Why do turning and milling SFM charts show different numbers?

Turning is a continuous cut — the edge stays engaged and reaches a stable temperature, so it tolerates higher surface speeds. Milling is interrupted: every revolution the edge slams into the material and then cools, which causes thermal and mechanical shock. Published milling speeds are therefore usually lower than turning speeds for the same material, and the two sets of figures must not be mixed. This page keeps them in separate tables for that reason.

SFM Chart: Cutting Speed by Material

Q: What SFM should I use for steel?

For carbide end mills in plain carbon steel such as 1018 or 1045, a conservative starting range is 250-350 SFM (76-107 m/min). Alloy steels like 4140 run similarly at 250-430 SFM when annealed, but drop sharply when hardened or heat treated. High speed steel tooling runs far slower — roughly 125-215 SFM in 1018 for turning. Always start at the low end of the range and adjust for rigidity, coolant and depth of cut.

Q: How much faster is carbide than HSS?

Carbide typically runs three to five times the surface speed of high speed steel in the same material, because it keeps its hardness at much higher temperatures. In mild steel that is roughly 125-215 SFM for HSS versus 800+ SFM for carbide in turning. Carbide is also more brittle, so it needs rigid setups and consistent feed — it fails by chipping when it is allowed to rub or when the machine chatters.

Q: What is the difference between SFM and RPM?

SFM is a property of the material and tool combination — how fast the cutting edge should travel through the workpiece. RPM is a machine setting. The same 300 SFM means a completely different spindle speed on a 1/8 inch end mill than on a 2 inch face mill, because RPM = (12 × SFM) / (π × D). Pick the SFM from a chart like this one, then convert it to RPM for your specific tool diameter.

Q: Do coolant and coatings change the recommended SFM?

Yes. Coated carbide (TiAlN, AlTiN and similar) tolerates more heat and is often run at the upper end of a published range or above it, while uncoated tooling should stay at the low end. Coolant matters most in materials that work-harden or gall, such as stainless and titanium. But the published figures are starting points from tooling manufacturers, not limits — machine rigidity and workholding usually constrain you before the tool coating does.

Recommended surface speeds for milling and turning, in both SFM and m/min, for HSS and carbide tooling. Every figure below is traced to a named tooling manufacturer — sources are listed at the bottom, and rows backed by only one source are marked as such.

Milling — carbide end mills

Conservative starting ranges for solid carbide end mills. Where two manufacturers disagreed, the lower (safer) range is shown and the disagreement is noted in the sources section.

Material	SFM	m/min	Confidence
Aluminum 6061	600–1500	183–457	3 sources
Aluminum 7075	600–1500	183–457	3 sources
Brass	800–1170	244–357	2 sources
Bronze	600–715	183–218	2 sources
Copper (oxygen-free)	700–1000	213–305	1 source
Mild steel 1018	250–350	76–107	3 sources
Steel 1045	250–350	76–107	3 sources
Alloy steel 4140 (annealed)	250–430	76–131	2 sources
Alloy steel 4340	50–250	15–76	2 sources, wide split
Tool steel A2	100–250	30–76	2 sources
Tool steel D2	200–280	61–85	1 source
Stainless steel 303 / 304 / 316	100–350	30–107	3 sources
Stainless steel 17-4PH	90–250	27–76	2 sources
Gray cast iron	100–400	30–122	3 sources
Ductile cast iron	80–400	24–122	1 source
Titanium Ti-6Al-4V	50–250	15–76	2 sources
Inconel 718	40–60	12–18	2 sources
Magnesium	1000+	305+	1 source, no upper limit given
Acrylic / polycarbonate	200–600	61–183	2 sources, wide split
Carbon fiber composite	400–825	122–251	1 source

SFM chart for turning

Turning is a continuous cut, so it runs faster than milling in the same material — these numbers are not interchangeable with the milling table above. Data is for lathe work with HSS and brazed/indexable carbide.

Material	HSS (SFM)	Carbide (SFM)	Confidence
Aluminum (wrought & cast)	500–600	2820	1 source
Brass	300–350	1170	1 source
Bronze	200–250	715	1 source
Mild steel 1018	125–215	800–885	1 source
Steel 1045	55–180	—	1 source
Alloy steel 4140	70–200	430–685	1 source
Tool steel A2	80–125	355–365	1 source
Stainless steel 303 / 304 / 316	115–135	—	1 source
Gray cast iron	145–215	410	1 source

Got your SFM? → Convert it to RPM for your tool diameter · Then → turn that RPM into a feed rate

How to use this chart

Surface speed is a property of the material and tool material — it does not depend on your machine. The workflow is always the same three steps:

1. Look up the SFM for your material and tool type in the tables above.
2. Convert to RPM for your actual tool diameter: RPM = (12 × SFM) / (π × D).
3. Convert to feed rate: IPM = RPM × chip load × number of flutes.

Start at the low end of every range. The published figures assume rigid setups, proper workholding and adequate coolant. A benchtop mill or a long tool stickout will chatter long before you reach the top of these ranges.

Turning vs milling vs drilling

The same material has three different practical speed ranges depending on how the edge engages it:

Turning — continuous cut, edge stays hot and stable. Highest SFM of the three.
Milling — interrupted cut, thermal and shock cycling every revolution. Lower SFM; this is the more conservative table above.
Drilling — poor chip evacuation and coolant reach at depth, and the speed at the drill centre is zero. Typically run at roughly half to two-thirds of the turning SFM for the same material, and peck deep holes.

What changes the right number

Hardness / heat treatment: 4140 annealed and 4140 hardened are effectively different materials — hardened alloy steel drops toward the bottom of its range or below it.
Coating: coated carbide (TiAlN, AlTiN) tolerates the upper end; uncoated stays low.
Coolant: critical in stainless and titanium, which work-harden and gall when the tool rubs. Flood or high-pressure coolant lets you hold the published speed.
Rigidity: stickout, workholding and spindle condition usually limit you before the tooling does.

Wood and MDF — why they are not in the chart

Router work in wood, MDF and plywood is not specified in SFM. Routers run at a fixed high spindle speed (typically 16,000–18,000 RPM) and the cut is controlled by chip load per tooth instead — around 0.003–0.008 in/tooth in MDF depending on cutter diameter. Putting a wood "SFM" figure in the table above would be using the wrong unit system for the job, so it is deliberately left out. Use the IPM calculator with your router's RPM and a chip load in that range.

Materials we could not source

Delrin / acetal and UHMW are not listed. No tooling manufacturer chart we checked gives a named SFM for either — they appear only inside generic "plastics" rows, and quietly reusing that figure would be presenting a guess as data. If you machine these, start from the acrylic / polycarbonate row and verify against your tool supplier.

Frequently asked questions

What SFM should I use for steel?

Carbide end mills in 1018 or 1045: start around 250–350 SFM (76–107 m/min). Annealed 4140 is similar at 250–430 SFM; hardened or heat-treated alloy steel drops sharply. HSS runs far slower — about 125–215 SFM in 1018 for turning.

Why do turning and milling charts show different numbers?

Turning is continuous, milling is interrupted. The milling edge is shock-loaded and thermally cycled every revolution, so published milling speeds are lower. Never mix figures between the two tables.

How much faster is carbide than HSS?

Roughly three to five times, because carbide keeps its hardness at much higher temperatures. It is also more brittle — it needs rigid setups and a consistent feed, and it chips when allowed to rub.

What is the difference between SFM and RPM?

SFM belongs to the material and tool; RPM is a machine setting. 300 SFM is a very different spindle speed on a 1/8″ end mill than on a 2″ face mill. Convert with RPM = (12 × SFM) / (π × D).

Do coolant and coatings change the recommended SFM?

Yes. Coated carbide runs at the top of a range or above; uncoated stays low. Coolant matters most in stainless and titanium. But rigidity usually limits you before the coating does.

Sources

Every figure in the tables above comes from one of the published references below. Where two sources disagreed, the lower range is shown and the row is flagged. Rows marked "1 source" have no independent confirmation — treat them as a starting point and verify with your tool supplier.

Harvey Tool — General Machining Guidelines — aluminium, copper alloys, magnesium, plastics, cast irons, alloy and tool steels, stainless grades, titanium, Inconel (carbide milling).
LittleMachineShop — Cutting Speeds — the turning table: HSS and carbide lathe speeds for carbon and alloy steels, stainless, cast iron, brass, bronze, aluminium.
Kennametal — Recommended Starting Speeds and Feeds (end mill catalogue) — carbide milling speeds and feed per tooth across steel, stainless, cast iron, titanium, nickel alloys, aluminium.
Amana Tool — Plastic O-Flute Speed Chart and Carbon / Graphite / CFRP chart — plastics and composites.
ShopBot Tools — Feeds and Speeds (after Onsrud) — the wood/MDF chip load figures cited in the section above.
Machining Doctor — D2 tool steel data — sole source for the D2 row; an aggregator rather than a tooling manufacturer, hence the flag.

Known disagreements between sources: 4340 (50–250 vs 150–550 SFM), acrylic (200–600 vs 500–1200 SFM, the higher figure being for dedicated O-flute plastic cutters), and gray cast iron (upper limit 400 vs 725 SFM depending on grade and hardness). The conservative value is shown in each case.