Milling Speed and Feed Calculator
In milling the tool spins and the work feeds past it: each tooth enters the material, cuts a comma-shaped chip, then swings out into fresh air. So the governing figure is not feed per revolution but feed per tooth fz — the chip load. This calculator turns that into spindle speed, feed rate, metal removal rate and power, and above all into the actual chip thickness, which is almost never equal to fz.
The milling trap: as soon as radial engagement ae drops below half the cutter diameter, the chip formed is thinner than the programmed feed. At 10% stepover, a 0.10 mm chip load produces a chip of only 0.04 mm: the edge rubs instead of cutting, heats up, and wears faster than it would at full engagement. This page works out that factor and the corrected chip load.
Other operations: turning, drilling, boring, threading, tapping.
Cutter and engagement
Cutter, chip and engagement terms marked with an asterisk are defined in the glossary at the foot of the page.
Climb versus conventional milling: backlash, tooth entry, surface finish
Two directions, two different cuts. In conventional milling* (up milling) the tooth lands at zero thickness and the chip thickens as the tooth leaves. In climb milling* (down milling) the tooth bites thick and exits at nothing. That contrast decides the heat in the edge, the wall finish, and whether a worn leadscrew will snatch the table.
Rubbing at the start of a conventional cut work-hardens the skin and dulls the edge. The force opposes the feed, so backlash in an Acme screw is taken up before metal comes off — the reason a 1960s Bridgeport is often left in conventional for roughing. Climb does the opposite: a clean shear, a better wall, less heat, and a force that pulls the work into the cutter. On a ballscrew machine with the axis preloaded, that pull is stable. On a loose knee mill the same pull is how a 2 mm unexpected bite appears and a 10 mm end mill breaks.
CNC finishing is climb. CNC roughing is climb unless the fixture is doubtful. A manual mill with visible backlash stays conventional until the last pass, and a tiny climb cut waits until the slack has been wound out. Aluminium takes climb well. A hard scale on a flame-cut plate sometimes suits conventional for the first skin cut, keeping the tooth off the crust at full chip thickness.
The control keeps no record of which direction was intended. Feed direction in the G-code and the sense of spindle rotation have to agree. Reverse either one and a climb path is suddenly conventional: a washboard finish, and an edge that fails early.
Chip thinning and trochoidal milling: why a light stepover allows a very deep cut
A slotting pass buries the cutter. Radial engagement ae equals D, and chip thickness sits near the feed per tooth. A light shoulder, or a trochoidal path, uses a sliver of the diameter. The chip comes out thinner than fz. That is radial chip thinning*, and it is why high-efficiency milling* can take a deep axial cut without snapping the tool.
cos φ = 1 − 2 · ae / D · hm = 360 · ae · fz / (π · D · φ°)
This page prints hm, hex and the factor fz / hm. At ae = 0.1 D the chip is only a fraction of the programmed chip load*. Left at the slotting value, fz lets the edge rub: heat, noise, a poor wall. Raised until hm is back where the grind was designed — often 0.05–0.12 mm for a carbide end mill in steel — the same edge starts cutting again.
Trochoidal and high-efficiency paths push the same idea: ae maybe 5–15% of D, ap up to 1–2 × D, table feed high. Radial force drops, and a long-reach tool survives. Heat leaves in the chip. Hardened steel that would snap on a 0.3 D slotting pass will take a skinny trochoid all day. The path is longer. The gain is engagement and tool life, not always minutes, once the CAM (computer-aided manufacturing) path is full of tiny loops a machine cannot accelerate through.
A face mill at 75% of diameter is a small thinning problem. A finishing wall at 5% of D is a large one. The factor printed here is the figure to trust, not a guess from the slotting chip.
Choosing ap and ae from machine rigidity and tool overhang
Metal removal is ap × ae × Vf. The product ap × ae is the cross-section of the chip, and that cross-section is what bends the tool. Overhang is the multiplier. A 12 mm end mill held 20 mm out will take a cut that the same mill, held 50 mm out, will chatter on. No coating repairs stick-out.
A short, stiff setup buries the axial depth — ap towards 1–1.5 D on a proper high-efficiency tool — keeps ae modest, and takes few passes at a high Q. A long reach, a skinny 40-taper, or a part sitting on parallels reverses that choice. Axial depth stays shallower, and ae can grow towards 0.5–0.7 D, spreading the load. The high-efficiency route remains open too: a tiny ae and a lot of axial engagement, provided the flute is long enough to use it. Finishing walls sit at ae of 0.02–0.1 D, with ap the full wall when the setup will stand it, or a few step-downs when the wall sings.
The first number to cut when the cut chatters is ae, not spindle speed. Spindle speed tunes a frequency. Engagement is the force, and the force is what the noise was.
A turning job has one depth of cut. Milling has two, axial and radial. Mixing them — the radial figure typed into the axial box — is a classic way to bury a tool.
Face mill, end mill, bull nose, ball nose: what each one is actually for
A face mill is a disc of indexable inserts, built for flats. Removal rate is high, ae is wide, ap stays modest. It will not plunge, it will not cut a square inside corner, and a pocket is not its job. It skins a plate, faces a boss, mills a datum. Lead angle changes both the thinning and the split of force: 45° against 90°. A 45° lead is kinder on a weak spindle. A 90° lead leaves a square shoulder.
A square end mill is the general-purpose stick: shoulders, slots, contours, ramps. Two flutes for aluminium, three or four for steel, and more for a finishing wall when the gullets can swallow the chip. A bull-nose, or corner-radius, mill is that stick with a small radius — 0.5, 1 or 2 mm — which keeps the corner from chipping and lets the floor blend. The CAM model has to carry the radius. Without it the wall comes in fat.
A ball nose is for 3D shapes: moulds, dies, impellers, a fillet that is not a single radius on the drawing. Cutting speed at the very tip is zero. That is geometry. The centre of the ball lies on the axis, where surface speed vanishes. A finish pass uses a tilt, a lead and a small stepover. A ball plunged into steel on the tip does not last. On a steep wall a bull-nose on a 3D path can outrun a ball, because more of the flute is moving.
The cutter follows from the geometry that must be left behind, and from the strategy after that. A ball pressed into service as a face mill is a slow way to burn an expensive stick.
Tooth count, variable pitch and variable helix: three ways to kill chatter
Chatter is a conversation between the tooth in the cut and the wave the tooth before it left behind. Break the rhythm and the conversation stops.
- Flute count — a 5-flute in a pocket that used to be a 4-flute shifts the frequency that excites the tool. More flutes also raise table feed, Vf = n · fz · z, when each tooth still receives its chip load. The gullet shrinks. Chip packing becomes the new limit, above all in aluminium.
- Variable pitch — unequal spacing, for example 68° / 76° / 72° / 64° / 80°. The time from tooth to tooth is never the same, and the wave left in the surface does not reinforce. Roughing end mills for steel are built on this.
- Variable helix — the helix angle changes along the flute, and the force falls out of phase along ap. Paired with variable pitch, it is the modern way to quiet a long reach.
A cheap 4-flute with even spacing will cut. It will also sing, at the stick-out where every other cheap 4-flute sings. When the only change available on the day is the cutter, a variable-pitch roughing mill is worth more than another 10% of spindle speed.
Entering the material: ramp, helical interpolation, plunge, pre-drilled hole
The first millimetre is where end mills die. A square end is a poor drill. Surface speed at the centre is low, the corners are overloaded, and the chips have nowhere to go.
- Ramp — feed along X or along Y while Z drops, 2–5° on carbide in steel, steeper in aluminium. Load builds gradually. Chips escape backward. This is the usual entry for an open pocket.
- Helical interpolation — a circle that descends as it turns. A hole without a drill, or a pocket entry in a tight bay. The helix stays wide enough that the core does not rub. Half a diameter of radius is a common floor for that circle.
- Plunge — only a centre-cutting end mill, or a real drill. A finishing ball, or a roughing mill that does not cut on centre, skates and breaks. Even a centre-cutting two-flute is happier on a ramp when a ramp is available.
- Pre-drilled hole — a hole at least as large as the mill, a drop straight in, and milling from there. The gentlest entry. It costs an extra tool and an extra cycle, and it earns that cost on a hardened block or on a long-reach cutter that cannot be replaced this week.
The drilling calculator covers that last option. A 20 mm hole in 4140 is not mill-plunged merely because a drill cycle looks like extra work.
Slotting: the worst case in milling, and how to avoid it
Full-width slotting is two cuts at once. Chips sit trapped in a trench, the flute sees no air, and radial engagement is 100%. Forces peak. Evacuation fails. The cutter is a buried shaft. Deeper than about 1 × D, the same slot is a chip-packed grave.
Where the drawing allows a way round it, the slot is milled as a pocket: a smaller cutter, ae of 0.3–0.5 D, climb on both walls, or a trochoid that never fills the width in a single pass. When the feature really is a slot — a keyway, a saw cut, a Woodruff — the tool is a dedicated slot drill or a two-flute. Depth is pecked, table feed comes down, and coolant is blown or pumped into the trench, not onto the spindle nose.
A four-flute in a deep slot packs. Two flutes, a three-flute with big gullets, or a stagger-tooth keyseat cutter gives the chip somewhere to sit. The habit of taking the slot full width “because it is only 8 mm” is how 8 mm end mills become 8 mm stubs.
A long-reach four-flute is a poor choice for slotting more than about one diameter deep, with a hose aimed at the guard. Packed flutes break the tool in the hole, not on the way in. Depth is pecked, the cutter goes to two flutes, or the feature stops being treated as a slot and is milled as a pocket.
Diagnosing chatter by ear and by surface finish, then fixing it with ae rather than RPM
Chatter has a voice and a handwriting. A high scream is usually the tool. A low growl is the part, or the vice. The wall shows even ripples, a fish-scale, a pitch that does not match feed per tooth. Feed marks are regular and small. Chatter marks are louder, taller, and diagonal.
ae is the first change. Less radial engagement drops the force and shifts the cut on the stability chart without a touch to spindle speed. More ae, sometimes, steps the cut onto a stable lobe: a full-width facing pass that went quiet once the width increased. That is lobe-jumping. It looks unlikely the first time it happens.
Spindle speed is the second knob. A shift of ±10–15% can walk off a bad phase match between the tooth-pass frequency and the natural frequency of the setup. Speed is a tuner, not a volume control. Dropping it by 50% “until the noise stops” produces a different bad cut: rubbing, and built-up edge*. The holder, the stick-out and a variable-pitch cutter are the mechanical fixes that remain after the headphones come off.
A part rattling in the vice chatters at every speed. A light tap on the work is the test. A ring means a clamp or a support is missing. The end mill is not the cause.
Milling aluminium: two flutes, big gullets, air blast or mist lubrication
Aluminium wants room for the chip. Two flutes on a 12 mm tool, three at most on a larger one, polished flutes, a high helix of 40–45°, and fat gullets. A 4-flute steel mill in 6061 packs those flutes in three seconds and breaks. High-silicon alloys — die-cast grades, and alloy 390 — are more abrasive and will accept a third flute. A packed gullet is unwelcome on those alloys as well.
Cutting speeds look extreme beside steel. On carbide, 300–800 m/min is a normal band, and higher again with a suitable coating or with diamond. Chip load is not a timid number. On a 12 mm two-flute, 0.08–0.20 mm/tooth is a starting band, not a dare. Built-up edge is the usual failure: silver welded to the edge, the surface torn. Speed goes up, the rake stays polished, and the chip keeps moving.
Flood coolant does the job. Many shops prefer an air blast, or minimum quantity lubrication*, which throws the chips clear and avoids recutting them in a wet slurry. Through-tool coolant in a pocket is a luxury on the machines that have it. A hose pointed at the wrong side of the cut plasters swarf back onto the wall.
Milling wood and panels: routers, feed direction, breakout at the end of a pass
A router spindle is a mill running at 18,000 rev/min, cutting fibre rather than forming a plastic chip. Climb and conventional both apply. On a joinery bench the same pair is called “with the rotation” and “against.” Anything fed by hand — a handheld router, work pushed past a router table or spindle moulder — runs conventional, against the rotation. In climb the bit pulls the machine or the workpiece, and the operator loses control. On a CNC with solid timber clamped down, climb often leaves the cleaner edge: the tooth slices the fibre before it can lever it up, where conventional lifts and tears it on reversing grain. Many shops rough conventional and finish with a light climb pass. On panels — melamine, particleboard, MDF — conventional is the rule, because climb chips the décor face. Breakout at the end of a pass across end grain is a separate problem: a backer board, end grain cut before long grain, and the last 10 mm slowed.
Particleboard and laminate chip on the top face, the bottom face, or both. A down-cut spiral keeps the top crisp and dumps dust into the kerf. An up-cut clears the chips and wrecks the top. A compression bit — up-cut on the lower part of the flute, down-cut on the upper — is the panel tool: the fibres are pushed towards the middle of the board. A shallow scoring pass, or a skin left for a later finish, protects an expensive laminate.
Feed stays high enough that the bit cuts, not burns. A router paused in MDF is a smoking hole. Dust extraction is not an optional extra. It is the chip clearance, it stands in for coolant, and it is what keeps the air in the shop breathable.
Holding the cutter: ER collets, hydraulic chucks, shrink fit — and the runout that follows
Total indicated runout* is a hidden extra chip on one tooth and a holiday for the others. At 0.02 mm TIR, a 3-flute mill has one flute doing roughly twice the work. That flute dies. The others look new. The coating collects the blame.
- ER collet — cheap and flexible, 8–20 µm when the collet is clean, free of cracks, and the nut is tight. Adequate for roughing. The pocket is wiped before the tool goes in. A single chip left in that pocket is 30 µm on its own.
- Hydraulic chuck — an oil jacket closed by a screw, 2–5 µm, with a little damping. The finishing holder. Temperature matters: a hot hydraulic chuck can loosen its grip. The actuating screw is not driven past its torque.
- Shrink fit — the holder is heated, the shank drops in, 1–3 µm, very stiff, slow to change. The choice for high-speed machining and for long reach, where deflection is the enemy. The shank has to match the bore. A shrink holder is not a collet that can be persuaded to grip.
A worn ER nut, or a 16 mm mill gripped in an 8–20 collet “because it held”, is how runout becomes a habit of that machine. The collet range matches the shank. The tool is pulled in short. An indicator check, made from time to time, says more than the name on the box.
Estimating pocket cycle time from toolpath length and removal rate
Volume divided by Q is a lower bound, not a quote. With ap and ae in millimetres and Vf in mm/min, Q = ap · ae · Vf / 1000 comes out in cm³/min. A pocket 50 × 40 × 12 mm is 24 cm³. At Q = 8 cm³/min the cutter is in the metal for 3 minutes — and only if it behaves like a plough that never lifts, never ramps and never runs a semi-finish.
Vf = n · fz · z · Q = ap · ae · Vf / 1000 · tcut ≈ V / Q
A CAM time adds the ramps, the links, the lead-ins, the finish pass at 5% ae, and the acceleration the machine can produce. A programmed 12,000 mm/min that the servo reaches only on a long straight is not 12,000 mm/min inside a 6 mm radius. A high-speed path of a thousand tiny trochoids can spend half the clock speeding up and slowing down. “Time remaining” on the control, read after the first part, is the number that belongs on the job card.
Tool changes, probing and deburr make up the rest of the quote. A pocket described as “only two minutes” usually lives in a five-minute neighbourhood.
Chip load on the control: feed per tooth, flute count, table feed
The catalogue prints feed per tooth, fz. The part programme carries table feed, Vf. Skipping the conversion is where speeds and feeds go wrong.
n = 1000 · Vc / (π · D) · Vf = n · fz · z
A 10 mm cutter, 4 flutes, 180 m/min, 0.06 mm/tooth: n is about 5,730 rev/min and Vf about 1,370 mm/min. The same cutter with 3 flutes, at the same chip load, drops table feed by a quarter. A 4-flute feed copied onto a 2-flute aluminium cutter gives each tooth twice the chip the edge was ground for. A 2-flute feed copied onto a 6-flute leaves each tooth rubbing.
After thinning, the fz in the programme is the corrected value this page prints. That correction is the point of the chip-thinning result. A slotting chip load left in a finish pass at 10% ae burns the wall. Opening the feed “a bit”, until the cut screams, is the usual next move, and it does not repair the rub.
When the spindle is out of torque: kilowatts at speed, newton-metres down low
A 15 kW spindle at 12,000 rev/min is not a 15 kW spindle at 800 rev/min. Power is torque times angular speed. Face milling a 50 mm cutter in 1045 at 80 m/min asks for torque. A 6 mm high-efficiency tool at 18,000 rev/min asks for power at speed, and for almost no torque. One machine can do both — until the heavy cut is demanded in a high-speed range, with the reduction in the wrong place.
A spindle that stalls, or a load meter that pins, is past “a bit over.” Axial depth or radial engagement comes down, or the tooth count comes down — a 3-flute in place of a 6 — or spindle speed drops into a band that has newton-metres left. Raising speed in order to “use the kilowatts” on a 40 mm face mill runs backwards. Vc climbs past what the insert grade tolerates and Taylor wear consumes the edges. The cut gains nothing: at the same chip, the torque it needs has not changed, and the torque the motor can give has fallen.
The motor curve is worth reading once. The useful rev/min band, written on the door of the machine, prevents a good deal of heroic CAM.
Through-tool coolant in a pocket versus a hose on the guard
A hose pointed at the guard cools the room. Coolant through the tool cools the edge and drives the chip up the flute. In a pocket deeper than about 1 × D the difference is not comfort. It decides whether the flute packs. Twenty to seventy bar through a carbide mill is a different process from a 3 bar flood. Cast iron prefers air. Aluminium takes a through-spindle blast well. Stainless wants oiliness and pressure together.
Where the jet points matters as much as the pressure. External coolant meets the tooth as the tooth leaves the cut, blowing the chip clear. A nozzle aimed at the entry plasters swarf into the next flute. Where flood is the only supply, a deep pocket is pecked: a retract every 1–2 D empties the nest of chips.
Minimum quantity lubrication on a wall finish can beat a flood on aluminium, with less thermal shock and less sticky paste. Heavy roughing in steel wants a wet chip conveyor, and a pump that has not been turned down merely to keep the floor dry.
Write the proven number down so the next shift can hit it
A milling speed that “worked on Thursday” is not a process until the setup sheet carries it: diameter, tooth count, holder, stick-out, Vc, fz together with the thinning-corrected fz, ap, ae, climb or conventional, the coolant, and the sound the cut ought to make. The night shift was not in the shop for the day-shift cut. The sheet has to say the thing that was heard — “quiet climb, 1.2 mm stepover, do not slot.”
This calculator is the first guess, and the check that the guess is sane. The second guess is the first part off the machine. The number that ships is the third. A tooling catalogue assumes a rigid block, a shrink-fit holder, and a spindle that is not the one on the floor. The start stays inside the published window. One knob moves at a time — radial engagement, followed by chip load, followed by spindle speed — and each change can be told apart from the others.
Boring and threading punish a milling speed copied across even faster. Separate sheets, separate tools, separate numbers.
Glossary
- Conventional milling
- Up milling. The tooth meets the surface at zero chip thickness and the chip thickens towards the exit. Cutting force opposes the feed, which takes up backlash in a worn leadscrew before the edge is cutting. The rub at entry can work-harden the skin.
- Climb milling
- Down milling. The tooth takes a thick chip at entry and leaves at nothing. The force pulls the work into the cutter. A preloaded ballscrew holds that pull; a loose knee mill can snatch an extra bite and break the tool.
- Radial chip thinning
- The drop in real chip thickness when radial engagement ae is only a fraction of the cutter diameter. Average thickness is hm = 360 · ae · fz / (π · D · φ°), with the engagement angle from cos φ = 1 − 2 · ae / D. The factor fz / hm is what the programmed feed is multiplied by if the edge is to see the thickness it was ground for.
- Chip load
- Feed per tooth, fz, in mm/tooth: the bite the programme asks of each tooth. Table feed is Vf = n · fz · z. Catalogues print fz. The control is given Vf.
- High-efficiency milling
- A trochoidal or similar path with a light radial stepover and a deep axial cut, table feed raised to keep average chip thickness where the edge was meant to cut. Radial force falls, which is why a long-reach tool can survive the pass. On this page the light stepover cited for that strategy is about 5–15% of diameter, with axial depth up to one or two diameters.
- Built-up edge
- Workpiece metal welded to the cutting edge and later torn off. On aluminium it shows as silver stuck to the edge, with the surface torn. A cutting speed that is too low, or a rake that rubs, encourages it. Shops abbreviate it BUE.
- Minimum quantity lubrication
- A fine mist of oil in place of a flood of emulsion. The chips leave the cut instead of being recut in a wet slurry. On an aluminium wall it can beat flood: less thermal shock, and less sticky paste on the surface.
- Total indicated runout
- The radial wobble of the cutter as it spins, read with a dial indicator and written TIR. Runout loads one tooth and spares the rest. At 0.02 mm on a three-flute cutter, one flute does roughly twice the work and wears out while the others look new.