Feeds and Speeds Calculator
Work out spindle rpm, feed rate and material removal rate for milling, drilling and turning from the cutting speed, diameter, teeth and chip load. Pick the workpiece and cutter material to start from a published speed range, set your machine's top speed, and copy the setup line into the job notes.
Material and tool
Chart range: 800–1,500 SFM (Harvey Tool, Aluminum 2024, 6061, 7075). The speed boxes start at the middle.
These are general starting points. Start from your tool maker's data for the exact cutter, coating and machine.
Milling (end mill)
Prefilled from the chart for the material and cutter. Change it to your tool maker's figure.
Chart start for a 0.5 in cutter: 0.004 in/tooth.
Set to your machine's maximum. Leave empty for no limit.
When the width of cut is under half the cutter diameter, the chip is thinner than the feed per tooth. This raises the feed to keep the chart chip thickness.
Result
Spindle speed
8,785 rpm
1,150 SFM
Feed rate
105.4 IPM
Feed per tooth used: 0.004 in/tooth
Metal removal rate
13.18 in³/min
Setup line
Milling | Aluminum (6061, 7075), Carbide | Ø 0.5 in, z 3 | 8,785 rpm (1,150 SFM) | 105.4 IPM | 0.004 in/tooth | ae 0.25 × ap 0.5 in | 13.18 in³/min
Drilling
Prefilled from the chart for the material and cutter. Change it to your tool maker's figure.
Placeholder; take the feed per rev from the drill or insert maker's chart.
Set to your machine's maximum. Leave empty for no limit.
Result
Spindle speed
8,785 rpm
1,150 SFM
Feed rate
35.14 IPM
Metal removal rate
6.9 in³/min
Setup line
Milling | Aluminum (6061, 7075), Carbide | Ø 0.5 in, z 3 | 8,785 rpm (1,150 SFM) | 105.4 IPM | 0.004 in/tooth | ae 0.25 × ap 0.5 in | 13.18 in³/min
Turning (lathe)
Prefilled from the chart for the material and cutter. Change it to your tool maker's figure.
Placeholder; take the feed per rev from the drill or insert maker's chart.
Set to your machine's maximum. Leave empty for no limit.
Result
Spindle speed
2,196 rpm
1,150 SFM
Feed rate
17.57 IPM
Metal removal rate
5.52 in³/min
Setup line
Milling | Aluminum (6061, 7075), Carbide | Ø 0.5 in, z 3 | 8,785 rpm (1,150 SFM) | 105.4 IPM | 0.004 in/tooth | ae 0.25 × ap 0.5 in | 13.18 in³/min
Starting cutting speeds by material
Carbide ranges from Harvey Tool's machining guidelines; HSS from the LibreTexts cutting speed table (plastics: University of Pennsylvania). Middle of the range is where the boxes start.
| Material | High-speed steel (SFM) | Carbide (SFM) |
|---|---|---|
| Aluminum (6061, 7075) | 300–400 | 800–1,500 |
| Mild steel (1018, 1020) | 40–140 | 100–300 |
| Stainless steel (304, 316) | 60–70 | 100–250 |
| Gray cast iron | 50–80 | 100–400 |
| Brass | 200–350 | 800–1,500 |
| Plastics (acrylic) | 400 | 200–600 |
| Titanium (6Al-4V) | 20–60 | 50–250 |
Everything is worked out in your browser. Nothing you type is sent to ParrotNotes.
How the feeds and speeds calculator works
Spindle speed comes from the cutting speed and the diameter: RPM = SFM × 3.82 ÷ D, where 3.82 is 12 ÷ π (3.8197) and D is the cutter, drill or workpiece diameter in inches. In metric, n = Vc × 1,000 ÷ (π × D) with Vc in m/min and D in mm.
Milling feed is RPM × number of flutes × chip load, in inches per minute (metric: vf = n × z × fz in mm/min). The metal removal rate is width of cut × depth of cut × feed, in cubic inches per minute. Drilling and turning feed is RPM × feed per revolution, and turning removes 12 × SFM × feed per rev × depth of cut in cubic inches per minute.
Worked examples
A textbook case from LibreTexts: a 3/8 in two-flute HSS end mill in mild steel at 90 SFM. The book rounds 3.82 up to 4 and gets 90 × 4 ÷ 0.375 = 960 RPM and 0.002 × 2 × 960 = 3.84 IPM. With the exact factor it is 916.7 RPM and 3.67 IPM; the rounded rule runs about 5% fast.
A 1/2 in three-flute carbide end mill in 6061 aluminum at 1,150 SFM, the middle of Harvey Tool's 800 to 1,500 SFM range: 1,150 × 12 ÷ (π × 0.5) = 8,785 RPM. At the chart chip load of 0.004 in per tooth the feed is 105.4 IPM, and a 0.25 in wide, 0.5 in deep cut removes 13.18 cubic inches a minute.
When the machine tops out
Small carbide cutters in aluminum ask for more speed than many spindles have. A 1/4 in cutter at 1,150 SFM needs 17,571 RPM. On a 10,000 RPM machine the calculator caps the speed, warns you, and works the feed out from 10,000 RPM: the cutter then runs at 654 SFM, and three flutes at 0.002 in per tooth feed 60 IPM.
Keeping the chip load and dropping the feed with the speed keeps the cutter safe. Raising the feed to make up for the lost speed would overload each tooth.
Chip thinning at light widths of cut
When the width of cut is under half the cutter diameter, each tooth takes a chip thinner than the feed per tooth. The adjusted feed per tooth is fz × D ÷ (2 × √(D × ae − ae²)), where ae is the width of cut. A 1/2 in cutter at a 0.05 in width of cut (10%) gets a factor of 0.5 ÷ (2 × √(0.025 − 0.0025)) = 0.5 ÷ 0.3 = 1.67, so a chart chip load of 0.003 in becomes 0.005 in.
Tick the chip thinning box only for light radial cuts such as finishing or high-efficiency milling, and check the adjusted figure against the tool maker's maximum.
Where the starting speeds come from
Carbide speed ranges are from Harvey Tool's General Machining Guidelines (for example aluminum 2024, 6061 and 7075 at 800 to 1,500 SFM, 304 and 316 stainless at 100 to 250 SFM). HSS ranges are from the cutting speed table in LibreTexts' Manufacturing Processes 4-5, and HSS plastics from the University of Pennsylvania's mechanical engineering feeds and speeds guide. Chip loads at 1/8, 1/4 and 1/2 in come from that same Penn guide, which lists no cast iron, so the calculator suggests none.
These are general starting points from published charts. Start from your tool maker's data for the exact cutter, coating, stick-out and machine, and adjust by the sound and the chips.
Sources
Harvey Tool, General Machining Guidelines and Milling Formulas (RPM = 3.82 × SFM ÷ D, IPM = RPM × IPT × T). LibreTexts, Manufacturing Processes 4-5, Unit 2: Speeds, Feeds, and Tapping, Table 1. University of Pennsylvania MEAM, Feeds and Speeds guide (carbide and HSS end mill chip loads). Sandvik Coromant, Milling formulas and definitions and Turning formulas and definitions (n, vf, Q, maximum chip thickness).
Results are starting points; tool life and finish depend on more than the numbers. Rigidity, stick-out, coolant, coating and the machine all change what a cutter can take. Use the tool maker's speeds and feeds for the exact tool, and run guards and PPE as your shop requires.
Selling cutting tools, machines or industrial supplies? See industrial distributor sales, manufacturers' reps, what a sales engineer does, running a plant tour.
Keep the setup from the shop floor
On a shop visit or a call, the machinist reads out the material, cutter size and the speeds they run faster than you can type them. Record the conversation with ParrotNotes and you get a transcript, a summary and the action items, so the details for the tooling quote are already written down.
Get Started FreeRelated tools
- Horsepower and Torque CalculatorConvert torque and rpm to horsepower and back in lb-ft, N·m, hp, kW and PS, with gearbox and electric motor tabs and the 5,252 rule explained.Open the tool
- Steel Weight CalculatorWeigh steel, stainless, aluminum and other metals as plate, sheet, bar, tube, pipe or angle, per foot or meter, per piece and for the order.Open the tool