Free tool

Feeds and speeds

Spindle speed, cutting feed and plunge feed for an end mill or router bit, from its diameter, flute count and the chipload the material wants. The numbers are conservative starting points: tune them by ear and by the chips.

Cutter

Units

mminch

Diameter, D

Flutes, z

flutes

Material

Material (carbide cutter)

Plywood at 6 mm: 0.15–0.25 mm per tooth.

Start the chipload at

Low endMiddleHigh end

Low end is the cautious start. Move up once the cut sounds and looks right.

Spindle

Spindle speed

Enter rpmFrom surface speed

Spindle speed, S

rpm

Spindle min

rpm

Spindle max

rpm

Optional. Your spindle’s range: min_rpm and max_rpm on a TNC-M34’s spindle page. Leave blank for no limit.

Machine and engagement

Machine max feed

mm/min

Optional. The lowest feed any of X, Y and Z can really deliver. Leave blank to skip.

Correct for chip thinning (optional)

Cutting feed 5 400mm/min

Within spindle rangeChipload clears rubbing limit

Spindle speed: 18 000 rpm
Plunge feed (50% of feed): 2 700 mm/min
Chipload per tooth: 0.15 mm
Surface speed: 339 m/min
Stepover (40% of D): 2.4 mm
Depth per pass (50% of D): 3 mm

G-code for this result
Block	What it does
G21 G94	Millimetres, feed per minute
M3 S18000	Spindle on, clockwise, at 18 000 rpm
G1 Z… F2700	Plunge to depth
G1 X… Y… F5400	Cut

By flute count, at S18000 and 0.15 mm per tooth
Flutes	Feed, mm/min	Plunge, mm/min	Machine max
1	2 700	1 350	—
2	5 400	2 700	—
3	8 100	4 050	—
4	10 800	5 400	—

Starting values, not guaranteesEvery number here is a conservative general starting point for a carbide cutter, not data for your cutter, machine or stock. Listen to the cut and look at the chips, then trim with the feed and spindle overrides.

How it is worked out

A cutter makes a good chip when each cutting edge takes a bite of the right thickness: the chipload, fz, in mm per tooth. Too thin and the edge rubs and heats up; too thick and the cutter or the machine is overloaded. Everything below follows from choosing fz and a spindle speed.

Spindle speed

RPM = Vc × 1000 / (π × D)
Vc  = π × D × RPM / 1000

D   cutter diameter, mm
Vc  surface speed at the cutting edge, m/min

Enter the spindle speed directly, or let the surface speed set it. If you give the spindle’s range, a speed outside it is clamped to the nearest end, and the feed is then worked out at the clamped speed so the chipload stays where it was.

Feed and plunge

feed   (mm/min) = RPM × z × fz
plunge (mm/min) = RPM × z × fz × plunge share

z   number of flutes
fz  chipload, mm per tooth

The plunge share is 50% of the feed for softwood, hardwood, MDF, plywood and HDPE, 40% for cast acrylic, and 30% for FR4, aluminium, brass, mild steel and a custom chipload. A plunge loads the whole tip, so it is worked from the chipload without any chip-thinning correction.

Stepover and depth per pass

Suggested as fractions of the diameter, for pocketing and profiling with a square-end cutter: 40% stepover and 50% depth for the woods, MDF and HDPE (40% depth in hardwood); 40% stepover and 30% depth in cast acrylic; 30% and 25% in FR4; 30% and 20% in aluminium and brass; 20% and 10% in mild steel; 25% and 25% for a custom chipload.

Chip thinning (optional)

if ae < D/2:   fz_adj = fz × D / (2 × √(D·ae − ae²))
otherwise:     fz_adj = fz

ae  radial engagement (width of cut), mm

When the cutter takes less than half its diameter sideways, each edge leaves a chip thinner than the feed per tooth. Programming fz_adj brings the real chip back up to fz. The correction is off unless you tick the box, and with it off the calculator assumes at least half-diameter engagement. It warns when the factor passes 3: numbers that high only hold on a rigid machine with a sharp cutter.

Rubbing threshold

minimum fz ≈ max(0.005 mm, 0.002 × D)

A rule of thumb, not a measured limit. No edge is perfectly sharp, and a chip thinner than the edge’s own rounding is pushed rather than cut. Below this figure the page flags the chipload as too small. At 6 mm that is about 0.012 mm per tooth.

Machine maximum feed

If the feed comes out above the machine maximum you entered, the page says so and does not quietly cap it. A lower feed at the same spindle speed thins the chip toward rubbing. It suggests the spindle speed that keeps the chipload at your maximum feed instead, or fewer flutes.

Worked example

A 6 mm, 2-flute carbide cutter in plywood, on a spindle that tops out at 18 000 rpm. The page opens with these values.

fz       = 0.15 mm             plywood at 6 mm is 0.15–0.25; start at the low end
RPM      = 18000               entered, and within the spindle’s range
Vc       = π × 6 × 18000 / 1000  ≈ 339 m/min
feed     = 18000 × 2 × 0.15    = 5400 mm/min
plunge   = 5400 × 50%          = 2700 mm/min
stepover = 40% × 6 mm          = 2.4 mm
depth    = 50% × 6 mm          = 3 mm

Starting values by material

For carbide cutters. Chipload is in mm per tooth at each listed diameter. Between them it is interpolated; below 3 mm it is scaled down in proportion to the diameter; above 12 mm it stays at the 12 mm value. These are conservative general starting points from common shop practice, not measurements and not a cutter maker’s data. Where the maker publishes a chipload for the cutter you are using, choose Custom chipload and use theirs.

Material	3 mm	6 mm	10 mm	12 mm	Vc, m/min	Plunge	Stepover	Depth per pass
Softwood	0.08–0.13	0.18–0.28	0.30–0.45	0.35–0.50	300–600	50%	40%	50%
Hardwood	0.06–0.10	0.15–0.23	0.25–0.38	0.30–0.43	250–500	50%	40%	40%
MDF	0.08–0.13	0.18–0.28	0.30–0.45	0.35–0.50	300–600	50%	40%	50%
Plywood	0.07–0.12	0.15–0.25	0.25–0.40	0.30–0.45	300–600	50%	40%	50%
Acrylic (cast)	0.05–0.08	0.10–0.18	0.18–0.28	0.20–0.30	200–400	40%	40%	30%
HDPE	0.08–0.12	0.15–0.25	0.25–0.38	0.28–0.43	250–500	50%	40%	50%
PCB (FR4)	0.02–0.04	0.04–0.08	0.06–0.10	0.07–0.12	150–300	30%	30%	25%
Aluminium 6061	0.013–0.025	0.03–0.05	0.05–0.08	0.06–0.10	150–300	30%	30%	20%
Brass	0.013–0.025	0.03–0.05	0.05–0.08	0.06–0.10	100–200	30%	30%	20%
Mild steel	0.008–0.015	0.020–0.035	0.035–0.055	0.040–0.065	60–100	30%	20%	10%

Reading the cut

Rules of thumb for moving off the starting value:

Fine dust instead of chips, a hot cutter, burn marks on wood or melted edges on plastic: the chipload is too low. Raise the feed, or lower the spindle speed.
Chatter, or a machine that labours: the cut is too heavy. Take less depth or less stepover before you lower the chipload.
Aluminium sticking to the flutes: clear the chips with air or mist, and prefer a 1- or 2-flute cutter.
Long stick-out, a light machine or a worn cutter: all of these call for lower numbers than the table.

On a TNC-M34

M3 S… starts the spindle clockwise at S rpm; M4 runs it counter-clockwise and M5 stops it. A lone S word changes the speed of a running spindle.
Feed is the F word in units per minute (G94): millimetres after G21, inches after G20. G95, feed per revolution, is refused when the program loads, and so is a G1 with no feed in effect.
The spindle settings hold min_rpm and max_rpm; enter those as the spindle range above. With a step-driven spindle (mode = STEP), max_rpm caps the commanded speed.
Every axis’s max_rate caps a move, but the step rate is limited to 100 kHz per axis, so an axis can deliver at most 6 000 000 ÷ steps_per_mm mm/min, whatever max_rate says: 7 500 mm/min at 800 steps/mm. Use the lower of the two as the machine max feed.
Feed-O and Spin-O set the feed and spindle overrides as percentages while the job runs. That is the way to tune a starting value by ear.

On a TNC-L32 lathe the work turns, not the cutter, so this calculator does not apply directly. The L32 also accepts G95 feed per revolution and G96 constant surface speed, with G50 clamping the spindle speed.

Limits

Carbide, square-end cutters on a mill or router. Not for high-speed steel, which wants far lower surface speeds, nor for ball-nose finishing, V-bits, drills or taps.
The stepover and depth suggestions are for pocketing and profiling. A full-width slot loads the cutter far more heavily: take a shallower pass.
Feeds are rounded to whole mm/min, or to a tenth of an inch per minute, in the G-code.