Machining cutting speeds (SFM) by material, spindle RPM by diameter, and milling chip load — plus the formulas to dial in any turning or milling job.
Feeds and speeds come down to two numbers: how fast the cutting edge moves across the material (surface speed, SFM) and how fast you advance the tool (feed). The rule mirrors drilling: soft materials and small diameters run fast; hard materials and large diameters run slow. The charts below give machining SFM by material, the RPM those speeds work out to by diameter, and milling chip loads — all for high-speed-steel (HSS) tooling. This is the machining companion to our Drill Speed Chart (drilling) and CNC Feeds & Speeds Chart (router bits).
Spindle speed is RPM = (SFM × 3.82) ÷ diameter (in.). With HSS tooling, aluminum runs ~300 SFM (about 1150 RPM on a 1" diameter), mild steel ~100 SFM (380 RPM), stainless ~50 SFM (190 RPM), and cast iron ~65 SFM (250 RPM). Carbide runs 2–3× faster. Milling feed is RPM × chip load per tooth × number of flutes. Full charts below.
Surface speed is the master number — every RPM below is derived from it. These are recommended surface feet per minute for turning and milling. Use the HSS column for high-speed-steel tools; carbide tooling runs 2 to 3 times faster on a rigid machine.
| Material | HSS Tooling (SFM) | Carbide Tooling (SFM) |
|---|---|---|
| Aluminum | 200–400 | 600–1000 |
| Brass / Bronze | 150–300 | 300–700 |
| Copper | 100–200 | 200–400 |
| Cast Iron (gray) | 50–80 | 150–300 |
| Mild Steel (1018) | 80–120 | 300–600 |
| Alloy Steel (4140) | 60–90 | 200–400 |
| Stainless (304/316) | 40–60 | 150–300 |
| Tool Steel | 40–70 | 150–300 |
| Titanium | 30–50 | 100–200 |
| Plastics / Delrin | 300–500 | 500–1000 |
Once you know the SFM for your material, you solve for the RPM that holds the cutting edge at that speed for a given diameter — the workpiece diameter on a lathe, or the cutter diameter on a mill.
RPM = (SFM × 3.82) ÷ Diameter (inches)
RPM = (1000 × surface speed in m/min) ÷ (π × Diameter in mm)
Milling feed (in/min) = RPM × chip load per tooth × number of flutes
Example: mild steel (100 SFM) turned at 1" diameter → (100 × 3.82) ÷ 1 = 382 RPM.
Recommended RPM for turning (by workpiece diameter) and milling (by cutter diameter) with HSS tooling, using mid-range SFM for each material. Round to the nearest speed your machine offers, and multiply by 2 to 3 for carbide.
| Diameter | Aluminum | Brass | Cast Iron | Mild Steel | Stainless |
|---|---|---|---|---|---|
| 1/4" | 4500 | 3050 | 990 | 1500 | 765 |
| 1/2" | 2300 | 1530 | 495 | 765 | 380 |
| 3/4" | 1530 | 1020 | 330 | 510 | 255 |
| 1" | 1150 | 765 | 250 | 380 | 190 |
| 1-1/2" | 765 | 510 | 165 | 255 | 127 |
| 2" | 575 | 380 | 125 | 190 | 95 |
| 3" | 380 | 255 | 83 | 127 | 64 |
| 4" | 285 | 190 | 62 | 95 | 48 |
Based on HSS mid-range SFM: aluminum 300, brass 200, cast iron 65, mild steel 100, stainless 50.
Dialing in these speeds needs a machine that holds them. The Grizzly G4000 9" x 19" Benchtop Metal Lathe (turning) and Grizzly G0761 10" x 32" HD Benchtop Mill/Drill (milling) are strong shop machines from Grizzly Industrial, often priced lower factory-direct than through a reseller and backed by full parts availability and U.S. support.
The RPM sets surface speed; the chip load sets how much each flute cuts. Multiply chip load by RPM and the number of flutes to get feed in inches per minute. Chip load per tooth in inches for HSS end mills:
| End Mill Diameter | Aluminum | Mild Steel | Stainless |
|---|---|---|---|
| 1/8" | 0.0010 | 0.0005 | 0.0005 |
| 1/4" | 0.0020 | 0.0010 | 0.0007 |
| 3/8" | 0.0030 | 0.0015 | 0.0010 |
| 1/2" | 0.0040 | 0.0020 | 0.0015 |
| 3/4" | 0.0050 | 0.0030 | 0.0020 |
| 1" | 0.0060 | 0.0040 | 0.0025 |
Chips tell the truth. Aim for tight commas or small curls, not dust and not long stringy ribbons. If the tool chatters or the finish is rough, first lower the RPM, then increase the feed slightly — a light, fast rub work-hardens steel and stainless and burns the edge. Use cutting oil on steels and stainless; aluminum cuts well dry or with a mist.
On the lathe, feed is set as inches per revolution rather than per tooth. Use light feeds for finishing and heavier feeds for roughing, then let the surface speed chart set your RPM.
| Operation | Feed (in/rev) | Notes |
|---|---|---|
| Roughing | 0.010–0.020 | Maximum material removal; heavier cuts on rigid machines |
| General turning | 0.005–0.012 | Everyday cuts on most bench and hobby lathes |
| Finishing | 0.002–0.005 | Fine surface finish; pair with a sharp, honed tool |
| Parting / grooving | 0.001–0.003 | Slow and steady; flood the cut and keep the tool on center |
This chart covers turning and milling. For drill-press RPM by bit and material, or CNC router feeds and speeds, use the matching references.
Drill Speed Chart CNC Feeds & SpeedsSharp, rigid tooling is what lets you actually run the numbers above.
As an Amazon Associate and Grizzly Industrial affiliate, WorkshopCalc earns from qualifying purchases. This helps support our free calculators and guides.
Spindle speed: RPM = (SFM × 3.82) ÷ diameter in inches, where SFM is the recommended surface feet per minute for the material and the diameter is the workpiece (turning) or the cutter (milling). Milling feed rate: Feed in inches per minute = RPM × chip load per tooth × number of flutes. Turning feed is set as feed per revolution, typically 0.005 to 0.015 inches per rev from finishing to roughing.
Mild steel (1018) machines at about 80 to 120 SFM with a high-speed-steel (HSS) tool, so use roughly 100 SFM. With carbide tooling you can run 300 to 600 SFM. At 100 SFM, a 1" diameter turns at about 380 RPM, a 1/2" bar at about 765 RPM, and a 2" bar at about 190 RPM.
Carbide tooling typically runs 2 to 3 times the surface speed of high-speed steel, provided the setup is rigid and you use coolant on steels. Run HSS at the SFM values in the charts, then multiply by roughly 2 to 3 for carbide. Coated carbide can go higher still on production machines.
Feed in inches per minute = RPM × chip load per tooth × number of flutes. Example: a 1/2" 2-flute end mill in aluminum at about 1150 RPM with a 0.004" chip load gives 1150 × 0.004 × 2 = about 9.2 inches per minute. Reduce the chip load for smaller cutters, harder materials, and deep slotting cuts.