United Kingdom version. Opens in metric (Vc in m/min, feed per tooth in mm, feed in mm/min) as UK tooling catalogues and CNC controls use it, with HSE guidance on lathes and metalworking fluids. US version
Cutting Speed and Feed Calculator (UK)
Spindle speed from cutting speed in m/min, table feed in mm/min, chip thinning and removal rate for milling, drilling and turning, set up in metric.
The interactive tool loads here when JavaScript runs.
About this toolWhat is the Speeds and Feeds Calculator?
UK cutter catalogues and CNC controls work in metric: cutting speed Vc in metres per minute, feed per tooth fz in millimetres and table feed in millimetres per minute. This version starts there, with a 10 mm three-flute carbide end mill in 6082 or 6061 aluminium.
At the preset 244 m/min that cutter wants 7,767 rpm (n = 1000 × Vc / (π × D)). Taking a 1 mm radial step at full 10 mm depth, chip thinning lifts the programmed feed per tooth from 0.08 to 0.133 mm and the feed to 3,107 mm/min, removing about 31 cm³ a minute. Put a 4,000 rpm limit on the machine, as on many small bench mills, and the tool can only reach 126 m/min, so the feed halves to 1,600 mm/min.
Drilling and turning work the same way. A 10 mm HSS jobber drill in mild steel runs at 872 rpm and 113 mm/min, and turning a 50 mm bar with carbide at 107 m/min needs 681 rpm. The presets are cautious starting points; your tool supplier's figures for that grade of insert or cutter always win.
- Milling, drilling and turning with inch (SFM, in/min) or metric (m/min, mm/min) units
- Conservative starting surface speeds and chip loads for ten common materials, HSS and carbide
- Radial chip thinning compensation for light stepovers
- Machine RPM limit with the resulting real surface speed
- Feed per revolution, material removal rate, formula panel, copy and share
Updated
How to use the Speeds and Feeds Calculator
- Choose inch or metric units and the operation: milling, drilling or turning.
- Pick the work material and tool material. The surface speed and chip load fill in from the presets; overwrite them with your tool maker's numbers if you have them.
- Enter the cutter, drill or workpiece diameter, the number of teeth for milling, and the depth and width of cut.
- Set your machine's maximum RPM so the calculator can cap the spindle speed, and choose whether to compensate for chip thinning.
- Read the RPM, feed rate, feed per revolution and metal removal rate, then copy the numbers into your program or CAM setup.
Worked examples
Side milling 6082 aluminium
Input
10 mm 3-flute carbide, Vc 244 m/min, fz 0.08 mm, ae 1 mm, ap 10 mm, chip thinning on
Output
7,767 rpm; factor 1.667; feed 3,107 mm/min; 31.07 cm³/min
A 10% radial step makes each chip only 60% as thick as the programmed feed, so the calculator raises fz to 0.133 mm to keep the chip at 0.08 mm.
Same cut on a 4,000 rpm bench mill
Input
As above with machine maximum 4,000 rpm
Output
4,000 rpm; real Vc 125.7 m/min; feed 1,600 mm/min; 16 cm³/min
Keep the feed per tooth and accept the lower feed rate. Raising fz to "make up" the speed overloads the edge.
Tapping drill for M10 in mild steel
Input
Drilling, 8.5 mm HSS, Vc 27.4 m/min, 0.13 mm/rev
Output
1,026 rpm; feed 133 mm/min
The 8.5 mm hole for an M10 x 1.5 thread. On a pillar drill with belt steps, take the nearest step below 1,026 rpm.
Turning a 50 mm mild steel bar
Input
Turning, 50 mm, carbide 107 m/min, 0.2 mm/rev, 1.5 mm depth of cut
Output
681 rpm; feed 136 mm/min; 32.1 cm³/min
With an HSS tool at 27.4 m/min the same bar runs at 174 rpm and removes only 8.2 cm³/min, a quarter of the carbide rate at the same feed and depth.
Background and insight
Spindle speed comes from the circumference of the tool or workpiece. In inch units n = 12 × SFM / (π × D), often rounded to the shop rule 3.82 × SFM / D or even 4 × SFM / D. In metric n = 1000 × Vc / (π × D) with Vc in m/min and D in mm. Feed rate is then rpm × number of teeth × chip load for milling and rpm × feed per revolution for drilling and turning.
The starting surface speeds in the presets are deliberately conservative. HSS values follow the shop tables derived from Machinery's Handbook that appear in many machine manuals, such as 90 SFM for mild steel and 300 SFM for aluminium; carbide values are about 2.5 to 3 times higher for general-purpose tools. Modern coated carbide in a rigid CNC can run much faster, so treat the preset as the low end and follow your cutter maker's data.
Radial chip thinning is the main correction. When the width of cut ae is less than half the cutter diameter, each tooth enters at a shallow angle and the maximum chip thickness is less than the programmed feed per tooth. Multiplying the feed by D / (2√(D·ae − ae²)) restores the intended chip. Ignore it and light finishing passes rub instead of cut, which shortens tool life in stainless and titanium.
Common use cases
CNC programming
Get RPM and feed for a new tool and material before running the first part, then fine-tune from the chips.
Manual mills and lathes
Pick the nearest belt or gear speed for a drill or end mill and set a sensible hand feed.
Hobby and benchtop machines
See when a low spindle limit forces you to drop surface speed, and keep chip load up so tools cut instead of rub.
Estimating cycle time
Use the metal removal rate and feed to estimate roughing time and compare tool options.
Tips and limitations
- HSE says it is never acceptable to hold emery cloth by hand on a rotating lathe workpiece; use a loop of cloth clamped in a holder on the tool post for outside work, or cloth wrapped on a holder in the boring bar position for bores.
- HSE warns that metalworking fluids can cause dermatitis and lung disease such as occupational asthma, and that health surveillance should be in place where exposure to fluid or mist cannot be prevented.
- Insert boxes and cutter catalogues often print Vc as a range for each material group. Start at the low end and raise it while watching wear and chip colour.
- Cutters over about three diameters of stick-out deflect; cut speed and feed back and take lighter radial steps.
Sources and further reading
- Using emery cloth on metalworking lathes, Health and Safety Executive. Hand-held emery cloth on rotating lathes is never acceptable; approved holder methods.
- Ill health from metalworking and water-mix wash fluids, Health and Safety Executive. Dermatitis, occupational asthma and hypersensitivity pneumonitis; health surveillance.
- Milling formulas and definitions, Sandvik Coromant. Metric spindle speed, table feed and chip thinning formulas.
Frequently asked questions
How do I convert cutting speed in m/min to RPM?
RPM = 1000 × Vc / (π × D), with Vc in m/min and D in mm. A 10 mm cutter at 244 m/min runs at 1000 × 244 / (π × 10) = 7,767 rpm. A quick shop version is RPM ≈ 318 × Vc / D.
What cutting speed should I use for mild steel with HSS?
The preset is 27.4 m/min, a cautious figure for plain HSS. That gives 872 rpm for a 10 mm drill and 174 rpm for turning a 50 mm bar. Coated HSS and carbide run several times faster.
What is feed per tooth (fz) and how does it give mm/min?
Feed per tooth is the chip each cutting edge takes, in millimetres. Table feed vf = rpm × number of teeth × fz, so 7,767 rpm × 3 × 0.08 mm is 1,864 mm/min before any chip-thinning correction.
Why does a light finishing pass need a higher feed?
When the radial step is under half the cutter diameter, the chip is thinner than fz. With a 1 mm step on a 10 mm cutter the factor is 1.667, so the feed rises to 3,107 mm/min. Without it the edge rubs, which wears tools fast in stainless.
My bench mill only reaches 4,000 rpm. What should I change?
Run at 4,000 rpm and keep fz the same. The feed drops in proportion (3,107 to 1,600 mm/min in the aluminium example) and so does removal rate, but the tool is safe. A smaller cutter or more flutes helps recover output.
Is it safe to polish work in the lathe with emery cloth?
Not by hand on a rotating chuck. HSE guidance says hand-held emery cloth on a turning CNC or manual lathe is never acceptable, because the cloth can snag and wrap round the work, taking the hand with it. Clamp a loop of cloth in a holder on the tool post instead.
Is there an in-depth guide to the Speeds and Feeds Calculator?
Yes. “Speeds and Feeds for Milling, Drilling and Turning, From First Principles” covers the background, how it works, common pitfalls and worked examples. Read the full guide.
Related Tools You May Like
Free, in-browser tools that pair well with this one.