These are baseline single-point turning speeds for HSS and uncoated carbide. Milling, drilling, coated tooling, high-feed strategies and flood coolant all shift them — see the adjustments below the table. To turn a cutting speed into spindle RPM for your tool or work diameter, use the SFM calculator.
| Material | Family | HSS (SFM) | HSS (m/min) | Carbide (SFM) | Carbide (m/min) | Notes |
|---|---|---|---|---|---|---|
| Aluminum | Light alloys | 300 | 91 | 800 | 244 | Free-machining; high speeds, watch built-up edge. |
| Brass | Copper alloys | 200 | 61 | 600 | 183 | Free-cutting brass; very machinable. |
| Bronze | Copper alloys | 120 | 37 | 350 | 107 | Harder than brass. |
| Cast iron (gray) | Cast iron | 60 | 18 | 200 | 61 | Abrasive; carbide preferred. |
| Mild steel (1018) | Carbon & alloy steel | 90 | 27 | 350 | 107 | General low-carbon steel. |
| Alloy steel (4140) | Carbon & alloy steel | 60 | 18 | 250 | 76 | Heat-treatable; lower when hardened. |
| Stainless (304) | Stainless steel | 50 | 15 | 200 | 61 | Work-hardens; keep feed up, avoid dwelling. |
| Tool steel | Carbon & alloy steel | 45 | 14 | 175 | 53 | Hard; reduce speed as hardness rises. |
| Titanium | High-temp & exotic | 35 | 11 | 150 | 46 | Low speed; heat builds fast. |
| Plastic | Non-metals | 400 | 122 | 800 | 244 | Sharp tools; clear chips. |
| Aluminum (cast A356) | Light alloys | 250 | 76 | 700 | 213 | Silicon content is abrasive; use flood coolant. |
| Magnesium | Light alloys | 400 | 122 | 900 | 274 | Excellent machinability; fine chips are a fire risk, never use water-based coolant. |
| Copper | Copper alloys | 150 | 46 | 400 | 122 | Gummy; sharp tools and positive rake reduce built-up edge. |
| Free-machining steel (12L14) | Carbon & alloy steel | 130 | 40 | 450 | 137 | Leaded/resulfurized; best machinability of the steels. |
| Medium-carbon steel (1045) | Carbon & alloy steel | 70 | 21 | 300 | 91 | Tougher than 1018; common shaft steel. |
| Alloy steel (4340) | Carbon & alloy steel | 50 | 15 | 220 | 67 | High-strength; reduce speed in the heat-treated condition. |
| Hardened steel (45-55 HRC) | Carbon & alloy steel | 20 | 6 | 100 | 30 | Hard turning; carbide or CBN only, light finishing cuts (HSS not suitable). |
| Stainless (303) | Stainless steel | 70 | 21 | 250 | 76 | Free-machining austenitic; the easiest stainless. |
| Stainless (316) | Stainless steel | 45 | 14 | 180 | 55 | Gummier than 304 and work-hardens; keep cuts positive. |
| Stainless (416) | Stainless steel | 90 | 27 | 280 | 85 | Free-machining martensitic stainless. |
| Stainless (17-4 PH) | Stainless steel | 40 | 12 | 150 | 46 | Precipitation-hardening; speed depends on condition (H900 lower). |
| Stainless (410) | Stainless steel | 60 | 18 | 220 | 67 | Martensitic; machine in the annealed condition where possible. |
| Ductile iron (65-45-12) | Cast iron | 50 | 15 | 180 | 55 | Nodular iron; tougher and less abrasive than gray. |
| Malleable iron | Cast iron | 80 | 24 | 250 | 76 | Machines more like steel than gray iron. |
| Inconel / nickel superalloy | High-temp & exotic | 15 | 5 | 60 | 18 | Very tough and work-hardens; low speed, positive rake, rigid setup. |
| Monel (Ni-Cu) | High-temp & exotic | 40 | 12 | 120 | 37 | Work-hardens; keep the feed up and never dwell. |
| Hastelloy | High-temp & exotic | 15 | 5 | 60 | 18 | Nickel superalloy; treat like Inconel. |
| Fiberglass / GFRP | Non-metals | 150 | 46 | 500 | 152 | Abrasive; carbide or diamond tooling and dust extraction. |
Source: Standard machining references (Machinery's Handbook turning-speed tables; common tooling-maker starting-speed data). Verify against your tooling maker's data.
How to use these speeds
Every value is a conservative starting point from standard references. Carbide runs 2–4× the HSS speed because it keeps its hardness at the higher temperatures fast cutting generates. Real cutting speed also depends on depth of cut, feed, tool coating, coolant, setup rigidity and the exact grade — so begin near these numbers and tune from there, and trust your tooling maker's data over any general chart.
Adjusting for operation and tooling (rules of thumb):
- Milling ≈ the same to 0.8× the turning speed; drilling ≈ 0.6× (HSS).
- Coated carbide (TiN, TiAlN) often runs 1.5–2× uncoated; coolant lets you push the top of the range.
- Drop toward the low end for interrupted cuts, hardened material, long overhangs or marginal rigidity.
Worked example — SFM to spindle RPM
Turning 1018 mild steel with a carbide insert at 350 SFM on a 1 in (25.4 mm) diameter: RPM = (SFM × 12) ÷ (π × D) = (350 × 12) ÷ (π × 1) ≈ 1,337 rpm. The same 350 SFM on a 2 in bar halves to ≈ 668 rpm — cutting speed is set by the material, so spindle RPM falls as the diameter grows. Give the SFM calculator your own diameter for the exact number, or use the CNC speeds & feeds calculator to carry it through to feed rate and material removal rate from this same table. For chip-load starting points by tool diameter, see the chip load chart.
Reuse this chart
This table is published as free, open data under CC BY 4.0 — you are welcome to reproduce it in articles, courses or shop documentation. The only ask is a link back to this page as the source so readers can find the latest version.