Speeds & Feeds Calculator
RPM, feed rate, metal removal and power — metric or inch, with every formula shown.
Feed for a surface finish
| Grade | Ra, µm | Largest feed |
|---|
From Ra ≈ f² ÷ (32 rε) with the nose radius above; real surfaces are usually rougher.
How it was calculated
Results are estimates from the formulas shown, not a professional design or certification. Have a qualified engineer verify anything safety-critical (structures, electrical installations, gas or pressure systems).
About the Speeds & Feeds Calculator
Pick the operation — milling, drilling, turning, reaming or tapping — the work material and the tool material, and the calculator fills in starting values for the cutting speed and the chip load or feed, which you can change. It gives the spindle speed, the feed rate, the metal removal rate and an estimate of the cutting power and spindle torque, in metric or inch units.
For milling it applies radial and axial chip thinning, so a light stepover gets the faster feed that keeps the chip load the tool is designed for. For turning it estimates the theoretical surface roughness from the feed and nose radius and shows the matching ISO 1302 N grade. A spindle-speed limit caps the rpm and recalculates the feed.
How to use it
- Choose the operation, the units (metric or inch), the work material and whether the tool is HSS or carbide. The cutting speed and feed boxes fill with starting values.
- Enter the tool diameter (the workpiece diameter for turning) and, for milling, the number of teeth, the radial stepover a_e and the axial depth a_p. For reaming, add the hole size before reaming to get the removal rate and power.
- Adjust the cutting speed and chip load to the tool maker’s figures if you have them. Leave chip thinning on for milling with a stepover below half the diameter.
- Optionally enter your spindle’s top speed, the machine efficiency and a length of cut for the time per pass.
- Read the spindle speed, feed rate, metal removal rate, power and torque, with the formulas. Copy result copies them as text.
Examples
v_c = 150 m/min, chip load 0.05 mm, a_e = 2 mm, a_p = 10 mm
4,775 rpm; chip thinning ×1.25 → f_z = 0.0625 mm, 1,194 mm/min; 23.9 cm³/min; about 1.6 kW at the cutter
v_c = 25 m/min, f_n = 0.12 mm/rev
796 rpm, 95.5 mm/min, 7.5 cm³/min, about 0.4 kW
v_c = 200 m/min, f_n = 0.2 mm/rev, a_p = 2 mm, nose radius 0.8 mm
1,273 rpm, 255 mm/min, 80 cm³/min; R_a ≈ 0.2² ÷ (32 × 0.8) = 1.56 µm (N7)
n = 3.82 × SFM ÷ D
3.82 × 500 ÷ 0.5 = 3,820 rpm
The formulas
- Spindle speed: n = 1000 × v_c ÷ (π × D) with v_c in m/min and D in mm; in inch units n = 12 × SFM ÷ (π × D) ≈ 3.82 × SFM ÷ D
- Milling feed rate: v_f = f_z × z × n (f_z feed per tooth, z teeth); metal removal rate Q = a_p × a_e × v_f
- Drilling, reaming, turning: v_f = f_n × n (f_n feed per revolution); drilling Q = π D² ÷ 4 × v_f, turning Q = v_c × a_p × f_n
- Reaming: from the hole size d before reaming, Q = π ÷ 4 × (D² − d²) × v_f, with the chip h = f_n ÷ z × sin κ_r (z teeth, κ_r the chamfer angle)
- Tapping: the feed per revolution is the pitch, so v_f = P × n
- Power: P_c = Q × k_c, with the specific cutting force k_c = k_c1 × h_m^(−m_c) taken at the mean chip thickness h_m; the motor needs P_c ÷ η, and the spindle torque is P_c × 9549 ÷ n (kW, rpm, N·m)
Chip thinning
With a stepover a_e smaller than half the cutter diameter, each tooth leaves the cut before reaching its full chip thickness: the maximum chip is f_z × sin φ, where φ = arccos(1 − 2 a_e ÷ D) is the engagement angle. A 10 mm cutter at a 2 mm stepover cuts a chip only 0.8 times the feed per tooth, so the feed can rise by 1.25 to keep the chip load. A face mill with a 45° entering angle thins the chip by sin 45° in the same way. Very light stepovers give large boosts — check them against the tool maker’s limits.
Surface finish and N grades
In turning, the nose radius leaves a scalloped surface whose theoretical roughness is R_a ≈ f_n² ÷ (32 × r_ε) and peak-to-valley R_t ≈ f_n² ÷ (8 × r_ε). Halving the feed quarters the roughness; a larger nose radius also helps but raises the cutting forces. The old ISO 1302:1992 roughness grades, still common on drawings, are N1 = 0.025 µm, N2 = 0.05, N3 = 0.1, N4 = 0.2, N5 = 0.4, N6 = 0.8, N7 = 1.6, N8 = 3.2, N9 = 6.3, N10 = 12.5, N11 = 25 and N12 = 50 µm R_a. Current standards (ISO 21920-1) write R_a values directly.
About the starting values
The cutting speeds, chip loads and k_c1 values filled in for each material are typical, conservative starting points for each ISO 513 material group (P steel, M stainless, K cast iron, N non-ferrous, S heat-resistant alloys and titanium, H hardened steel). The right numbers depend on the exact grade and hardness, the tool’s coating and geometry, the coolant and the rigidity of the machine and set-up. Start with them, watch the chips and the sound, and adjust — or use the tool maker’s data from the start.
Sources
- Machinery’s Handbook, 32nd ed. (2024) — cutting speeds, feeds and power; reaming at about 2/3 of the drilling speed
- Sandvik Coromant, metal cutting formulas and definitions for milling, drilling and turning — chip thinning, specific cutting force and power
- ISO 1302:1992, roughness grade numbers N1–N12 (later replaced; ISO 21920-1:2021 is current)
- ISO 513, classification of hard cutting materials by application group (P, M, K, N, S, H)
Limitations
- The material starting values are typical, not guaranteed: tool life, finish and chatter depend on the actual tool, holder, machine and set-up.
- Power is an estimate for a sharp tool from typical k_c1 values; worn tools and negative rake need more. Check the machine’s power and torque at the speed used.
- Power, torque and removal rate are estimated for milling, drilling, turning and — when you enter the hole size before reaming — reaming. Tapping torque depends strongly on the tap, the thread depth and the lubricant, so only the speed and feed are given for tapping.
- Ball-nose effective diameter, helical interpolation, ramping, plunge milling and high-feed cutters are not modelled.
- The surface finish is the theoretical value from geometry; real surfaces are usually rougher.
Privacy
Everything happens in your browser. What you enter or open here is not uploaded or stored by MySmartCoPilot.
Frequently asked questions
How do I calculate spindle speed (rpm)?
n = 1000 × v_c ÷ (π × D). A 10 mm end mill at 150 m/min runs at 1000 × 150 ÷ (π × 10) = 4,775 rpm. In inch units, rpm ≈ 3.82 × SFM ÷ diameter in inches.
How do I calculate the feed rate for milling?
Multiply the feed per tooth by the number of teeth and the rpm: v_f = f_z × z × n. At 0.05 mm per tooth, 4 teeth and 4,775 rpm that is 955 mm/min — or 1,194 mm/min once chip thinning for a 2 mm stepover is applied.
What is chip thinning?
With a stepover under half the cutter diameter the chip never reaches the feed per tooth, so the tool rubs instead of cutting. Raising the feed by D ÷ (2√(a_e × (D − a_e))) brings the real chip back to the intended chip load.
What is the difference between SFM and m/min?
Both are cutting speeds — the speed of the cutting edge over the work. SFM is surface feet per minute; 1 m/min = 3.281 SFM, so 100 m/min is 328 SFM.
How much power does a cut need?
About the removal rate times the specific cutting force: P_c = Q × k_c. Milling 24 cm³/min of medium-carbon steel with a thin chip takes about 1.6 kW at the cutter, roughly 2 kW at the motor. The calculator shows both and the spindle torque.
What does N7 surface finish mean?
An ISO 1302 roughness grade of R_a 1.6 µm (63 µin). N6 is 0.8 µm and N8 3.2 µm. A turned surface with a 0.8 mm nose radius at 0.2 mm/rev is about R_a 1.6 µm in theory, which is N7.