The field that lies by omission
Open any CAM operation for a 3 mm carbide end mill in 6061 and you will find a chip-load field. It accepts a number in mm/tooth. That number is feed per tooth — the distance the tool advances per cutting edge per revolution. It is not the maximum thickness of the chip the edge will actually cut. At full slotting the two are close enough that the distinction rarely matters. At 10% radial engagement they diverge by a factor of 1.67, and at 5% by 2.30. The field does not tell you this. It is a feed-per-tooth input, and treating it as a statement about chip thickness is the root error behind a large share of small-tool failures in aluminum.
The correction is not folklore. It is geometry, it is computable from the stepover you already programmed, and it belongs in the tool library rather than in one programmer’s spreadsheet.
Three quantities, not one
Keep these separate or the arithmetic will not close:
- Feed rate (F) — table advance, mm/min. This is what the post writes into the G-code.
- Feed per tooth (fz) — the programmed chip load, mm/tooth. This is what the CAM field accepts.
- Maximum chip thickness (hex) — what the cutting edge actually bites, mm. This is what the tool cares about.
The core relationship is F = fz × n × Z, where n is spindle speed in rev/min and Z is the flute count. Harvey Tool’s milling formula states the same thing in imperial units as IPM = RPM × IPT × T, with IPT defined as chip load and T as number of teeth. That equation is exact. The problem is that fz and hex are only equal under specific engagement conditions.
The geometry: why a light stepover thins the chip
When the radial depth of cut (Ae) is at least the cutter radius, the edge engages past the tool centerline and the maximum chip thickness equals the feed per tooth. When Ae is less than the radius, the edge sweeps a short arc and the chip is a wedge — thick at entry, tapering to zero at exit. The maximum thickness of that wedge is smaller than fz, and the shortfall grows as the stepover shrinks.
The effective maximum chip thickness is:
hex = fz × √(1 − (1 − 2Ae/D)²)
valid for Ae < D/2. The compensation factor is the reciprocal of that square-root term. At Ae/D = 10% the factor is 1.67×; at 5% it is 2.30×; at 1% it climbs past 5×. These are geometric ratios, independent of tool diameter and material. A 3 mm cutter and a 12 mm cutter at the same percentage stepover see the same multiplier.
Two consequences follow directly. First, if you program a chip load from a datasheet and take a 10% radial cut without compensation, the edge sees only 60% of the intended bite. Second, if that reduced thickness falls below the minimum needed for proper chip formation, the edge rubs instead of cutting — which accelerates wear and work-hardens the material. A chip load that is too low is not a safe chip load; it is a different failure mode.
Worked example: 3 mm tool, 6061, 10% stepover
Take a 3 mm diameter carbide end mill, two flutes, cutting 6061-T6 at a 0.30 mm radial stepover — 10% of diameter. Suppose the programmer enters fz = 0.010 mm/tooth, a plausible starting figure for a small aluminum-optimized cutter.
- 2Ae/D = 2 × 0.30 / 3.0 = 0.20
- 1 − 0.20 = 0.80
- 0.80² = 0.64
- 1 − 0.64 = 0.36
- √0.36 = 0.60
- hex = 0.010 × 0.60 = 0.006 mm
The edge cuts 0.006 mm, not 0.010 mm. To restore the intended 0.010 mm bite, multiply the programmed feed per tooth by 1/0.60 = 1.67, giving fz = 0.0167 mm/tooth. At 18,000 rev/min and two flutes, the feed rate moves from 360 mm/min to 601 mm/min.
That arithmetic is not a cutting recommendation. It shows what the geometry does to a number you supply. The number itself has to come from the tool maker’s data for that specific carbide grade, edge geometry, and coating — and Harvey Tool’s published non-ferrous table, which starts at 1/8″ (3.175 mm) and lists 0.001 IPT for 6061-T6/T651 at 800–1500 SFM, is a starting point, not a mandate. A 3 mm tool sits just below that table’s smallest column, so the datasheet for the exact cutter you own governs.
Radial is not the only correction
Radial chip thinning and axial (approach-angle) thinning are independent factors and stack multiplicatively. A ballnose or chamfer cutter approaches the material at an angle below 90°, so its feed per tooth also exceeds the chip thickness even at full radial engagement. If you apply the radial factor and forget the axial one on a ballnose finishing pass, you will under-feed the tool twice. The two corrections are computed separately and multiplied.
Where the multiplier becomes dangerous
The compensation factor rises steeply as stepover falls. At 1% Ae/D it exceeds 5×. A programmer who applies the full multiplier at a 0.03 mm stepover on a 3 mm tool has just multiplied the feed rate by five, and the machine will attempt it. The geometry is correct; the machine may not be.
Three practical controls keep the correction honest:
- Reduce axial depth before abandoning the correction. If the compensated feed loads the spindle or the sound changes, take a lighter axial pass rather than reverting to an under-fed rub.
- Verify chip evacuation. A 3 mm cutter in a 0.3 mm slot has almost no room for chips. Recut chips destroy small tools faster than any feed error. Air blast or through-tool coolant is not optional at these engagements.
- Derate for rigidity. Long stickout, light fixturing, and small machines all force the programmed value below the datasheet figure. The multiplier corrects geometry; it does not correct a tool hanging 40 mm out of a collet.
Adaptive and trochoidal paths rarely hold one exact stepover through corners. A defensible shop rule is to size the correction from the highest sustained radial engagement for thermal safety, and from the average engagement for cycle-time planning. Using the minimum instantaneous stepover produces an absurd multiplier in every corner.
Put the correction in the tool library, not in a habit
The reason this error persists across seats is that the correction lives in one programmer’s head or one spreadsheet. A new hire inherits the habit, not the number. For a firm standardizing CAM templates, the deliverable is a documented, versioned feed-calculation procedure that states:
- the geometry formula and the engagement range over which it applies;
- the source of the target chip load (tool maker, part number, revision date);
- the rigidity derating rule and who signs off on exceptions;
- the verification step — spindle load, sound, chip color — before a compensated feed is released to the shop.
Where the CAM platform supports it, the multiplier belongs in the operation template as a function of engagement, so it is applied consistently rather than per-operator. Where it does not, the procedure document is the control. Either way, the number a new hire produces should be reproducible from the document, not reconstructed from memory.
The 3 mm cutter in 6061 is a useful teaching case because the same math that justifies a higher feed also shrinks the margin for every rigidity error. Get the geometry right, then respect the margin.
FAQ
Does the 1.67× factor at 10% stepover depend on tool diameter?
No. The factor is a function of Ae/D, the ratio of radial depth to diameter. A 3 mm and a 12 mm cutter at 10% stepover share the same multiplier. What changes with diameter is the absolute chip thickness and the rigidity margin.
My CAM software has a chip-thinning checkbox. Can I trust it?
Only if you know what it multiplies and against which engagement value. Verify the output against the formula above for one operation before releasing a template. A checkbox that applies the factor at the minimum corner engagement will over-feed straight sections.
What if my stepover is above 50% of diameter?
No radial compensation applies. At Ae ≥ D/2 the edge engages past the centerline and the maximum chip thickness equals the programmed feed per tooth. Axial/approach-angle correction may still apply for ballnose or chamfer geometry.
Is a lighter chip load always safer?
No. Below the minimum chip thickness for the tool’s geometry, the edge rubs rather than cuts, which accelerates wear and work-hardens the material. Under-feeding is a failure mode, not a safety margin.
Sources
- Pi Fabricators, chip load calculator and radial chip thinning formula, including the compensation factor table (1.67× at 10% Ae/D, 2.30× at 5%). pifabricators.com
- Machining Doctor, chip thinning calculator — radial and axial factors, independence and stacking. machiningdoctor.com
- Harvey Tool, general machining guidelines — non-ferrous chip load table and milling formulas. harveytool.com
- Sandvik Coromant, machining formulas and definitions — cutting speed and spindle speed as primary parameters. sandvik.coromant.com