Calculate CNC feed rate from spindle RPM, flutes and chip load, or find RPM from cutting speed (SFM) and chip load from table feed, in inches or mm.
Feed Rate Formula
The calculator solves feed from RPM, feed from cutting speed, feed per tooth, or spindle RPM. Surface speed, removal rate and cutting time are optional outputs.
Feed from RPM:
Feed from cutting speed (SFM):
Feed per tooth (often called chip load):
- F = feed rate (in/min or mm/min)
- RPM = spindle speed (revolutions per minute)
- CL = chip load per tooth (in/tooth or mm/tooth)
- N = effective cutting teeth per revolution for the feed formula, not the number simultaneously in contact
- SFM = surface feet per minute (cutting speed)
- D = tool diameter (inches)
Inputs are normalized to millimeters before calculation. One inch is exactly 25.4 mm; one foot is 304.8 mm. The 12 in the SFM formula converts feet to inches. The tool maker’s effective tooth count must match the cutter. Feed per tooth is nominal advance per tooth and may differ from maximum chip thickness. Optional removal rate assumes a rectangular steady cut: MRR = feed × axial depth × radial width. Time = cutting path ÷ feed and excludes rapid moves, acceleration and tool changes.
The four solve modes cover these common unknowns. “Feed from RPM” is the direct multiplication when you already set spindle speed on the machine. “Feed from SFM” first solves RPM from the recommended cutting speed and tool diameter, then computes feed. “Chip load” reverses the feed equation when you want to verify the per-tooth engagement of a program already running.
Find material and tool cutting data
For sourced material SFM and chip-load charts, see Harvey Tool’s carbide end-mill tables by material grade and cutter diameter. The tables give surface-speed ranges and chip load in inches per tooth. For a Harvey cutter, use its product-specific speeds and feeds chart instead of a general material row. For another brand or HSS cutter, use that tool maker’s data.
Choose Feed and RPM from cutting speed (SFM) above, enter the cutting speed selected from the applicable chart, then enter the effective cutter diameter, flute count and chip load. Choose in/tooth for an IPT value; multiply by 25.4 only if entering it as mm/tooth. Chart values are starting references, not universal settings: match the cutter, material grade, engagement, coolant and machine limits. Do not interpolate chip load or apply carbide values to HSS without the tool maker’s guidance.
Reference Tables
The following legacy intervals illustrate approximate inch-to-millimeter conversion only; they are not validated cutting recommendations. Select actual feed per tooth from the specific tool maker’s data for the material, diameter, engagement and machine. Do not scale these intervals proportionally with diameter.
| Material | Chip load (in/tooth) | Chip load (mm/tooth) |
|---|---|---|
| Aluminum | 0.005 – 0.010 | 0.13 – 0.25 |
| Brass | 0.004 – 0.008 | 0.10 – 0.20 |
| Mild steel | 0.002 – 0.005 | 0.05 – 0.13 |
| Stainless steel | 0.001 – 0.004 | 0.03 – 0.10 |
| Titanium | 0.001 – 0.003 | 0.03 – 0.08 |
| Hardwood | 0.008 – 0.015 | 0.20 – 0.38 |
| Plastic | 0.005 – 0.012 | 0.13 – 0.30 |
The following legacy SFM intervals are illustrative arithmetic values, not validated recommendations for a specific grade, cutter or setup. Use the tool maker’s recommended cutting speed.
| Material | Carbide SFM | HSS SFM |
|---|---|---|
| Aluminum | 600 – 1200 | 250 – 400 |
| Brass | 300 – 700 | 150 – 300 |
| Mild steel | 300 – 500 | 80 – 120 |
| Stainless steel | 150 – 350 | 40 – 80 |
| Titanium | 100 – 250 | 30 – 60 |
| Cast iron | 250 – 450 | 60 – 100 |
Worked Examples and FAQ
Example 1: Feed from RPM. A 4-flute end mill at 3500 RPM with a 0.002 in/tooth chip load.
F = 3500 × 0.002 × 4 = 28 in/min.
Example 2: Feed from SFM. A 0.5 in carbide end mill in aluminum at 800 SFM, 3 flutes, 0.005 in/tooth.
RPM = (800 × 12) / (π × 0.5) ≈ 6,111.55 RPM. Using the unrounded RPM gives F ≈ 91.67325 in/min. These are arithmetic example inputs, not aluminum cutting recommendations.
Example 3: Chip load check. Program runs at 40 in/min, 5000 RPM, 2 flutes.
CL = 40 / (5000 × 2) = 0.004 in/tooth.
What if feed per tooth is too low? Rubbing and wear may occur. Check the specific cutter’s recommended data, runout, engagement and machine limits before changing feed or RPM.
What if it is too high? Excessive load can cause deflection, damaged edges or machine overload. Reconcile the tool maker’s cutting data and setup limits; adding flutes alone is not a general remedy.
Do I scale chip load with tool diameter? There is no universal proportional rule. Use the tool maker’s cutting data for the actual cutter diameter, material, engagement and machine.
Does flute count change feed? Yes, directly. Doubling flutes at the same RPM and chip load doubles the feed rate. That is why 3-flute and 4-flute end mills feed faster than 2-flute at the same per-tooth load.
Why is the SFM formula 12 / π and not something simpler? SFM is feet per minute at the cutting edge. Diameter is in inches. The 12 converts feet to inches and π converts a circumference to a diameter so you can solve for RPM.
