, the stroked cut in a machining center is the cheaper route overall.