Speeds and feeds
Drilling speeds and feeds calculator
RPM = (SFM x 12) / (pi x D) and IPM = RPM x IPR; a 3/8 in HSS drill in mild steel at 100 SFM and 0.005 IPR runs 1,019 RPM at 5.09 IPM.
Technical review pending. Formulas and values are cited. This notice comes down after a machinist review.
Spindle speed
RPM
RPM = (SFM x 12) / (pi x D) = (100 x 12) / (3.1416 x 0.375) = 1,019 RPM
Starting point. 100 SFM is 30.48 m/min; 0.3750 in is 9.53 mm. Low-carbon (mild) steel, 0.2 to 0.3% carbon: 95 to 100 SFM (29 to 30 m/min) with HSS.
Feed rate
IPM
IPM = RPM x IPR = 1,018.6 x 0.005 = 5.09 IPM
129.36 mm/min at 0.127 mm/rev. A 0.3750 in drill is in the HSS feed band 1/4 to 1/2 in: 0.004 to 0.007 IPR (0.102 to 0.178 mm/rev).
Reamer speed (rule of thumb)
RPM
Reamer SFM = (1/2 to 2/3) x SFM = (1/2 to 2/3) x 100 = 50 to 67 SFM
Rule of thumb. Feed 2 x 0.005 = 0.0100 IPR: 5.09 to 6.79 IPM.
Source: Machinery's Handbook (cutting speed, spindle speed and feed formulas); starting SFM and feed per revolution from published drill data by Viking Drill and Tool, ICS Cutting Tools and Redline Tools, and University of Florida Mechanical and Aerospace Engineering design lab notes. Reamer speed and feed are rules of thumb.
Starting points only. Adjust by chip, sound and hole finish; the drill maker's chart for your drill governs.
| Work material | Cutting speed (SFM) | Cutting speed (m/min) |
|---|---|---|
| Aluminum alloys | 200 to 300 | 61 to 91 |
| Brass, free-machining | 200 to 300 | 61 to 91 |
| Bronze, high tensile | 70 to 150 | 21 to 46 |
| Magnesium alloys | 250 to 400 | 76 to 122 |
| Cast iron, soft | 70 to 150 | 21 to 46 |
| Cast iron, medium hard | 80 | 24 |
| Low-carbon (mild) steel, 0.2 to 0.3% carbon | 95 to 100 | 29 to 30 |
| Alloy steel, 300 to 400 HB (Brinell hardness) | 30 | 9 |
| Stainless steel, free-machining | 30 to 50 | 9 to 15 |
| Stainless steel, work-hardening (300 series) | 20 to 26 | 6 to 8 |
| Titanium alloys | 20 | 6 |
| Acetal and similar plastics | 100 to 300 | 30 to 91 |
m/min = SFM x 0.3048, rounded to whole numbers. Carbide drills: take speed and feed from the drill maker's chart.
| Drill diameter (in) | Drill diameter (mm) | Feed (IPR) | Feed (mm/rev) |
|---|---|---|---|
| Under 1/8 (0.125) | Under 3.18 | 0.001 to 0.002 | 0.025 to 0.051 |
| 1/8 to 1/4 (0.125 to 0.250) | 3.18 to 6.35 | 0.002 to 0.004 | 0.051 to 0.102 |
| 1/4 to 1/2 (0.250 to 0.500) | 6.35 to 12.70 | 0.004 to 0.007 | 0.102 to 0.178 |
| 1/2 to 1 (0.500 to 1.000) | 12.70 to 25.40 | 0.007 to 0.015 | 0.178 to 0.381 |
| Over 1 (1.000) | Over 25.40 | 0.015 to 0.025 | 0.381 to 0.635 |
Each range is the band every source above contains. mm/rev = IPR x 25.4. On a band boundary (1/8, 1/4, 1/2 or 1 in), the value both bands share is the starting point.
Reaming the same hole
Rule of thumb: run a reamer at about 1/2 to 2/3 of the drilling speed with about twice the feed per revolution. For the 3/8 in hole above in mild steel, that is 50 to 67 SFM, 509 to 679 RPM, at 0.010 IPR. Choose "Also show reamer speed and feed" in the calculator to get it for your numbers.
How it works
Pick a starting cutting speed for the work material from the first table and a feed per revolution for the drill size from the second. The spindle speed comes from the cutting speed and the drill diameter; the feed rate is spindle speed times feed per revolution. To turn an RPM back into SFM, or to work with a tool other than a drill, use the spindle speed calculator.
Inch
RPM = (SFM x 12) / (pi x D); IPM = RPM x IPR
| Symbol | Meaning | Unit |
|---|---|---|
| RPM | Spindle speed | rev/min |
| SFM | Cutting speed, surface feet per minute | ft/min |
| D | Drill diameter | in |
| IPR | Feed per revolution, inches per revolution | in/rev |
| IPM | Feed rate, inches per minute | in/min |
| 12 | Inches per foot | in/ft |
Metric
RPM = (Vc x 1000) / (pi x D); vf = RPM x fn
| Symbol | Meaning | Unit |
|---|---|---|
| RPM | Spindle speed | rev/min |
| Vc | Cutting speed | m/min |
| D | Drill diameter | mm |
| fn | Feed per revolution | mm/rev |
| vf | Feed rate | mm/min |
| 1000 | Millimeters per meter | mm/m |
Conversions: m/min = SFM x 0.3048; mm/rev = IPR x 25.4; mm/min = IPM x 25.4. The feed rate is worked from the unrounded RPM, then both are rounded for display.
Worked example: 3/8 in drill in mild steel
A 3/8 in (0.375 in) HSS drill in low-carbon steel at 100 SFM (top of the 95 to 100 SFM range) and 0.005 IPR (inside 0.004 to 0.007 IPR for 1/4 to 1/2 in).
- Multiply the cutting speed by 12: 100 x 12 = 1,200.
- Multiply pi by the diameter: 3.1416 x 0.375 = 1.1781.
- Divide: 1,200 / 1.1781 = 1,018.6 RPM, shown 1,019 RPM.
- Feed rate: 1,018.6 x 0.005 = 5.09 IPM (5.0930 unrounded).
- Metric alongside: 9.53 mm drill, 30.48 m/min, 0.127 mm/rev, 129.36 mm/min.
- Reaming the same hole (rule of thumb): 1/2 x 100 = 50 SFM, 509.3 RPM; 2/3 x 100 = 66.7 SFM, 679.1 RPM.
- Reamer feed 2 x 0.005 = 0.010 IPR: 509.3 x 0.010 = 5.09 IPM to 679.1 x 0.010 = 6.79 IPM.
Result: 1,019 RPM at 5.09 IPM to drill; 509 to 679 RPM at 0.010 IPR to ream. Starting points.
Worked example: 10 mm drill in aluminum
A 10 mm HSS drill in aluminum alloy at Vc 75 m/min (246 SFM, inside 200 to 300 SFM) and fn 0.15 mm/rev (10 mm = 0.3937 in, the 1/4 to 1/2 in band, 0.102 to 0.178 mm/rev).
- Multiply the cutting speed by 1,000: 75 x 1,000 = 75,000.
- Multiply pi by the diameter: 3.1416 x 10 = 31.416.
- Divide: 75,000 / 31.416 = 2,387.3 RPM, shown 2,387 RPM.
- Feed rate: vf = 2,387.3 x 0.15 = 358.10 mm/min (358.0986 unrounded) = 14.10 IPM.
- Reamer (rule of thumb): 37.5 to 50.0 m/min, 1,193.7 to 1,591.5 RPM.
Result: 2,387 RPM at 358.10 mm/min (14.10 IPM). Starting points.
Shop notes
- Tool-maker speeds assume a rigid machine, sharp drills and coolant. On a drill press or a light mill, start at the low end of the range.
- Belt and step-pulley drill presses: pick the step at or below the result.
- Holes deeper than a few diameters: peck, and set the peck depth with the peck drilling calculator. Add the point length from the drill point length calculator to the programmed depth.
- Pilot or starter hole for a long drill: drill it slightly larger than the long drill, with a point angle equal to or larger than the long drill's.
- Carbide drills: rule of thumb from tool-maker data, about 2 to 4 times the HSS speed in the same material. Take speed and feed from the drill maker's chart.
FAQ
What RPM and feed for a 3/8 in drill in mild steel?
At 100 SFM, 1,019 RPM; at 0.005 IPR that is 5.09 IPM. Treat both as a start.
What feed per revolution for a 1/2 in drill?
1/2 in sits where two bands meet: 0.004 to 0.007 IPR (1/4 to 1/2 in) and 0.007 to 0.015 IPR (1/2 to 1 in), so 0.007 IPR (0.178 mm/rev) is a starting value both bands share.
How fast should a reamer run?
Rule of thumb: about 1/2 to 2/3 of the drilling speed with about twice the feed. For a 3/8 in reamer in mild steel: 50 to 67 SFM, 509 to 679 RPM, 0.010 IPR.
What speed for drilling aluminum?
200 to 300 SFM (61 to 91 m/min) with HSS. A 10 mm drill at 75 m/min runs 2,387 RPM.
How much faster do carbide drills run?
Rule of thumb from tool-maker data: about 2 to 4 times the HSS speed in the same material. Use the drill maker's chart for the grade.
What speed for drilling 304-type stainless?
20 to 26 SFM (6 to 8 m/min) with HSS for work-hardening stainless; free-machining stainless takes 30 to 50 SFM.
Last updated