Construction

Speeds & Feeds Chart

Starting SFM (m/min) and chip loads for milling, turning and drilling with HSS and carbide, by material, plus RPM = 3.82 × SFM ÷ D and the feed formulas.

Spindle speed: RPM = SFM × 3.82 ÷ D (D in inches; 3.82 = 12 ÷ π), or RPM = 1000 × Vc ÷ (π × D) ≈ 318.3 × Vc ÷ D in metric (Vc in m/min, D in mm). Feed: in/min = RPM × number of teeth × chip load. Starting surface speeds for HSS end mills are 400–1,000 SFM in aluminum, 45–100 SFM in soft steel and 25–70 SFM in hard steel (US Army TC 9-524). Solid carbide end mills start at about 1,000 SFM in wrought aluminum, 600 SFM in free-machining steel, 200 SFM in alloy steel and 150 SFM in titanium (Harvey Tool, 29–37 HRC for the steels). These are starting values. Harvey says its figures "may be increased given optimal setup conditions", and the right number for a given job depends on the tool, its coating, the machine and how rigid the setup is. Example: a 1/2 in 4-flute carbide end mill in 4140 at 200 SFM runs at 1,528 RPM, and at Harvey's 0.00179 in/tooth it feeds at 10.9 in/min. To check a G-code program's S and F words, use the G-code Explainer & Simulator.

Speed and feed formulas

RPM (inch)RPM = SFM × 12 ÷ (π × D) = 3.82 × SFM ÷ D. D is the cutter diameter (milling, drilling) or the work diameter (turning), in inches. Sandvik Coromant: n = vc × 12 ÷ (π × DCap). TC 9-524 prints the same formula as 12 × SFM ÷ (3.1416 × D).
Why 3.82Each revolution moves the cutting edge π × D inches, or π × D ÷ 12 feet. RPM = SFM ÷ (π × D ÷ 12) = (12 ÷ π) × SFM ÷ D, and 12 ÷ π = 3.8197. TC 9-524 also gives a mental-arithmetic version, RPM ≈ 4 × SFM ÷ D, which runs about 4.7 % faster. Its RPM tables (8-2 and 4-4) use 3.82: for example 300 SFM with a 1/4 in drill = 4,584 RPM.
RPM (metric)n = Vc × 1000 ÷ (π × D) = 318.3 × Vc ÷ D (Vc in m/min, D in mm; 1000 ÷ π = 318.31). TC 9-524 rounds the constant to 320.
Surface speed from RPMSFM = π × D × RPM ÷ 12; Vc (m/min) = π × D × n ÷ 1000 (Sandvik Coromant).
Milling feedFeed (in/min or mm/min) = RPM × number of effective teeth × chip load per tooth. Sandvik: vf = fz × n × ZEFF.
Drilling and turning feedFeed (in/min) = RPM × feed per revolution (in/rev). Sandvik: fn = vf ÷ n.
Metal removal rateQ = axial depth × radial width × feed rate (in³/min); in metric, Q (cm³/min) = ap × ae × vf ÷ 1000 (Sandvik Coromant).
Unit conversionSFM × 0.3048 = m/min; m/min × 3.281 = SFM; in × 25.4 = mm.

HSS milling cutter speeds by material (TC 9-524 Table 8-1)

MaterialPlain mill, roughing (SFM)Plain mill, finishing (SFM)End mill, roughing (SFM)End mill, finishing (SFM)End mill, overall (m/min, calc.)
Aluminum400–1,000400–1,000400–1,000400–1,000122–305
Brass, composition125–20090–20090–15090–15027–46
Brass, yellow150–200100–250100–200100–20030–61
Bronze, phosphor and manganese30–8025–10030–8030–809–24
Cast iron, hard25–4010–3025–4020–456–14
Cast iron, soft and medium40–7525–8035–6530–809–24
Monel metal50–7550–7540–6040–6012–18
Steel, hard25–5025–7025–5025–708–21
Steel, soft60–12045–11050–8545–10014–30

Notes on HSS milling speeds

  • TC 9-524 gives these as approximate starting values for high-speed steel cutters. Its footnotes say to reduce them by 50 % for carbon-steel cutters and increase them by 100 % for carbide-tipped cutters.

Solid carbide end mill speeds and chip loads by material (Harvey Tool)

Material (examples)Hardness (HRC)Speed (SFM)Speed (m/min, calc.)Chip load, 1/4 in cutter, roughing (in/tooth)Chip load, 1/2 in cutter, roughing (in/tooth)
Aluminum, wrought
1xxx–3xxx, 5xxx–8xxx
≤ 28 HRC1,0003050.00316 (0.080 mm)0.00633 (0.161 mm)
Aluminum, castings
2xx, 5xx, 7xx, 8xx
≤ 28 HRC7502290.00316 (0.080 mm)0.00633 (0.161 mm)
Aluminum-silicon castings, 3–5 % Si
3xx, 4xx
≤ 28 HRC7502290.00285 (0.072 mm)0.00569 (0.145 mm)
Aluminum-silicon castings, 5–8 % Si
3xx, 4xx
≤ 28 HRC7002130.00285 (0.072 mm)0.00569 (0.145 mm)
Aluminum-silicon castings, 8–12 % Si
3xx, 4xx
≤ 28 HRC6501980.00285 (0.072 mm)0.00569 (0.145 mm)
Aluminum-silicon castings, 12–16 % Si
3xx, 4xx
≤ 28 HRC4751450.00285 (0.072 mm)0.00569 (0.145 mm)
Aluminum, wrought, 5–8 % Si
4xxx
≤ 28 HRC1,0003050.00285 (0.072 mm)0.00569 (0.145 mm)
Aluminum, wrought, 8–12 % Si
4xxx
≤ 28 HRC8002440.00285 (0.072 mm)0.00569 (0.145 mm)
Magnesium alloys≤ 28 HRC1,5004570.00316 (0.080 mm)0.00633 (0.161 mm)
Zinc alloys≤ 28 HRC8002440.00316 (0.080 mm)0.00633 (0.161 mm)
Brass
C2xxxx–C4xxxx, C66400–C69800
≤ 28 HRC5001520.00253 (0.064 mm)0.00506 (0.129 mm)
Aluminum and silicon bronzes
C60600–C66100
≤ 28 HRC5001520.00253 (0.064 mm)0.00506 (0.129 mm)
Cast copper alloys
C83300–C99700 (ranges)
≤ 28 HRC5501680.00253 (0.064 mm)0.00506 (0.129 mm)
High coppers, phosphor bronzes, copper-nickels
C1xxxx, C5xxxx, C7xxxx
≤ 28 HRC225690.00253 (0.064 mm)0.00506 (0.129 mm)
Free-machining and low-carbon steels
10xx–1029, 11xx–1139, 12xx, leaded grades
29–37 HRC6001830.00098 (0.025 mm)0.00196 (0.050 mm)
Medium/high-carbon and alloy steels
1030–1095, 13xx, 15xx, 2xxx–9xxx (e.g. 4140)
29–37 HRC200610.00089 (0.023 mm)0.00179 (0.045 mm)
Free-machining stainless
303, 416, 420F, 430F, 440F
29–37 HRC4501370.00098 (0.025 mm)0.00196 (0.050 mm)
Austenitic and ferritic stainless
304, 316, 321, 410, 430 and others
29–37 HRC200610.00089 (0.023 mm)0.00179 (0.045 mm)
Austenitic and ferritic stainless38–45 HRC100300.00045 (0.011 mm)0.00089 (0.023 mm)
Martensitic and PH stainless
414, 431, 440A–C, 13-8, 15-5, 17-4, 17-7
29–37 HRC150460.00056 (0.014 mm)0.00112 (0.028 mm)
Martensitic and PH stainless38–45 HRC90270.00028 (0.007 mm)0.00056 (0.014 mm)
Tool steels, A, L, O, P, W series29–37 HRC200610.00089 (0.023 mm)0.00179 (0.045 mm)
Tool steels, A, L, O, P, W series38–45 HRC100300.00045 (0.011 mm)0.00089 (0.023 mm)
Tool steels, D, H, M, T, S series29–37 HRC150460.00056 (0.014 mm)0.00112 (0.028 mm)
Tool steels, D, H, M, T, S series38–45 HRC90270.00028 (0.007 mm)0.00056 (0.014 mm)
Titanium alloys29–37 HRC150460.00056 (0.014 mm)0.00112 (0.028 mm)
Titanium alloys38–45 HRC75230.00028 (0.007 mm)0.00056 (0.014 mm)
High-temperature alloys
Inconel, Hastelloy, Waspaloy, Monel, Incoloy
29–37 HRC70210.00056 (0.014 mm)0.00112 (0.028 mm)
High-temperature alloys38–45 HRC50150.00028 (0.007 mm)0.00056 (0.014 mm)

Carbide end mill chip load by operation (Harvey Tool)

Material groupSlotting, Ø 1/8 / 1/4 / 1/2 in (in/tooth)Roughing, Ø 1/8 / 1/4 / 1/2 in (in/tooth)Finishing, Ø 1/8 / 1/4 / 1/2 in (in/tooth)
Aluminum (wrought and 2xx/5xx/7xx/8xx castings), magnesium, zinc0.00121 / 0.00242 / 0.004840.00158 / 0.00316 / 0.006330.00174 / 0.00348 / 0.00695
High-silicon aluminum0.00109 / 0.00218 / 0.004360.00142 / 0.00285 / 0.005690.00156 / 0.00313 / 0.00626
Copper alloys0.00097 / 0.00194 / 0.003870.00127 / 0.00253 / 0.005060.00139 / 0.00278 / 0.00556
Free-machining steel and stainless0.00042 / 0.00083 / 0.001660.00049 / 0.00098 / 0.001960.00054 / 0.00109 / 0.00217
Alloy steel, austenitic stainless, A/L/O/P/W tool steel (29–37 HRC)0.00038 / 0.00076 / 0.001520.00045 / 0.00089 / 0.001790.00050 / 0.00099 / 0.00199
Martensitic/PH stainless, D/H/M/T/S tool steel, titanium, high-temp alloys (29–37 HRC)0.00024 / 0.00048 / 0.000950.00028 / 0.00056 / 0.001120.00031 / 0.00062 / 0.00124

Notes on the carbide figures

  • Harvey Tool's chart is for its uncoated solid carbide square end mills, 1/64–1/2 in, 4 flutes, 1.5 × D length of cut (series 140xx and 503xx). Harvey publishes a separate chart for each tool family (flute count, length of cut, reach), with different chip loads, so check the chart for the cutter you have.
  • The depths of cut behind those chip loads, for 1/16–1/2 in cutters, are: slotting at full width and 0.5 × D deep; roughing at 0.6 × D radial and 1 × D axial; finishing at 0.25 × D radial and 1 × D axial.
  • Harvey notes that chip loads may be raised 10–20 % for coated cutters, and 10–20 % for ferrous materials at or below 28 HRC. The steel rows are printed for 29–37 HRC and 38–45 HRC; free-machining and carbon/alloy steels have no 38–45 HRC entry.
  • The two sources differ a lot. TC 9-524 (1996) gives 45–100 SFM for HSS end mills in soft steel and says to double it for carbide-tipped cutters, about 90–200 SFM. Harvey's current solid carbide chart gives 600 SFM for free-machining steel and 200 SFM for alloy steel. Modern coated carbide runs much faster than the older guidance, so use the tool maker's own chart where you have one.

Chip load per tooth by cutter type: HSS (TC 9-524 Table 8-3)

Cutter (HSS)Aluminum (in/tooth)Bronze (in/tooth)Cast iron (in/tooth)Free-machining steel (in/tooth)Alloy steel (in/tooth)
Face mills.007–.022.005–.014.004–.016.003–.012.002–.008
Helical mills.006–.018.003–.011.004–.018.002–.010.002–.007
Side cutting mills.004–.013.003–.008.002–.009.002–.007.001–.005
End mills.003–.011.003–.007.002–.008.001–.006.001–.004
Form relieved cutters.002–.007.001–.004.002–.005.001–.004.001–.003
Circular saws.002–.005.001–.003.001–.004.001–.003.005–.002 *

Chip load per tooth by cutter type: carbide (TC 9-524 Table 8-3)

Cutter (carbide)Aluminum (in/tooth)Bronze (in/tooth)Cast iron (in/tooth)Free-machining steel (in/tooth)Alloy steel (in/tooth)
Face mills.007–.020.004–.012.006–.020.004–.016.003–.014
Helical mills.006–.016.004–.010.002–.018.003–.013.003–.012
Side cutting mills.004–.012.003–.007.003–.012.003–.009.002–.008
End mills.003–.010.002–.006.003–.010.002–.008.002–.007
Form relieved cutters.002–.006.001–.004.002–.006.002–.005.001–.004
Circular saws.002–.005.001–.003.002–.006.001–.004.001–.004

Notes on chip load

  • Chip load (feed per tooth) is the thickness of material each cutting edge removes per revolution. Multiply by 25.4 for mm/tooth: 0.004 in = 0.10 mm.
  • * TC 9-524 prints ".005 to .002" for HSS circular saws in alloy steel, with the larger number first. Every other cell runs small to large, and the carbide cell for the same case is .001–.004, so the first figure is probably a misprint for .0005. It is shown as printed.

HSS lathe turning and threading speeds (TC 9-524 Table 7-2)

MaterialTurning (SFM)Turning (m/min)Threading (SFM)Threading (m/min)
Low-carbon steel80–10024.4–30.535–4010.7–12.2
Medium-carbon steel60–8018.3–24.425–307.6–9.1
High-carbon steel35–4010.7–12.215–204.6–6.1
Stainless steel40–5012.2–15.215–204.6–6.1
Aluminum and its alloys200–30061.0–91.450–6015.2–18.3
Ordinary brass and bronze100–20030.5–61.040–5012.2–15.2
High-tensile bronze40–6012.2–18.320–256.1–7.6
Cast iron50–8015.2–24.420–256.1–7.6
Copper60–8018.3–24.420–256.1–7.6

Notes on turning speeds

  • These speeds are for HSS tool bits under normal lathe conditions, with normal feeds and depths of cut. TC 9-524 says to use the low end of each range for roughing and the high end for finishing, and that carbide-tipped bits can run 2 to 3 times as fast.
  • In turning, D is the diameter being cut, not the stock size. A 1/2 in aluminum bar at 200 SFM runs at 3.82 × 200 ÷ 0.5 = 1,528 RPM (TC 9-524 rounds this to 1,600 RPM with its 4 × SFM ÷ D shortcut).

HSS drill speeds by material (TC 9-524 Table 4-2)

MaterialCutting speed (SFM)Cutting speed (m/min, calc.)RPM for a 1/2 in (12.7 mm) drill (calc.)
Aluminum and alloys200–30061–911,528–2,292
Armor plate40–5012–15 *306–382
Brass200–30061–911,528–2,292
Bronze200–30061–911,528–2,292
Bronze, high tensile70–15021–46535–1,146
Cast iron, soft100–15030–46764–1,146
Cast iron, medium70–10021–30535–764
Cast iron, hard70–10021–30535–764
Cast iron, chilled30–409–12229–306
Copper200–30061–911,528–2,292
Copper-graphite alloy (carbide drills)60–7018–21458–535
Glass (carbide drills)20–306–9153–229
Iron, malleable50–9015–27382–688
Magnesium and alloys250–40076–1221,910–3,056
Monel30–509–15 *229–382
Nickel alloys40–6012–18306–458
Plastic, hot set100–30030–91764–2,292
Plastic, cold set100–30030–91764–2,292
Steel, low carbon (0.2–0.3 % C)80–11024–34611–840
Steel, medium carbon (0.4–0.5 % C)70–8021–24535–611
Steel, high carbon (1.2 % C)50–6015–18382–458
Steel, forged50–6015–18382–458
Steel, alloy50–7015–21382–535
Steel, alloy 300–400 Brinell20–306–9153–229
Stainless steel, free machining30–809–24229–611
Stainless steel, hard15–505–15115–382
Steel, manganese12–154–592–115
Stone (carbide drills)25–308–9191–229
Wood300–40091–1222,292–3,056

Drill feed per revolution by drill size (TC 9-524 Table 4-4)

Drill diameter (in)Drill diameter (mm)Feed (in/rev)Feed (mm/rev)RPM in mild steel at 110 SFM (calc.)
1/161.60.00150.0386,723
1/83.20.002–0.0030.051–0.0763,361
3/164.80.00400.1022,241
1/46.40.00500.1271,681
5/167.90.00500.1271,345
3/89.50.00600.1521,120
7/1611.10.00700.178960
1/212.70.00800.203840
9/1614.30.00800.203747
5/815.90.00900.229672
11/1617.50.00900.229611
3/419.10.01000.254560
13/1620.60.01000.254517
7/822.20.01100.279480
15/1623.80.01200.305448
125.40.01300.330420
1-1/431.80.01500.381336
1-1/238.10.01500.381280
1-3/444.50.01600.406240
250.80.01600.406210

Notes on drilling

  • The drill speeds are for high-speed steel drills except where carbide drills are named. TC 9-524 says rotational speeds for carbide twist drills are 200 to 300 percent higher. In its own RPM examples it uses the slower end of each range, because of variations in setup rigidity, machine size and required finish.
  • * Two metric figures in Table 4-2 do not match the ft/min column (armor plate: 12.20–18.25 m/min printed for 40–50 ft/min; Monel: 4.15–15.28 m/min printed for 30–50 ft/min). The m/min column here is calculated from ft/min × 0.3048 for every row.
  • Feed per revolution rises with drill diameter, from 0.0015 in at 1/16 in to 0.016 in at 1-1/2 in and above. Table 4-4 gives one feed per diameter for all materials; TC 9-524 adds that the best feed depends on the drill size, the material and the condition of the drilling machine.
  • For the drill point angle to grind for each material, see twist drill point angles. For tap drill sizes, see the inch and metric tap drill charts.

Sources

  • Headquarters, Department of the Army, TC 9-524, Fundamentals of Machine Tools, 1996 (armypubs.army.mil/epubs/DR_pubs/DR_a/pdf/web/tc9_524.pdf). Used for: Table 4-2 (HSS drill cutting speeds), Table 4-4 (drill feeds and RPM), Table 7-2 (HSS turning and threading speeds), Table 8-1 (HSS milling cutter speeds), Table 8-2 (cutter RPM) and Table 8-3 (chip per tooth, HSS and carbide), plus the RPM formulas on pp. 4-17 and 7-26.
  • Harvey Tool (Harvey Performance Company), Speeds & Feeds: Miniature End Mills – Square – Stub & Standard, 1.5x Length of Cut, 4 Flutes (series 140xx, 503xx), chart SF_14000, viewed October 2026 (harveyperformance.widen.net/content/bp6raj7qwr/pdf/SF_14000.pdf). Used for: solid carbide end mill SFM and chip load per tooth by workpiece material and hardness.
  • Sandvik Coromant, Milling formulas and definitions, viewed October 2026 (sandvik.coromant.com/en-us/knowledge/machining-formulas-definitions/milling-formulas-definitions). Used for: spindle speed n = vc × 1000 ÷ (π × DCap) in metric and n = vc × 12 ÷ (π × DCap) in inch units; cutting speed vc = π × DCap × n ÷ 1000 (m/min) or ÷ 12 (ft/min); table feed vf = fz × n × ZEFF (effective number of teeth); metal removal rate Q = ap × ae × vf (÷ 1000 for cm³/min).
  • Earlier versions of this page gave SFM ranges, chip loads by diameter, lathe feeds and rules of thumb with no source. They have been replaced by the published figures above.

Frequently asked questions

How do you calculate RPM from SFM?

RPM = SFM × 12 ÷ (π × D), with D in inches, which simplifies to RPM = 3.82 × SFM ÷ D. A 1/2 in cutter at 100 SFM runs at 3.82 × 100 ÷ 0.5 = 764 RPM, the figure in TC 9-524 Table 8-2. In metric units, RPM = 1000 × Vc ÷ (π × D) = 318.3 × Vc ÷ D, with Vc in m/min and D in mm.

Where does the 3.82 in the RPM formula come from?

It is 12 ÷ π = 3.8197. One revolution moves the cutting edge π × D inches, which is π × D ÷ 12 feet, so RPM = SFM ÷ (π × D ÷ 12) = 12 × SFM ÷ (π × D). TC 9-524 rounds the constant up to 4 for mental arithmetic, which gives about 4.7 % more speed. Its own RPM tables use 3.82.

What SFM should I use for aluminum and steel?

HSS end mills (TC 9-524 Table 8-1): aluminum 400–1,000 SFM, soft steel 45–100 SFM, hard steel 25–70 SFM, soft cast iron 30–80 SFM. Solid carbide end mills (Harvey Tool): 1,000 SFM in wrought aluminum, 600 SFM in free-machining steel and 200 SFM in alloy steel at 29–37 HRC. Both are starting values.

How do I calculate the feed rate in inches per minute?

Feed (in/min) = RPM × number of teeth × chip load (in/tooth). For a 1/2 in, 4-flute carbide end mill in 4140 at 200 SFM: RPM = 3.82 × 200 ÷ 0.5 = 1,528, and with Harvey's roughing chip load of 0.00179 in, feed = 1,528 × 4 × 0.00179 = 10.9 in/min.

What chip load should I use for an end mill?

TC 9-524 Table 8-3 gives 0.003–0.011 in/tooth for HSS end mills in aluminum, 0.001–0.006 in free-machining steel and 0.001–0.004 in alloy steel. Carbide end mills get 0.003–0.010, 0.002–0.008 and 0.002–0.007 in. Harvey Tool's figures for 1/2 in 4-flute carbide end mills when roughing are 0.00633 in for aluminum and 0.00179 in for alloy steel.

Was this article helpful?