What table feed rate is and where it comes from
Table feed is the speed at which the machine drives the tool along the toolpath, and it is the only feed number a CNC control understands. Everything else — chip load, feed per revolution, feed per tooth — is a way of describing what that speed does to the cutting edge. The conversion is a single multiplication, but it is the multiplication that decides whether a tool survives the job.
The chain runs in one direction. The material and the tool grade give you a surface speed. The surface speed and the cutter diameter give you a spindle RPM, which is what the spindle RPM calculator handles. The tool maker's data sheet gives you a chip load for that diameter and material. Multiply the chip load by the number of flutes and by the RPM and you have the feed rate. Change any link and the feed changes with it.
The mistake this fixes is the habit of copying a feed rate from a previous job. A feed of 48 in/min is correct for a four-flute cutter at 3,000 rpm taking 0.004 in per tooth, and it is four times too fast for the same tool at 750 rpm. Feeds do not travel between setups; chip loads do.
The formula, and the correction most people skip
In one minute the spindle turns n times, and each turn brings Z teeth past the work, so n × Z teeth cut in that minute. If each one is to remove a chip fz thick, the work must advance fz × Z × n inches. That is the whole derivation, and it works identically in metric with fz in mm/tooth.
Feed per revolution, fz × Z, is worth knowing separately because it is diameter-independent and it is how lathes and drills quote feed. A four-flute cutter at 0.004 in per tooth advances 0.016 in each revolution regardless of spindle speed.
The correction is radial chip thinning. A milling cutter forms a comma-shaped chip: zero thickness at entry, maximum somewhere in the arc, zero at exit. The maximum equals the feed per tooth only when the tooth reaches the point where its motion is perpendicular to the feed direction, which happens only once radial engagement reaches half the cutter diameter. Below that, the thickest chip formed is 2√(ae/D − (ae/D)²) times the feed per tooth. Divide by that ratio to recover the intended chip, and the corrected feed comes out at or above the uncorrected one — never below it, since the ratio never exceeds 1.
This is what makes high-efficiency roughing possible. At a 10% stepover the ratio is 0.600, so you must feed 1.667 times faster just to make the same chip the tool was rated for. That is not a productivity trick; it is a correction for a geometric fact, and skipping it is the reason light-stepover paths so often rub tools to death.
Worked example: 1/2 in four-flute carbide at 10% stepover
A 0.500 in four-flute carbide end mill, data sheet chip load 0.004 in per tooth, running at 3,000 rpm with a 0.050 in stepover.
- Tooth passes per minute. 3,000 × 4 = 12,000.
- Feed per revolution. 0.004 × 4 = 0.016 in/rev.
- Base table feed. 0.004 × 4 × 3,000 = 48.0 in/min, which is 48 × 25.4 = 1,219.2 mm/min.
- Radial engagement ratio. 0.050 ÷ 0.500 = 0.100.
- Chip thickness ratio. 2√(0.100 − 0.100²) = 2√(0.100 − 0.010) = 2√0.090 = 2 × 0.30 = 0.600.
- Thinning factor. 1 ÷ 0.600 = 1.667.
- Corrected feed. 48.0 × 1.667 = 80.0 in/min, or 2,032 mm/min.
At 80 in/min the edge is finally taking the 0.004 in chip the catalogue assumed. Check what that does to the removal rate: at 0.050 in stepover and, say, 0.500 in of axial depth, the material removal rate is 0.050 × 0.500 × 80 = 2.00 in³/min, against 1.20 in³/min at the uncorrected feed. Same tool, same wear per edge, 67% more metal.
Sanity-checking the feed before you run it
Start with feed per revolution. On a solid end mill it should normally sit well under 10% of the cutter diameter; a 0.500 in tool advancing more than about 0.050 in per revolution is taking a very heavy bite no matter how the flutes divide it. That check catches flute-count errors instantly, because doubling the flute count doubles feed per revolution while leaving chip load alone.
Next check the machine. A feed is only real if the control can execute it. On a toolpath full of short segments and small arcs, block processing time and acceleration limits can leave the machine running well below the commanded feed, which quietly reduces the actual chip load and reintroduces rubbing at exactly the corners where the tool is most engaged. Look-ahead settings, high-speed machining modes and segment length matter more than the F word on those paths.
Finally check the direction of travel around corners. On an inside corner the effective radial engagement rises sharply — a cutter of radius r following a corner of radius R sees a momentary engagement much greater than the programmed stepover — so a feed corrected for a 10% stepover is badly wrong for those few milliseconds. Modern CAM handles this with automatic feed reduction in corners; if yours does not, arc the corners rather than sharpening them.
Table feed for common chip loads and flute counts at 3,000 rpm
| Chip load (in/tooth) | 1 flute | 2 flutes | 3 flutes | 4 flutes | 6 flutes |
|---|---|---|---|---|---|
| 0.0005 | 1.5 | 3.0 | 4.5 | 6.0 | 9.0 |
| 0.001 | 3.0 | 6.0 | 9.0 | 12.0 | 18.0 |
| 0.002 | 6.0 | 12.0 | 18.0 | 24.0 | 36.0 |
| 0.003 | 9.0 | 18.0 | 27.0 | 36.0 | 54.0 |
| 0.004 | 12.0 | 24.0 | 36.0 | 48.0 | 72.0 |
| 0.005 | 15.0 | 30.0 | 45.0 | 60.0 | 90.0 |
| 0.006 | 18.0 | 36.0 | 54.0 | 72.0 | 108.0 |
| 0.008 | 24.0 | 48.0 | 72.0 | 96.0 | 144.0 |
These are uncorrected feeds. Multiply by the chip thinning factor if your radial engagement is below half the cutter diameter.
Ways a feed rate calculation goes wrong
- Applying the thinning correction while slotting. At full width the factor is exactly 1. Multiplying a slotting feed by 1.67 because the toolpath elsewhere in the program is light is a reliable way to break a cutter.
- Using nominal flute count on a cutter with unequal spacing. Variable-pitch and variable-helix tools still have the stated number of edges, but a wiper insert or a non-cutting pocket does not remove metal — count only what cuts.
- Forgetting that the correction is radial only. A ball nose or a round insert taking a shallow axial cut is thinned in the axial direction too, by a different geometry this calculator does not cover.
- Programming a feed the machine cannot execute. Small arcs, short line segments and low acceleration limits mean the achieved feed is often well below the commanded one, which lowers the actual chip load.
- Ignoring inside corners. Engagement spikes at corners, so a feed tuned for the straight sections is too aggressive there. Corner feed reduction, or an arc-in toolpath, solves it.
- Changing spindle speed without changing feed. Chip load is feed ÷ (RPM × flutes), so an RPM change alone moves the chip load in the opposite direction — check with the chip load calculator.
How feed relates to the other cutting parameters
Feed rate is the last number you calculate and the first one that gets edited at the machine, which is why it is worth understanding what an override actually does. A 120% feed override raises chip load by 20% and leaves surface speed untouched, so it trades edge strength for cycle time. A spindle override does the reverse. Neither is free, and pushing both at once compounds them.
Metric shops calculate the identical quantity in mm/min, and the arithmetic is slightly friendlier because the chip load is already in millimetres: 0.1 mm/tooth on three flutes at 5,000 rpm gives exactly 1,500 mm/min with no conversion. The chip thinning correction is unit-free, so it applies unchanged.
Turning and drilling use feed per revolution rather than feed per tooth, because a turning tool has one edge and a twist drill has two symmetric lips. That is why lathe feeds are quoted in in/rev or mm/rev and why the drilling speed and feed calculator asks for feed per revolution directly. The link back to milling is feed per revolution = chip load × flutes, which is one of the outputs above. Machinery's Handbook is the standard reference for these conventions and for the feed-per-tooth tables that supply the input.