Speed and Feed Calculator for Tapping
Tapping is the one CNC operation where feed rate is not a free parameter. The feed must equal RPM times thread lead so the tap advances exactly one thread per revolution, or the tap breaks, snaps, or strips the thread. This calculator returns the matched RPM, SFM, and IPM feed rate for common UNC, UNF, and metric tap sizes in every shop metal, using separate SFM tables for HSS cutting taps, solid carbide taps, and form (roll) taps.
The tapping feed equation
A tap threads the workpiece by cutting one thread pitch per revolution. So feed rate is locked to RPM through the thread lead:
Feed rate (IPM) = RPM x (1 / TPI) for imperial, or Feed rate (mm/min) = RPM x pitch for metric. TPI is threads per inch; pitch is the axial distance between threads in millimeters.
For a 1/4-20 tap at 600 RPM: feed = 600 x (1/20) = 30 IPM. For an M6 x 1.0 tap at 500 RPM: feed = 500 x 1.0 = 500 mm/min.
Tapping SFM by material and tap type
| Material | HSS cutting tap | Carbide cutting tap | Form (roll) tap |
|---|---|---|---|
| Aluminum 6061 | 80 SFM | 250 SFM | 150 SFM |
| Mild steel 1018 | 35 SFM | 90 SFM | 65 SFM |
| Alloy steel 4140 | 20 SFM | 60 SFM | 40 SFM |
| Stainless 304 | 15 SFM | 50 SFM | 30 SFM |
| Cast iron | 35 SFM | 80 SFM | N/A |
| Brass | 70 SFM | 150 SFM | 100 SFM |
| Titanium | 10 SFM | 30 SFM | 20 SFM |
Form taps cannot be used in cast iron or brittle materials because the metal must plastically deform without cracking. Aluminum, mild steel, stainless, and copper all form-tap cleanly.
RPM from SFM for taps
The same cutting speed equation applies: RPM = (SFM x 12) / (pi x D) with D in inches. For a 3/8 inch HSS cutting tap in mild steel at 35 SFM: RPM = (35 x 12) / (pi x 0.375) = 356 RPM. Feed at 1/16 thread lead (16 TPI) = 356 x 0.0625 = 22.3 IPM. A rigid-tapping spindle cuts this cleanly; a floating tap holder needs a bit less rigidity tolerance in the feed-to-RPM match.
Rigid tapping vs tension-compression
Modern CNC mills with encoder-synchronized spindles (Haas, Mazak, Okuma, Tormach PCNC with Path Pilot) tap rigidly: the feed follows RPM exactly through a G84 cycle. Older machines use a tension-compression tap holder that allows a small mismatch between programmed feed and actual RPM. Either way, the calculator output is the programmed value. Reduce RPM 20-30 percent for blind holes under 1/4 inch diameter where chip evacuation is marginal.