Chip thinning: radial, axial and feed correction

In milling, the programmed feed per tooth and the thickness of the chip the cutting edge actually removes are often not the same. When the radial engagement narrows, or when cutting takes place in a spherical or radiused edge region, the chip cross-section becomes thinner; if the feed is not corrected, the tool works below the intended load and, contrary to expectation, dulls earlier. This guide covers the geometric origin of radial and axial chip thinning, the calculation of the correction factors and the minimum chip thickness limit through worked examples.

1. The difference between fz and the actual chip thickness

Feed per tooth (fz) is the distance the machine travels during one tooth period and is a programmed quantity. The actual chip thickness, on the other hand, is the thickness of the cross-section the cutting edge separates perpendicular to the material along the engagement. In milling this thickness varies continuously along the engagement arc; it starts from zero, reaches a maximum (hex) and falls back to zero.

The feed recommendations given by tool manufacturers describe the target chip thickness at which the edge works soundly. In full side milling (ae = D/2) these two quantities are taken to be equal. Once the engagement conditions move away from this reference, a conversion factor comes into play between fz and hex. For the basic relationships between cutting speed, spindle speed and feed, the cutting speed, spindle speed and feed calculation guide is complementary.

The basic relationships are as follows:

• n = (1,000 × vc) / (π × D)
• vf = fz × Z × n
• hex = fz / CTF

Here the correction factor is used in moving from the target chip thickness to the fz to be programmed: fz = target hex × CTF.

2. Radial chip thinning

2.1 Geometric origin

When the radial engagement (ae) is smaller than the tool radius, the cutting edge no longer enters the material perpendicularly but at an angle close to the tangent. The arc travelled by the edge becomes shorter and the component of the feed vector perpendicular to the chip thickness decreases. As a result, a thinner chip is removed at the same fz value. The effect grows at an accelerating rate as the ae/D ratio decreases.

Geometrically, the correction factor is obtained from the following relationship:

RCTF = 1 / √[1 − (1 − 2 × ae/D)²]

The relationship is valid over the range ae/D ≤ 0.5. For ae/D = 0.5 the factor comes out as 1.0; that is, no correction is needed at half-diameter engagement. The same relationship is also written in the equivalent form RCTF = D / (2 × √(ae × (D − ae))). Since the angle of the engagement arc is found from θ = arccos(1 − 2 × ae/D), the factor can also be expressed as RCTF = 1 / sin θ.

2.2 Numerical values

The table below shows the factors calculated from the relationship and the programmed fz values these require for a target chip thickness of 0.05 mm. The values are of the same order as the radial engagement correction table published by Sandvik Coromant.

Critical point: while the ae/D ratio is above 0.25 the correction is modest; once it drops below 0.10, the feed has to be increased by close to a factor of two. This is the fundamental reason why trochoidal and high-efficiency machining strategies work with high feed values. The subject is treated separately in the trochoidal milling and high-efficiency machining guide.

2.3 Worked example 1: radial correction

Data: D = 10 mm four-flute carbide end mill, Z = 4, ae = 1 mm, target hex = 0.05 mm, target vc = 120 m/min.

1. Spindle speed: n = (1,000 × 120) / (π × 10) = 3,820 rpm
2. Ratio: ae/D = 1 / 10 = 0.10
3. Factor: RCTF = 1 / √[1 − (1 − 0.2)²] = 1 / √0.36 = 1.67
4. Feed to be programmed: fz = 0.05 × 1.67 = 0.083 mm/tooth
5. Table feed: vf = 0.083 × 4 × 3,820 ≈ 1,270 mm/min

Without the correction the feed would be 0.05 × 4 × 3,820 = 764 mm/min and the edge would work at a chip thickness of around 0.030 mm. The difference is not merely a loss of productivity; a thin chip also makes it harder for the heat in the cutting zone to be carried away with the chip.

3. Axial chip thinning

3.1 Effective entering angle on a corner radius cutter

On a corner radius cutter, when the axial depth of cut remains smaller than the corner radius, cutting takes place only in the radius region. In this region the effective entering angle (κ) of the edge drops below 90° and the chip thickness decreases according to hex = fz × sin κ. The correction factor in this case becomes ACTF = 1 / sin κ.

The effective entering angle within the radius is found from cos κ = (R − ap) / R. From this, the factor is tied directly to the ap/R ratio:

The same logic also applies to straight-edged tools in cases where the entering angle is determined directly by the tool geometry: while the factor is 1.0 at a 90° entering angle, it rises to approximately 1.4 at 45° and to the order of 5.8 in the high-feed geometries around 10°. The ability of high-feed cutters to work at unusually high feeds at small axial depths rests on this geometric effect.

For the definitions of dimensions such as R, D1 and L1 in the tool geometry, the end mill dimensions guide can be consulted.

3.2 Effective diameter in ball nose milling

In ball nose milling, cutting takes place not at the nominal diameter but on a smaller circle determined by the axial depth of cut. The diameter of this circle is called the effective diameter (Deff):

Deff = 2 × √(ap × (D − ap))

The axial chip thinning factor is written as ACTF = D / √[D² − (D − 2·ap)²] and is numerically equal to the ratio D / Deff. The table below shows the values for a ball nose cutter of 10 mm diameter.

Zero speed at the axis: On the axis of rotation of a ball nose cutter the diameter is zero, and therefore the cutting speed at that point is zero as well. Since crushing and rubbing occur in the axis region instead of cutting, positioning the tool axis perpendicular to the machined surface has to be avoided. In practice, giving the tool or the workpiece a tilt angle of the order of 10–15° allows cutting to take place at a larger effective diameter and improves both surface quality and tool life. For the link with surface quality, the surface roughness and finish milling guide can be examined.

3.3 Worked example 2: ball nose cutter

Data: D = 10 mm two-flute ball nose cutter, Z = 2, ap = 0.5 mm, target vc = 150 m/min, target hex = 0.04 mm.

1. Effective diameter: Deff = 2 × √(0.5 × 9.5) = 2 × 2.18 = 4.36 mm
2. Spindle speed, from the effective diameter: n = (1,000 × 150) / (π × 4.36) ≈ 10,950 rpm
3. Axial factor: ACTF = 10 / 4.36 = 2.29
4. Feed to be programmed: fz = 0.04 × 2.29 = 0.092 mm/tooth
5. Table feed: vf = 0.092 × 2 × 10,950 ≈ 2,015 mm/min

Where the spindle speed is calculated from the nominal 10 mm diameter, n = 4,775 rpm is obtained and the actual cutting speed remains at a level of vc = π × 4.36 × 4,775 / 1,000 ≈ 65 m/min. This is approximately 44% of the intended 150 m/min. The most frequently seen reason why the coating and carbide grade fail to deliver the expected performance in ball nose milling is that the cutting speed remains low in this way without being noticed.

4. Combining the two effects

Radial and axial thinning arise from independent geometric causes. Where both apply at once, the factors are applied by multiplication:

CTF = RCTF × ACTF

A die surface finished with a ball nose cutter using a raster path at small stepover is the typical example. For instance, on a 10 mm ball nose cutter with ap = 0.5 mm and a stepover of 0.5 mm, the axial factor is 2.29 while the radial factor, calculated over the effective diameter of 4.36 mm, comes out at approximately 1.57; the total factor rises to the order of 3.6. At this point the limiting element is no longer the geometry but the feed and acceleration capacity of the machine tool together with the edge strength of the tool.

In practice three limits have to be checked:

• Edge strength: the corrected fz must not exceed the maximum chip thickness given by the tool manufacturer for the relevant diameter and material group.
• Machine dynamics: on small-radius toolpaths the machine tool cannot reach the programmed feed; unless the achieved feed is checked, the correction remains ineffective.
• Engagement angle stability: since the instantaneous engagement angle grows at corner entries, a high feed can lead to breakage. On the tendency to vibrate, the chatter in milling: causes and solutions guide offers guidance.

5. Minimum chip thickness and ploughing

The physical justification for chip thinning correction is the lower limit in cutting mechanics. The cutting edge is not an ideal line; it has a particular edge radius (re). When the chip thickness drops to a level comparable with this radius, the effective rake angle of the edge becomes strongly negative and the material, rather than being cut, is first crushed and pushed aside.

The research literature reports that this transition occurs while the ratio of chip thickness to edge radius (h/re) is roughly between 0.25 and 0.33. Across different materials, rake angles and measurement methods, the range given spreads over a band of approximately 0.2–0.35; the sources do not converge on a single definite value. Below this limit three phenomena appear together:

The result runs counter to intuition: reducing the feed does not protect the tool but instead accelerates flank wear. This effect is particularly marked in stainless steels and heat-resistant alloys, because these materials have a high tendency to work harden. The detail of the wear mechanisms is treated in the tool wear mechanisms and tool life guide.

Since the edge radius grows as the tool wears, the minimum chip thickness also rises over time. A feed value that works soundly with a new tool can fall into the ploughing region with a worn tool. For this reason, monitoring tool life trials with standardised wear criteria such as ISO 8688-2 is necessary for repeatable results.

6. Verification in practice

Whether the chip thinning correction has been applied correctly can be checked through three observations. The first is the chip form: if powder-like, very fine and colourless chips are seen instead of curled chips that carry the heat away, the thickness is insufficient. The second is sound and surface; in rubbing mode the cutting sound becomes shriller and a bright, crushed appearance forms on the machined surface. The third is the wear pattern; a uniform flank wear spread along the edge, rather than a depth-of-cut notch, points to ploughing.

For quick verification of the calculations, the cutting parameter tool can be used. Since geometry and parameter compatibility are assessed together in the selection of ball nose and corner radius tools, the diameter and length options under the ball nose end mills category have to be determined according to the slope distribution of the surface to be machined.

Sources

• Sandvik Coromant — Entering angle and chip thickness in milling (entering angle and radial engagement correction factor tables). sandvik.coromant.com
• Sandvik Coromant — Milling formulas and definitions (definitions of vc, n, vf, fz, hex). sandvik.coromant.com
• Harvey Performance Company (Harvey Tool) — Ball Nose Milling Strategy Guide (effective cutting diameter and compensated spindle speed calculation, tilt angle). harveyperformance.com
• ISCAR / IMC — Adjustments for Ball Nose Endmills (ball nose effective diameter and feed correction). cms.imcousa.com
• ISO 8688-2:1989 — Tool life testing in milling — Part 2: End milling (milling tool life and wear criteria).
• ISO 3685:1993 — Tool-life testing with single-point turning tools (reference standard for wear measurement definitions).
• Machinery's Handbook, Industrial Press — Milling section; chip thickness, entering angle and feed relationships.
• The International Journal of Advanced Manufacturing Technology (2020) — Determination of minimum uncut chip thickness and size effects in micro-milling of P-20 die steel using surface quality and process signal parameters (minimum chip thickness / edge radius ratio). doi.org/10.1007/s00170-020-04926-6