Speeds and feeds
CNC milling calculators
RPM = (SFM x 12) / (pi x D), then IPM = RPM x IPT x Z, then MRR = WOC x DOC x IPM; the form below chains all three.
Technical review pending. Formulas and values are cited. This notice comes down after a machinist review.
Inch
RPM = (SFM x 12) / (pi x D); IPM = RPM x IPT x Z; MRR = WOC x DOC x IPM
| Symbol | Meaning | Unit |
|---|---|---|
| SFM | Cutting speed, surface feet per minute | ft/min |
| D | Cutter diameter | in |
| IPT | Feed per tooth (chip load) | in/tooth |
| Z | Number of flutes | count |
| IPM | Feed rate, inches per minute | in/min |
| WOC, DOC | Width (radial) and depth (axial) of cut | in |
| MRR | Metal removal rate | in³/min |
Metric
RPM = (Vc x 1000) / (pi x D); vf = RPM x fz x Z; Q = (ae x ap x vf) / 1000
| Symbol | Meaning | Unit |
|---|---|---|
| Vc | Cutting speed | m/min |
| D | Cutter diameter | mm |
| fz | Feed per tooth | mm/tooth |
| vf | Feed rate | mm/min |
| ae, ap | Width (radial) and depth (axial) of cut | mm |
| Q | Metal removal rate | cm³/min |
Source: Machinery's Handbook (speeds and feeds; metal removal rate); cutting tool makers' published data for SFM and chip load.
One cut: RPM, feed and removal rate
Spindle speed
RPM
RPM = (SFM x 12) / (pi x D) = (100 x 12) / (3.1416 x 0.5) = 764 RPM
Starting point. Feed 6.1 IPM; removal rate 0.76 in³/min.
| Value | Result | Formula with your numbers |
|---|---|---|
| Spindle speed | 764 RPM | RPM = (SFM x 12) / (pi x D) = (100 x 12) / (3.1416 x 0.5) = 764 RPM |
| Feed rate | 6.1 IPM (155 mm/min) | IPM = RPM x IPT x Z = 764 x 0.002 x 4 = 6.1 IPM |
| Metal removal rate | 0.76 in³/min (12.52 cm³/min) | MRR = WOC x DOC x IPM = 0.25 x 0.5 x 6.112 = 0.76 in³/min |
Milling tools
- The formulas behind this form, with a worked cut and the common mistakes, are on the machining formulas page.
- RPM from SFM or m/min, and back again, comes from the spindle speed calculator.
- IPT, IPR, IPM and the metric feeds convert in one form on the feed rate conversion calculator.
- Removal rate with horsepower at the cutter and at the motor is on the metal removal rate calculator.
- Scallop height from stepover for a ball end mill, h = R - sqrt(R^2 - (s / 2)^2), comes from the surface finish calculator.
- The G83 peck depth (Q value) for a drilled hole comes from the peck drilling calculator.
- Rigid tapping feed from the thread pitch is on the tapping calculator.
- Hole coordinates for the DRO or the program come from the bolt circle calculator.
- Cutting soft jaws to hold a part in the vise is covered in the vise soft jaws guide.
- Mill G-codes and M-codes are in the mill column of the G and M codes list.
- Codes for the Fadal VMC have their own Fadal G-code list.
- Drilling speeds and feeds. Coming
How to choose a starting point
- Material first. The cutting speed and chip load come from the tool maker or the Handbook for the material you are cutting.
- Carbide runs several times the HSS speed in the same material.
- Tool-maker charts assume a rigid machine. On a light mill, start at the low end of the range.
- Dry cuts and deep pockets call for lower numbers.
- Treat the result as a start, then adjust by sound, chip color and finish.
Worked example: inch
A 1/2 in 4-flute HSS end mill, 100 SFM, 0.002 in per tooth, WOC 0.250 in, DOC 0.500 in.
- RPM = (100 x 12) / (3.1416 x 0.500) = 763.9, so 764 RPM.
- IPM = 764 x 0.002 x 4 = 6.112, so 6.1 IPM.
- MRR = 0.250 x 0.500 x 6.112 = 0.764, so 0.76 in³/min.
Result: 764 RPM, 6.1 IPM, 0.76 in³/min. These match the cut on the machining formulas page.
Worked example: metric
A 12 mm 3-flute end mill, Vc 120 m/min, fz 0.05 mm, ae 3 mm, ap 12 mm. Vc and fz are example inputs, not recommendations.
- RPM = (120 x 1000) / (3.1416 x 12) = 3,183 RPM.
- vf = 3,183 x 0.05 x 3 = 477.45 mm/min.
- Q = (3 x 12 x 477.45) / 1000 = 17.19 cm³/min.
Result: 3,183 RPM, 477.45 mm/min, 17.19 cm³/min.
FAQ
How do you calculate milling feed rate?
IPM = RPM x IPT x Z. At 764 RPM, 0.002 in per tooth and 4 flutes, the feed is 6.1 IPM.
What SFM do you start with?
It depends on the tool material and the machine. Take SFM from the tool maker's data or the Machinery's Handbook, and start low on a light mill.
Is SFM different for HSS and carbide?
Yes. Rule of thumb from tool-maker data: carbide runs about 2 to 4 times the HSS surface speed in the same material.
The mill tops out below the RPM the tool maker wants. Now what?
Run top speed and hold the chip load. The cutter runs below its ideal surface speed, and the IPM drops in proportion to the lower RPM.
Should you use an AI chatbot for speeds and feeds?
Use it to learn the formulas, not to trust a number. Check any number it gives against a chart and the formula.
Last updated