EN

Turning Speed and Feed Calculator

Three numbers govern a turning operation: cutting speed Vc (m/min — how fast the workpiece surface passes the cutting edge), feed per revolution f (mm/rev) and depth of cut ap (mm). The lathe only understands revolutions per minute, so this calculator does the conversion, then works out the metal removal rate and the power and torque the spindle actually has to deliver.

If you already know your cutting speed — the insert manufacturer prints it on the box — type it straight in. The material and tool selector is only there to suggest one when you have nothing to hand.

Other operations: drilling, milling, boring, threading, tapping.

Cutting conditions

nfapD = 50 mmVc
Step 1 — Recommended cutting speed

These three choices only suggest a cutting speed, which is copied straight into the Vc field in step 2. You are free to replace it with your own.

≈ 180–260 HB

Only tool materials that suit the chosen workpiece are offered.

Recommended range: 180 to 320 m/min — starting value 240 m/min

Step 2 — Cutting conditions

Filled in by step 1. Editable: if your tooling supplier gives you a figure, theirs wins.

The diameter at the cutting point, not the stock size. When facing it changes constantly — see the second calculator below.

Roughing 0.2 to 0.5; finishing 0.05 to 0.15. This is what sets the surface finish.

Measured on the radius: each pass takes 2 × ap off the diameter.

Halve the feed for grooving and parting off: the tool cuts across its whole width.

Optional: adds the cutting time for one pass.

0.7 to 0.75 for a belt-and-step-pulley drive; 0.85 to 0.9 for a direct drive.

Facing: which diameter should you use?

When facing, the tool starts at the outside diameter and works towards the centre, so the diameter at the cutting point — and with it the cutting speed — changes the whole way across. On a lathe running at constant spindle speed you have to pick one reference diameter. The right choice is not the arithmetic mean, which under-weights the outer edge where most of the swept area lies, but the root mean square of the two diameters.

Start and finish diameters

Enter 0 if you are facing all the way to the centre.

Equivalent diameter to use above 58.3 mm
Arithmetic mean, for comparison 50.0 mm

Deq = √( (Dmax² + Dmin²) / 2 )

Put 58.3 mm in the Diameter being cut field of the main form. Near the centre the cutting speed still falls away to nothing — that is where the finish deteriorates and the tool starts to rub rather than cut. A lathe with constant surface speed (G96) removes the problem by winding the spindle up as the tool moves in, right up to its RPM ceiling.

On first use, an asterisk leads to the definition in the glossary.

Reading an insert box: ISO grade, chipbreaker, nose radius and the published Vc range

The box is not packaging. It is the data sheet, folded into a code. Four marks on it decide whether the edge lasts a shift or dies in twenty parts: the ISO grade, the chipbreaker, the nose radius, and the cutting speed* window the maker tested.

ISO 513* paints the workpiece family on the insert. P (blue) is steel. M (yellow) is stainless. K (red) is cast iron. N (green) is aluminium, brass and copper. S (brown) is nickel and titanium. H (grey) is hardened steel, typically 45 HRC and up. The letter is the family; the number is the compromise inside it. A P10–P20 is hard and wear-resistant: finishing, a high cutting speed, no shock. A P30–P40 is tougher: roughing, scale, interrupted cuts. A P10 on a rusty hex bar chips before lunch.

The chipbreaker* is the small form pressed into the rake face. It is built for a feed* band, not for a preference. Finishing geometries want something like 0.08–0.20 mm/rev and a light depth of cut*. Medium sits around 0.20–0.40. Roughing starts near 0.40 and goes up. A finishing breaker run at 0.5 mm/rev never curls the chip. The chip ribbons, wraps the chuck, and polishes the flank away. A roughing breaker at 0.08 mm/rev leaves a chip too thin to break, and the chip smears.

Nose radius* rε is printed as the last digits of a code like CNMG 12 04 08: that 08 is 0.8 mm. Common shop sizes are 0.4, 0.8, 1.2 and 2.4 mm. A larger radius means a stronger corner and a better Ra at a given feed, and a larger radial push, which a slender bar will not accept. The published cutting-speed range is the maker's tested band, often 120–200 m/min for a coated P15 in 1045. A new job stays inside that band. A move outside it waits until the wear has been read.

A worn turret, a 40-year-old headstock, a part hanging 200 mm out of the chuck: the sensible place is the low end of the printed window. The insert grade is a starting number, not a law.

Choosing feed per revolution from nose radius and target roughness

The scallop left by the nose is a circle of radius rε, spaced one feed apart. That is the whole kinematic story. Peak-to-valley height is f² / (8 rε). A profilometer reporting Ra sits closer to a quarter of that height, which is why some catalogues print the 8 and some print the 32. This page uses the shop form, the one that can be worked at the machine.

Rt ≈ f² / (8 · rε)  ·  Ra ≈ f² / (32 · rε)

With f and rε in millimetres, and roughness in micrometres: Rt(µm) ≈ 125 · f² / rε and Ra(µm) ≈ 31 · f² / rε. A target of Ra 1.6 µm on a 0.8 mm nose calls for a feed around 0.20 mm/rev. On that same nose, 0.32 mm/rev is a 4 µm Ra. Feed marks a fingernail can feel. A roughing finish wearing a finishing name.

The other limit is mechanical. Feed much past about 0.7 × rε and the tool is no longer cutting on the radius. It is plowing with the straight side, and the formula stops meaning anything.

A 0.4 mm nose is a finishing tool. It is not a 0.4 mm/rev tool. A 1.2 mm nose will take that feed, and will shove the part off centre if the stick-out is long.

  • Roughing — feed comes from the chipbreaker and the horsepower. Ra is ignored.
  • Finishing — rε is picked from the drawing first, and f is back-calculated.
  • Compromise — one insert, two feeds: 0.30 mm/rev in, 0.12 mm/rev for the last pass.

Roughing and finishing: two sets of conditions, two conflicting goals

Roughing wants metal in the bin. Depth of cut as deep as the insert and the machine will stand, feed at the top of the chipbreaker, cutting speed a notch below the catalogue, so the edge survives the scale. Surface finish is not a parameter. The pass is making a shape for the next tool.

Finishing wants a number on a drawing: a diameter, an Ra, a cylindricity. Depth of cut drops to 0.2–0.5 mm, enough to get under the previous tool's work-hardened skin, not enough to bend the part. Feed comes from the roughness formula. Cutting speed often goes up. A hotter, cleaner shear leaves a brighter finish and keeps built-up edge off the nose.

Those two jobs do not share one line in the program. The insert may be the same. Vc, f and ap are not. The roughing edge is a different corner of the same CNMG, or a tougher grade altogether. The finishing edge is honed, positive, and expensive. The corner is indexed before the last pass. The extra twenty seconds costs less than a scrapped shoulder.

A spring pass — same offset, no extra depth — is the smaller sibling of a finishing cut. It takes the elastic push out of the tool and the part. On a slender shaft it is the difference between a ring gauge that goes and one that does not.

Constant surface speed (G96) versus constant spindle speed (G97), and when each one wins

Cutting speed is a speed at the cut, not a spindle RPM. Vc = π · D · n / 1000, with D in millimetres, n in rev/min and Vc in m/min. Change the diameter, or change n, and Vc walks off. That relation is what this turning calculator inverts to get spindle speed. A lathe has two answers when the diameter changes under the tool.

Vc = π · D · n / 1000  ·  n = 1000 · Vc / (π · D)  ·  SFM = Vc / 0.3048

G96 is constant surface speed. The program carries Vc, or SFM on an inch control. The CNC winds the spindle up as the tool moves in, and down as the tool moves out. Longitudinal turning on a taper, a facing cut, a profile: wear stays even, Ra stays even, and the insert sees the speed printed on the box. G97 locks one RPM. Vc is then left to change. Parting, grooving, drilling from the tailstock, threading: the diameter is fixed, or it falls fast enough that G96 would try to hit 8,000 rev/min at the centre. The chuck will not enjoy that.

G96 is clamped with a G50 maximum RPM, or a Fanuc G92. Facing a 20 mm face down toward a hole, the control will chase an infinite n. The clamp is not optional. A manual lathe is in G97 either way. The RPM is taken from the largest diameter, the centre is accepted as a rub, or the gears are changed on the way in — which nobody does.

US tooling lists live in SFM. 100 m/min is 328 SFM. The inch shortcut is n ≈ 3.82 × SFM / D(in). Metric: n ≈ 318 × Vc / D(mm). Same physics. Different clipboard.

Tool life and the Taylor equation: what a 20% speed increase really costs

Raise cutting speed 20% and the clock on that pass drops about 17%. The edge does not lose 17%. Taylor wrote it as V · Tn = C. The exponent n is small. That is the trap.

V · Tn = C  ·  T2 / T1 = (V1 / V2)1/n

For coated carbide, n sits around 0.25. A 20% rise in Vc gives (1.20)4 ≈ 2.07. Tool life is cut in half. HSS is worse: n ≈ 0.1–0.15, and the same 20% can cost a factor of four to six. Ceramic is kinder, with n toward 0.4. A ceramic insert will take a speed carbide is not asked to take. Slowing a ceramic down is a common way to break the edge.

C is the cutting speed that would last one minute. Nobody runs there. Catalogue Vc is usually a 15-minute life, sometimes 30. The economic speed sits a bit below the catalogue maximum once indexing time, the price of the edge, and the scrap from a cratered nose are in the sum. A 20% push is a common late-shift temptation. The Taylor sum comes before that push is treated as free time.

Feed is the cheaper lever. Life is far less sensitive to f than to Vc. Where the motor has the amps, metal comes off with feed and depth of cut, not with speed.

Reading abnormal wear: flank wear, cratering, built-up edge, notching, chipping

The insert is a report. It gets read under the shop light before the offset is touched.

  • Flank wear (VB) — a uniform land on the clearance face. That is the wear the edge is meant to show. The corner is changed at about 0.3 mm on roughing, 0.15 mm on finishing. When the land grows too fast, Vc is high or the grade is too soft.
  • Crater wear — a pit on the rake, behind the edge, where the chip has been welding and diffusing. Vc is too high, or the grade has no alumina layer for steel. A deep crater undercuts the edge and the whole corner lets go.
  • Built-up edge (BUE) — workpiece metal welded to the edge, torn off later, and taking coating with it. The finish looks torn. Speed is too low, or the material is sticky (304, 316, aluminium). A higher Vc, a sharper rake, and coolant on the nose are the usual fixes.
  • Notching — a gash exactly at the depth-of-cut line. Scale, sand, a work-hardened skin, or a depth of cut that never changes, with the same millimetre of edge taking the beating on every pass. Vary ap. Move to a tougher grade. The finishing pass does not reuse the roughing corner that has already notched.
  • Chipping — a bite missing from the edge. An interrupted cut, too much feed for a brittle grade, a hammered setup, or built-up edge that pulled a lump of carbide away. Feed comes down, the edge is honed, and a P35 replaces a P15.

Thermal cracks, comb lines across the edge, mean the insert is quenched on every revolution. Flood on, flood off, or a wet-dry cycle on a ceramic. One condition, not both. Wet or dry.

Parting off and grooving: overhang, blade width, reduced feed, the risk of jamming

A parting blade is narrow, and it deflects. Width 2–4 mm. Stick-out as short as the diameter allows. The blade can sing even then. This page derates feed to about 45% of ordinary turning for grooving and parting. That factor is not timid. It is how the blade is kept from walking.

RPM stays locked on G97. G96 at the centre is a wreck: speed climbs, the blade rubs, the part pinches. Feed goes in at a modest rate and eases over the last few millimetres, once the remaining disc is thin and tries to climb the blade. Coolant has to reach the groove, not the splash guard. A slight side clearance, or a twisted chipbreaker, helps. A square blade in a closing groove is a jam waiting.

The two faces of the cut close as the blade goes deeper. Mild steel will pinch the blade and snap it. A small back-rake, a peck out to break the ring, or a 0.05 mm retract at the bottom of a groove, saves more blades than a grade change. A long bar is not parted off without a catcher, or without a tailstock backed off at the right moment. The stub that flies is a projectile.

Slender workpieces, tailstock and steady rest: when the part vibrates instead of cutting

When the part is what rings, no insert grade saves the diameter. A shaft with L/D past about 4 starts to bow under the radial force. Past 6 or 8 the bar whips. The finish becomes a chatter spiral, the diameter goes barrel-shaped, and the tool rubs on the way back.

First support is a live centre in the tailstock. That halves the bending length. The end is faced and centre-drilled properly. A badly drilled centre is a second chatter source. On longer work the next support is a steady rest, or a follower rest that travels with the tool. Cast-iron shoes sit on a finished diameter. Rollers sit on a rough one. The shoes are oiled. A dry rest marks the job in one pass.

Rather than dropping RPM first, depth of cut comes down, and the radial component with it. A small entering angle, a CSNM instead of a 90° facing tool, sends more of the force along the axis, where the part is stiff. A smaller nose radius does the same. Feed can stay where it is. A feed that is too light rubs, work-hardens, and chatters harder. If the bar sings after that, the missing piece is a rest, not a slower spindle.

A boring bar is the same physics inside a hole. Deflection grows with the cube of the stick-out. Same lesson, turned inside out.

Flood coolant, minimum quantity lubrication or dry cutting, material by material

Coolant has three jobs: carry heat off the edge, lubricate the rake, and shove the chip clear. Not every material wants all three.

  • Steels (P) — flood emulsion at 6–8%, aimed at the nose, not at the sky. Stainless wants more pressure and an oiliness package, or the chip welds.
  • Cast iron (K) — dry, or an air blast. Water plus graphite dust is a grinding paste on the ways and on the insert. When a wet cut cannot be avoided, the filter has to be up to the dust.
  • Aluminium (N) — flood, or MQL. MQL, a few millilitres of oil per hour in a mist, is plenty for turning aluminium. It limits built-up edge without drowning the chip conveyor. Some shops run dry, with a polished diamond-coated insert and air.
  • Superalloys (S) — flood, high pressure where the machine has it. The edge is not starved. Heat is the failure mode.
  • Hardened (H) — often dry, with CBN or ceramic. Thermal shock from flood is how those edges crack.

MQL is not a thin flood. It is a metered aerosol on the rake. It suits aluminium and brass. It is a weak heat sink on a heavy steel roughing cut. Dry cutting in steel is possible with the right coating and a chip that carries the heat away, in a shop that can live with hot blue spirals.

Turning wood and plastics: what changes compared with metal

Wood is not a slow steel. It wants a knife. High-speed steel, or a very sharp carbide: rake 20–40°, clearance generous, Vc from the hundreds of metres per minute up to a couple of thousand. The edge shears fibres. It does not plastic-flow a chip. Dust extraction does the job coolant would do on metal. A dull tool burns, raises the grain, and invites a catch that snatches the gouge out of the hand.

Plastics melt. That is the failure, not a slow version of a steel chip. Nylon, acetal, acrylic, PTFE conduct heat badly, and the heat stays in the cut. Sharp HSS or polished carbide, a large clearance (12° and up), a moderate Vc (often 50–150 m/min), and an air blast so the swarf does not weld back on. Flood water can help acrylic. Oil on nylon can swell it. Feed stays high enough that the tool cuts, rather than rubs. A rubbed plastic diameter is glazed, oversize once it cools, and ugly.

Fibreglass and carbon fibre are the other case. The workpiece grinds the edge. Carbide or diamond, dust under control, and an edge that dulls by abrasion rather than by cratering.

Lathe safety: chuck key, guarding, wood blanks bursting, stringy chips

The chuck key is the classic failure. It stays in the hand, or in a spring-loaded holder. Never in the chuck. A key left in the chuck becomes a missile the moment the spindle is jogged. Every old turner has that story. A new one has no need to collect one.

A long chip is not picked off a rotating part with the fingers, a rag, or compressed air aimed at the face. The spindle stops. A hook takes the chip, or the chipbreaker has already broken it. Mild steel and aluminium will wrap a wrist.

Guards are closed before the spindle starts, chuck guard included on a CNC. A file on a running lathe is a 19th-century habit, and it takes fingertips. Wood blanks, green or cracked ones in particular, can burst. The first speed is a low one, the glue line on a bowl blank is checked, and nobody stands in the line of fire. Unbalanced work at speed walks the machine across the floor.

Stringy chips call for another chipbreaker, a higher feed, or a peck. Reaching into the cut is not the remedy. A chip hook costs nothing. A tendon does.

Costing a part from cutting time and the price of an edge

Cycle time is not the cost. Cost is machine minutes, plus edges, plus the minutes spent changing those edges. A high Vc that halves tool life can lose money while the stopwatch looks good.

cost / part ≈ tcycle · Rmachine + (tcut / T) · Cedge

Rmachine is the burdened rate: depreciation, labour, lights, the inspector. Cedge is the insert price divided by the corners actually used. A CNMG has four, unless a corner is chipped. T is the Taylor life at the Vc in use. Raise speed 20% on carbide and tcut drops about 17%, while T drops about 50%. Twice the edges are bought for a modest saving in time. On a 40-dollar-an-hour machine and a 4-dollar corner, that arithmetic is worth doing once.

Roughing is usually limited by how fast metal leaves, and by how full the chip conveyor gets. Milling has the same trade. On a lathe it is harder to miss, because the one edge dies in plain sight.

Surface feet per minute, metres per minute, and the RPM the spindle actually sees

Catalogues do not share a unit. European and ISO sheets speak in m/min. North American shops speak in SFM. The insert does not care which label is on the box. 1 m/min = 3.281 SFM, which makes 200 m/min equal to 656 SFM, and 400 SFM equal to 122 m/min. Both figures belong on the setup sheet when two people share the machine.

The number entered on the control is n. That is where the mistakes sit. A 50 mm bar at 180 m/min wants about 1,150 rev/min. The same Vc on a 12 mm stub wants 4,770. Leave the 1,150 in from the previous job and the stub crawls, builds built-up edge, and looks sticky. Leave 4,770 in on an 80 mm chucking and the insert fails at once. The calculator is there so the conversion is not a felt-tip sum on the wall.

On a dual-mode control, G20 and G21 (inch and metric) have to agree with the units G96 is using. Mix them once and the error is a factor of 25.4. It happens.

Depth of cut versus insert size: using the edge already paid for

An insert has an inscribed circle. CNMG 120408 is a 12.7 mm IC, 4.76 mm thick, with a 0.8 mm nose. The chipbreaker is sized for a band of ap as well as a band of f. Bury a finishing geometry 4 mm deep and the chip forms behind the breaker, where there is no breaker. Tickle a roughing geometry at 0.15 mm and the cut is only on the radius: rubbing, pushing, notching.

A shop rule that holds up: ap at least around two-thirds of rε, which puts the straight cutting edge in the work, and ap no more than about a third of the IC unless the holder and the machine are built for more. A 12 mm IC insert is a 2–4 mm roughing tool on the machine, not an 8 mm one. The pocket and the clamp are the other limit. A screw-down positive insert takes less abuse than a double-clamp negative.

Depth of cut is a radial figure. A 2 mm ap takes 4 mm off the diameter. That sentence catches an apprentice on the second day.

Interrupted cuts, mill scale and a rusty hex: the insert killers

A round bright bar is a courtesy the insert does not always get. A flame-cut plate, a weld, a hex turned down to round, a keyway already milled: those cuts are hammers. The edge enters, leaves, and enters again. Carbide dislikes the cycle. Vc comes down 20–30%. The grade moves up in toughness: a P35, a honed edge, a thicker insert. Feed stays up, so each entry is a cut and not a bounce. Dropping the feed “to be gentle” work-hardens the skin and chips the next corner.

Scale and rust act as sandpaper on the depth-of-cut line. Notch wear is the mark they leave. Where the stock allows it, a cheap roughing corner skins the bar first, and ap is then changed so the finishing edge sits under the scale. A ceramic that runs happily on a continuous 1045 cut will shatter on a weld bead. It stays in the drawer until the diameter is clean.

Single-point threading on a rusty bar has the same entry shock, and a worse one: the tip is a 60° point. The bar is skinned before the thread starts.

Three numbers that have to agree: n, f, and ap

Spindle speed comes from Vc and D. Feed rate is Vf = n · f, in mm/min, which is the figure a CNC wants on the finish as well as on the rough. Metal removal is Q = ap · f · Vc. With ap and f in millimetres and Vc in m/min, that product is already in cm³/min. Power is about Q times the specific cutting force* kc, divided by 60,000 to reach kW at the cut, and divided again by efficiency to reach motor kW.

Kienzle corrects kc for chip thickness. On a 90° tool this calculation takes the undeformed thickness h as the feed per revolution. A thinner chip raises kc. A finishing feed can therefore demand more specific force than the roughing feed on the same steel, even while Q falls.

kc = kc1.1 / hmc  ·  Vf = n · f  ·  Q = ap · f · Vc  ·  Pc ≈ kc · Q / 60 000

With the motor already at its limit, a higher RPM is not a way out. ap or f comes down. With a dirty finish, a deeper ap is not a way out either. f comes down, or Vc goes up, where Taylor still leaves room. With a chattering part, RPM is the last knob: stick-out, the rest and the nose radius come first, and a 10% speed change only after that, to step off a bad frequency.

Drilling and tapping use the same cutting-speed idea, with a much smaller number on the dial. A turning speed left parked in a tap program is how a tap snaps in the hole.

Glossary

Cutting speed
Surface speed of the work past the edge, Vc, in m/min. Vc = π · D · n / 1000, with D in millimetres and n in rev/min. Inch catalogues print the same speed as SFM. 1 m/min = 3.281 SFM, and 100 m/min is 328 SFM.
Feed
Advance of the tool per revolution, f, in mm/rev. The control is often given the feed rate Vf = n · f in mm/min. On this page, grooving and parting use about 45% of an ordinary turning feed. Theoretical roughness follows f² against the nose radius.
Depth of cut
Radial engagement ap, in millimetres. It is measured on the radius: a 2 mm depth of cut takes 4 mm off the diameter. A chipbreaker is built for a band of ap as well as a band of feed. Finishing depths on this page sit around 0.2–0.5 mm.
Specific cutting force
Force per unit area of the chip, kc, in N/mm². Kienzle writes kc = kc1.1 / hmc, with h the undeformed chip thickness. For a 90° tool this page sets h equal to the feed. Cutting power is Pc ≈ kc · Q / 60 000, in kW when Q is in cm³/min.
ISO 513
The workpiece-family code on the insert. P (blue) steel, M (yellow) stainless, K (red) cast iron, N (green) aluminium and other non-ferrous metals, S (brown) nickel and titanium, H (grey) hardened steel, typically from 45 HRC up. Inside a family a P10–P20 is hard and wear-resistant; a P30–P40 is tougher.
Nose radius
Corner radius rε. In a code such as CNMG 12 04 08 the last two digits, 08, are 0.8 mm. Common sizes are 0.4, 0.8, 1.2 and 2.4 mm. Peak-to-valley height of the feed mark is Rt ≈ f² / (8 · rε). Feed much past about 0.7 × rε leaves the radius and cuts on the straight side.
Chipbreaker
The form pressed into the rake, sized for a feed band. Finishing geometries sit near 0.08–0.20 mm/rev, medium geometries near 0.20–0.40 mm/rev, and roughing geometries from about 0.40 mm/rev upward. Outside that band the chip ribbons, or it smears, instead of breaking.

Related calculators