A neutral machinist workbench: RPM/SFM solver, feed-rate calculator, curated material speed database, chip-load advisor, tapping speeds & feeds, metal-removal-rate + spindle-power estimator, and printable reference charts. Imperial and metric, no sign-up.
This SFM calculator solves the speeds and feeds formula in both directions and both unit systems. RPM = SFM × 3.82 ÷ diameter (inches); metric: Vc = π × D × RPM ÷ 1000. For lathe work, enter the workpiece diameter — the solver doubles as a lathe RPM calculator for steel, aluminum, stainless, and other materials.
Enter values and press Calculate. Example: 600 SFM on a 1/2″ end mill in aluminum → 4,584 RPM.
Example: Vc = 183 m/min on a 12 mm end mill → ≈ 4,854 RPM. This is the sfm to rpm calculator metric shops use: enter SFM as Vc = SFM × 0.3048.
Tip speed is SFM itself — the surface speed of the tool's outer edge. “RPM to tip speed calculator” = the RPM → SFM direction above.
This milling feed rate calculator solves feed (IPM) = chip load per tooth (IPT) × flutes × RPM, and the reverse. Lathe & drilling mode: feed (IPM) = feed per rev (IPR) × RPM.
Example: 0.004″ IPT × 4 flutes × 4,584 RPM → 73.34 IPM.
Example: 0.008 IPR × 1,500 RPM → 12 IPM. Typical HSS drill feeds: 0.001–0.003 IPR under 1/8″, 0.004–0.010 IPR for 1/4″–1/2″, 0.007–0.015 IPR for 1/2″–1″.
Curated SFM starting ranges per workpiece material and tool material, compiled from published charts (sources keyed below the table). Use the HSS column for HSS end mill speeds and feeds, the carbide column for solid-carbide tools. Cobalt ≈ 25% above HSS (shop rule of thumb). Always start at the low end and verify — these are planning estimates, not manufacturer data.
| Material | HSS (SFM) | Carbide (SFM) | Cobalt ≈ (SFM) | Unit power hp per in³/min | Sources |
|---|
Sources: [A] OpenOregon Manufacturing Processes Table 1 (openoregon.pressbooks.pub) · [B] Bridgeport speeds & feeds chart (hotteam67.org) · [C] Amana Tool carbide end-mill material chart (toolstoday.com) · [D] Amana shop formulas: RPM = SFM × 3.82 / D, SFM = 0.262 × D × RPM · [H] MSU ME477 specific-energy table (egr.msu.edu)
This chip load calculator suggests feed per tooth by cutter diameter — the trap most charts mention but never compute: smaller tools tolerate much lower chip loads. The chip load formula runs both ways here: IPT = IPM ÷ (flutes × RPM), or get a starting IPT from the chart below. Carbide chart data from the Amana material chart [C]; HSS = 70% of carbide [J]. Output is a starting band (±25%), not a manufacturer guarantee.
Example: 1/2″ carbide end mill in steel → 0.0028 in/tooth (band 0.0021–0.0035).
This speed and feed calculator for tapping uses HSS tap SFM by thread coarseness band (3–7½ | 8–15 | 16–24 | 25+ TPI) from the Hertel tap chart [E]. Coarse taps run slower — the table handles it automatically. Feed must equal exactly one thread pitch per revolution: IPM = RPM ÷ TPI (imperial) or mm/min = RPM × pitch (metric).
Example: 1/4-20 UNC in mild steel → band 16–24 TPI = 70 SFM → ≈ 1,070 RPM at 53.5 IPM.
For rigid tapping, feed must equal exactly one thread pitch per revolution. With a floating/compression tap holder, reduce feed ~5–10%. Drill the tap-drill hole first — use the correct tap drill size for the thread (a dedicated tap drill chart covers every size).
Metal removal rate = width of cut × depth of cut × feed [G]. Power = MRR × unit power (hp per in³/min). Unit-power method is accurate to about ±15% [G].
Example: 0.5″ WOC × 0.25″ DOC × 73.344 IPM in aluminum → 9.17 in³/min, 2.75 HP at the cutter.
| Material | HSS | Carbide | Cobalt ≈ |
|---|
| Diameter | Steel | Stainless | Titanium | Aluminum | Brass | Cast iron |
|---|
| SFM | 1/8″ | 1/4″ | 3/8″ | 1/2″ | 3/4″ | 1″ |
|---|
| Material | 3–7½ TPI | 8–15 TPI | 16–24 TPI | 25+ TPI |
|---|
| Material | hp / (in³/min) |
|---|
Planning estimates — verify against Machinery's Handbook and your tool manufacturer's data. Always wear eye protection.
Every number in the calculators traces to a cited published source below. Where sources disagree, the tables use conservative ranges and say so. Nothing here replaces your tool manufacturer's data or Machinery's Handbook.
The two core formulas: spindle speed RPM = SFM × 3.82 ÷ tool diameter (inches), and feed rate IPM = chip load per tooth (IPT) × number of flutes × RPM. Metric: Vc (m/min) = π × D(mm) × RPM ÷ 1000, and mm/min = mm/tooth × flutes × RPM. The calculators above solve all four directions.
Drill RPM uses the same formula: RPM = SFM × 3.82 ÷ drill diameter. Use the HSS column of the material table (twist drills run about 50–70% of milling SFM). Drill feed is expressed per revolution: IPM = IPR × RPM, with typical HSS feeds of 0.001–0.003 IPR under 1/8″, 0.004–0.010 IPR for 1/4″–1/2″, and 0.007–0.015 IPR for 1/2″–1″. Start low and verify.
Convert SFM to cutting speed Vc in m/min first (Vc = SFM × 0.3048), then RPM = Vc × 1000 ÷ (π × D) with D in mm. Example: 600 SFM = 182.9 m/min; on a 12 mm end mill that is 182.9 × 1000 ÷ (π × 12) ≈ 4,852 RPM. The metric solver on the RPM/SFM tab does this both directions.
Chip load (IPT, inches per tooth) = feed rate (IPM) ÷ (flutes × RPM). It is the thickness of material each tooth removes per revolution. The Chip Load tab works the other way: pick a material and tool diameter and it suggests a starting IPT from published carbide end-mill charts, interpolating between charted diameters.
Typical carbide starting ranges: aluminum 450–650 SFM, low-carbon steel 300–500 SFM, 304/316 stainless 200–300 SFM; HSS runs much slower (aluminum 200–300, steel 80–110, stainless 60–80). See the Material DB tab for all ten materials with HSS, carbide, and cobalt ranges. Always start at the low end of the range and verify against your tool manufacturer's data.
Tap RPM = tap SFM × 3.82 ÷ tap diameter, where tap SFM depends on thread coarseness — coarse taps run slower (see the TPI-band chart). Feed must equal exactly one pitch per revolution: IPM = RPM ÷ TPI for imperial taps, or mm/min = RPM × pitch for metric. For rigid tapping keep the feed exact; with a floating holder reduce it ~5–10%.
MRR is the volume of material removed per minute: MRR (in³/min) = width of cut × depth of cut × feed rate (IPM). Metric: cm³/min = WOC × DOC × feed ÷ 1000. It is the key number for comparing how aggressive two cuts are — the MRR + Power tab computes it and converts it to spindle power.
Spindle power ≈ MRR × unit power, where unit power is hp per cubic inch per minute for the material (e.g. ~0.3 for aluminum, ~1.0 for mild steel and stainless, ~1.3 for titanium). Divide by ~0.8 for a suggested motor size. The method is accurate to about ±15%. Hobby machines often deliver far less than nameplate HP — treat the result as a planning estimate.
Use the same formulas but with the effective diameter at your depth of cut, not the shank diameter. A ball nose cutting shallow behaves like a much smaller tool — at 10% depth of cut a 1/2″ ball end mill has an effective diameter of about 0.3″, so it needs roughly 65% more RPM than the nominal diameter suggests. Feed per tooth stays the same.
Same SFM formula, applied to the workpiece diameter: RPM = SFM × 3.82 ÷ workpiece diameter (inches). For mild steel with carbide at ~350 SFM on a 2″ bar: 350 × 3.82 ÷ 2 ≈ 669 RPM. Lathe feed is per revolution: IPM = IPR × RPM, with roughing around 0.010–0.020 IPR and finishing 0.002–0.005 IPR.
SFM (surface feet per minute) is how fast the cutting edge moves through the material — it depends only on the material and tool type. RPM is how fast the spindle turns — it depends on SFM and tool diameter. Two different-size tools cutting the same material run at the same SFM but very different RPM: a 1/4″ tool needs twice the RPM of a 1/2″ tool at the same SFM.
Tip speed is SFM: SFM = 0.2618 × RPM × diameter (inches). Metric: Vc (m/min) = π × D(mm) × RPM ÷ 1000, or Vc = SFM × 0.3048. The RPM/SFM tab's reverse direction is exactly an RPM-to-tip-speed calculator.
Carbide runs 3–5× faster SFM and holds an edge far longer, so it wins for production and hard materials. HSS is cheaper, tougher (less likely to chip), and more forgiving on light or shaky machines — many hobbyists get better results with HSS because their machine can't use carbide's speed. Cobalt (HSCO) sits between, roughly 25% faster than HSS.
Chip load scales with tool strength, which drops fast as diameter shrinks — a 1/8″ end mill tolerates about 0.0006 in/tooth while a 1/2″ tool in the same material takes about 0.0028 in/tooth (roughly 5×). Feeding a small tool like a big one snaps it; feeding a big tool like a small one rubs and burns the edge. The Chip Load tab computes the diameter-adjusted value so you don't have to guess.
Use them as starting points, not gospel. They are planning estimates compiled from published charts — your tool manufacturer's data and Machinery's Handbook take precedence. Start at the low end of every range, listen to the cut, and adjust. Always wear eye protection, never wear gloves near rotating tools, and secure workholding before cutting.
FSWizard is a strong single-operation calculator with a PRO upsell. This suite is a neutral, vendor-independent alternative that covers seven operations in one place — RPM/SFM, feed rates, a curated material database, chip-load-by-diameter advice, tapping, MRR + power, and printable charts — with full metric support and no account or paywall. Use both: cross-check one tool's answer against the other.
Free tool by NRTechStudio
Explore similar math tools and calculators. 100% free, accurate, and runs completely in your browser without sign-up.
2 taps, no typing needed — diagnostics are sent automatically.