Running Drills at Correct SFM: Speed-Feed Charts Explained

The SFM Formula Every Machinist Should Know

Surface feet per minute (SFM) measures how fast the cutting edge moves across the workpiece material. It's the fundamental parameter that determines cutting temperature, tool wear rate, and chip formation. Yet a surprisingly large number of production shops set spindle speed by feel or habit rather than calculation, and pay for it in shortened tool life and inconsistent hole quality.

The formula is straightforward: RPM = (SFM × 3.82) / Diameter. The 3.82 factor is the constant 12/π rounded to three significant figures — it converts the diameter in inches and the surface speed in feet per minute into revolutions per minute. For metric users: RPM = (SMM × 1000) / (π × Diameter_mm), where SMM is surface meters per minute.

Example: drilling 3/8" (0.375") holes in 1018 mild steel. Recommended SFM for HSS in mild steel is 80 to 100 SFM. Take the midpoint at 90 SFM: RPM = (90 × 3.82) / 0.375 = 343.8 / 0.375 = 917 RPM. That's your starting spindle speed. If your machine doesn't hit exactly 917, the closest available speed below that target is the safer choice — running under the recommended SFM is conservative; running over generates more heat and shortens tool life.

The calculation changes with every diameter change. A 1/4" drill in the same material at the same SFM needs 1,375 RPM — 50% higher spindle speed. Shops that set RPM once and drill multiple hole sizes are either running some holes too fast or some too slow. The proper approach is a posted SFM-to-RPM chart or a calculator at the machine, and the discipline to use it.

SFM Values by Material: A Working Reference

Recommended SFM values for HSS drills (reduce by 20-30% for carbide inserts, increase by 20-30% for carbide drills):

• Free-machining steel (12L14, 1213): 100–130 SFM
• Mild steel (1018, A36): 80–100 SFM
• Medium-carbon steel (1045, 4140 annealed): 60–80 SFM
• 4140 pre-hard (28-32 HRC): 40–55 SFM
• Tool steel (D2, H13 annealed): 30–50 SFM
• 304/316 stainless steel: 40–60 SFM
• 17-4 PH stainless: 30–45 SFM
• Cast iron (gray): 50–80 SFM
• Aluminum alloys (6061, 7075): 200–300 SFM
• Brass/bronze: 150–200 SFM
• Copper: 100–150 SFM
• Titanium (Grade 5): 20–30 SFM
• Inconel 718: 10–20 SFM
• Plastics (Delrin, nylon): 150–250 SFM

These ranges reflect starting points for standard HSS jobber drills. Cobalt grades allow the upper end of the range or slightly above. Coatings (TiN, TiAlN) can push speeds 10 to 20 percent higher. Material condition matters — normalized steel vs. stress-relieved vs. hardened can shift the recommended SFM significantly.

Feed Rate: The Other Half of the Equation

Feed rate — inches per revolution (IPR) — determines chip load, cutting forces, and how efficiently material is removed. Unlike SFM, feed rate scales with drill diameter rather than remaining constant across sizes.

General starting feeds for HSS in mild steel:

• Under 1/8" diameter: 0.001–0.002 IPR
• 1/8" to 1/4": 0.002–0.004 IPR
• 1/4" to 1/2": 0.004–0.007 IPR
• 1/2" to 1": 0.007–0.015 IPR
• Over 1": 0.015–0.025 IPR

Feed that's too light is almost as bad as feed that's too heavy. Light feed causes rubbing instead of cutting, which generates heat without removing material. Heavy feed causes excessive thrust, drill flexion, and potential breakage. The sweet spot is a feed that produces a well-formed chip — not dust, not stringy coils, but short, controlled segments that evacuate cleanly.

On CNC machines, feed rate is programmed in inches per minute (IPM) = IPR × RPM. At 917 RPM with 0.005 IPR feed: 917 × 0.005 = 4.6 IPM. That's your F value in the program. Document these values in a setup sheet — it takes two minutes per job and saves the next operator from guessing.