CNC Formulas

How to Calculate CNC Feeds, Speeds, and Cycle Time Step by Step

A worked walkthrough of the five formulas every machinist runs before cutting metal: spindle RPM, feed rate, chip load, MRR, and cycle time, with real inputs.

Every CNC job starts from one number: cutting speed, expressed as surface feet per minute (SFM) or meters per minute. It comes from the tool and material, not the machine. A carbide end mill in 6061 aluminum runs 800 to 1000 SFM; the same tool in 304 stainless drops to 150 to 300 SFM; in 4140 steel expect 250 to 400 SFM. Coated carbide in gray cast iron sits near 350 SFM. You pull this value from the tooling catalog or a Surface Speed reference, then convert it to spindle RPM for the specific cutter diameter. SFM is the anchor; get it wrong and the other four calculations inherit the error.

Spindle speed converts SFM into revolutions per minute using RPM = (SFM times 3.82) divided by tool diameter in inches. The 3.82 is 12 divided by pi, folding inches per foot into the circle. Take a 0.5 inch carbide end mill in 6061 at 900 SFM: RPM = (900 times 3.82) / 0.5 = 6,876 RPM. Metric version: RPM = (surface speed in m/min times 1000) / (pi times diameter in mm). A 12 mm cutter at 275 m/min gives (275,000) / (37.7) = 7,294 RPM. Round to what your control accepts and confirm it is under the spindle's rated ceiling. The CNC Spindle Speed calculator handles both unit systems.

Feed rate is the table or tool travel in inches per minute (IPM), and it is built from chip load, not guessed. The formula is IPM = RPM times number of flutes times chip load per tooth. Chip load, the feed per tooth (IPT), is the real design variable: 0.001 to 0.003 inch for a 1/8 inch tool, 0.004 to 0.006 inch for a 1/2 inch tool, higher in aluminum than in stainless. Using our 6,876 RPM, 4 flute, 0.004 inch example: IPM = 6,876 times 4 times 0.004 = 110 IPM. Drop to 2 flutes and feed halves to 55 IPM. Run the numbers on the CNC Feed Rate and Chip Load calculators before committing a program.

Chip load is worth isolating because it is where tool life and finish are won or lost. Rearrange the feed equation: IPT = IPM / (RPM times flutes). If a program feeds 60 IPM at 6,876 RPM with 4 flutes, actual chip load is 60 / (6,876 times 4) = 0.00218 inch per tooth. That is thin. Below roughly 0.001 inch the tool rubs instead of cuts, generating heat and work hardening, which murders coated carbide in stainless. Too thick past 0.006 inch on a small tool and you chip the edge. The Chip Load calculator lets you back-solve the target IPT and verify you are inside the tool maker's window.

Material Removal Rate (MRR) tells you how fast you are actually cutting metal, in cubic inches per minute, and it drives cycle time and horsepower load. For milling, MRR = width of cut times depth of cut times feed rate (IPM). A 0.375 inch wide, 0.100 inch deep pass at 110 IPM removes 0.375 times 0.100 times 110 = 4.13 cubic inches per minute. Aluminum needs about 0.3 HP per cubic inch per minute, so that pass draws roughly 1.2 HP at the cutter; steel needs 1.0 to 1.4 HP per cubic inch per minute, so the same MRR would demand 4 to 6 HP. The Material Removal Rate calculator flags when a pass will stall an undersized spindle.

Cycle time is the number that reaches the quote and the schedule. Break it into cutting time plus non-cutting time. Cutting time for a single pass is length of cut divided by feed rate: a 10 inch pass at 110 IPM takes 10 / 110 = 0.091 minute, or 5.5 seconds. Multiply by the number of passes, which is total depth divided by depth of cut. Cutting 0.400 inch total at 0.100 inch per pass is 4 passes, so 4 times 5.5 = 22 seconds of cutting. Then add rapids, tool changes at 3 to 6 seconds each, and approach or retract moves. The Milling Cycle Time calculator sums these so you are not eyeballing them.

Turning follows the same logic with different geometry. Spindle RPM uses the workpiece diameter, not the tool: RPM = (SFM times 3.82) / diameter. Because diameter shrinks as you face or profile, constant surface speed (G96) mode holds SFM by raising RPM as diameter falls, capped by a G50 limit. Feed in turning is inches per revolution (IPR), typically 0.005 to 0.015 IPR for roughing and 0.002 to 0.006 IPR for finishing. Cutting time per pass is length divided by (RPM times IPR). Turning 4 inches of a 2 inch bar at 400 SFM and 0.010 IPR gives 764 RPM, so 4 / (764 times 0.010) = 0.52 minute. The Turning Cycle Time calculator applies the CSS ramp automatically.

Chain the formulas in order and every downstream number stays consistent. Pick SFM from the material and coating, convert to RPM for the exact diameter, multiply by flutes and target chip load for IPM, verify chip load is inside 0.001 to 0.006 inch, compute MRR to check spindle horsepower, then roll length, passes, and tool changes into cycle time. A worked example end to end: 0.5 inch 4 flute carbide, 6061, 900 SFM gives 6,876 RPM and 110 IPM at 0.004 IPT, 4.13 cubic inches per minute MRR at about 1.2 HP, and 22 seconds of cutting per part. Change any one input and rerun the chain; the CNC Feed Rate and Material Removal Rate calculators keep the arithmetic honest.

Published 2026-07-01.