Speeds and Feeds Calculator
Every speeds and feeds answer comes from three numbers — surface speed, chip load, and the size of the cut — run through a short chain of formulas. This page lays out the formulas, a worked example, and the recommended starting tables for common materials. When you want the math done for you, these same tables drive the Mill and Lathe wizards in the ChipLoad app — and the Calculator tab runs free in your browser.
The formulas
Spindle speed from surface feet per minute and tool (or work) diameter in inches. The constant 3.8197 is 12 ÷ π — it converts the circumference of the cutter into revolutions. Metric shops use RPM = (m/min × 318.3) ÷ D in mm, the same math.
Milling feed rate. Chip load is inches per tooth (IPT) — how thick a chip each flute takes. Multiply by the number of flutes and the spindle speed and you get inches per minute at the table.
Material removal rate in in³/min. Power follows from it: HP ≈ MRR × the material's unit power (about 0.9–1.0 for mild steel, 0.25 for aluminum, 1.3+ for stainless and titanium). If the HP answer is bigger than your spindle, the RPM and feed on paper won't happen in the cut.
On the lathe and the drill press, feed is set per revolution instead of per tooth. A tap is the strict case: feed per rev must equal the thread pitch exactly — RPM × pitch is the only correct feed for rigid tapping.
Worked example — ½″ carbide end mill in 1018 steel
From the tables below: 1018 steel runs 500 SFM with carbide, and a ½″ end mill carries a 0.0050″ chip load. Four flutes, profiling at 0.50″ deep × 0.25″ wide:
FEED = 0.0050 × 4 × 3,820 = 76.4 IPM
MRR = 76.4 × 0.25 × 0.50 = 9.55 in³/min
POWER = 9.55 × 0.90 = ≈ 8.6 HP
That is exactly the readout ChipLoad's Mill wizard gives for this setup — the app just does the chain instantly, caps the RPM at your machine's limit, and warns you when the cut asks for more horsepower than the spindle has.
Recommended surface speeds & chip loads
These are the starting values the ChipLoad calculator itself uses — mid-range published shop numbers, not catalog maximums. Chip load is shown for a ½″ end mill; the app scales it by cutter diameter and material.
| Material | Mill SFM — carbide | Mill SFM — HSS | Lathe SFM — carbide | Drill SFM — HSS | Chip load, ½″ EM (in/tooth) |
|---|---|---|---|---|---|
| Aluminum 6061 | 900 | 280 | 1000 | 250 | 0.0090 |
| Aluminum 7075 | 800 | 250 | 900 | 220 | 0.0085 |
| Brass | 700 | 250 | 800 | 200 | 0.0070 |
| Bronze | 500 | 180 | 550 | 150 | 0.0060 |
| Copper | 500 | 200 | 550 | 150 | 0.0060 |
| Steel 1018 | 500 | 110 | 550 | 100 | 0.0050 |
| Steel 1045 | 450 | 95 | 480 | 90 | 0.0050 |
| Steel 4140 | 400 | 85 | 450 | 80 | 0.0048 |
| A2 Tool Steel | 300 | 60 | 330 | 55 | 0.0043 |
| Stainless 304 | 250 | 50 | 300 | 45 | 0.0035 |
| Stainless 316 | 220 | 45 | 260 | 40 | 0.0033 |
| Stainless 17-4 | 300 | 60 | 340 | 50 | 0.0040 |
| Cast Iron | 400 | 100 | 450 | 90 | 0.0045 |
| Titanium 6Al-4V | 160 | 40 | 180 | 35 | 0.0030 |
| Inconel 718 | 100 | 25 | 120 | 20 | 0.0025 |
| Delrin / Plastic | 600 | 300 | 700 | 250 | 0.0075 |
Chip load scales with cutter size. The base values the app uses for steel, before the material factor: ⅛″ → 0.0015, ¼″ → 0.0030, ⅜″ → 0.0040, ½″ → 0.0050, ¾″ → 0.0070, 1″ → 0.0090 in/tooth. Softer materials take a bigger bite (aluminum ×1.8), tougher ones a smaller one (Inconel ×0.5).
How to run a speeds and feeds calculation
- Identify the material — the actual alloy, not just "steel." 1018 and 4140 differ by 100 SFM in the table; 304 stainless runs at half the speed of mild steel.
- Pick the SFM for your tool material — carbide and HSS live in different worlds (roughly 3–5× apart in steel). Coated carbide generally takes a bump up from uncoated.
- Compute the RPM — SFM × 3.8197 ÷ diameter. Then check it against your machine's top speed before you fall in love with the number.
- Set the chip load for the cutter diameter, scaled for the material. This is the number that decides tool life — too light rubs, too heavy snaps.
- Compute the feed — chip load × flutes × RPM. On a light stepover (under half the cutter diameter), the real chip is thinner than the programmed one, so the feed can come up to match — that's chip thinning.
- Sanity-check power and rigidity — MRR × unit power against your spindle HP, then honestly grade your setup: vise or toe clamps, stickout, machine size. Back the cut intensity down before you back it down with a broken end mill.
Or skip the pencil work: ChipLoad's Mill and Lathe wizards run this whole chain — material, cutter, operation, coolant, rigidity and chip thinning included. They are in the ChipLoad app; on the web, only the Calculator tab is free.
Common mistakes
304 work-hardens the instant a cutter rubs instead of cutting. It needs roughly half the SFM of 1018 and a chip load heavy enough to stay under the hardened layer — slow and light is the worst combination there is.
Carbide at HSS speeds just wastes the tool's potential; HSS at carbide speeds burns up in seconds. The SFM column has to match the tool in the spindle.
At a 10% stepover, the actual chip is a fraction of the programmed feed per tooth. If you don't raise the feed to compensate, the cutter rubs, heats up, and dulls — while the control says everything is "correct."
A formula doesn't know your spindle tops out at 3,000 RPM, your end mill is hanging 3 inches out of the collet, or the part is held by hope and one strap clamp. Rigidity and stickout move the safe answer more than a second decimal place ever will.
Published SFM and chip load are starting points for a prove-out pass, not guarantees. Listen to the cut, look at the chips — blue straw-colored chips in steel mean heat is leaving with the chip, which is where you want it.
Put the calculator in your pocket
ChipLoad's Mill and Lathe wizards run these exact formulas and tables — plus coatings, coolant, interrupted cuts, rigidity and your own machine's limits — and they're part of a 17-tool machinist calculator that works fully offline. Free to download, one-time Pro unlock, no subscription.