KEY TAKEAWAYS

✓
Broaching removes material in a single linear pass using a multi-tooth tool, making it exceptionally fast for high-volume production of repeating features.

✓
Internal broaching handles keyways, splines, hex bores, and round holes; external broaching handles flat surfaces, slots, and gear teeth.

✓
Tolerances of 0.001 inch and surface finishes as fine as 32 Ra microinch are routinely achievable with proper tooling and setup.

✓
Broaching is a high-tooling-cost, low-per-part-cost process — it becomes economically viable at moderate-to-high production volumes.

✓
Always evaluate stock allowance, material hardness (ideally below 40 HRC), and part rigidity before specifying broaching in your design.

Broaching is a machining process that uses a toothed tool — called a broach — to remove material in a single, controlled linear stroke. Each tooth on the broach is slightly larger than the one before it, so the tool progressively cuts deeper with every inch of travel until the final geometry is achieved. The result: a finished feature produced in one pass, often in under ten seconds of cutting time. No multiple setups, no tool changes, no interpolated paths.

The broach itself is typically a long, hardened steel or carbide tool with roughing, semi-finishing, and finishing teeth ground into its body. The roughing teeth hog out the bulk of material, semi-finishing teeth approach final geometry, and finishing teeth bring the surface to spec. This staged cutting geometry is what makes broaching both fast and dimensionally consistent — every part produced from the same broach is effectively identical until the tool wears.

Broaching is used across aerospace, automotive, defense, and industrial equipment manufacturing. Common applications include cutting internal keyways in gears and hubs, producing splined bores in transmission components, generating hex or square internal sockets, and finishing flat external surfaces on high-volume parts. When a feature must be held to tight tolerances at volume, broaching is often the correct answer.

Rule of Thumb: If you need the same internal or external profile repeated across hundreds or thousands of parts, broaching will almost always beat milling on cycle time and per-part cost — once tooling is amortized.

Broaching operations are broadly classified as internal or external, and further divided by the direction of tool travel — linear pull, linear push, or rotary. Understanding the distinction helps engineers select the right process during design review.

Internal broaching operates inside a pre-existing hole. The broach is inserted through the hole and pulled (or pushed) through, enlarging or reshaping it. Internal keyways in gears, spline bores in drive shafts, and non-circular through-holes (square, hex, D-profile) are classic internal broaching applications. The starting hole must be drilled or bored first — broaching does not create the initial hole, it reshapes it.

External broaching — also called surface broaching — moves a broach across the outside of a workpiece to generate flat surfaces, slots, or contoured profiles. Automotive connecting rods are frequently surface-broached on both parting faces in a single pass. Pot broaching is a specialized external variant where the part is pushed through a stationary ring-shaped tool, common for producing external splines.

Continuous chain broaching is used for very high-volume flat work — parts are fixtured to a continuous conveyor and dragged past stationary broach sections. This variant is common in automotive body and engine component production where millions of identical parts are needed annually.

A broaching machine is fundamentally a high-force linear actuator designed to pull or push a broach through or across a workpiece with controlled speed and force. Machines are categorized as vertical or horizontal, and as pull-type or push-type. Vertical pull-down machines are the most common for internal broaching — the broach is pulled downward through the fixtured part using a hydraulic or electromechanical ram.

Cutting speeds in broaching are relatively slow compared to milling or turning — typically 20 to 50 surface feet per minute — but this is largely irrelevant to cycle time because the entire feature is cut in one pass. Setup time dominates the economics. Modern CNC broaching machines add programmable control over stroke length, speed profiles, and return stroke, reducing operator error and enabling faster changeovers.

Fixturing is critical. The workpiece must be rigidly supported to resist the broaching force, which can reach tens of thousands of pounds for large tools in hard materials. Poor fixturing leads to part movement, tool deflection, and out-of-tolerance geometry. Coolant — typically a sulfurized cutting oil for ferrous materials — is applied to lubricate the tool teeth and flush chips. Chip gullets machined between each tooth carry swarf away from the cutting zone, preventing re-cutting and surface damage.

Warning: Never attempt to broach a part without adequate pilot hole size and surface finish. An undersized or rough pilot hole overloads the roughing teeth and can snap a broach — a costly and potentially dangerous failure.

Broaching delivers some of the tightest tolerances achievable in production machining. Dimensional tolerances of ±0.001 inch are standard; ±0.0005 inch is achievable with sharp tooling and stable fixturing. Surface finish typically falls in the 32 to 63 Ra microinch range, with finishing-quality broaches achieving 16 Ra microinch or better. For many applications — keyways, splines, gear bores — this eliminates the need for secondary grinding.

Material hardness is the primary constraint. Broaching works best on materials at or below 38–40 HRC. Softer steels (1018, 1045), aluminum alloys, brass, bronze, and cast iron are all excellent candidates. Stainless steels and nickel superalloys can be broached but demand premium carbide or coated HSS tooling, reduced cutting speeds, and more frequent resharpening. Hardened tool steels above 45 HRC are generally not candidates — grinding or EDM are more appropriate for post-hardening internal features.

Ductility matters too. Highly ductile materials like pure copper or annealed aluminum can smear rather than shear cleanly, generating built-up edge on tool teeth and degrading surface finish. A light work-hardened condition or alloyed grade often machines better. Material selection should be confirmed with your manufacturing partner early — especially for aerospace and defense components where material certs are mandatory.

Key Insight: Broaching is a shear-dominant process. The cleaner the shear — meaning the sharper the tooling and the better the material machinability — the closer you get to the tolerance and finish floor of the process.

The broach is a precision, application-specific tool — there is no universal broach. Every profile geometry (keyway width, spline tooth count, hex size) requires a dedicated tool ground to that specification. This is the central economic reality of broaching: tooling cost is high, but per-part cost is extremely low once tooling is amortized. A high-speed steel internal keyway broach might cost $500 to $2,000; a complex multi-tooth external broach in carbide can run $10,000 or more. Standard keyway and spline sizes have off-the-shelf tooling available, which dramatically reduces upfront cost.

Broach teeth are ground with specific geometry parameters: hook angle (rake), back-off angle (relief), pitch, and rise-per-tooth. Hook angle controls how aggressively the tooth shears — high hook angles (15–20 degrees) for ductile materials, lower angles for brittle ones. Rise-per-tooth (chipload per tooth) is typically 0.001 to 0.003 inch for internal broaching in steel. Total tool length is a function of rise-per-tooth multiplied by the number of teeth needed to achieve full depth of cut.

Broaches can be resharpened multiple times by re-grinding the face of the teeth — extending tool life significantly. A well-maintained broach in production can produce tens of thousands of parts before retirement. Tracking resharpening history and maintaining dimensional logs of pilot hole size versus finished bore is standard practice in any quality-controlled broaching operation.

Designing for broachability starts with understanding what the process can and cannot do geometrically. Broaching requires a straight-line path through or across the workpiece — any undercut, taper, or interrupted geometry breaks this constraint and may require a different process. The entry and exit of the tool must be clear; a blind keyway (closed at one end) is not broachable with a standard pull broach and requires either a push broach (limited depth) or a milling operation instead.

Wall thickness and part rigidity are critical. Thin-walled parts can deflect under broaching load, causing out-of-round bores or mislocated keyways. A general rule: the wall thickness between the broached feature and the nearest external surface should be at least 1.5 times the depth of cut. This varies with material and feature size, but it is a useful starting point for preliminary design review.

Feature location relative to part datums also matters. Keyway angular position, spline clocking, and hex flat-to-flat orientation must be established by fixturing — the broach itself does not locate the feature angularly. If angular position is critical, the fixturing design must incorporate a locating pin or nest that references the correct datum. Specifying angular tolerances without accounting for fixturing capability is a common source of quality escapes. Reviewing your broached feature drawings with an experienced manufacturing partner before releasing to production can catch these issues early — Nimble’s certified partner network offers free DFM review on every submitted part.

DFM Warning: A blind keyway on a production drawing is a frequent cause of quoting delays and re-design cycles. Always specify whether a keyway is through or blind — and confirm your shop has push-broaching capability if blind features are required.

The most common alternative to broaching for internal features is CNC milling with a keyway or slotting cutter. Milling is more flexible — it can produce blind keyways, work on complex geometries, and requires no dedicated tooling per profile. But milling an internal keyway is dramatically slower than broaching: a broached keyway takes seconds; a milled equivalent can take minutes. At volumes above a few hundred parts, this cycle-time gap dominates the cost equation. At prototype or very low-volume quantities, milling usually wins on total cost because there is no tooling amortization burden.

Electrical Discharge Machining (EDM) — specifically wire EDM and sinker EDM — can produce internal splines, hex bores, and complex profiles in hardened materials that broaching cannot touch. EDM is slow and expensive per part but material-hardness-agnostic. It is the go-to process for post-hardening internal features or exotic superalloy components where broaching is not viable.

Gear shaping and hobbing are related processes used specifically for internal and external gear teeth. Shaping uses a reciprocating cutter and can produce internal gear forms that broaching cannot efficiently generate at small production volumes. For high-volume external splines, rotary broaching (a spinning broach driven by a lathe or mill turret) is an increasingly popular alternative — it works on CNC turning centers without a dedicated broaching machine, though it is limited in depth and profile complexity.

Process Selection Rule: Use broaching when you have a repeating, straight-through internal or external profile at moderate-to-high volume. Use milling for low volume or blind features. Use EDM for hardened materials or complex post-heat-treat geometry.

Not every machine shop has broaching capability — the machines are specialized, the tooling is application-specific, and the process knowledge required to hold tight tolerances consistently is not trivial. When sourcing broached components, verify that your supplier has the correct machine type (horizontal vs. vertical, pull vs. push) and that off-the-shelf tooling exists for your profile — or that custom tooling lead time is factored into your schedule. Standard ANSI and DIN keyway and spline profiles typically have stocked tooling; non-standard profiles require custom broach fabrication, which can add four to eight weeks to first-article lead time.

Inspection of broached features requires appropriate gauging. Internal keyways are typically checked with keyway gauges or CMM probing routines. Splines require spline gauges (go/no-go ring gauges for external, plug gauges for internal) or full CMM analysis for critical aerospace and defense applications. CMM inspection is the only way to fully characterize a spline profile, lead, and runout simultaneously. Ensure your supplier documents this data and provides it with each production lot — not just first article.

When you submit broached parts through Nimble’s certified partner network, quotes are returned within 24 hours and every order includes CMM inspection documentation. The network is AS9100 and ISO 9001 certified, covering the documentation and traceability requirements that aerospace and defense procurement teams require. If your part requires ITAR compliance, that coverage is in place as well.

READY TO SOURCE?

Table of Contents

Related Services

Get a Quote in 24h

Upload your drawing and get a detailed quote with free DFM review.