Hong Life CalculatorsUnderstanding the speeds and feeds calculator — concept and principle
Milling needs two settings: how fast the spindle turns and how fast the table moves. This calculator converts a cutting speed and chip load into spindle rpm and table feed, corrects the feed for radial chip thinning when the cut is narrow, and estimates the material removal rate. Machinists and CNC programmers use it to set up a new tool or material.
How it is calculated
n = 1000 × vc ÷ (π × D)
vf = fz × z × n
hmax = fz × 2√((ae/D)(1 − ae/D)) when ae < D/2, otherwise hmax = fz
Corrected fz = fz² ÷ hmax; corrected feed = corrected fz × z × n
Q = ae × ap × vf ÷ 1000 (cm³/min)
- vc cutting speed (m/min), D cutter diameter (mm), z number of flutes, fz feed per tooth (mm).
- ae radial width of cut and ap axial depth of cut (mm).
The principle
The cutting edge travels π × D millimetres per revolution, so the rpm needed for a given surface speed is the speed divided by the circumference. Each tooth removes a chip whose nominal thickness is the feed per tooth, and with z teeth the table must advance fz × z per revolution. When the cutter engages only a narrow strip (less than half its diameter), each tooth enters and leaves the work at a shallow angle and never cuts the full fz thickness. The chip is thinner, which rubs and wears the tool. Raising the feed so that the maximum chip thickness equals the intended chip load restores proper cutting.
Worked example
Default inputs: vc 150 m/min, D 10 mm, 3 flutes, fz 0.05 mm, ae 3 mm, ap 10 mm.
- n = 1000 × 150 ÷ (π × 10) = 4,775 rpm.
- Feed per revolution = 0.05 × 3 = 0.15 mm/rev; vf = 0.15 × 4,775 = 716 mm/min (28.2 in/min).
- ae/D = 0.3, so hmax = 0.05 × 2√(0.3 × 0.7) = 0.0458 mm.
- Corrected fz = 0.05² ÷ 0.0458 = 0.0546 mm; corrected feed = 0.0546 × 3 × 4,775 = 781 mm/min.
- Q = 3 × 10 × 716 ÷ 1000 = 21.49 cm³/min.
| Cutting speed vc (m/min) | Spindle speed n (rpm) |
|---|---|
| 37.5 | 1,194 |
| 75 | 2,387 |
| 112 | 3,581 |
| 150 | 4,775 |
| 188 | 5,968 |
| 225 | 7,162 |
| 300 | 9,549 |
How to read the result
Cutting speed and chip load come from the tool maker's tables for your material and coating; this calculator only converts them. If the rpm is above your machine's maximum, run at the maximum and keep the chip load, which lowers the feed. Chip thinning matters most in light radial cuts such as finishing or high-efficiency milling. The removal rate lets you compare strategies and estimate cycle time and spindle power.
Common mistakes
- Using cutting speed in surface feet per minute while entering millimetres.
- Applying the chip-thinning correction to full-width slots, where it does not apply.
Frequently asked questions
What is chip load?
The thickness of material each tooth removes per revolution, also called feed per tooth.
Why does a narrow cut need a higher feed?
The actual chip becomes thinner than the feed per tooth, so the feed is raised to keep the real chip thickness on target.
Does more flutes mean a faster feed?
At the same chip load, yes, because more teeth cut per revolution. Chip evacuation may limit flute count in soft materials.
Sources: Standard machining formulas: n = 1000vc/(πD), vf = fz·z·n, radial chip thinning and Q = ae·ap·vf