← AskMachinist · Guides · Calculator · 🔎 Search

Turning Speeds and Feeds

Guide · Updated October 28, 2026

On a lathe the work spins, so cutting speed depends on the diameter being cut right now. You pick a surface speed (SFM) for the material and tool, turn it into RPM for the diameter, then choose a feed per revolution (IPR) and depth of cut for the insert.

Run the numbers

Use the free speeds and feeds calculator for RPM and feed, and the free Gage Block Calculator when you need an exact gage stack to check a shoulder or length.

Step by step

Pick SFM: Choose a surface speed for the work material and tool: for example around 500–800 SFM for carbide in mild steel, or about 80–100 SFM for HSS.
Convert to RPM: RPM = SFM × 3.82 ÷ diameter in inches (metric: RPM = Vc × 1000 ÷ (π × D mm)). Use the diameter being cut.
Check machine limits: Cap the RPM at the chuck and spindle rating and at what the setup can safely hold, especially for long or unbalanced work.
Choose feed per rev: Pick IPR from the insert chipbreaker range: roughly 0.008–0.015 IPR roughing and 0.003–0.006 IPR finishing for common inserts.
Set depth of cut: Stay inside the chipbreaker depth range; finishing passes usually leave 0.010–0.030 in per side.
Cut and adjust: Watch chip color and shape, sound and finish, then adjust speed first for tool wear and feed for chip control and finish.

Worked example

Rough turning 1018 steel at 2.000 in diameter with a coated carbide insert. Start at 600 SFM: RPM = 600 × 3.82 ÷ 2.000 = 1,146 RPM.

At 0.010 IPR the carriage moves 1,146 × 0.010 = 11.5 in/min. A 4 in long pass takes about 21 seconds.

Finish at 1.900 in with 0.004 IPR: RPM = 600 × 3.82 ÷ 1.9 ≈ 1,206 RPM, feed ≈ 4.8 in/min. With HSS at 90 SFM the same 2 in bar would run about 172 RPM.

Constant surface speed (CSS)

On CNC lathes G96 holds SFM as the diameter changes, and G50 (or G92 on some controls) caps the spindle RPM. Always set the cap before facing toward center, or the spindle will try to run to its maximum.

Starting surface speeds

These are conservative starting points, not limits. Aluminum: 800–1,500+ SFM carbide. Mild steel: 500–800 carbide, 80–100 HSS. 4140 prehard: 350–550 carbide. 304 stainless: 300–500 carbide. Cast iron: 300–600 carbide. Always check the insert maker’s chart first.

Tips

Inserts come with a recommended feed and depth window for each chipbreaker: see carbide insert basics.
Coolant choice changes tool life and finish: cutting fluid and coolant basics.
Finish depends mostly on feed and nose radius: surface finish basics.
Set the tool on center first: how to set tool height.
The same SFM-to-RPM logic drives milling, drilling and tapping.

FAQ

How do you calculate lathe RPM?

RPM = SFM × 3.82 ÷ diameter in inches. For example 600 SFM on a 2 in bar is about 1,146 RPM.

What is IPR in turning?

Inches per revolution: how far the tool advances each time the part turns once. Feed rate in in/min equals RPM × IPR.

What feed should I use for finishing on a lathe?

Commonly 0.003–0.006 IPR with a 1/32 in (0.8 mm) nose radius, adjusted for the finish you need and the insert chipbreaker.

Why does my finish get worse near the center when facing?

At fixed RPM the surface speed drops toward zero as the diameter shrinks. Use constant surface speed with an RPM cap, or raise the RPM as you go.

Is there a free calculator for speeds and feeds?

Yes. AskMachinist has a free speeds and feeds calculator, and the Gage Block Calculator at gageblockcalc.com is free with no login.

Related guides and calculators

Build your stack in seconds

The free Gage Block Calculator finds the fewest-block combination for inch and metric sets, with wear blocks. No login.

Questions? Ask a machinist.

General shop information only — follow your tooling, machine and gage manufacturers' instructions and your quality system.