Cutting Speed, Spindle Speed and Feed Rate
Surface speed and RPM, feed per tooth and per revolution, feed rate, metal removal rate and the unit conversions between metric and inch.
Cutting speed and spindle speed
The cutting speed (surface speed) Vc is how fast the cutting edge moves across the material: the speed of the tool rim in milling and drilling, or of the workpiece surface in turning. It depends on the material and on the tool, not on the machine. The spindle speed n (RPM) is what you set on the machine, and it follows from the surface speed and the diameter.
n = 1 000 × Vc ÷ (π × D)
Worked example: a 10 mm end mill in aluminum
- Surface speed 100 m/min, diameter 10 mm: n = 1 000 × 100 ÷ (π × 10) = 3 183 rpm.
- The same surface speed on a 20 mm cutter needs only 1 592 rpm, and on a 3 mm cutter 10 610 rpm: halving the diameter doubles the RPM.
- A tool’s speed is limited by heat, not by RPM: a small tool must spin much faster to reach the same rim speed.
Metric and inch units
US shops quote surface speed in surface feet per minute (SFM) and diameters in inches. The formula becomes RPM = 12 × SFM ÷ (π × D) ≈ 3.82 × SFM ÷ D, with D in inches. The two systems are exactly equivalent (1 m = 3.28084 ft).
| Surface speed (metric) | Surface speed (inch) |
|---|---|
| 30 m/min | 100 SFM |
| 60 m/min | 195 SFM |
| 100 m/min | 330 SFM |
| 200 m/min | 655 SFM |
| 300 m/min | 985 SFM |
| 600 m/min | 1 970 SFM |
Worked example: a 1/2 inch drill in mild steel
- A high-speed steel drill in mild steel starts at about 100 SFM. RPM = 12 × 100 ÷ (π × 0.5) = 764 rpm (the shortcut 3.82 × 100 ÷ 0.5 = 764 agrees).
- At a feed of 0.007 inch per revolution the feed rate is 764 × 0.007 = 5.3 in/min (136 mm/min).
- A hole 1.0 inch deep takes about 11 s of cutting.
Feed: per tooth, per revolution, per minute
Feed is quoted three ways, and mixing them up is the commonest mistake.
| Name | Symbol | Unit | Used for |
|---|---|---|---|
| Feed per tooth (chip load) | fz | mm/tooth, in/tooth | Milling: the chip thickness each tooth takes |
| Feed per revolution | f | mm/rev, in/rev (IPR) | Drilling, turning, tapping, reaming |
| Feed rate | Vf | mm/min, in/min (IPM) | What the controller is told to do |
milling: Vf = n × z × fz drilling, turning: Vf = n × f
Worked example: milling feed rate
- A 4-flute 10 mm end mill at 3 183 rpm and a chip load of 0.05 mm per tooth: Vf = 3 183 × 4 × 0.05 = 637 mm/min.
- A two-flute tool at the same speed and chip load feeds at half that rate (318 mm/min): more flutes allow a faster feed for the same chip thickness, but leave less room for chips.
- Doubling the RPM at the same chip load doubles the feed rate; the tool covers the work faster but wears faster too (see Tool Life, Wear and Cutting Economics).
Metal removal rate
The volume of material removed per minute, Q, measures how productive a cut is and what power it needs (see Cutting Force, Power and Torque).
milling: Q = ap × ae × Vf ÷ 1 000 (cm³/min) turning: Q = Vc × ap × f (cm³/min)
Worked example: how much metal per minute
- The mill above with a 8 mm depth and 5 mm stepover removes 8 × 5 × 637 ÷ 1 000 = 25 cm³/min.
- To get more, increase the depth, the width or the feed: depth and width are cheap, speed is expensive, because speed shortens tool life far more than the others.
- Doubling the removal rate by doubling the depth of cut costs about double the power; doubling it by doubling the cutting speed also costs double the power and cuts tool life sharply.
When the spindle cannot reach the speed
Small tools in soft materials want very high speeds, and many hobby spindles and routers stop at 10 000 to 24 000 rpm. When the ideal RPM is out of reach, run at the maximum and keep the chip load the same, so the feed rate falls in proportion. Never keep the feed rate and lower the RPM: the chip load would rise and the tool would break.
Worked example: a 3 mm cutter on an 18 000 rpm spindle
- The ideal speed for 200 m/min is 21 221 rpm, beyond the spindle’s 18 000 rpm.
- At 18 000 rpm the real surface speed is 170 m/min (85 % of the target): perfectly acceptable, as long as the material is not one that rubs and burns at low speed.
- The ideal feed rate would be 21 221 × 2 × 0.02 = 849 mm/min; at the limit it is 18 000 × 2 × 0.02 = 720 mm/min. Keep the chip load and the feed follows the RPM.
RPM quick tables
Spindle speeds from the formula, in metric and inch. Read across from the diameter to the surface speed you want.
| Diameter | 20 m/min | 30 m/min | 60 m/min | 100 m/min | 150 m/min | 250 m/min | 400 m/min |
|---|---|---|---|---|---|---|---|
| 3 mm | 2 120 | 3 180 | 6 370 | 10 610 | 15 920 | 26 530 | 42 440 |
| 6 mm | 1 060 | 1 590 | 3 180 | 5 310 | 7 960 | 13 260 | 21 220 |
| 10 mm | 637 | 955 | 1 910 | 3 180 | 4 770 | 7 960 | 12 730 |
| 12 mm | 531 | 796 | 1 590 | 2 650 | 3 980 | 6 630 | 10 610 |
| 16 mm | 398 | 597 | 1 190 | 1 990 | 2 980 | 4 970 | 7 960 |
| 20 mm | 318 | 477 | 955 | 1 590 | 2 390 | 3 980 | 6 370 |
| 25 mm | 255 | 382 | 764 | 1 270 | 1 910 | 3 180 | 5 090 |
| Diameter | 50 SFM | 100 SFM | 200 SFM | 300 SFM | 500 SFM | 800 SFM |
|---|---|---|---|---|---|---|
| 1/8 in | 1 530 | 3 060 | 6 110 | 9 170 | 15 280 | 24 450 |
| 1/4 in | 764 | 1 530 | 3 060 | 4 580 | 7 640 | 12 220 |
| 3/8 in | 509 | 1 020 | 2 040 | 3 060 | 5 090 | 8 150 |
| 1/2 in | 382 | 764 | 1 530 | 2 290 | 3 820 | 6 110 |
| 3/4 in | 255 | 509 | 1 020 | 1 530 | 2 550 | 4 070 |
| 1 in | 191 | 382 | 764 | 1 150 | 1 910 | 3 060 |
Turning is the same idea
On a lathe the workpiece rotates, the diameter is the workpiece diameter, and the feed is per revolution. The details are in Turning, Threading and Surface Finish.
Worked example: turning a 50 mm bar
- At 120 m/min on a 50 mm bar: n = 764 rpm. With a feed of 0.20 mm/rev the feed rate is 153 mm/min, so a 100 mm pass takes 39.3 s.
- The removal rate at a 2 mm depth is 120 × 2 × 0.20 = 48 cm³/min.
- As the diameter turns down, the RPM must rise to keep the same surface speed: constant surface speed (G96) does this automatically.
Troubleshooting
| Symptom | Likely cause | Try |
|---|---|---|
| Tool is very hot or turns blue | Surface speed too high, no coolant | Lower the RPM; use coolant or air; check the speed against the material data |
| Tool wears fast on the flank | Speed too high for the tool material | Reduce the speed 20 %; use a harder coating or carbide |
| Edge rubs, glazes the surface, makes dust not chips | Feed too low for the speed | Raise the feed until real chips form |
| Tool snaps or chips | Feed too high, or RPM too low for the feed rate | Reduce the feed per tooth; keep it with the RPM |
| Feed rate looks right but the cut is heavy | Mixed up feed per tooth and per revolution | Recalculate Vf = n × z × fz |
| Controller shows a different feed than the program | Units: mm/min against in/min, per rev against per minute | Check the G-code units and the feed mode (G94, G95) |
Related
- Speeds and Feeds: the overview of this guide.
- Chip Load, Chip Thinning and Engagement: chip load and chip thinning.
- Speeds and Feeds by Material: the speeds and chip loads to use.
- CNC Feeds and Speeds Calculator and G-code and Programming (feed modes and units).
FAQ
How do I convert SFM to RPM?
RPM = 3.82 × SFM ÷ diameter in inches. For 100 SFM and a 1/2 inch tool that is about 764 rpm.
What is the difference between chip load and feed rate?
Chip load (feed per tooth) is the thickness each tooth cuts; the feed rate is how fast the tool moves: feed rate = RPM × number of teeth × chip load.
Should I change speed or feed to fix a problem?
One at a time. Heat and fast flank wear point to speed; rubbing, dust and poor chips point to feed; breakage points to chip load or depth.
What do I do if my machine cannot reach the RPM?
Run at the maximum and keep the same chip load; the feed rate falls with the RPM.
References
- Oberg, E., et al., Machinery’s Handbook (cutting speed and RPM formulas, SFM tables).
- ISO 3002 (basic quantities in cutting and grinding) and ISO 3685.
- Tool makers’ catalogs (Sandvik, Kennametal, Harvey, OSG) for speeds and feeds of specific tools.
Last reviewed: October 2026. Speeds and feeds are typical starting values: follow your tool maker’s data.