Worked examples
- Lathe: f = 0.2 mm/rev at 1,273 RPM → F = 0.2 × 1,273 ≈ 255 mm/min.
- Mill: Ø10 mm 3-flute end mill, fz = 0.05 mm at 3,820 RPM → F = 0.05 × 3 × 3,820 ≈ 573 mm/min.
- Finish: with f = 0.2 mm/rev and a 0.8 mm nose radius, Ra ≈ 0.2² / (32 × 0.8) × 1000 ≈ 1.6 µm.
Feed chart by material
Starting values for coated carbide and a medium cut, the same ones the site's calculator uses: mm/rev for turning and drilling and mm per tooth for milling. For finishing, lower the feed; for roughing, raise it if the machine and tool can take it.
| Material | ISO | Turning f (mm/rev) | Milling fz (mm/tooth) | Drilling f (mm/rev) |
|---|---|---|---|---|
| Low-carbon steel S235 / St37 | P | 0.30 | 0.12 | 0.20 |
| Medium-carbon steel C45 / 1045 | P | 0.28 | 0.10 | 0.18 |
| Alloy steel 42CrMo4 / 4140 | P | 0.25 | 0.09 | 0.16 |
| Austenitic stainless 304 / 1.4301 | M | 0.22 | 0.08 | 0.12 |
| Austenitic stainless 316 / 1.4401 | M | 0.20 | 0.07 | 0.10 |
| Gray cast iron GG25 / EN-GJL-250 | K | 0.30 | 0.12 | 0.22 |
| Aluminum 6082 / AlMgSi1 | N | 0.25 | 0.15 | 0.25 |
| Aluminum 7075 / AlZnMgCu | N | 0.22 | 0.13 | 0.22 |
| Brass CuZn39Pb3 | N | 0.20 | 0.10 | 0.20 |
| POM-C / Delrin plastic | N | 0.20 | 0.15 | 0.15 |
| Titanium Ti6Al4V | S | 0.15 | 0.06 | 0.08 |
| Inconel 718 | S | 0.12 | 0.05 | 0.06 |
| Hardened steel 50-55 HRC | H | 0.10 | 0.04 | 0.05 |
01mm/rev or mm/min: G95 and G94
Lathes are almost always programmed in mm/rev (G95, or G99 on Fanuc lathes): the actual feed then adapts by itself when RPM changes with G96. Mills are programmed in mm/min (G94). Mixing them up is a serious error: 0.2 in mm/min is almost standing still, and 200 in mm/rev is a crash.
02Feed per tooth is what the part feels
On a mill, the value that matters is feed per tooth fz: the chip thickness each edge removes. If you raise RPM without touching mm/min, fz drops and the edge may rub instead of cutting. Remove a flute and the same F means more load per tooth.
03Chip thinning on narrow passes
With a small radial depth (ae less than half the diameter), the actual chip is thinner than the programmed fz. At ae = 10% of the diameter the chip is only about 60% of fz, so feed can be raised to stop the edge rubbing. This is the basis of trochoidal and high-speed milling.
04Signs that the feed is wrong
Too high: chatter, broken edges, poor finish and a struggling machine. Too low: the edge rubs, heats up and wears sooner; in stainless steel it work-hardens the surface, and on a lathe chips do not break and wrap around. A slightly higher feed with less depth usually works better than the opposite.
05Common mistakes
Copying the F from another machine's program without recalculating with its RPM, forgetting the number of flutes, using the roughing feed for finishing and programming G95 on a mill by accident. Always calculate F with the machine's actual RPM.
Frequently asked questions
What is feed rate?
It is how fast the tool advances while cutting. Turning and drilling use mm/rev (f) and milling uses feed per tooth (fz); the machine converts it to mm/min with the RPM.
How do you calculate milling feed rate?
F = fz × z × n: feed per tooth times number of teeth times RPM. For example, 0.05 mm × 3 flutes × 3,820 RPM ≈ 573 mm/min.
What is the difference between G94 and G95?
G94 programs feed in mm/min and G95 in mm/rev. On Fanuc lathes the equivalents are G98 and G99. Lathes almost always use per revolution and mills per minute.
How does feed affect surface finish?
When turning, theoretical roughness grows with the square of the feed: Ra ≈ f² / (32 × r). Lowering the feed or using a larger nose radius improves the finish.
Indicative starting values. Confirm them with the tool maker's data, the actual material and your machine's rigidity. Last updated: