Speeds and Feeds
How fast to spin the tool and how fast to push it: cutting speeds, chip loads and the formulas behind them, for milling, drilling, turning and routers, with worked numbers.
Every cut comes down to two numbers. Speed is how fast the cutting edge moves across the material (the surface speed), which sets the spindle RPM. Feed is how far the tool advances per tooth or per revolution, which sets the chip thickness. Get the speed wrong and the tool overheats and wears out; get the feed wrong and the tool either rubs and glazes or is overloaded and breaks. This guide takes the subject in eleven pages: the basic formulas, chip load and chip thinning, data by material, cutting force and power, tool life and economics, tool materials and geometry, holes, turning, coolant, hobby machines and routers, and how to dial in a cut and fix chatter. Every worked number is computed so that you can check your own setup. The machines, workholding, G-code and CAM are in CNC Machining; the values here are starting points, and the tool maker’s data for the tool you bought always wins.
Start here: what do you need?
| I need to… | Go to |
|---|---|
| turn a surface speed into RPM, or a chip load into a feed rate | Cutting Speed, Spindle Speed and Feed Rate |
| choose a stepover, or understand why a light cut needs more feed | Chip Load, Chip Thinning and Engagement |
| look up starting speeds and chip loads for a material | Speeds and Feeds by Material |
| check whether my machine has the power and torque | Cutting Force, Power and Torque |
| make a tool last, or find the cheapest speed per part | Tool Life, Wear and Cutting Economics |
| choose between HSS, carbide and coatings, or understand rake and relief | Tool Materials, Coatings and Geometry |
| drill, ream, tap or bore a hole | Drilling, Reaming, Tapping and Boring |
| set up turning or threading, or predict the finish | Turning, Threading and Surface Finish |
| decide on coolant, mist or air, or clear chips from a pocket | Coolant, Lubrication and Chip Evacuation |
| set up a router or a small hobby machine | CNC Routers and Hobby Machines |
| fix chatter, bad finish or broken tools | Dialling In: Chatter, Rigidity and Troubleshooting |
A suggested order
Start with Cutting Speed, Spindle Speed and Feed Rate and Chip Load, Chip Thinning and Engagement (the two ideas everything else uses), then Speeds and Feeds by Material for starting numbers. Cutting Force, Power and Torque, Tool Life, Wear and Cutting Economics and Tool Materials, Coatings and Geometry explain what limits a cut; Drilling, Reaming, Tapping and Boring, Turning, Threading and Surface Finish and CNC Routers and Hobby Machines apply it to each process; Coolant, Lubrication and Chip Evacuation and Dialling In: Chatter, Rigidity and Troubleshooting finish with the shop floor.
- Cutting Speed, Spindle Speed and Feed Rate: Surface speed and RPM, feed per tooth and per revolution, feed rate, metal removal rate and the unit conversions between metric and inch.
- Chip Load, Chip Thinning and Engagement: Chip thickness, why a light radial cut needs a higher feed, arc of engagement, high-efficiency milling and how to choose a stepover.
- Speeds and Feeds by Material: Starting surface speeds and chip loads for aluminum, steels, stainless, titanium, cast iron, brass, plastics and wood, for HSS and carbide.
- Cutting Force, Power and Torque: Specific cutting force, how it rises as the chip gets thin, spindle power and torque checks, and whether the machine can take the cut.
- Tool Life, Wear and Cutting Economics: Taylor tool life, how speed shortens life, the cost-per-part and production-rate speeds, and when to change an edge.
- Tool Materials, Coatings and Geometry: HSS, cobalt, carbide, ceramic, CBN and diamond; coatings; rake and relief angles, flutes, helix and edge preparation.
- Drilling, Reaming, Tapping and Boring: Drill speeds and feeds, thrust and torque, pecking, reaming, tapping speeds, boring bars and hole accuracy.
- Turning, Threading and Surface Finish: Surface speed and feed per revolution, depth of cut, constant surface speed, threading, nose radius and the finish you get.
- Coolant, Lubrication and Chip Evacuation: Where the heat goes, flood, mist and air, minimum-quantity lubrication, chip control and clearing chips from a pocket.
- CNC Routers and Hobby Machines: Feeds and speeds for routers, small mills and desktop CNCs: limited rigidity, high RPM, plastics, wood and aluminum.
- Dialling In: Chatter, Rigidity and Troubleshooting: Listening to the cut, chatter and stability, rigidity, how to adjust speed and feed one step at a time, and a troubleshooting table.
The two numbers behind every cut
Surface speed depends on the material and the tool; the RPM follows from the diameter. The feed is set by the chip load the tool can take, not by what feels fast. The CNC Feeds and Speeds Calculator does the arithmetic; the pages here explain it so that you can judge the answer.
A first cut in five steps
Worked example: slotting 6061 aluminum with a 12 mm three-flute carbide end mill
- 1. Pick the surface speed from the material data (see Speeds and Feeds by Material): carbide in aluminum starts at about 300 m/min.
- 2. Turn it into RPM: n = 1 000 × 300 ÷ (π × 12) = 7 958 rpm. If the spindle tops out at 12 000 rpm, run at that limit (452 m/min) and keep the chip load.
- 3. Pick the chip load: about 0.08 mm per tooth for a 12 mm tool in aluminum.
- 4. Find the feed rate: Vf = n × z × fz = 7 958 × 3 × 0.08 = 1 910 mm/min (2 880 mm/min at the 12 000 rpm limit).
- 5. Check the load: a 6 mm deep, full-width slot removes 6 × 12 × 1 910 ÷ 1 000 = 138 cm³/min and needs about 3.2 kW at the cutter (see Cutting Force, Power and Torque). Reduce the depth if the machine cannot supply it, and listen to the cut (see Dialling In: Chatter, Rigidity and Troubleshooting).
Quick reference: formulas
| What you need | Metric | Inch |
|---|---|---|
| Spindle speed | n = 1 000 Vc ÷ (π D) | RPM = 12 SFM ÷ (π D) ≈ 3.82 SFM ÷ D |
| Milling feed rate | Vf = n z fz | IPM = RPM × teeth × chip load |
| Drilling and turning feed rate | Vf = n f | IPM = RPM × IPR |
| Metal removal rate, milling | Q = ap ae Vf ÷ 1 000 (cm³/min) | in³/min = depth × width × IPM |
| Chip thinning | fz = chip load × D ÷ (2 √(D ae − ae²)) | Same |
| Cutting power | Pc = Q kc ÷ 60 000 (kW, Q in cm³/min, kc in N/mm²) | hp = in³/min × unit power (hp per in³/min) |
| Tool life (Taylor) | V Tn = C | Same |
| Turned finish | Ra ≈ f² ÷ (32 r) | Ra ≈ f² ÷ (32 r) |
D is the tool diameter (or the workpiece diameter when turning), z the number of teeth, fz the feed per tooth, ap the axial depth of cut, ae the radial depth, kc the specific cutting force of the material and r the tool nose radius. Details and worked examples are on the pages above.
Related guides and tools
- CNC Machining: the machines, workholding, G-code, CAM and design for milling and turning.
- Material Properties (in the Structures guide): strength, hardness and thermal properties that set the cutting data.
- Tolerances by Process and Surface Finish: what finish and accuracy each process holds.
- CNC Feeds and Speeds Calculator, Lathe Turning Calculator and Tap Drill Calculator.
- Laser Cutting and 3D Printing: the processes that avoid cutting forces.
- Shop Tools: the drill press speeds, workholding and measuring that go with a good cut.
Safety first
- A tool that breaks throws pieces at tip speed. Use a guard or an enclosure, wear safety glasses, and keep your face out of the line of the cutter (see Machine and Hand Tool Safety).
- No gloves, loose sleeves or long hair near rotating tools; keep a hand on the stop for the first run of any program.
- Hold the work properly (see Workholding and Fixturing) and never clear chips by hand while the spindle is turning.
- The numbers here are starting values. Follow the machine and tool makers’ limits, begin conservatively and increase one parameter at a time.
FAQ
What is the difference between speed and feed?
Speed is how fast the cutting edge moves past the material (surface speed, which sets the RPM). Feed is how far the tool advances per tooth or per revolution (which sets the chip thickness). See Cutting Speed, Spindle Speed and Feed Rate.
Why do two charts give different speeds for the same material?
Because speeds depend on the tool material, coating, geometry, coolant and rigidity, and charts are conservative or aggressive by design. Use the chart for the tool you have, and treat any number as a starting point. See Speeds and Feeds by Material.
Why is my small cutter breaking?
Usually too little chip load (the edge rubs and heats), too deep a cut, too much stick-out or chips packed in the flutes. See Dialling In.
My spindle cannot reach the calculated RPM. What now?
Run at the maximum RPM and keep the chip load the same: the feed rate drops with the RPM. See CNC Routers and Hobby Machines.
Where did the old Speeds and Feeds sections go?
All of them are in this guide with much more depth: the formulas, the RPM tables, chip thinning, drilling, turning and routers each have their own page.
References
- Oberg, E., et al., Machinery’s Handbook, Industrial Press (cutting speeds and feeds, tool materials, power).
- Sandvik Coromant, Metal Cutting Technology and Modern Metal Cutting (specific cutting force kc1 and mc, chip thickness).
- Kalpakjian, S. and Schmid, S., Manufacturing Engineering and Technology, Pearson; Trent, E. M. and Wright, P. K., Metal Cutting, Butterworth-Heinemann.
- Taylor, F. W., On the Art of Cutting Metals, ASME (1907); ISO 3685 (tool-life testing with single-point turning tools).
Last reviewed: November 2026. All speeds, feeds and cutting forces are typical starting values: use your tool maker’s data and your own machine’s limits, and test on scrap.