Free Speeds and Feeds Calculator

Two formulas do most of the work:

RPM = (SFM × 12) ÷ (π × D)    (metric: RPM = Vc × 1000 ÷ (π × D))
Feed rate = chip load × number of flutes × RPM

You need three inputs: surface speed (SFM) for the material, chip load per tooth, and the tool diameter + flute count. Pick the material in this calculator and the SFM and chip load defaults fill in automatically. See the Show Math panel for the exact arithmetic on every result.

For 6061-T6 with a carbide end mill: SFM 800–1,200, chip load 0.001–0.003″ per tooth at 1/4″ (0.025–0.075 mm at 6 mm). 7075-T6 is slightly tougher: SFM 600–900 with the same chip-load range. Aluminum is forgiving — err on the faster side, because slow rubbing causes built-up edge on the cutter. The calculator scales chip load by tool diameter, so a 1/2″ end mill gets ~0.004–0.006″ automatically.

For 304 / 316 stainless with carbide: SFM 200–400, chip load 0.0015–0.003″ per tooth at 1/4″. Stainless work-hardens, so never rub — keep chip load up and use TiAlN or AlTiN coating. 17-4 PH in the H900 condition is harder still: drop to SFM 150–250. Coolant and proper chip evacuation matter more here than in mild steel.

Ti 6Al-4V is ISO group S (superalloy). Use SFM 100–200 with carbide, chip load 0.001–0.0025″ per tooth at 1/4″. Heat is the enemy — titanium has poor thermal conductivity so the heat goes into the tool. Use AlTiN coating, plenty of coolant, short stickout, and high-pressure flood if available. Conservative RPM with a healthy chip load beats high RPM every time.

Chip load (also called feed per tooth) = feed rate ÷ (RPM × number of flutes).

Example: 1/4″ 3-flute carbide end mill at 12,000 RPM, 60 IPM feed → 60 ÷ (12,000 × 3) = 0.00167″ per tooth.

A good rule of thumb for end mills is 1–3 % of tool diameter as a starting chip load. This calculator does it the other way: pick a target chip load from the material database, get the required feed rate. That keeps tool wear predictable.

When your radial depth of cut (stepover) is less than 50 % of tool diameter, the actual chip is thinner than the programmed feed per tooth — because the cutter rolls into the material at an angle instead of taking a full slot. To keep effective chip load on target, you have to multiply feed rate by the chip thinning factor, roughly √(D ÷ (2 × ae)) for light radial engagement.

It matters most for high-feed milling (HEM), trochoidal and adaptive toolpaths where radial engagement is 10–25 % of diameter. Without thinning compensation those toolpaths rub the tool to death.

A ball end mill cuts at its full diameter only when fully engaged. At light axial depth the effective cutting diameter is smaller:

D_eff = 2 × √(R² − (R − ap)²)    where R = tool radius, ap = axial depth of cut.

Example: 1/2″ ball mill at 0.020″ axial DOC has an effective diameter of only ~0.20″. Plug 0.20″ into the SFM formula instead of 0.5″ and the required RPM roughly doubles. The calculator does this automatically when you pick "ball nose" as the tool type.

For drilling, use the same SFM → RPM formula and a feed per revolution (IPR) instead of feed per tooth:

RPM = (SFM × 12) ÷ (π × D)
Feed rate = feed per revolution × RPM    (typically 1–3 % of drill diameter)

A carbide drill in 6061 aluminum at 1/4″: SFM 300–500, 0.004–0.008 IPR → roughly 6,000 RPM at 30 IPM. Pick "Drill" as the tool type in the calculator and the chip-load defaults shift to drilling values.

Results assume ideal rigidity, short stickout and good chip evacuation. If the calculator flags warnings or you see chatter:

1. Reduce the aggressiveness slider (start at 70–80 %).
2. Shorter stickout — every extra diameter of length cubes deflection.
3. Check workholding and machine rigidity (1–10 slider).
4. Verify spindle power against the power-check value.
5. Make sure the SFM you picked matches your tool coating.

Yes. G-Wizard (Bob Warfield, $79+ /year) and HSMAdvisor (Eldar Gerfanov, $129 perpetual) ship with bigger material/tool databases and more advanced features (tap calc, lathe inserts, real-time tweak). This calculator covers the core milling/drilling math — RPM, feed, chip load, chip thinning, ball-nose, power — for $0, in a browser, with the formulas visible. If you outgrow it, the paid options are worth the money. For most shops, this is enough.

Yes. Set rigidity to 3–5 for hobby/desktop routers (Shapeoko, Carbide 3D), 5–7 for prosumer (Onefinity, Avid CNC, X-Carve Pro), and use lower SFM than industrial machines. The calculator does not magically make a desktop router cut like a Haas — but it will tell you what your machine can do and warn you when chip load is too low (rubbing) or feed rate is too high.

Right now the calculator is focused on milling and drilling. Lathe / turning (feed per revolution, no flutes), tapping (feed = pitch × RPM) and threading are not yet first-class — tell us at hello@puida.com if you want them prioritised.

Both. Toggle between imperial (inches, SFM, IPM, HP) and metric (mm, m·min⁻¹, mm·min⁻¹, kW) anywhere in the UI. All values convert consistently — pick one system and stay in it. Material database covers both unit systems.

No. Everything runs in your browser. Machine profiles and tool library save to your browser's local storage only — never uploaded. No account, no telemetry, no subscription. Works offline after the first page load.