Broaching machining process explained for keyways, splines and precision profiles
What the broaching machining process does
The broaching machining process uses a multi-tooth cutting tool, called a broach, to remove material in a controlled sequence. The tool is pushed or pulled through a hole or across a surface, with each tooth taking a small part of the total cut. Broaching is commonly selected for repeated features such as keyways, internal splines, square or hexagonal holes, serrations, slots and shaped external profiles. Its main advantage is that roughing, semi-finishing and finishing can be built into one stroke, which makes the process productive when the part geometry and production volume justify dedicated tooling.
For readers comparing machining processes, broaching is best viewed as a precision profile-generating operation, not a general-purpose cutting method. It can hold accurate forms and produce a good surface finish, but it is less flexible than milling or EDM because the broach is usually designed around one feature, one size range and one family of parts.
How broaching works
A broach may look simple from a distance, but its geometry is carefully staged. Each cutting tooth is slightly higher, wider or otherwise more advanced than the tooth before it. This gradual increase is often called tooth rise or rise per tooth. As the broach travels through the workpiece, each tooth removes a small chip. The total stock removal comes from many small cuts rather than one heavy cut.
Standard machining references, including ISO 6779:2019 for vertical internal broaching machines, describe internal broaching as a linear cutting process in which a broach is pushed or pulled through a hole. The same basic principle applies to surface broaching, except that the cut is made across an outside face rather than inside a bore.
Roughing, semi-finishing and finishing teeth
The cutting section of a broach is normally divided into roughing teeth, semi-finishing teeth and finishing teeth. Roughing teeth remove most of the stock. Semi-finishing teeth reduce the remaining allowance and stabilize the profile. Finishing teeth are usually the same size and establish the final form and surface. This tooth sequence is the reason a single broaching stroke can replace several conventional cutting passes in suitable applications.
Pilots, gullets and chip control
Internal broaches often include a front pilot to align the tool in the starting hole and a rear pilot to support the tool as the finishing teeth pass through the part. The spaces between teeth, called gullets, provide room for chips. If the gullets are too small for the chip volume, chips can pack in the tool and damage the workpiece or the broach. For ductile materials, chipbreakers may be used to split chips and support evacuation.
Main types of broaching operations
Internal broaching
Internal broaching is used when the feature is inside a part. Common examples include internal keyways in hubs, involute splines, round holes sized from a pilot bore, square holes, hexagonal holes, serrations and special non-round profiles. The workpiece normally needs a starting hole large enough for the broach to enter. That starting bore is a process-control feature, not just clearance; its size, straightness, roundness and location all influence the finished feature.
Pull broaching is common for long internal broaches because pulling keeps the tool in tension. Push broaching is also used, especially for shorter tools, keyway broaching and press-style setups. In either case, the machine or press must provide enough force over the full stroke while keeping the tool aligned.
Surface and external broaching
Surface broaching removes material from the outside of a workpiece. It can generate flats, slots, grooves, external keyways, bearing surfaces and contoured forms. In production environments, surface broaching can be faster than milling or planing because the complete profile is distributed along the length of the broach. This makes it useful for parts where the same external form is repeated in significant quantities.
Rotary broaching
Rotary broaching, also called wobble broaching, is a related but distinct method often used on lathes or machining centers to create small polygonal or shaped holes. The tool is held at a slight angle and rotates with a wobbling action while being fed into the part. It is not the same as conventional linear broaching, but it serves a similar design need when a compact internal form must be produced without moving the work to a dedicated broaching machine.
Where broaching performs best
Broaching performs best when the feature is difficult or slow to produce by ordinary milling, drilling or shaping, but simple enough to be built into a dedicated tool. The process is especially attractive when many parts need the same geometry and inspection requirements are stable over time.
| Application | Why broaching fits | Key planning point |
|---|---|---|
| Internal keyways | The slot can be cut straight and repeatably through a hub or gear bore. | Confirm bushing, shim and broach size before machining the bore. |
| Internal splines | Many teeth can be generated at once instead of indexing around the part. | Control pilot hole quality and concentricity to the datum structure. |
| Square or hex holes | A non-round internal form can be produced from a prepared hole. | Provide enough relief and through-clearance for the broach and chips. |
| Surface slots and flats | Multiple cutting teeth produce the surface in one pass. | Use rigid fixturing to resist cutting forces and avoid chatter. |
| Production drivetrain parts | Cycle time and repeatability can justify dedicated tooling. | Balance tool cost against annual volume and changeover frequency. |
Broaching is not limited to steel, but material behavior matters. Too-soft materials may smear or adhere to the tool, while very hard materials accelerate wear and increase cutting force. Published technical guidance for gear and spline broaching often treats medium-hard ferrous materials as a favorable range and warns that work-hardening alloys, gummy aluminum grades and interrupted cuts require extra attention to tool coating, lubrication and chip flow.
Process planning checklist
A broaching operation should be planned from the finished feature backward. The following checklist helps avoid the common mistake of treating broaching as only a tooling decision. It is a system involving part design, starting stock, fixture stiffness, machine stroke, cutting force, lubrication, inspection and tool maintenance.
- Define the final profile. Specify the keyway, spline, polygon, serration or surface form with a complete drawing, datum scheme and inspection method.
- Check whether the feature is through or blind. Through features are usually easier because the broach and chips can exit. Blind features may require special tools or an alternative process.
- Prepare the starting hole or surface. For internal broaching, the pilot hole must allow tool entry while leaving the correct stock for the broach teeth.
- Confirm machine capacity. Stroke length, tonnage, pulling or pushing arrangement, tool length and part loading must all fit the machine.
- Plan chip evacuation. Chip gullet volume, coolant direction, lubrication and chipbreaker design should match the material and cut length.
- Choose tool material and coating. High-speed steel is common for many broaches, while powder metallurgy high-speed steels, carbide sections or coatings may be used for wear resistance and longer tool life.
- Set inspection before production. Go/no-go gauges, spline gauges, coordinate measurement, surface finish checks and concentricity checks should be defined before the first run.
The cost decision is simple in concept but specific in practice. Broaches can be expensive to design, manufacture and sharpen, yet part cost can be attractive when one tool runs many cycles with short stroke times. Low-volume prototypes, frequently changing designs and one-off repair work often lean toward milling, shaping, keyseating or EDM instead.
Advantages, limitations and alternatives
The main advantage of broaching is repeatable form generation in a short cycle. Because the broach carries the complete cutting sequence, the machine motion can be relatively simple. This helps maintain consistency across batches. Broaching can also reduce indexing errors in splines because many or all profile elements are cut in one guided pass.
The limitations are just as important. The broach is not flexible. A change in spline class, keyway width, corner radius, tooth form or bore condition may require a different tool. The process also creates high axial cutting forces, so thin-walled parts may distort if fixturing and tooth design are not matched to the workpiece. Long broaches need careful handling, storage and sharpening because small tool errors can show up directly in the finished feature. See also: CNC Machining.
| Process | Best fit | Typical trade-off |
|---|---|---|
| Broaching | Repeated internal or external profiles with stable geometry | High tooling commitment but fast and repeatable production |
| Milling | Flexible slots, pockets and external forms | More adaptable but may need multiple passes or indexing |
| Keyseating or shaping | Internal keyways and repair work | Lower tool cost for small runs but slower cycle time |
| Reaming | Finishing round holes | Good for cylindrical accuracy, not for splines or non-round forms |
| Wire EDM | Hard materials, sharp internal features or low-volume precision profiles | High accuracy and flexibility but often slower than production broaching |
Common quality risks and controls
Loss of concentricity
In internal spline and keyway work, the finished feature must often be concentric or correctly oriented to an existing bore or datum. Poor pilot hole quality, excessive clearance between pilot and bore, worn guides, uneven tooth wear or a misaligned pulling mechanism can shift the broach. A practical control plan starts with the pilot hole, then checks machine alignment, fixture seating and tool runout.
Poor surface finish
Surface finish problems can come from dull teeth, incorrect cutting speed, inadequate lubrication, chip packing, material adhesion or chatter. Since the finishing teeth determine the final surface, tool wear near the finishing section should be monitored closely. Grinding during resharpening must preserve tooth size relationships; otherwise the broach may cut undersize, oversize or unevenly.
Burrs and edge breakout
Exit burrs are common when a tooth leaves the cut, especially on ductile materials. Design engineers can help by specifying deburr requirements, providing accessible exit edges and avoiding fragile thin sections near the broached feature. Manufacturing teams can reduce burr formation through tool condition control, support at the exit side and suitable cutting fluid.
Tool breakage
Broach breakage is costly because the tool is a dedicated precision asset. Causes include insufficient starting-hole clearance, hard spots in the material, chip packing, machine misalignment, excessive cutting load, interrupted geometry and mishandling. Preventive maintenance should include cleaning, inspection for chipped teeth, controlled resharpening and protected storage.
Design guidelines for broached parts
Good broached parts are designed with the cutting direction in mind. Internal forms should be parallel to the broach travel; undercuts, reverse tapers and trapped chips complicate the operation. If a through hole is possible, it usually simplifies tooling and chip evacuation. If a blind feature is unavoidable, the design should allow relief for chips and should be reviewed before the broach is ordered.
Datum strategy also matters. A spline that transmits torque, a keyway that locates a pulley and a polygonal drive hole all depend on functional relationships to other surfaces. Those relationships should be shown clearly on the drawing. If the bore is machined in one setup and broached in another, the fixture must reproduce the intended datum location, not merely hold the part tightly.
Designers should also avoid specifying tighter tolerances or smoother finishes than the function requires. Broaching is capable of precision, but tighter requirements increase tool cost, setup effort and inspection burden. A realistic drawing gives manufacturing more room to choose the most reliable process.
Frequently asked questions
Is broaching a finishing process or a roughing process?
It can be both in one operation. A conventional broach includes roughing, semi-finishing and finishing teeth, so stock removal and final sizing occur during the same stroke. The amount of work assigned to each tooth group depends on material, allowance, profile and tool design.
Why does internal broaching need a pilot hole?
The pilot hole allows the broach to enter the workpiece and helps establish alignment. It also sets the starting condition for stock removal. If the pilot hole is out of position, out of round or incorrectly sized, the broached profile may inherit those errors or create excessive cutting load.
When is broaching better than milling?
Broaching is often better when the same keyway, spline or shaped profile must be produced repeatedly with short cycle time and stable dimensions. Milling is usually better when the design changes often, production volume is low, or the feature can be produced easily with standard cutters.
Can broaching be used for blind holes?
Blind-hole broaching is possible in some cases, but it is more difficult than through-hole broaching because the tool and chips need space at the end of the cut. Many blind internal profiles should be evaluated against shaping, slotting, rotary broaching or EDM before committing to a custom broach.
What is the biggest cost driver in broaching?
The dedicated broach is usually the major cost driver, followed by machine capacity, fixtures, setup and maintenance. Broaching becomes more economical as the same tool is used across enough parts to offset design, manufacturing and sharpening costs.