Lathe turning SFM by material and tool type, IPR feed bands, depth-of-cut guidance, and example RPM at common diameters from 0.25″ to 6″ (RPM = SFM × 3.82 ÷ diameter). Starting points for manual and CNC lathes — verify on scrap before production cuts.
How to Use This Chart
Choose SFM from material and insert type, convert to RPM for your workpiece diameter, then pick roughing or finishing IPR and depth of cut. Calculator: lathe turning calculator. Guide: lathe speeds & feeds guide.
Turning speed is limited by workholding, machine horsepower, and insert geometry as much as by the material table. Start at the low end of the SFM band for HSS, mid-band for carbide, and increase only when chips are consistent and surface finish is acceptable.
SFM by Material & Tool
| Material | HSS | Carbide | Coated carbide | Ceramic |
|---|---|---|---|---|
| Mild steel (1018/1045) | 80–120 | 300–600 | 400–800 | 800–1500 |
| Tool steel (annealed) | 40–60 | 150–300 | 200–400 | 400–800 |
| Stainless (304/316) | 40–60 | 150–250 | 200–350 | 300–600 |
| Cast iron (class 30–40) | 60–80 | 200–400 | 300–500 | 600–1000 |
| Aluminum (6061) | 300–500 | 800–1500 | 1000–2000 | — |
| Brass | 200–300 | 500–800 | 600–1000 | — |
| Copper | 100–200 | 300–500 | 400–600 | — |
| Plastic (Delrin/acrylic) | 200–400 | 500–1000 | 500–1000 | — |
| Titanium (Grade 5) | 20–35 | 60–120 | 80–150 | 200–400 |
RPM = SFM × 3.82 ÷ diameter (in). Constant SFM (G96 on CNC) automatically reduces RPM as diameter increases — essential for facing and taper turns.
HSS vs Carbide — Practical Differences
| Factor | HSS | Carbide / coated |
|---|---|---|
| Typical SFM | 0.25–0.35× carbide values | Use table bands directly |
| Feed (IPR) | ≈ 0.7× carbide feeds | Baseline in IPR table below |
| DOC roughing | 0.050–0.125″ common | 0.100–0.250″ when rigid setup |
| Edge prep | Positive rake, sharp edge | Negative rake holders for heavy cuts |
| Best for | Small lathes, threading, odd alloys | Production OD/ID, hard materials |
HSS tolerates interrupted cuts and low rigidity better than brittle carbide but cannot sustain high surface speed. Coated carbide adds heat resistance — use coated inserts above ~400 SFM in steel.
IPR Feed Ranges (carbide baseline)
HSS feeds ≈ 0.7× these values. Reduce 30–50% for finishing passes or poor rigidity.
| Material | Roughing IPR | Finishing IPR |
|---|---|---|
| Mild steel | 0.010–0.020 | 0.003–0.008 |
| Tool steel | 0.008–0.015 | 0.003–0.006 |
| Stainless | 0.008–0.015 | 0.002–0.006 |
| Cast iron | 0.010–0.018 | 0.004–0.008 |
| Aluminum | 0.015–0.030 | 0.005–0.010 |
| Brass | 0.012–0.022 | 0.005–0.010 |
| Copper | 0.010–0.018 | 0.004–0.008 |
| Plastic | 0.012–0.025 | 0.005–0.012 |
| Titanium | 0.004–0.008 | 0.002–0.004 |
Depth of Cut (DOC) Guidance
| Operation | Carbide DOC (typical) | HSS DOC (typical) | Notes |
|---|---|---|---|
| Roughing OD | 0.100–0.250″ | 0.050–0.125″ | Machine and holder limited |
| Finishing OD | 0.010–0.030″ | 0.005–0.020″ | Spring pass if deflection |
| Boring ID | 0.050–0.150″ | 0.025–0.080″ | L/D ratio reduces DOC |
| Parting off | 0.040–0.080″/pass | 0.020–0.050″/pass | Reduce feed vs turning |
Material removal rate (MRR) ≈ DOC × IPR × SFM factor — doubling feed or DOC increases load faster than doubling speed. Chatter means reduce DOC or speed, not both blindly.
Example RPM — Carbide Mid SFM
Midpoints: mild steel 450 SFM, stainless 200 SFM, aluminum 1150 SFM. RPM = SFM × 3.82 ÷ D.
| Diameter | Mild ~450 SFM | SS ~200 SFM | Al ~1150 SFM |
|---|---|---|---|
| 0.25″ | 6876 | 3056 | 17,572 |
| 0.5″ | 3438 | 1528 | 8786 |
| 1.0″ | 1719 | 764 | 4393 |
| 2.0″ | 860 | 382 | 2196 |
| 3.0″ | 573 | 255 | 1464 |
| 4.0″ | 430 | 191 | 1098 |
| 5.0″ | 344 | 153 | 878 |
| 6.0″ | 287 | 127 | 732 |
Example RPM — HSS (Mild Steel ~100 SFM)
| Diameter | ~100 SFM RPM | ~50 SFM RPM (tool steel) |
|---|---|---|
| 0.5″ | 764 | 382 |
| 1.0″ | 382 | 191 |
| 2.0″ | 191 | 96 |
| 3.0″ | 127 | 64 |
| 4.0″ | 96 | 48 |
| 6.0″ | 64 | 32 |
Small diameters at high RPM overheat HSS quickly — use coolant and keep passes light. Many manual lathes cap spindle speed below carbide recommendations for small work — that is normal; reduce feed to compensate or use HSS.
Calculate SFM, RPM, feed, and MRR for your cut
WeldKit — Welding Calculators Offline
MIG, TIG, Stick, speeds/feeds, and more on Android.
Related Calculators & Guides
Machining
Machining Speeds & Feeds Card
One page. Speeds, chip load and drill feed, imperial and metric.
$3.99
Buy
Complete Machining Speeds & Feeds Guide
27 pages. Milling, drilling, tapping, turning and CNC routing.
$12.99
Buy
Machining Job Estimator
Quote shop work and check operations against your spindle's top speed.
Excel or Google Sheets. Best on a computer.
$29.00
Buy
Machining Complete Bundle
Card, 27-page guide and the estimator workbook. All six files.
Excel or Google Sheets. Best on a computer.
$34.99
$45.98 if bought separately — save $10.99
BuyCheckout opens in a new tab.