Why drilling needs its own speed and feed rules
A twist drill is not a milling cutter with two flutes. Three things make it a different problem. Its cutting speed varies from the rated figure at the outside corner to exactly zero at the axis, so the centre of the drill never cuts — the chisel edge extrudes material sideways instead. The chip has to reverse direction and climb out through the flutes, so evacuation, not edge wear, limits deep holes. And because the whole circle is being removed, torque and thrust are far higher than a mill cut of the same diameter.
Feed is therefore quoted per revolution rather than per tooth. A drill has two symmetric lips, so feed per revolution splits between them and each lip takes half. Published drill feed tables give feed per revolution directly, and the practical starting rule is 0.01 to 0.02 times the drill diameter for steel — 0.005 to 0.010 in/rev on a 1/2 in drill.
That rule has a consequence worth seeing. Since the required RPM falls as 1/D and the feed per revolution rises as D, the penetration rate in inches per minute is nearly constant across drill sizes at the same surface speed. A 1/8 in and a 1 in drill in the same material both penetrate at roughly the same inches per minute. What changes enormously is the torque, which scales with D².
The four calculations, and where each constant comes from
Spindle speed. The outside corner of the drill travels πD per revolution, so to reach a surface speed of SFM feet per minute the spindle must turn 12 × SFM ÷ πD times. That is the same identity the spindle RPM calculator uses; the 12 is simply inches per foot. Metric: n = 1000 Vc ÷ πD with D in millimetres.
Penetration feed. Multiply feed per revolution by the spindle speed. Nothing subtler is involved, and it is what the control needs as an F word in G81 or G83.
Torque. A solid drill removes a chip whose total cross-section is f × D/2 per lip pair, and the specific cutting force kc gives the tangential force per unit area. Working the force through the mean radius at which it acts gives M = kc f D² / 8000 in newton-metres with f and D in millimetres. The square on the diameter is the important part: doubling the drill size at a fixed feed per revolution quadruples the torque, and with the feed scaled to diameter as well it multiplies it by eight.
Cycle time. Axial travel divided by penetration feed. The travel is not just the hole depth: a conical drill point extends (D/2) ÷ tan(θ/2) beyond the full diameter, which is 0.3004 D for a 118° point and 0.2071 D for a 135° point. For a through hole the point must clear the far face, so that length is added.
Worked example: a 1/2 in HSS drill through 1 in of mild steel
A 0.500 in high-speed steel jobber drill, 118° point, in 1018 steel one inch thick. The handbook figure for HSS in mild steel is around 100 SFM, and you choose 0.005 in/rev — the conservative end of the 0.01–0.02 D rule.
- Spindle speed. 12 × 100 ÷ (π × 0.500) = 1,200 ÷ 1.5708 = 764 rpm.
- Penetration feed. 0.005 × 764 = 3.82 in/min, which is 97.0 mm/min.
- Point length. (0.500 ÷ 2) ÷ tan 59° = 0.250 ÷ 1.6643 = 0.1502 in.
- Axial travel. 1.000 + 0.1502 = 1.1502 in, because the point must break through.
- Cutting time. 1.1502 ÷ 3.82 = 0.3011 min = 18.1 seconds.
- Torque. In metric, D = 12.70 mm and f = 0.127 mm/rev, with kc ≈ 1,800 N/mm² for low-carbon steel: 1,800 × 0.127 × 12.70² ÷ 8,000 = 4.61 N·m, or 3.40 lb·ft.
- Power at the cut. 4.61 × 2π × 764 ÷ 60 = 369 W = 0.37 kW, about half a horsepower.
Half a horsepower is trivial; 4.6 N·m is not, on a hand-fed drill press. Now scale to a 1 in drill at the same 0.01 D feed rule — 0.010 in/rev, 382 rpm — and the torque becomes 1,800 × 0.254 × 25.4² ÷ 8,000 = 36.9 N·m, eight times as much, which is why a 1 in hole gets a pilot drill and a 1/2 in hole does not.
Reading the numbers before you cut
Check torque against the machine first. A bench drill press typically stalls or spins the work well below 20 N·m; a knee mill with a drill chuck is limited by the quill's rack and pinion; a CNC machining centre will normally have plenty. If the torque figure looks high, a pilot hole at roughly the width of the drill's web removes the chisel-edge contribution and cuts the required thrust dramatically, though it does less for the torque because the lips still cut the same annulus.
Check depth next. Standard jobber drills evacuate chips reliably to about three diameters; beyond that a peck cycle (G83) becomes necessary, and beyond five diameters you want a parabolic-flute drill or through-coolant. The feed and speed above assume free chip flow, so a hole that packs will jam at parameters that are correct on paper.
Then check the feed against the diameter. Below about 0.005 D per revolution the chisel edge does more extruding than the lips do cutting, which raises thrust, work-hardens the hole bottom and is a common cause of drill failure in austenitic stainless. Above about 0.03 D the lips take a chip the flute cannot clear. The band between those is where drills are meant to live.
Finally, treat the surface speed figure as belonging to the drill material, not the hole. HSS in mild steel sits around 80–110 SFM; carbide roughly triples that; stainless and titanium want considerably less than steel, and hardened material wants a solid carbide drill designed for it rather than a slower feed on an HSS one.
Speed, feed and torque for HSS drills in mild steel at 100 SFM
| Drill | Speed (rpm) | Feed (in/rev) | Feed (in/min) | Torque (N·m) |
|---|---|---|---|---|
| 1/8 in | 3056 | 0.003 | 9.17 | 0.17 |
| 1/4 in | 1528 | 0.005 | 7.64 | 1.15 |
| 3/8 in | 1019 | 0.007 | 7.13 | 3.63 |
| 1/2 in | 764 | 0.010 | 7.64 | 9.22 |
| 3/4 in | 509 | 0.015 | 7.64 | 31.10 |
| 1 in | 382 | 0.020 | 7.64 | 73.74 |
Penetration rate barely changes across the range while torque rises more than four hundredfold from the 1/8 in drill to the 1 in drill. That contrast is the reason large holes are stepped and small ones are not.
Assumptions, limits and common errors
- Torque is a sharp-tool estimate. Specific cutting force values assume a correctly ground drill with equal lips and a normal chip. A dull drill, an off-centre web or a rubbing margin can draw well above the figure shown.
- Thrust is not calculated here. Axial thrust is dominated by the chisel edge and depends on web thickness and point grind, which no diameter-and-feed formula captures. Machinery's Handbook gives empirical thrust constants by material and point geometry.
- Chip evacuation is not modelled. Beyond about three diameters of depth the limit is getting chips out, not cutting them. Use a peck cycle and expect to reduce the feed.
- The cycle time excludes rapids and pecks. It is the in-cut time only. A pecked hole spends much of its cycle retracting.
- Cutting speed refers to the outside corner. The corner is the fastest-moving and hottest point on the drill, which is where wear begins and why it is the reference point for the speed table.
- Core drills and insert drills remove less material. They cut an annulus rather than a full circle, so the torque estimate here is conservative for them.
Drilling in the wider sequence of operations
A drilled hole is usually a means to something else, and the something else sets the tolerance you need. A drill produces a hole that is typically oversize by a few thousandths and not especially round or straight, which is fine for a clearance hole and unacceptable for a bearing fit — that needs reaming or boring, and the fit itself is defined by the tolerance symbols the ISO hole and shaft fit calculator resolves.
When the hole is going to be tapped, the drill diameter is set by the thread rather than by convenience, and the choice of drill decides the percentage of thread engagement you end up with. That is a calculation in its own right; the tap drill size calculator works it out for unified and metric threads and reports the nearest standard drill.
The speed and feed logic here is the drilling case of the same three-parameter framework used in milling and turning: surface speed sets temperature, feed sets mechanical load per edge, and the product with the engaged area sets removal rate. The material removal rate calculator covers the drilling geometry alongside milling and turning, and the cutting speed calculator converts in the reverse direction when you already have a spindle speed and want to know what it means. Machinery's Handbook is the standard reference for drilling feeds, point geometry and the empirical constants behind thrust and torque.