CNC Machining Feeds and Speeds Calculator

A feeds and speeds calculator connects a documented cutting speed and feed per tooth to the spindle speed and linear table feed used for a milling operation. Cutting speed describes the relative surface speed at the cutter circumference. Feed per tooth describes the nominal linear advance assigned to each effective cutting tooth. Cutter diameter converts surface speed into revolutions per minute, while RPM and effective teeth convert feed per tooth into table feed.

This calculator deliberately asks you to name the supplier-data basis. A carbide end mill, indexable cutter and high-speed-steel tool can require very different data in the same work material. Tool geometry, grade, coating, radial and axial engagement, coolant and operation also matter. The equations can translate selected data, but they cannot select suitable cutting data from tool diameter or material name alone.

The result separates theoretical values from values adjusted by the machine limits you enter. That distinction matters when a small cutter would require more RPM than the spindle can provide, or when the calculated table feed exceeds a control or axis limit. The tool recalculates the actual cutting speed and feed per tooth after those caps so the final condition remains visible.

All inputs are converted to a consistent metric basis. Spindle speed is cutting speed multiplied by 1,000 and divided by pi times effective cutter diameter. Table feed is feed per tooth multiplied by spindle RPM and effective cutting teeth. These are the milling relationships published in Sandvik Coromant’s metric reference; the inch presentation is checked against the corresponding inch reference and the exact inch conversion.

Limits are applied in a defined sequence. RPM is capped first because changing RPM changes the feed required to preserve feed per tooth. Feed is recalculated at that adjusted RPM, then capped by the entered table-feed maximum. If the feed cap applies, actual feed per tooth falls below the target. The calculator reports that change rather than concealing it.

Metric milling calculation: For a 10 mm effective diameter, 100 m/min cutting speed, 0.050 mm per tooth and four effective teeth, theoretical speed is about 3,183 RPM. Multiplying 0.050 by 3,183 and four gives about 636.6 mm/min. If entered machine limits exceed both results, no adjustment is made.

RPM and feed limits: With the same inputs, an entered 3,000 RPM limit reduces feed to 600 mm/min to preserve 0.050 mm per tooth. If the entered feed limit is 500 mm/min, final chip load becomes about 0.04167 mm per tooth. The actual cutting speed is then about 94.25 m/min.

US customary entry: A diameter, SFM, IPT and IPM entered in US units are converted internally before the same equations run. Switching units changes the display, not the physical cutting condition. Small display differences can occur from rounding, so retain the precision needed by the shop’s documentation.

Use effective cutting diameter, especially when the contact diameter differs from a nominal tool diameter. Confirm whether the supplier line applies to slotting, side milling, roughing or finishing and whether it assumes a particular engagement. Enter the effective tooth count stated for the cutter rather than automatically counting every visible flute or insert.

Treat the entered maximums as comparison limits, not evidence of capacity at the calculated condition. Check the actual machine manual and setup for torque, power, holder balance, tool projection and axis behavior. Review runout, workholding, entry moves, corners, chip evacuation and coolant before programming, then use the shop’s normal prove-out process.