Drilling Speed and Feed Calculator
Drilling is the most common machining operation — and the one that breaks the most tools. The drill works buried at the bottom of its own hole, packed in its own chips, with coolant that never really reaches the cutting edge. Hence cutting speeds well below turning, and two figures this calculator gives you alongside the RPM: the thrust force and the torque, which tell you whether your machine will cope.
A quirk of the twist drill: the quoted cutting speed is the one at the periphery. At the centre, along the web, it is zero — the tool does not cut there, it extrudes the material. That is where the thrust force comes from, and why a pilot hole pays off on larger diameters.
Other operations: turning, milling, boring, threading, tapping.
Drill and hole
Drill features and cutting quantities marked with an asterisk are defined in the glossary, in the sense a twist drill uses them on this page.
Anatomy of a twist drill: web, flutes, margins, helix angle, clearance
A twist drill is a pair of cutting edges mounted on a screw conveyor. The lips do the cutting. Everything else keeps those lips alive and carries the chip up the hole.
The web* is the solid spine between the flutes. It supplies the stiffness in torsion, and at the point it is a blunt chisel. Webs thicken towards the shank — a broken drill in section shows it — so a long jobber is stiffer back at the chuck, and every regrind moves the point into a thicker web. Thin the web at the point, with a split point or a notched point, and the thrust force* drops by a third or more. Leave the web thick and the tool is not drilling. It is extruding a dimple with a cold chisel.
Flutes carry chips and coolant. Deep, wide and polished suits aluminium and a long chip. Shallower and harder-backed suits cast iron and a short chip, with more body behind the margin. The margins are the thin cylindrical lands that size the hole: two of them, 180° apart, rubbing at cutting speed* Vc. Too wide, and they burn. Worn, and the hole goes taper.
Helix angle* is the pitch of the flute. 10–15° for brass and hard iron, where the chip should break and the tool should not screw itself in; ~30° for general steel; 35–40° for aluminium and copper. Clearance behind the lip — the relief — stops the heel rubbing. No relief means heat. Too much relief leaves a weak edge that chips on the first hard spot.
A 118° jobber off the rack is a compromise of all of that. It is not a gun drill, not a stub, and not a wood bit. It is a starting geometry, changed to suit the hole required.
Point angle by material: 118°, 135°, 140° — and why wood wants 60°
Point angle* is the included angle of the two lips. A flatter point, the larger number, gives stronger corners and a shorter entry, which suits hard material, but it skates on a flat face unless the point is split or spotted. A sharper point centres more readily on a punch mark, makes longer and thinner lips, and pulls harder on breakthrough.
- 118° — the HSS default. Steel, general iron, a mixed drawer of work. Sound on a drill press that has a centre-punch mark to follow.
- 135° — harder steels, stainless, and a lot of carbide drills. Often paired with a split point, which keeps the web from staying a chisel. Less wandering on a mill with no spot.
- 140° — carbide on tough alloys, and some through-coolant drills. Very flat, very strong at the corners, and it needs a machine that can push.
- ~60°, wood — a brad-point or a lip-and-spur. The centre spike locates, the outer spurs shear the fibres, and only then do the lips scoop. A 118° metal drill in oak blows the exit out.
Brass often needs a flattened point and a reduced helix. Without that, the bit grabs and screws the work up the flutes. Acrylic likes a small included angle and chips that are scraped, not melted. The angle on the grinding rest is not a fixed creed. It matches the material in the vice that day.
Sharpening a drill and thinning the web: the two moves that change everything
A dull drill is a blunt cone that rubs, blues, and then walks. Sharpening means two lips of the same length, the same angle and the same relief. A longer lip takes the whole cut, and the hole goes oversize on a banana axis. Off-hand grinding can produce the match. A drill grinder produces it before the first cup of coffee. A drill gauge checks the result or, more bluntly, the chip from each flute: the two chips should look like twins.
Web thinning is the second move, and the one most bench grinders skip. Each resharpening eats into a thicker part of the web, and a freshly sharpened drill gets harder to push. A split-point grind — an S-point, a notched point — cuts the chisel edge down to two small secondary lips. Thrust collapses. The drill starts on a mill without a spot. Deep holes stop smoking.
A carbide drill is not a bench-grinder job. It goes back for a proper grind, or it is replaced. HSS is the grade that can be saved at the wheel, provided the point stays cool: dipped, not cooked. A blued lip has lost its hardness in the last two millimetres, which is exactly the length that had to stay hard.
Pilot holes, spotting drills and step drills: setting up a large-diameter hole
Above about 12–16 mm, the web of a standard jobber is a large fraction of the diameter. Thrust on a 20 mm drill in 1045 is already a two-handed lean on a small press. A pilot hole the size of the web, or a hair under, turns the chisel into a pair of lips and dumps most of that thrust. This calculator flags the case on large diameters. The flag belongs in the setup, not in a footnote.
A spotting drill is not a centre drill. A centre drill, the combined drill and countersink, is for a tailstock centre. A spot is a short, stiff drill, 90° or 120°, that leaves a shallow cone for the twist drill to follow. On a mill, that cone is what holds location. Pressed into service as a spot, a centre drill works until the tiny tip snaps in a hard skin. The rest of the hole then follows a bent start.
Step drills and subland drills put two diameters on one tool: a lead diameter that pilots, and a second diameter that opens the hole. Sheet metal, a clearance hole plus a screw head, a dozen identical holes in a panel. They are not gun drills, and they hate depth. The work stays flat and is backed up. A step drill is not the tool for a 30 mm hole in plate thicker than the step was designed for.
A large hole on a mill is often a helical milling pass, or a boring pass, after a modest drill. The twist drill is the start, not the tolerance.
Peck cycles on CNC: G81, G83 and how to set their parameters
G81 is the cycle for a hole that can be trusted: in, to depth, out. It suits a shallow hole, short chips, through-coolant, or a material that makes dust, such as cast iron. G83 is the peck cycle* for a deep hole: peck, full retract, re-enter, and the nest of chips leaves the flutes. G73 is the impatient cousin, a small chip-break retract that does not come all the way out. Faster, and it clears less. Fine until the flutes pack.
- Q — peck depth. A starting figure is around 1 × D in steel, 2–3 × D in aluminium with through-coolant, and less in stainless. The peck deepens only once the chips look like chips, not like packing.
- R — the retract plane. Above the burrs, not 0.1 mm above a rough casting.
- F — feed, held constant. Easing off at the bottom in stainless is how the last millimetre work-hardens and the corners snap.
- Dwell — almost never at the bottom of a blind hole in gummy material. Spinning in place is rubbing.
A G83 that pecks 0.5 mm in a 10 mm hole wastes time and hammers the lips. A G81 taken to 8 × D in mild steel, with no coolant through, leaves a blue drill and an oversized hole. The cycle has to match the depth this page reports as a ratio of D.
Beyond 10 × D: through-coolant drills, guide bushings, gun drilling
Past about 5 × D the job has changed. Past 10 × D, pecking harder is not a method. Chips will not climb a 15 × D flute on a jobber on the strength of the cycle alone.
Through-coolant carbide, at 20–70 bar, is the usual answer on a machining centre. Oil or emulsion reaches the lips, chips come up the flutes, and the hole stays on line: the drill is cutting, not walking on packed swarf. A bushing in a drill jig, or a start-bush on a lathe tailstock, holds the margins for the first few diameters and keeps the drill from wandering. After that the hole is its own bushing, for better or worse.
Gun drilling is the specialist tool: a single lip, a kidney-shaped oil hole, 50–100 bar, a guide, and an L/D into the dozens. A long HSS drill is not a gun drill with the name left off. A drawing that calls for 200 mm deep at 6 mm diameter belongs in a gun-drill shop, or on a purpose-built deep-hole cycle. It is not a Friday-afternoon G83.
Coolant in drilling: neat oil, emulsion, mist, compressed air
In a hole the fluid has to arrive at a point that cannot be seen. That is the whole problem.
- Neat oil — the best film on stainless, on aluminium, and on a tap-drill that must stay round. Messy. A fire risk on a rag. Superb on a small press.
- Emulsion — the CNC default, at 6–10%. Cooling first, lubrication second. Sent through the tool, it becomes a chip pump.
- Mist or MQL — enough for shallow holes in aluminium. Not a substitute for 40 bar at 12 × D.
- Air — cast iron, graphite, some composites. It blows the dust out. An air blast into a nest of steel chips is not coolant. It is shrapnel.
A dry HSS drill in 304 will blue in one hole. A wet carbide drill in the same hole will make a thousand. The fluid is part of the tool.
Diagnosis: oversize hole, bell-mouthed hole, torn breakout, a drill that squeals or blues
The hole reports the fault. Oversize or oval points to unequal lips, a drill spinning in a worn chuck, or a spot that was never there. Bell-mouth, big at the top, means the drill wandered for the first millimetre and then followed itself. A spot or a bush stops that wander, unless the margins have already gone.
A torn exit is a feed too high for the last 0.5 mm of unsupported skin, a missing backing block, or a point too sharp for the material. A squeal is rubbing: a dull lip, a feed that is too slow, or a drill that is walking. Blue means Vc too high, or no coolant at the lips. The temper is gone. The drill is scrap, or it is ground back past the colour. It is not kept “for aluminium”.
A drill that screams and then goes quiet has not settled in. It has work-hardened the hole and is polishing a hard skin with dead lips. It comes out, it is sharpened, and the next entry uses a feed that cuts. Otherwise the next drill dies in the same place.
A hole the right size at the top and tight at the bottom is a taper, from worn margins or from a packed flute that pushed the tool off line. More frequent pecks, coolant through the tool, or a shorter drill.
Drilling stainless and titanium: why work hardening forbids slowing down mid-hole
Austenitic stainless and titanium harden under a dull push. The cut has to stay under the skin the lip has produced. Feed goes up, not down. A hesitation — a dwell, a peck that sits, an ease-off at the bottom — and the next lip meets 40 HRC that was 20 HRC a second earlier. The corners snap.
The workable set is a split point, 135°, carbide if the machine can hold it, through-coolant, a constant feed, and G83 pecks that leave the hole and take the heat with them. HSS cobalt will manage small holes if it stays wet and is never allowed to rub. Titanium needs stricter care: a lower Vc than stainless, plenty of fluid, no rubbing, and a sharp edge. On a 10 mm hole, 0.08–0.15 mm/rev is a cutting feed. 0.02 mm/rev is a burnishing feed, and burnishing is how a hole becomes tap-proof.
A drill is not stopped in stainless or titanium and then restarted in the same spot. It retracts, the hole is cleared, and the next entry uses the feed that was intended. A pause at mid-depth is a broken-corner appointment.
Drilling wood and panels: brad point bits, Forstner bits, hole saws
Wood is fibre. The surface has to be sheared before the core is lifted. A brad point does that: a spike in the middle, spurs on the rim, lips behind. Entry is clean, and the exit is decent once the work is backed up. A metal jobber in pine wanders and tears.
Forstner bits make flat-bottomed holes — hinge cups, a recess, a hole that must not blow through. They need spindle speed, not pressure, and they hate a handheld drill used as a ram. Hole saws take large diameters by cutting a kerf, not a chip. The plug is the waste. The work is clamped and rim speed stays low. The diameter is huge, and Vc at the teeth is what burns. Sawdust left in the kerf cooks it.
Plywood and laminate need the face scored, or a down-cut or a brad that shears the veneer. A backing board saves the exit. MDF is dust, and the dust is extracted. The speed looks high next to steel. Smoke means the edge is rubbing, not cutting.
Drilling plastics: melting, breakout on exit, the rake angles that suit
Plastics fail in two ways. They melt onto the flutes, and they chip out the last millimetre. Both come from heat and a dull edge.
Sharp HSS, polished flutes, a little more helix, and a point that is not too flat. Air, or a drop of water on acrylic. A slow-to-moderate Vc, and a feed that produces a chip that can be picked up, not dust that smears. Pecking clears the gum. A flute that loads is withdrawn and peeled. A loaded flute is a reamer that melts a triangle-shaped hole, which then shrinks as it cools and binds the drill.
Breakout is handled by backing the sheet, dropping the feed for the last millimetre, or drilling from both sides to a meeting point. Acrylic cracks if it is punched through, and chips if it is grabbed on breakthrough. Polycarbonate is tougher: it smears and builds a burr rather than cracking. A small relief on the point, of the sort used on a brass grind, reduces the grab. This is the opposite of stainless: here the feed does ease off at the end.
Safety: the drill grabbing on breakthrough, clamping the work, thin sheet
Breakthrough is the moment the lips stop being a drill and become a screw. The web has nothing left to push, the margins take a bite, and the work climbs the flutes. On a press, with the work held in the hand, that ends in A&E. A clamp, a vice, a step clamp. Not a glove and a hope.
Thin sheet is the worst case. It flexes, the point pops through, the hole grabs, and the sheet becomes a rotating knife. Scrap behind it, a step drill, and a lighter feed before breakthrough. A small drill in sheet, even on a mill, is clamped. “Only 3 mm” is the sentence that comes just before the part spins.
The guard on a drill press is there because chips, the workpiece and hair all meet at the same spindle. Long chips off a 12 mm hole in mild steel will wrap a wrist. They come away with a brush, not a finger. The tap that follows this hole grabs even harder if it is given the chance. Same vice. Same rule.
Jobber, stub and extra-length: picking a drill by stick-out
A jobber is the default length. A stub drill, the screw-machine length, is shorter and stiffer, starts straighter, and will not reach through a tall fixture. An extra-length drill, or an aircraft extension, is a flute on a fishing rod. It wanders, it whistles, and it follows every hard spot unless it is bushed, or started with a stub and then changed for the long tool.
Stick-out is the accuracy. The same 8 mm point, 20 mm out of the chuck, drills a hole that can be reamed. At 80 mm out it draws a cone. Where reach is required, a stub start plus a long drill to finish is two tools and one good hole. One long drill is one tool and a lottery. Carbide through-coolant drills are stubby for this reason. The catalogue length is a warning, not a dare.
A worn chuck that holds 12 mm on three jaws of unequal grip is stick-out of another kind. The drill becomes a lever running out. An indicator on the shank, or a collet chuck, settles it. The grind is not the first suspect.
Thrust on the handle: the push a drill press has to give
Thrust force Ff is the push along the axis. This page estimates it from chip thickness, the specific cutting force* kc and the point. On a CNC machine the figure is a load-meter reading. On a drill press it is the shoulder on the handle. A 16 mm HSS drill in 1045, at a proper feed, is tens of kilograms on that handle. If the feed cannot be kept steady without bouncing, the feed is too high, the point is dull, or a pilot is required — not a longer lever welded onto the handle.
n = 1000 · Vc / (π · D) · Vf = n · f · h = (f / 2) · sin(κr)
A pilot the size of the web cuts that thrust by roughly two thirds, which is why a large hole is stepped. Pecking does not reduce thrust. It only clears chips. When the press walks across the floor, the work lifts, or the belt slips, the cut is past what the machine will give. The job moves to the mill, or the diameter is stepped.
Reaming allowance: how much to leave after the drill
A twist drill makes a hole. A reamer makes a size. Too little stock — 0.05 mm on a 10 mm hole — and the reamer rubs, chatters, and goes oversize on the bell. Too much — 1 mm — and the reamer is a poor mill: it follows the drilled axis, tapers and tears. Shop starting figures are 0.2–0.3 mm on a 6–10 mm hole, 0.3–0.5 mm on 12–20 mm, and a bit more in gummy aluminium when the reamer has a proper lead.
The drilled hole has to be straight. A reamer will not pull a banana into a cylinder. It follows the curve and polishes it. Spot, bush, stub-drill, then ream. Speed on the reamer stays low, and the feed is surprisingly high: the tool has to cut, not glaze. Flood coolant in steel. A boring bar is the other way to true a hole that started off line.
Insert drills on a lathe: the U-drill versus the twist drill
An indexable insert drill — a U-drill: a short body carrying two inserts, one at the centre and one at the periphery — is how a CNC lathe opens a 20–60 mm hole without 400 mm of HSS hanging out of the tailstock. The speed sits in the range used for turning, the feed is high, coolant goes through the tool, and the machine has to accept an interruption on every revolution. A handheld press is the wrong machine.
The hole is typically a few tenths over nominal, and it is not a reamer finish. Suitable for a relief, for a thread core that will be tapped or bored, for a hole whose job is to save weight. Not suitable for an H7 on its own. Stick-out matters here as well: these bodies are short on purpose. A worn insert on the periphery walks the size. Both inserts are indexed, not only the outer one.
A twist drill in the tailstock remains the better choice on small diameters, on a mill, and on a job that has neither through-coolant nor the power. The tool follows from the hole, the machine, and the chip that can be evacuated — not from whatever is left in the drawer.
Glossary
- Web
- The solid core of a twist drill, between the flutes. It stiffens the tool in torsion. At the point it forms the chisel edge, which pushes the material aside instead of cutting it.
- Thrust force
- The axial push the drill needs in order to keep feeding, written Ff. On a twist drill most of it comes from the web, not from the cutting lips.
- Cutting speed
- The speed of the cutting edge relative to the work, written Vc and quoted at the outside diameter. On a drill it is highest at the periphery and zero at the centre of the web.
- Helix angle
- The angle of the flute spiral. A steep helix lifts a long chip quickly. A shallow helix is less likely to screw the drill into the work.
- Point angle
- The included angle between the two cutting lips. A larger angle gives a flatter, stronger point. A smaller angle bites more sharply and wanders more readily.
- Peck cycle
- A drilling move that advances a short distance, withdraws to clear the chips, and advances again. On a CNC control, G83 retracts clear of the hole and G73 makes only a short chip-break.
- Specific cutting force
- The force needed to cut one square millimetre of chip, written kc. It depends on the material and on the thickness of the chip.