India version. Set up in metric for the drilling and lathe work in Indian ITI and tool-room practice: HSS drills in mild steel by default, cutting speed in m/min and feed in mm/rev. US version

Cutting Speed and RPM Calculator

Find spindle RPM from cutting speed in m/min for drilling, turning and milling, with feed in mm/min, worked for HSS drills and lathe tools in mild steel.

The interactive tool loads here when JavaScript runs.

About this tool

What is the Speeds and Feeds Calculator?

The ITI Fitter curriculum asks trainees to choose "cutting speed, feed, R.P.M. for different materials" for drilling and to compare cutting speed and feed for HSS and carbide lathe tools. The calculation behind both is N = 1000 × V / (π × D), with cutting speed V in metres per minute and diameter D in millimetres. This version opens on that case: a 10 mm HSS drill in mild steel.

At the preset 27.4 m/min, N = 1000 × 27.4 / (π × 10) = 872 rpm. With a feed of 0.13 mm per revolution the drill advances 113 mm per minute. On a pillar or bench drill with fixed belt speeds, choose the nearest step below 872 rpm. Larger drills need slower speeds: the same steel with a 20 mm drill needs 436 rpm.

For turning, D is the job diameter. A 50 mm mild steel bar turned with an HSS tool at 27.4 m/min runs at 174 rpm; with a carbide tip at 107 m/min it runs at 681 rpm and removes about four times as much metal at the same feed and depth of cut. The presets are cautious starting values for plain tools; a tool maker's figure for a coated tool or insert takes priority.

  • 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
Read the guide: Speeds and Feeds for Milling, Drilling and Turning, From First Principles

Updated

How to use the Speeds and Feeds Calculator

  1. Choose inch or metric units and the operation: milling, drilling or turning.
  2. 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.
  3. Enter the cutter, drill or workpiece diameter, the number of teeth for milling, and the depth and width of cut.
  4. Set your machine's maximum RPM so the calculator can cap the spindle speed, and choose whether to compensate for chip thinning.
  5. Read the RPM, feed rate, feed per revolution and metal removal rate, then copy the numbers into your program or CAM setup.

Worked examples

10 mm HSS drill in mild steel

Input

Drilling, D = 10 mm, V = 27.4 m/min, feed 0.13 mm/rev

Output

872 rpm; feed 113.4 mm/min

N = 1000 × 27.4 / (3.1416 × 10) = 872.2. Feed rate = 872.2 × 0.13 = 113.4 mm/min.

Tap drill for M10 before tapping

Input

Drilling, D = 8.5 mm, V = 27.4 m/min, feed 0.13 mm/rev

Output

1,026 rpm; feed 133.4 mm/min

The smaller drill runs faster at the same cutting speed. The 8.5 mm size comes from the tap drill rule for M10 x 1.5.

Turning a 50 mm bar: HSS against carbide

Input

Turning, D = 50 mm, feed 0.2 mm/rev, depth of cut 1.5 mm; V = 27.4 then 107 m/min

Output

HSS 174 rpm, 34.9 mm/min, 8.22 cm³/min. Carbide 681 rpm, 136 mm/min, 32.1 cm³/min

Metal removal rate = V × depth × feed. Carbide takes the same chip about four times as fast, which is the comparison the syllabus asks for.

20 mm drill on a pillar drill

Input

Drilling, D = 20 mm, V = 27.4 m/min, feed 0.25 mm/rev

Output

436 rpm; feed 109 mm/min

Doubling the diameter halves the RPM. Big drills in mild steel are often piloted with a smaller drill first so the chisel edge does not have to push through solid metal.

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

  • If the machine has stepped pulleys, always take the speed step below the calculated RPM, not above it.
  • When the drill squeals or the chips turn blue with an HSS tool, the speed is too high.
  • For a deep hole, withdraw the drill now and then to clear chips, and slow down once the hole is more than about three diameters deep.

Sources and further reading

  1. Competency based curriculum: Fitter (CTS, NSQF level 4), Directorate General of Training, Ministry of Skill Development and Entrepreneurship. Drill cutting speed, feed and RPM for different materials; lathe cutting speed and feed for HSS and carbide tools.
  2. Milling formulas and definitions, Sandvik Coromant. Spindle speed n = vc × 1000 / (π × D) and table feed vf = fz × n × z.

Frequently asked questions

What is the formula for RPM from cutting speed?

N = 1000 × V / (π × D), where V is cutting speed in m/min and D is the drill, cutter or job diameter in mm. For a 10 mm drill at 27.4 m/min, N = 27,400 / 31.42 = 872 rpm.

What cutting speed should I take for mild steel with an HSS drill?

The calculator uses 27.4 m/min as a cautious starting value for plain HSS in mild steel. Coated HSS drills and carbide tools can run much faster; follow the tool maker's figure when you have it.

How do I find the feed in mm/min from feed per revolution?

Multiply by the RPM. A drill at 872 rpm with 0.13 mm/rev feed advances 872 × 0.13 = 113 mm/min. For milling, feed = RPM × number of teeth × feed per tooth.

What RPM should I use to turn a 50 mm mild steel bar?

About 174 rpm with an HSS tool at 27.4 m/min, or about 681 rpm with a carbide tool at 107 m/min. Use the job diameter, and raise the RPM as the diameter comes down if you want to keep the same cutting speed.

Why is carbide run faster than HSS?

Carbide keeps its hardness at much higher cutting temperatures, so it can take a higher cutting speed for the same tool life. In the presets carbide runs about four times faster than HSS in mild steel (107 against 27.4 m/min).

How do I calculate metal removal rate in turning?

MRR = V × depth of cut × feed, in cm³/min when V is m/min and depth and feed are in mm. At 27.4 m/min, 1.5 mm depth and 0.2 mm/rev that is 27.4 × 1.5 × 0.2 = 8.22 cm³/min.

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.