Broached Square Bores: Why Do Square Shafts Jam?

A broached square bore looks like the easiest feature on a drive hub, right up to the moment the shaft will not go in. Job 260616007 arrived in November 2023 from a maker of valve drive components whose previous supplier had shipped black anodized hubs that were assembled by hand with a mallet on one shift and dropped together by gravity on the next: the square measured correctly at the mouth of the bore and wrong at the far end, and on a share of the parts the flats had come out rotated, so a square shaft that fitted perfectly lined up wrong against the flange hole pattern and the assembly clocked into the wrong position.

The hubs in the photographs are the production parts from the order that followed: an AL6061-T6 twin-flange hub, turned and finished in one mill-turn setup, with a broached square bore through the body, six holes in each flange, a retaining groove on the far end, a radial cross hole, a black anodized finish and a laser mark on the body between the flanges. A broached square bore is the feature that decides whether the part works, and it is the one feature that cannot be corrected after it is cut.

What this hub has to do?

Four jobs, and the square bore is the one that carries the drive.

The square bore takes the shaft and transmits torque. A round bore with a key would do the same duty, but a square lets the shaft be indexed to the hub in four positions and needs no key, no keyway and no separate locking feature.

The two flanges locate the assembly. Both flange patterns are indexed at equal spacing, and the six holes on each flange have to line up with the mating bolt pattern, which means the two patterns have to be drilled from one datum rather than from two separate setups.

The retaining groove and the radial cross hole hold the assembly together. The groove takes the retaining ring that stops the hub sliding along the shaft, and the cross hole takes the pin that locks the shaft axially.

The anodized film and the laser mark are the finish and the identity of the part. Both are applied last, which means both have to work around the tolerances that the earlier operations already set.

Why a square bore is harder than a round bore?

A round bore is judged at one place, a square bore has to be judged along its depth

A round bore is measured with a pin gauge or a bore gauge at one depth, and if it is in size there, it is almost always in size through the rest of the bore, because a reamer or a boring bar cuts a consistent cylinder.

A square bore is cut by a broach: a long bar of stepped cutting teeth that is pushed or pulled once through a pilot hole, each tooth taking a small step deeper than the one before it. The width across the flats is therefore decided progressively, tooth by tooth, along the whole depth of the bore. If the cutting load changes along the stroke, or if the tool wears during the run, the bore ends up slightly different at the entry face than at the exit face. The part passes a check at the mouth and fails at the far end, which is exactly the symptom that made this job difficult to quote.

That is why the inspection on this order measures width across the flats at three depths down the bore rather than at the face only. A square that is uniform at the face and 0.02 mm different at the exit will still pass a face check, and it will still jam a shaft.

The broach also decides the clocking, and clocking cannot be fixed later

The angular position of the flats relative to the flange hole pattern is set by the broach. Whatever clocking the broach enters at is what the finished part has, because no later operation can rotate a square bore inside the part.

On a hub like this one the consequence is specific: a square shaft can fit the bore perfectly and still present its own flats at the wrong angle relative to the flange pattern, so the assembly bolts up but sits in the wrong rotational position. If the drawing does not call out the clocking tolerance, the shop has to guess whether the broach is guided from a flange hole or from a machined flat, and the guess is what produces a batch that is dimensionally perfect and functionally wrong.

The fix is procedural rather than expensive. The pilot hole is drilled and the broach is entered from the same datum that the flange patterns were drilled from, with a guide bushing that keeps the broach from rotating as it starts. The clocking is then checked against a flange hole on a gauge, not estimated by eye.

A broached square always has a corner radius

No broach can cut a mathematically sharp internal corner, because the cutting teeth have a finite corner radius. The corners of a broached square therefore carry a radius, and the mating square shaft must be relieved to match. When it is not, the shaft contacts on the flats and rides on the corner radii instead of seating, which feels like interference even though the width across the flats is correct.

The drawing should say what corner radius is allowed in the bore and what relief is provided on the shaft. Leaving both to assumption is how a part that measures in tolerance is rejected at assembly.

How the hub was made, step by step?

Step 1 - Turn the profile, the steps and the retaining groove in one setup

The outside profile, both flange faces, the stepped shaft and the retaining groove are turned in one setup with the part held on the main axis. One setup keeps the two flanges concentric to each other and to the bore axis, which is what the 0.02 mm flange concentricity call on this drawing depends on.

Step 2 - Mill the flange hole patterns in the same clamping

The six holes in each flange are milled in the same clamping as the turning, indexed from one datum, so both patterns share an axis and an angular reference. Drilling the two flanges in separate setups is what produces a hub whose holes each line up with the drawing and not with each other.

Step 3 - Drill the pilot hole to the size the broach expects

The pilot hole is drilled to the diameter the broach is designed to follow. Cutting it oversize leaves every tooth taking a lighter cut than intended, which lets the broach shift instead of cutting, and the resulting bore is wider at the exit than at the entry. Cutting it undersize overloads the teeth and promotes a heavy burr at the exit face.

Step 4 - Broach the square, guided from the flange datum

The broach is entered through a guide that holds its angular position, with the part oriented so the flats clock to the flange pattern as drawn. This is the step that fixes the part's clocking for good, so it is the step where the operator checks the setup rather than the finished part.

Step 5 - Deburr the exit edge and hold the corner radius

Broaching pushes a burr ahead of the last tooth, and the burr collects on the exit face. The exit edge is deburred without breaking the chamfer the drawing calls for, and the corner radii in the bore are checked against the radius the mating shaft is relieved to.

Step 6 - Black anodize to a uniform film

The hub is anodized black. The film grows out of the aluminum surface as well as into it, so the bore and the flange holes both tighten slightly, and the anodize line is told which dimensions matter for fit and which are protected. A part that fits before anodizing and does not fit afterwards has usually gone wrong here rather than at the machine.

Step 7 - Laser mark from the same datum

The identification mark is applied on the body between the flanges, referenced to the same datum that set the square and the flange patterns, so the mark lands in the same place relative to the flats on every part. On a black anodized surface the contrast of the mark is what makes it readable, so the mark is verified on the finished part rather than on a sample before anodizing.

Step 8 - Inspect the square along its depth, and the clocking against a flange hole

Final inspection covers width across the flats at three depths, the clocking of the flats to the flange hole pattern, flange concentricity, the groove position, the film and the mark. Checking the square at the face only is the one inspection habit that lets a bad batch leave the shop.

What the 1,600-piece run measured?

Sixteen hundred hubs shipped in 22 days, and the customer reported no hand fitting at assembly and no clocking errors on the line.

The fault we found in our own trial run

The fifty-piece trial run passed at the inspection bench and failed on the gauge, and the cause was our pilot hole.

Every trial part measured inside the width-across-flats band at the entry face. When we measured the same parts at the exit face, the width was running 0.02 mm wide, with a heavy burr on the exit edge. We had drilled the pilot hole 0.04 mm above the size the broach was designed to follow, on the reasoning that a slightly larger pilot hole would ease the cutting load and extend broach life. The opposite happened: with less material to remove, the teeth cut light, the broach was free to shift in the bore instead of being guided by the cut, and the last teeth opened the bore at the exit end.

Three changes went into production. The pilot hole diameter was pinned to the broach's requirement and checked on the first part of every batch. A guide bushing was added so the broach starts in a fixed angular position. And the width across the flats was measured at three depths every 100 pieces, which is the check that would have caught the drift on the trial parts in a single measurement.

Between the trial and the production run, the taper across the bore disappeared and the exit burr stopped being a deburring problem.

Three ways to cut an internal square, compared

The practical rule: broaching wins on unit cost once the shape repeats, milling wins when the geometry is still changing, and EDM wins when the corner radius or the material rules the other two out. On this part the square repeats on every piece, so the broach paid for itself inside the first order.

FAQ

Why is a broached square bore tight at one end and loose at the other?

Because a broach cuts progressively, tooth by tooth, along the depth of the bore. If the cutting load varies along the stroke, or if the tool wears during the run, or if the pilot hole is not the size the broach is designed to follow, the flats end up a few hundredths of a millimeter different between the entry face and the exit face. A check at the mouth of the bore will not show it, so the width across the flats has to be measured at several depths.

Can a square bore be milled instead of broached?

Yes, and for prototypes it usually is. A small cutter forms the corners and a larger one clears the flats. It works well when the square is large, the quantity is low, or the geometry is still changing, but the corner radius is limited by the smallest cutter you can run, and the unit cost stays high because every part follows the whole tool path.

How much corner radius does a broached square have?

It is set by the corner radius of the broach teeth and cannot be zero, because a cutting edge with a sharp internal corner would fail immediately. The drawing should state the radius the bore may carry, and the mating square shaft should be relieved to match it. When the shaft is left sharp, it contacts on the corner radii instead of the flats and feels like an interference fit even when the width across the flats is correct.

How do you check the clocking of a square bore to the flange holes?

With a gauge that references a flange hole and reads the angular position of the flats, rather than by eye or by fitting a shaft. It has to be done on every part, because clocking is fixed by the broach entry and no later operation can rotate the bore. On this order the check runs on 100 percent of the parts, alongside the flange index and the flange concentricity.

What to put on your drawing?

Six lines settle almost every argument about a broached square bore:

1. Give the width across the flats with a tolerance, and say that it applies along the full depth of the bore rather than at the entry face.
2. Give the clocking of the flats to a named flange hole, with a tolerance, and name the datum it is measured from.
3. State the corner radius the bore may carry, and state the relief on the mating shaft.
4. State the bore's relationship to the flange axis as a concentricity or runout call.
5. Say which surfaces are protected during anodizing, and what the film may do to the bore and the flange holes.
6. State where the laser mark goes relative to the flats, so the mark and the square are set from the same datum.

A hub is a stack of features that all reference one axis and one angular position, and the square bore is the feature that locks the angular position in place. Specify the square properly and the rest of the part is ordinary turning and milling work: concentric flanges, holes that line up, and a mark that lands in the same place on every piece.

PFT - turning, mill-turn machining, broaching and anodizing for aluminum drive components, prototype to production. Send us your drawing for a DFM review and a same-day quote.