Sheet metal
Drill speed calculator
In short
Drill speed is n = 1000 × Vc / (π × D), in rpm, with Vc the cutting speed in m/min from manufacturer data sheets and D the diameter in mm. For tapping, the tap drill is about d − P (ISO 2306 series) and the tap feed equals the pitch × n.
Calculation
Example calculated with the tool’s default values.
Inputs
- What to compute
- Tapping (tap drill + tap)
- ISO metric thread
- M10 (pitch 1.5)
- Drill
- HSS / HSSCo
- Workpiece material
- Non-alloy steel (S235, S355, annealed C45)
Results
- Tap drill Ø
- 8.5 mm
Worked example
Every value in this section belongs to the example, calculated with the tool’s default values.
Other results of the example
- Pitch
- 1.50 mm
- Drill speed
- 936 rpmRange: 824 to 1011 rpm
- Cutting speed Vc
- 25 m/minHSS / HSSCo, standard and jobber series (Ø ≤ 20 mm)
- Feed per revolution
- 0.130mm/rev
- Spindle feed rate
- 122 mm/min
- Tap speed
- 477 rpmMachine tap, uncoated HSS-E
- Tap Vc
- 15.0 m/min
- Tap feed (= pitch × n)
- 716 mm/min
- The standard tap drill (≈ d − P) gives roughly 75 to 80 % thread height. In stainless and soft materials the metal flows: a drill 0.1 mm larger is common.
- Starting values from manufacturers’ catalogues (see sources), ± 25 % depending on machine, coolant and drill length. Beyond 5 × D depth, reduce Vc by about 20 %. Indicative.
Step-by-step calculation
Tap drill
drill Ø ≈ d − P (drill series, ISO 2306)
M10: 10.0 − 1.50 = 8.50 → ISO 2306 table: 8.5 mm
Starting cutting speed
Vc: Europa: non-alloy steel < 25 HRc (VDI 1-5)
Vc = 25 m/min (range 22 to 27)
Spindle speed
n = 1000 × Vc / (π × D)
1000 × 25 / (π × 8.5) = 936 rpm
Feed
Vf = fn × n
0.130 mm/rev × 936 = 122 mm/min
Tapping
n = 1000 × Vc / (π × d); feed = pitch × n
HSS-E tap Vc (group P1) = 15.0 m/min → n = 477 rpm; feed 1.50 × 477 = 716 mm/min
How to use it
- Pick what to compute: tapping (tap drill and tap) or drilling only.
- Pick the ISO metric thread, or enter the drill diameter (1 to 60 mm).
- Pick the drill: HSS / HSSCo or solid carbide.
- Pick the workpiece material.
- Read the tap drill Ø when tapping, or the spindle speed when drilling only.
Frequently asked questions
How do I calculate drill RPM?
n = 1000 × Vc / (π × D), with Vc the cutting speed in m/min and D the drill diameter in mm. Example: 8.5 mm HSS drill in non-alloy steel, Vc = 25 m/min: 1000 × 25 / (π × 8.5) = 936 rpm, range 824 to 1011 rpm. The feed is Vf = fn × n: 0.130 mm/rev × 936 = 122 mm/min.
What drill speed for steel?
With an HSS / HSSCo drill up to Ø 20 mm, the Europa Tool sheet gives Vc = 25 m/min (22 to 27) for non-alloy steel and 22 m/min (20 to 25) for low-alloy steel. For HSS Ø 21 to 60 mm, Vc = 20 m/min (18 to 22). With solid carbide, Carbide s.r.o. gives 92 m/min for non-alloy steel up to 650 N/mm².
What tapping speed should I use?
For a machine tap in uncoated HSS-E, the D 396 catalogue gives Vc = 15 m/min in steel (groups P1, P7), 5 in stainless (M1), 20 in cast iron (K3), 10 in aluminium (N1), 5 in copper (N7) and 25 in brass (N8). For M10 in steel: n = 477 rpm and a feed of 1.50 × 477 = 716 mm/min.
Which tap drill size for a metric thread?
The tap drill is about d − P, rounded to the ISO 2306 drill series: M10 with a 1.5 pitch gives 10.0 − 1.50 = 8.50, so an 8.5 mm drill. It gives roughly 75 to 80 % thread height; in stainless and soft materials the metal flows, and a drill 0.1 mm larger is common.
Should the speed go down for deep holes?
Yes: beyond 5 × D depth, reduce Vc by about 20 %. The values are starting values from manufacturers' catalogues, ± 25 % depending on machine, coolant and drill length.
Limits
Indicative results: manufacturer starting values (Europa Tool, Carbide s.r.o., D 396 tapping catalogue), to adapt to the machine and coolant, not maxima. With no sourced value for a material / drill pair, the calculation refuses rather than extrapolates. In stainless, keep a positive feed, never dwell (work hardening), flood coolant.
Sources
- Avant-trou des filetages métriques : diamètre ≈ nominal − pas, série des forets : ISO 2306:1972, tableaux 1 et 2 ; recoupé AmesWeb et Fractory (link)
- Vc et avance des forets HSS / HSSCo par groupe de matière VDI : Europa Tool, fiches cutting data 0001 / 820902 (Ø ≤ 20) et 821901 (Ø 21-60) (link)
- Vc et avance des forets carbure monobloc : Carbide s.r.o., recommandations de coupe pour forets VHM (link)
- Vc du taraudage machine (HSS-E non revêtu), groupes P1 P7 M1 K3 N1 N7 N8 : Catalogue technique, « Schnittdaten für das Gewindebohren », D 396 (link)
- Vitesse de rotation : n = 1000 × Vc / (π × D) (Europa Tool ; Dormer Pramet)