Home » Milling » SFM Chart by Material: Max’s Guide to Speeds, RPM and Chip Load

SFM Chart by Material: Max’s Guide to Speeds, RPM and Chip Load

Filed under , ,

A blown up end mill. A chattered finish. A burned edge on a part that should have come off clean. Walk the floor of a shop after a bad run and the tool can get blamed first. Sometimes, it is not the tool. It is the math.

Category: Milling  •  Updated October 2026  •  Reading Time: ~10 minutes  •  Audience: Intermediate to Advanced Machinists

SFM Chart by Material

Every number below comes from a tool maker’s published cutting data, and every cell names its source. Where two makers publish different numbers for the same material and tool type, the cell shows the spread from lowest to highest. Where none of them publish a number, the cell says n/p. We would rather leave a blank than fill it with a guess.

Material Example grades Carbide end mill HSS end mill Carbide drill HSS-Co drill Tap (HSS-E)
Aluminum, wrought 6061, 7075 1,000 H1 260–395 D2 250–360 G, M n/p 30–80 O3, D4
Aluminum, cast A356, 380 650–750 H1 235 D2 n/p 205–330 O2 30–110 O3, D4
Brass / bronze C360 / C932 225–500 H1 165–275 D2 160 G n/p 30–195 O3, D4
Low-carbon steel 1018, 12L14 560–755 D1 320–430 D2 215–395 O1, G, M 105–130 O2 50–130 O3, D4
Medium-carbon steel 1045 490 D1 280 D2 195–395 O1, M 70–100 O2 40–80 O3, D4
Alloy steel, annealed 4140, 4340 365 D1 195 D2 195–395 O1, G, M 65–80 O2 40–80 O3, D4
Alloy / tool steel, pre-hard 4140 HT, P20 (28–36 HRC) 150–310 H1, D1 120–165 D2 180–280 M, G n/p 20–60 O3, D4
Tool steel, annealed A2, D2, H13 270 D1 145 D2 180 G 25–40 O2 35 D4
Hardened steel 45–55 HRC 210–255 D3 * n/p 65–100 M ** n/p n/p
Cast iron, gray Class 30–40 475 D1 135 D2 230–395 O1, G, M 105–130 O2 35–80 E, D4
Cast iron, ductile 65-45-12 445 D1 215 D2 195–330 O1, G, M n/p 35–80 E, D4
Stainless, free-machining 303, 416 450 H1 n/p 130–230 O1 n/p 40–80 O3
Stainless, austenitic 304, 316 200–310 H1, D1 n/p 65–230 O1, G, M n/p 25–80 O3, D4
Stainless, PH 17-4 PH 150 H1 n/p 120–230 O1, G n/p n/p
Titanium Ti-6Al-4V 150–225 H1, D1 115 D2 100–180 O1, G n/p n/p
Nickel alloys Inconel 625 / 718 70–130 H1, D1 80 D2 65–110 O1, G, M n/p n/p
Plastics, unfilled Delrin, nylon, acrylic 800–1,200 H3 275 D2 n/p n/p 85 D4

Values in SFM. n/p = not published by the sources below. Letters in each cell refer to the source list. * Dormer S561 hard-milling end mill; Harvey’s 7-flute hardened-steel finisher is published at 60 SFM (45–55 Rc). ** Mitsubishi MVE, published for 40–55 HRC.

Starting values. Always check the maker’s data for your exact tool.

How to read this chart

  • These are starting points, not limits. Rigid setups often run above them; long stickout and light workholding run below.
  • Milling numbers assume side or profile milling with flood coolant. For a full-width slot, Dormer recommends dropping cutting speed roughly 20 to 25 percent.
  • Harvey Tool publishes its steel, stainless, titanium and nickel speeds for 29–37 Rc material. That is why the Harvey numbers sit in the pre-hard and stainless rows, and the annealed steel rows come from Dormer.
  • The OSG carbide drill numbers are for through-coolant drills. The tap numbers are OSG’s standard column for a rigid setup on a machining center; coolant-through taps can run considerably faster.
  • Metric catalog values were converted at m/min × 3.281 and rounded to the nearest 5 SFM.

Where these numbers come from

  • H1 Harvey Tool, Speeds & Feeds, Miniature End Mills, Square, Stub & Standard (4 flute). Published on Harvey tool pages and on shop.wcchapman.com.
  • H2 Harvey Tool, End Mills for Hardened Steels, Square, For Steels 45–68 Rc (7 flute).
  • H3 Harvey Tool, End Mills for Plastics, Square Upcut, 2 Flute, High Helix.
  • D1 Dormer Pramet Solid Milling catalog 2024, S716 4-flute solid carbide end mill, AlCrN, p.100.
  • D2 Dormer Pramet Solid Milling catalog 2024, C246 multi-flute HSS-E-PM end mill, TiCN, p.40.
  • D3 Dormer Pramet Solid Milling catalog 2024, S561 4-flute solid carbide end mill for hard materials, TiSiN, p.144.
  • D4 Dormer Pramet Threading catalog 2024, EP00TIN HSS-E-PM spiral point machine tap, TiN, p.126.
  • M Mitsubishi Materials catalog C010A, MVE solid carbide drill, recommended cutting conditions (inch), pp. L085–L086.
  • G Garr Tool, General Purpose Drilling Guide, Bright Finish table, 1200/1205/1520 series, p.328.
  • O1 OSG, A Brand ADO carbide drill, Lists 6500/6510/6520, technical page 306.
  • O2 OSG, EX-GOLD HSS-Co drill, Lists 1000/1500, technical page 352.
  • O3 OSG, HY-PRO cut taps, Recommended Tapping Conditions, technical page 415.
  • E Emuge-Franken, Rekord 1A-H-NT machine tap specification sheet (cast iron).

Three numbers control almost everything that happens at the spindle: surface feet per minute (SFM), revolutions per minute (RPM), and chip load. Here is how they work together, and how to calculate them for your next job.

What Is SFM (Surface Feet per Minute)?

Surface feet per minute is how fast the cutting edge travels through the material, not how fast the spindle turns. It is a property of the material and the tool, not the machine.

Materials tend to have a sweet spot. Push SFM too high on a tough alloy and the tool can burn up before the part is finished. Run it too low and the edge can rub instead of cutting, which can wear the tool just as fast, only less obviously. That is why tool makers publish SFM ranges, and why that number is step one. RPM and chip load get built on top of it.

SFM vs. SFPM vs. RPM

SFM and SFPM are the same thing: surface feet per minute, two abbreviations for one unit. RPM is different. RPM is spindle speed, the number you actually dial in at the control. The same SFM gives a different RPM for every tool diameter.

How to Convert SFM to RPM

Bigger tool at the same SFM means lower RPM. Smaller tool at the same SFM means higher RPM. That is why swapping a 1/2″ end mill for a 1/4″ and leaving the spindle speed alone is an easy mistake to make. The dial did not move, but the surface speed at the cutting edge was cut in half.

RPM at 100 SFM by tool diameter

Pure math, no recommendation. Multiply the RPM by your SFM ÷ 100. For 300 SFM on a 1/2″ tool: 764 × 3 = 2,292 RPM.

Tool diameter 1/8″ 1/4″ 3/8″ 1/2″ 3/4″ 1″
RPM at 100 SFM 3,056 1,528 1,019 764 509 382

Metric: SMM and Vc

Metric catalogs list cutting speed as Vc in meters per minute (sometimes written SMM). SFM × 0.3048 = m/min, and m/min × 3.281 = SFM.

Chip Load and Feed Rate: Learn to Read Your Chips

Chip load (feed per tooth) is how far the tool advances each time one cutting edge enters the cut. It is a number that sometimes gets skipped, and skipping it can lead to expensive failures.

  • Too light: the edge rubs instead of shearing. Heat can build at the tip and the tool can fail from the inside, before it looks worn.
  • Too heavy: the edge is overloaded on each pass. That can lead to chipping and breakage rather than gradual wear.

Dial chip load in correctly and the benefit is not just tool survival. Finish improves and cycle time drops in the same pass, because the tool is cutting the way it was designed to cut instead of fighting the material.

Feed rate formula

Chip thinning at light radial engagement

When the radial depth of cut (ae) is less than half the tool diameter (D), the chip the tool actually makes is thinner than the feed per tooth you programmed:

Divide your target chip load by that factor to get the feed per tooth to program. At 10 percent radial engagement the factor is 0.6, so a .002″ target becomes about .0033″ programmed. Dormer’s published correction factor for 10 percent radial engagement is 1.67, which is the same math. For full slotting, go the other way and run below the chart’s chip load.

Worked Example: 1/2″ Carbide End Mill in 4140

Take a 1/2″, 4-flute carbide end mill roughing annealed 4140. Dormer publishes 365 SFM for this material with its S716 4-flute carbide end mill. Start a little under that, at 325 SFM.

  • RPM: (325 × 3.82) ÷ 0.5 = 2,483. Call it 2,480 RPM.
  • Chip load: Dormer’s feed table gives .0020″ per tooth for a 1/2″ tool in this material; Harvey publishes .0018″ uncoated for roughing this alloy group (at 29–37 Rc). Use .002″.
  • Feed rate: 2,480 × 4 × .002 = 19.8. Call it 20 IPM.

That is the whole system. SFM sets the pace based on the material. RPM translates that pace to the spindle based on tool diameter. Chip load protects the edge and sets how fast the tool moves through the part. If your radial engagement is light, adjust the chip load for chip thinning before you touch anything else.

When to Run Above or Below the Chart

Published speeds and feeds are the right starting point, not the finish line. A rigid setup on a heavy machine can sometimes push past the published number. A long stickout or a marginal fixture sometimes needs to back off. Start with the chart, then adjust from the cut (or the GUT, once you get comfortable). The chip and the finish can tell you which way to go.

Signs you are running too fast

Rapid flank wear, discolored chips, cratering, or a burned edge on the part. If the wear shows up early and evenly, speed is the first suspect. Our guide on how to diagnose end mill wear walks through what each wear pattern means.

Signs you are running too slow or rubbing

Built-up edge, a smeared finish, and squealing instead of cutting. In stainless and other work-hardening alloys, rubbing hardens the surface for the next pass and makes everything worse. Stop smoking your end mills covers the heat side of this.

Coolant and coating shift the number

How much heat you can pull out of the cut affects how hard you can push SFM. If you are deciding between flood coolant, MQL, or running dry, the tradeoffs are in Flood Coolant vs. MQL vs. Dry Machining. Coatings matter too: Harvey notes its chip loads are for uncoated tools and can go up 10 to 20 percent coated. See the cutting tool coatings guide for which coating suits which material, and Killing Chatter if vibration, not speed, is the real problem.

SFM for Drilling and Tapping

Drills and taps run on the same formula, but the numbers are lower and the range is tighter. A drill cuts at the center where surface speed falls to zero and has to clear chips from the bottom of a hole. A tap is pulling a full thread form at once and has to stop and reverse.

  • Carbide drills in steel typically start between 195 and 395 SFM in the chart above, depending on the maker and on whether coolant comes through the drill.
  • HSS-Co drills run much slower: OSG publishes 65–80 SFM for 4140 and 105–130 SFM for 1018.
  • Taps run slowest in the chart above. In 4140, OSG and Dormer publish 40–80 SFM for HSS-E machine taps. Coolant-through taps can run considerably faster in the right setup.

For tough materials, read How to Thread Inconel Without Breaking Taps. Indexable drills cover the larger hole sizes; see Indexable Tooling vs. Solid Carbide for where each one makes sense.

Watch: Max Math, CNC Speeds & Feeds Explained

Max walks through the same SFM, RPM and chip load math on camera, start to finish, with a real tool and a real material. If you would rather watch it than read it, start here.

SFM FAQ

What is SFM in machining?

SFM (surface feet per minute) is the speed of the cutting edge across the material, measured in feet per minute. It depends on the workpiece material and the tool, not the machine. Tool makers publish starting SFM ranges for each material.

What is the difference between SFM and RPM?

SFM is how fast the cutting edge moves. RPM is how fast the spindle turns. The same SFM means a different RPM for every tool diameter: RPM = (SFM × 3.82) ÷ diameter.

How do I convert SFM to RPM?

Multiply SFM by 3.82 and divide by the tool diameter in inches. At 300 SFM, a 1/2″ end mill runs (300 × 3.82) ÷ 0.5 = 2,292 RPM. In metric, RPM = (Vc × 1,000) ÷ (π × diameter in mm).

What does SFPM mean?

SFPM means surface feet per minute, the same as SFM. Two abbreviations, one unit.

What SFM should I run for mild steel with a carbide end mill?

Dormer publishes 560 SFM for 1018 with its S716 4-flute carbide end mill, and 755 SFM for free-machining steels like 12L14. Start mid-range for your tool and adjust from the cut.

What SFM should I run for aluminum?

Harvey Tool publishes 1,000 SFM for wrought aluminum with its miniature carbide end mills, and Dormer publishes 260–395 SFM for HSS end mills. Published aluminum ranges vary widely by tool and coating, so use the maker’s number for your tool.

What is chip load?

Chip load is the feed per tooth: how far the tool advances each time one cutting edge enters the cut, in inches. Too light and the edge rubs and overheats; too heavy and it chips. Feed rate is RPM × flutes × chip load.

Does SFM change for HSS vs. carbide?

Yes, a lot. In annealed 4140, Dormer publishes 365 SFM for its carbide end mill and 195 SFM for its HSS end mill. Coatings move the number too. See Carbide vs. HSS End Mills for when each makes sense.

Get the Tools

W.C. Chapman & Sons stocks cutting tools from Mitsubishi Materials, Iscar, Helical Solutions, Harvey Tool, Garr Tool, OSG, Dormer Pramet, and Emuge-Franken, all backed by published speeds and feeds data and a technical team that can help you dial in a specific application, not just hand you a chart.

Need it today? Maryland stock items are available for same-day will-call at our Rosedale location. Or call us at 410.686.6860 to talk through your setup with a member of our team.

Order online or talk to the team

The store is open around the clock. The sales desk is open Monday through Friday, 7:30am to 5:00pm EST.

Call (410) 686-6860 or write sales@wcchapman.com.