For a rotating multi-edge cutter, programmed table feed is the distance each effective cutting edge should advance, multiplied by the number of effective edges and the number of spindle revolutions per minute.
Feed rate = RPM × number of effective flutes × chip load per tooth
Metric inputs produce mm/min; inch chip load produces inches per minute (IPM).
CNC feed rate formula
The same relationship can be rearranged when a different value is unknown:
- Chip load:
fz = vf ÷ (RPM × flutes) - RPM:
n = vf ÷ (fz × flutes) - Feed per revolution:
fn = fz × flutes = vf ÷ RPM
Worked example
A four-flute end mill is programmed at 6,000 RPM with a target chip load of 0.05 mm per tooth.
- Feed per revolution:
0.05 × 4 = 0.20 mm/rev. - Table feed:
0.20 × 6,000 = 1,200 mm/min.
| Variable | Value | Meaning |
|---|---|---|
| n | 6,000 RPM | Spindle speed |
| zc | 4 | Effective cutting edges |
| fz | 0.05 mm/tooth | Programmed advance per edge |
| vf | 1,200 mm/min | Calculated table feed |
Chip load is not the same as table feed
Chip load is the programmed advance per effective cutting edge. Table feed is the machine-axis speed needed to deliver that advance at the current RPM. If RPM changes while chip load and flute count stay constant, table feed must change in direct proportion.
A manufacturer’s chip-load recommendation is normally a starting range tied to a tool family, diameter, cutting-edge geometry, work material, and engagement condition. Do not copy a value from a different diameter or tool construction without checking the manufacturer’s guidance.
Count effective cutting edges
Use the number of edges that actually participate in the operation. A four-flute end mill generally has four effective edges in side milling. Some indexable cutters have unequal pitch, wiper inserts, or insert arrangements where the effective count requires the toolmaker’s definition. Drilling is normally expressed as feed per revolution rather than milling chip load, even though the drill has multiple lips.
When the simple feed formula needs adjustment
Radial chip thinning
At light radial engagement, the actual maximum chip thickness can be smaller than the programmed feed per tooth. Constant-engagement toolpaths may use a compensated feed. Do not carry that compensation into full-width slots or tight corners. Use the Radial Chip Thinning Calculator for the geometric correction.
Entry, corners, and machine acceleration
The formula assumes the commanded feed is achieved and engagement is stable. Short moves, small arcs, plunges, corners, and frequent direction changes can be limited by acceleration or by a CAM feed reduction.
Runout and rigidity
Runout can make one flute carry more than its share of the chip. Tool overhang, holder condition, spindle condition, workholding, and machine rigidity can all require a more conservative starting value.
Practical workflow
- Select cutting speed and chip load from current tooling data.
- Calculate RPM from cutting speed and effective diameter.
- Calculate table feed from RPM, effective edges, and chip load.
- Apply engagement-specific corrections only where they are valid.
- Check spindle, feed-axis, holder, tool, and workholding limits.
- Prove the cut conservatively and inspect chips, sound, load, size, and finish.
For the full chain, start with the RPM & Surface Speed Calculator and compare the result with the Milling Speeds & Feeds Calculator.
Technical references
Published and formula-checked by MfgWorkbench. Last reviewed September 4, 2026. See our editorial method.