Cutting data: what happens between the catalogue and the machine
The two formulas it comes down to
Cutting speed and feed per tooth come from the tool catalogue. What the machine needs is spindle speed and feed rate. Two conversions sit in between.
n = vc · 1000 / (π · d) spindle speed [rpm]
vf = n · fz · z feed rate when milling [mm/min]
vf = n · f feed rate when turning [mm/min]
One example carries this whole article: a Ø 12 mm end mill with four flutes, coated carbide, workpiece material S235. The catalogue gives vc = 180 m/min and fz = 0.05 mm.
n = 180 · 1000 / (π · 12) = 4775 rpm
vf = 4775 · 0.05 · 4 = 955 mm/min
You could set off with that. For a full-width slot it would even be right. For a finishing pass with 1.2 mm of radial engagement it is a mistake that costs tools.
Chip thinning: the feed that is too low
Feed per tooth is not chip thickness. It is the distance the tool advances per cutting edge. How thick the chip actually gets depends on how far the edge dips into the material.
At full slot width the maximum chip thickness is roughly the feed per tooth. Cut with only a tenth of the diameter engaged radially and the edge grazes the material along a shallow arc and takes far less with it. The chips get thin, the edge rubs instead of cutting, and the heat goes into the tool instead of into the chip.
fz,corr = fz / √( 1 − (1 − 2·ae/d)² )
Example: ae = 1.2 mm at d = 12 mm → ae/d = 0.1
fz,corr = 0.05 / √(1 − 0.8²) = 0.05 / 0.6 = 0.083 mm
vf = 4775 · 0.083 · 4 = 1585 mm/min
So the feed has to rise by two thirds, not fall. That runs against instinct, because less engagement looks like a reason to be careful. Which is precisely why it is one of the most common causes of tool failure in finishing.
At very small stepovers the correction gets large. At ae/d = 0.03 the factor is already above 2.9. Then a second limit takes over: the feed must not overwhelm the edge geometry and the runout. Common practice is to use the corrected value and to cap the factor below ae/d of about 0.05.
What the catalogue value quietly assumes
Every cutting recommendation applies to conditions that are rarely written next to it. As a rule those are: short overhang, rigid clamping, sufficient cooling, a tool in good condition, and a workpiece material that matches its data sheet.
Overhang
Tool deflection grows with the cube of the free length. Twice the overhang means eight times the deflection at the same force. A cutter that runs cleanly at 30 mm of overhang chatters at 60 mm and leaves marks no finishing pass will remove. In practice: find the shortest possible setup first, then the cutting data.
Cooling and chip evacuation
When milling aluminium, chip evacuation is often the real limit rather than cutting speed. A chip left in the slot is cut a second time and welds itself to the edge. With stainless steel it is the opposite, the heat: the material conducts poorly and the heat stays in the cutting zone. There, more feed helps rather than less, because the heat has to leave with the chip.
Machine power
At larger depths of cut the spindle power becomes the limit. The estimate is simple enough to do in your head:
P = Q · kc / 60000
Q material removal rate [cm³/min] = ap · ae · vf / 1000
kc specific cutting force [N/mm²], steel roughly 2000
For the example above with ap = 12 mm, Q comes to 22.9 cm³/min and from that about 0.76 kW. Any milling machine manages that. A roughing slot 20 mm wide with 40 mm of depth is a different calculation, and then the spindle decides rather than the catalogue.
Tool life: why cutting speed costs more than feed
Cutting speed and tool life are connected by a relationship Frederick Taylor described back in 1907, and it still holds.
vc · T^n = C
T tool life [min]
n material exponent, around 0.25 for coated carbide
With n = 0.25, doubling the cutting speed leaves a sixteenth of the tool life. So turning up the spindle to save ten percent of cycle time is paid for with considerably more tool changes.
Feed is better behaved. It enters tool life with a much smaller exponent. That is why the order of optimisation is almost always: use up the feed first, then the depth of cut, and only touch the cutting speed last.
| Material | vc in m/min | fz at Ø 12 mm |
|---|---|---|
| Aluminium, unalloyed to AlSi | 400 … 1000 | 0.06 … 0.12 mm |
| Structural steel S235, S355 | 150 … 250 | 0.05 … 0.09 mm |
| Quenched and tempered 42CrMo4 | 100 … 160 | 0.04 … 0.08 mm |
| Grey cast iron EN-GJL-250 | 120 … 200 | 0.05 … 0.10 mm |
| Stainless steel 1.4301 | 80 … 120 | 0.04 … 0.07 mm |
| Titanium Ti-6Al-4V | 30 … 60 | 0.03 … 0.06 mm |
Guide values for coated solid carbide in milling. The tool manufacturer knows their product better than any general table, so their data sheet always wins.
The speed limit small tools run into
At small diameters the arithmetic tips over. A Ø 2 mm cutter would need close to 48,000 rpm for vc = 300 m/min. Few machines manage that. At a maximum of 12,000 rpm what is left is an actual cutting speed of 75 m/min.
That is not a calculation error but a physical limit of the machine. You just have to know about it instead of wondering why the small tool leaves poor surfaces. Anyone regularly working below Ø 3 mm needs a high-frequency spindle or has to adjust their expectations of surface finish and tool life.
The reverse holds as well: with large face mills, speed is never the problem; there the power is the limit. Between those two ends lies the range where catalogue values actually apply.
Frequently asked questions
Climb milling or conventional milling?
On a backlash-free CNC machine, climb milling as a rule. The edge enters at full chip thickness and leaves thin, which extends tool life and improves the surface. Conventional milling only makes sense on manual machines with backlash in the feed screw, where climb milling can pull the workpiece into the cutter.
Why do catalogues sometimes give fz and sometimes hm?
hm is the average chip thickness and therefore the physically relevant quantity. fz is what the machine needs. If a catalogue quotes hm, you have to convert to fz yourself, and the radial engagement enters that conversion. That conversion is exactly the chip thinning correction.
How do you tell the cutting data is wrong?
By the colour of the chips and by the sound. Blue chips when milling steel mean a lot of heat in the chip, which can still be acceptable with enough coolant. Silvery, dust-fine chips and a whistling noise mean too little chip thickness, the tool is rubbing. A deep, irregular rumble is chatter, and then the overhang is usually the culprit.
Is trochoidal milling worth it?
For deep slots in tough materials, markedly so. Instead of full width and shallow depth you cut narrow and full depth along circular paths. The engagement angle stays small and constant, the heat spreads over the whole cutting length, and tool life rises considerably. The feed has to be raised properly according to the chip thinning correction, otherwise the advantage turns into the opposite.