Speeds & Feeds Chart

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 / D_in
RPM (metric)	RPM = (V_m/min × 1000) / (π × D_mm) — shortcut: RPM ≈ V × 318 / D_mm
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.

Was this article helpful?