Drill Speeds and Feeds: A Practical Reference for Common Materials

Speeds and feeds for drilling get treated like a dark art in a lot of shops — machinists run whatever sounds right and adjust based on feel. That works once you've developed the feel, but it's slow to learn and easy to get wrong in new materials. This reference gives you the math, the starting points for common materials, and the indicators that tell you whether you need to adjust up or down.

The Core Formula

Drilling speed (RPM) is derived from surface feet per minute (SFM), which is a property of the material and tool combination — not the machine or the diameter. The formula:

The 3.82 constant is derived from 12 ÷ π, converting surface speed from feet-per-minute to revolutions-per-minute for a given diameter. On a CNC with metric inputs, the equivalent formula using m/min is RPM = (SFM_in_meters × 1000) ÷ (π × diameter_in_mm).

Example: drilling 1/2" diameter in mild steel at 90 SFM:

Round to the nearest available spindle speed. On a manual drill press with stepped pulleys, pick the closest step at or below the calculated RPM — running a touch slow is safer than running hot.

SFM Reference by Material

The values below are starting points for quality HSS (M2) or M42 cobalt drills with flood coolant or appropriate cutting oil. Adjust based on results. Dry drilling typically requires reducing SFM by 25–40%.

Material	SFM (HSS)	SFM (Cobalt M42)	Notes
Mild Steel (1018, A36)	80–100	100–120	Water-soluble coolant or cutting oil
Alloy Steel (4140, 4340)	50–80	70–100	Lower end for harder conditions
304/316 Stainless	30–50	40–60	Sulfurized cutting oil; cobalt preferred
Aluminum (6061, 2024)	200–300	250–400	High helix drills; flood or light oil
Cast Iron (gray)	50–80	70–100	Dry; air blast for chip clearing
Brass (free-cutting)	150–250	200–300	Zero-rake geometry required; dry or light oil
Copper	150–250	200–300	Zero-rake geometry; cutting oil reduces BUE
Bronze	100–150	130–200	Light cutting oil; watch for grab on leaded grades
Tool Steel (pre-hard, ~30 HRC)	30–50	40–60	Cutting oil; cobalt required above 28 HRC
Inconel 625/718	—	10–20	Cobalt minimum; straight cutting oil; no hesitation
Titanium Grade 2	25–40	35–55	Flood coolant; sharp tooling essential
Acrylic / Polycarbonate	150–250	—	High SFM, low feed; backing board to prevent cracking

Feed Rate: IPR as the Starting Point

Feed rate for drilling is expressed in inches per revolution (IPR) — how far the drill advances axially per full spindle rotation. Unlike SFM which is tied to surface speed, IPR scales with drill diameter: larger drills use higher IPR values.

General starting points for HSS in 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": 0.003–0.006 IPR
• 1/2" to 1": 0.005–0.010 IPR

Scale down by 30–40% for stainless and alloy steels. Scale up for aluminum and free-machining brass.

To convert IPR to IPM for CNC programming:

Reading the Results

After your first hole or two, chip formation tells you whether you're in the right zone:

Correct parameters

In steel: short, curled chips, silver to light straw color. The spindle sounds steady. Feed advances without forcing. The hole is at nominal diameter.

SFM too high

Chips turn blue or purple. Tip discoloration on the drill. Heat at the workpiece surface. Reduce SFM by 20% and check again.

Feed too low / rubbing

Fine, dusty, powdery chips. The drill sounds like it's sliding rather than cutting. The bit runs hot without removing much material. This is the dangerous condition in work-hardening materials — increase feed until you're generating a visible chip.

Feed too high

Long, stringy chips that pack in the flutes. The spindle sounds labored. Breakthrough is violent. Reduce IPR and re-run.

The Most Common Mistake: Feeding Too Slow

In manual drilling, machinists tend to go light on the feed because it feels more controlled. In most materials, this is the wrong instinct. A light feed at full RPM means rubbing, not cutting — which generates more heat, more wear, and less hole quality than a proper cutting feed. When in doubt, increase feed until the drill is making clean chips, then adjust SFM as needed for temperature.

---

Correct speeds and feeds only work with sharp tooling. A dull drill behaves erratically at any feed rate. MachinistPost resharpens HSS and cobalt drills by mail from anywhere in the US, restoring proper geometry so your speeds and feeds actually produce the results the table says they should.