Speeds & Feeds Chart

Starting surface speeds (SFM) and chip loads (IPT) for milling, turning, and drilling across common materials. HSS and carbide values plus the RPM / feed-rate formulas machinists use every day.

Reference Reference Updated Apr 24, 2026
X Facebook LinkedIn Reddit Email
Reference

Starting values for milling, turning, and drilling. All SFM figures are conservative — OK to bump 20-40% once the setup is dialled in and chip formation looks right. Carbide columns are 3-4× HSS for the same material. Always verify against your specific tool and machine; chatter, rubbing, or glazed chips mean back off 10-20% and try again.

Milling — end mill surface speeds (SFM)

Material HSS SFM Carbide SFM Notes
Aluminum 6061 300 – 1000 800 – 3500 Use 2-flute to prevent chip packing; WD-40 / alcohol lubricant.
Aluminum 7075 250 – 800 700 – 2500 Harder than 6061; higher silicon content dulls HSS fast.
Brass / free-mach. 200 – 350 500 – 1200 Dry or light coolant; 360 brass is ideal.
Bronze 100 – 200 300 – 800 Bearing bronze is gummy — use positive rake.
Copper 100 – 250 300 – 900 Gummy; sharp tools and positive rake essential.
Cast iron (gray) 60 – 90 250 – 500 Dry machining — coolant can cause thermal cracks.
Cast iron (ductile) 50 – 80 200 – 400 Slightly tougher than gray iron.
Mild steel 1018 80 – 120 300 – 600 Standard reference. Flood coolant.
Medium carbon 1045 70 – 110 250 – 500 Flood coolant mandatory.
Alloy steel 4140 60 – 100 200 – 450 Pre-hardened: reduce to 40-60 SFM HSS.
Tool steel (annealed) 50 – 80 180 – 400 H13, D2, A2 at low hardness.
Tool steel (hardened) — 80 – 200 Rc > 40: carbide only, reduce depth of cut.
Stainless 303 80 – 120 250 – 500 Most machinable SS; free-cutting.
Stainless 304 / 316 40 – 70 150 – 350 Work-hardens fast — feed hard, stay in the cut.
Stainless 17-4 PH 50 – 80 200 – 400 Condition A; reduce 30% for H900/H1025.
Inconel / Hastelloy 15 – 30 60 – 150 Super-alloy: slow, heavy feed, flood coolant.
Titanium Ti-6Al-4V 20 – 40 80 – 200 Low RPM, aggressive feed; never dwell in cut.
Plastic (Delrin, UHMW) 400 – 800 800 – 2000 Sharp tools; dry or air blast.
Plastic (acrylic) 200 – 500 500 – 1500 Polished flutes; slow feed to avoid melt.
Wood / MDF — 1500 – 5000 High RPM, low DOC, chip clearance is key.

Milling — end mill chip load (IPT, inches per tooth)

Tool Ø Aluminum Brass Mild Steel Stainless Titanium
1/8 (3 mm) 0.0010 – 0.002 0.0008 – 0.0015 0.0005 – 0.0010 0.0004 – 0.0008 0.0003 – 0.0006
1/4 (6 mm) 0.002 – 0.004 0.0015 – 0.003 0.001 – 0.002 0.0008 – 0.0015 0.0006 – 0.0012
3/8 (10 mm) 0.003 – 0.006 0.0025 – 0.004 0.0015 – 0.003 0.0012 – 0.0020 0.0010 – 0.0018
1/2 (12 mm) 0.005 – 0.009 0.004 – 0.007 0.002 – 0.005 0.0015 – 0.003 0.0012 – 0.0025
3/4 (20 mm) 0.008 – 0.014 0.006 – 0.010 0.004 – 0.008 0.003 – 0.006 0.0020 – 0.005
1 (25 mm) 0.010 – 0.018 0.008 – 0.014 0.005 – 0.010 0.004 – 0.008 0.0025 – 0.006

Turning — starting SFM on a lathe (single-point HSS / carbide)

Material HSS Rough HSS Finish Carbide Rough Carbide Finish
Aluminum 400 – 700 600 – 1000 800 – 1500 1200 – 3000
Brass 150 – 300 250 – 400 400 – 800 600 – 1500
Cast iron 50 – 80 80 – 120 200 – 400 300 – 600
Mild steel 80 – 110 100 – 150 300 – 500 400 – 900
Alloy steel 60 – 90 80 – 120 200 – 400 350 – 700
Tool steel 40 – 70 60 – 100 150 – 350 250 – 600
Stainless 304 40 – 60 60 – 90 150 – 300 250 – 500
Titanium 20 – 35 30 – 50 80 – 160 120 – 250
Plastic 300 – 600 400 – 800 600 – 1500 1000 – 2500

Turning — feed rate (IPR, inches per revolution)

Operation DOC (in) Aluminum Steel Stainless / Titanium
Rough 0.050 – 0.250 0.010 – 0.025 0.007 – 0.020 0.005 – 0.012
Finish 0.005 – 0.030 0.002 – 0.008 0.002 – 0.007 0.0015 – 0.005

Drilling — starting SFM (HSS twist drill)

Material SFM Feed per rev (IPR)
Aluminum 6061 200 – 400 0.004 – 0.016
Brass 150 – 300 0.004 – 0.012
Cast iron 50 – 80 0.004 – 0.015
Mild steel 60 – 100 0.004 – 0.015
Alloy steel (4140) 40 – 60 0.003 – 0.012
Tool steel 30 – 50 0.002 – 0.010
Stainless 304 25 – 50 0.002 – 0.010
Titanium 15 – 30 0.002 – 0.008
Plastic 150 – 400 0.008 – 0.020

Formulas

RPM (inch)
RPM = (SFM × 12) / (π × D) — shortcut: RPM ≈ SFM × 3.82 / Din
RPM (metric)
RPM = (Vm/min × 1000) / (π × Dmm) — shortcut: RPM ≈ V × 318 / Dmm
SFM from RPM
SFM = (π × D × RPM) / 12
Milling feed
IPM = RPM × IPT × (# of teeth)
Turning feed
IPM = RPM × IPR
MRR (milling)
MRR (in³/min) = WOC × DOC × IPM
SFM ↔ m/min
SFM × 0.3048 = m/min · m/min × 3.28 = SFM

Rules of thumb

  • Start at the low end of each SFM range, then increase until you hear chatter or see tool wear accelerate.
  • For HSS end mills: chip load ≈ 1% of tool diameter for steel, 2% for aluminum.
  • Carbide generally wants 3-4× the HSS SFM and 1.5× the chip load. Use coated carbide (TiN, TiAlN, AlTiN) for higher ranges.
  • Slot milling (full-width cut) halve the chip load — the tool is doing ~2× the work of a side cut.
  • Ramp or helical into pockets instead of plunging; plunge-cut chip evacuation fails above ~0.5 × tool diameter depth.
  • Work-hardening materials (stainless, Inconel, Ti) hate light passes. Feed hard (≥ 0.002 IPT) to stay under the hardened skin.
  • Thin-wall parts: reduce DOC and use climb milling to keep deflection in.

Last updated: