Home / Metal cutting / Milling / Reference
Every milling field, and what it actually controls
This is the milling tab of the desktop application with its help text printed rather than hidden behind a hover. If you've ever wondered why a calculator gave you a feed you didn't trust, the answer is usually in one of these fields.
Milling — cut parameters
Values shown are a worked example: face milling low alloy steel with a 50 mm cutterISO material group, not a specific alloy. The group sets the starting cutting speed and the specific cutting force used for power. P covers unalloyed through low alloy steels; M is austenitic stainless, which work hardens and needs speed reduced and a positive edge; K is grey and nodular iron, abrasive but low in cutting force; N is aluminium and non-ferrous, where speed is limited by the machine rather than the tool; S is heat resistant and titanium alloys, where speed drops sharply and edge security governs everything.
The driver variable, and the field the whole tab hangs from. A grade is proposed automatically from your operation conditions, snapped to the ISO 1302 preferred steps N4 to N12. Dragging it picks the nearest step and switches Set Manually on, so an overridden value always reads as a deliberate choice rather than something inherited. Feed per tooth is then back-solved from it — which is why feed appears below as a result rather than an input.
Only needed for cutting time. Leave it blank and speeds, feeds and power still calculate. Fill it in and you get time per part, which is also what turns a part count into a tool life for the two-speed test below — the reason the optimization asks how many parts an edge lasted rather than how many minutes.
Grade sets how much speed the edge can survive; geometry sets what the cut does. The two are chosen separately and the code carries both. Geometry — rake face, chipbreaker, edge preparation — decides chip formation and evacuation, the direction and size of the cutting forces, whether a marginal setup rings, and the finish those four arrive at. None of it is in this calculation. The application range runs from wear resistance at one end to toughness at the other. A hard, wear-resistant grade takes more speed but chips under interruption; a tough grade survives the interruption but wears faster in a continuous cut. Pick from the interruption in the cut first, then take the speed the grade allows — not the other way round.
Determines how the cutter is engaged, which changes both speed and feed. Face milling is the most forgiving: the load is spread across several teeth and chip evacuation is easy. Peripheral and shoulder cuts load fewer teeth at a time. Slotting is the hardest case — full width engagement, both climb and conventional cutting on the same tooth, and chips that must exit through the cut they came from. Speed and feed are reduced accordingly.
Measured at the cutting edge, not the body. This is what converts cutting speed to spindle speed, so an error here scales every result. For round inserts and ball nose cutters the effective diameter at your depth of cut is smaller than the nominal diameter, and using the nominal value will leave you cutting slower than you intended.
The cutter's flute count — all of them, not the number engaged at any instant. Every flute passes through the cut once per revolution, so table feed is feed per tooth multiplied by the full flute count and the spindle speed, whatever the radial engagement happens to be. How many teeth are in cut simultaneously is a different question, and it governs force fluctuation, stability and whether the cut is continuous rather than intermittent — it does not enter the feed calculation. Count the flutes on the cutter and enter that.
Controls how feed per tooth becomes chip thickness. A 90° entering angle puts the full feed into the chip. As the entering angle drops, the same feed is spread over a longer cutting edge, so the chip gets thinner and feed can be raised to compensate. That's the whole principle behind high feed milling, where very small entering angles allow feeds several times higher at shallow depths. Lower entering angles also push cutting force into the spindle axis rather than sideways, which helps on long overhangs and weak fixturing.
Axial engagement — how deep the cutter is set into the material. This scales removal rate and power almost directly, and it's usually the first thing to reduce when the spindle can't deliver. It does not change chip thickness, which is why increasing depth is a safer way to add removal rate than increasing feed when edge life is marginal.
Radial engagement — how much of the cutter diameter is buried in the cut. This is the field that quietly ruins most calculations. Below about half the diameter, the chip is thinner than the programmed feed per tooth and the feed must be raised to compensate. Above about three quarters, teeth stay engaged long enough that heat becomes the limit and speed should come down.
Back-solved from the finish grade, not entered. Feed follows from Ra and the assumed corner radius, so it is a result you check rather than a number you tune. It is also not the chip the edge actually cuts: entering angle and radial engagement both thin it further, which is what the mean chip thickness result reports. Where the derived feed drives that chip under the rubbing floor, the finish grade is the thing that has to move — feed cannot, because the drawing is holding it.
Calculated results
Surface speed at the cutting edge. The single strongest influence on tool life — roughly, a 20% increase in speed can halve it. This is the number to reduce first when inserts are wearing too fast, and the last one to raise when chasing cycle time.
Cutting speed converted through the cutter diameter. Check it against your machine's usable range, not its maximum. Many spindles lose available torque well below top speed, so a result inside the rev range can still be outside the power range.
What the edge is actually cutting, after entering angle and radial engagement are accounted for. This is the number that should sit inside the insert's designed range — not feed per tooth. When the two diverge sharply, the radial engagement is doing something the programmed feed doesn't reflect.
The feed rate programmed at the control. Feed per tooth multiplied by teeth in cut and spindle speed. Worth sanity checking against your machine's rapid and acceleration limits on short moves — a high feed that the machine never reaches on a 20 mm cut is a feed that only exists on paper.
Volume of material removed per minute. The honest measure of roughing productivity, and the right thing to compare two strategies with — a shallow, fast, wide cut against a deep, slow, narrow one.
Net power at the cut, plus drive losses. Compare against continuous rated power at your working speed, not peak. If it exceeds what the machine has, the calculation can be inverted to solve depth of cut back from available power instead of you guessing at a reduction.
Starting values for coated carbide in good conditions. Verify against your insert manufacturer's data and your machine's rigidity before cutting.
The relationships behind the fields
Four calculations do most of the work. None of them are secret, and knowing them tells you when a result is wrong.
Spindle speed
n = Vc × 1000 / (π × Dc)
Cutting speed is a property of the material and the grade. Spindle speed is what the machine does about it, and depends entirely on cutter diameter. The same 200 m/min is 1,270 rpm on a 50 mm cutter and 3,180 rpm on a 20 mm one, which is why a parameter set copied between cutters is almost always wrong.
Chip thinning
hm ≈ fz × sin κ × f(ae/Dc)
Two separate effects thin the chip. A reduced entering angle spreads the feed along a longer edge. A light radial engagement means the tooth enters and leaves before it reaches full depth of engagement. Both reduce actual chip thickness below programmed feed per tooth, and both are additive.
The consequence is counterintuitive and it costs shops a lot of inserts: on a light radial cut you must feed harder, not softer. A cutter taking a 10% radial pass at a conservative feed is rubbing, not cutting, and will wear faster than the same cutter fed twice as hard.
Specific cutting force
kc = kc1 × hm−mc
The force needed to shear one square millimetre of chip. It is not a constant — it rises steeply as chips get thinner, which is why a thin chip costs disproportionately more energy per unit of material removed than a thick one.
This is the quiet argument for heavier feeds wherever the setup allows them: thick chips are cheaper to make, carry more heat away with them, and leave less of it in the edge.
Removal rate and power
Q = ap × ae × vf / 1000
Pc = Q × kc / (60 × η)
Power follows removal rate almost directly, scaled by specific cutting force and divided by drive efficiency. That gives the useful inversion: given the power a machine actually has, the maximum depth of cut can be solved rather than guessed.
It also explains why a small machine is not simply a slow big machine. Below a certain power, some cuts are not available at any feed, and the answer is a different strategy rather than a reduced one.
Run these numbers on your own cutThe browser calculator covers milling with the same model described here. Turning and drilling are in the desktop application, along with the grade cross-reference tables.
Open the calculator