Speeds and Feeds Calculator
Spindle RPM from surface speed, feed rate from chip load, chip thinning and metal removal rate for milling, drilling and turning, with material starting speeds.
The interactive tool loads here when JavaScript runs.
About this toolWhat is the Speeds and Feeds Calculator?
Every machining recipe starts with two numbers: how fast the cutting edge moves through the material (surface speed) and how thick a chip each edge takes (chip load or feed per revolution). From those, the spindle speed and the table feed follow by simple arithmetic. This calculator does that arithmetic for milling, drilling and turning in inch or metric units, and adds the corrections that catch people out: radial chip thinning on light stepovers and the speed limit of your spindle.
Choose the work material and HSS or carbide and the calculator fills in a conservative starting surface speed and chip load. The default, a 1/2 inch three-flute carbide end mill in aluminium at 800 SFM, runs at 6,112 rpm. With 0.004 in per tooth and a 0.1 in stepover, chip thinning raises the programmed chip load to 0.005 in and the feed to 91.7 in/min, removing 2.29 cubic inches a minute at 0.25 in deep.
If the ideal RPM is above your machine's maximum, the calculator caps it, shows the real surface speed you will get and recalculates the feed so the chip load stays where you set it.
- 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
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
Aluminium slotting and side milling
Input
1/2 in 3-flute carbide, 800 SFM, 0.004 in/tooth, 0.1 in stepover, 0.25 in deep
Output
6,112 rpm; chip thinning 1.25x; feed 91.7 in/min; MRR 2.29 in³/min
Without the chip-thinning correction the feed would be 73.3 in/min and each tooth would take a 0.0032 in chip.
Drilling mild steel with HSS
Input
1/4 in HSS drill, 90 SFM, 0.005 in/rev
Output
1,375 rpm; feed 6.9 in/min
The shortcut 4 × 90 / 0.25 gives 1,440 rpm, close enough for a drill press with stepped pulleys.
Turning a 50 mm bar
Input
Metric, 200 m/min carbide, 50 mm diameter, 0.25 mm/rev, 2 mm depth
Output
1,273 rpm; feed 318 mm/min; MRR 100 cm³/min
Keep surface speed constant as the diameter drops by using constant surface speed (G96) on a CNC lathe.
Small end mill on a slow spindle
Input
1/8 in carbide in mild steel, 350 SFM, machine limit 10,000 rpm
Output
Ideal 10,695 rpm, capped at 10,000; real surface speed 327 SFM
The cap is close enough here, but with a 4,000 rpm benchtop mill the same tool would run at only 131 SFM, and the feed drops with it.
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
- Start at the low end of the speed range and raise it while watching tool wear and chip colour. Blue chips in steel with carbide are fine; with HSS they mean too fast.
- Do not cut chip load to be gentle. Too thin a chip rubs and work-hardens stainless; reduce depth of cut instead.
- Long tools deflect. Above about 3 diameters of stick-out, cut both speed and feed by 20 to 50% and take lighter radial cuts.
- Check spindle power for heavy roughing: material removal rate times a unit power factor (about 0.3 hp per in³/min in aluminium, 1 to 1.5 in steel).
- Drill speeds should be about the same as milling for HSS but peck deep holes and slow down past 3 diameters deep.
Frequently asked questions
How do you calculate spindle RPM from SFM?
RPM = 12 × SFM / (π × diameter in inches), or about 3.82 × SFM / D. For a 1/2 inch cutter at 800 SFM that is 12 × 800 / (π × 0.5) = 6,112 rpm. In metric, RPM = 1000 × Vc / (π × D) with Vc in m/min and D in mm.
How do you calculate feed rate for milling?
Feed rate = RPM × number of teeth × chip load per tooth. A 3-flute end mill at 6,112 rpm and 0.004 in per tooth feeds at 6,112 × 3 × 0.004 = 73.3 in/min.
What is chip load?
Chip load, or feed per tooth, is the thickness of material each cutting edge removes per revolution. It is the number tool makers specify and the one that controls heat and tool life; RPM and feed rate are derived from it.
What is chip thinning and when should I use it?
When the radial width of cut is less than half the cutter diameter, the actual chip is thinner than the programmed feed per tooth. Multiply the chip load by D / (2√(D·ae − ae²)) to compensate. At a 10% stepover the factor is about 1.67.
What surface speed should I use for aluminium and steel?
As starting points, about 300 SFM (90 m/min) for HSS and 800 SFM (245 m/min) or more for carbide in aluminium; about 90 SFM (27 m/min) for HSS and 350 SFM (105 m/min) for carbide in mild steel. Coated carbide tool makers often recommend higher values.
How do I calculate metal removal rate?
For milling, MRR = width of cut × depth of cut × feed rate. For turning, MRR = 12 × SFM × depth of cut × feed per rev in cubic inches per minute, or Vc × ap × f in cubic centimetres per minute. Multiply by the material's unit power to estimate spindle load.
What should I do if my machine cannot reach the calculated RPM?
Run at the maximum spindle speed and keep the chip load the same, which lowers the feed rate in proportion. Do not raise the chip load to make up the difference. A smaller-diameter tool or one with more flutes can also help keep productivity up.
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.