More HSS drill bits die from wrong speeds than from any other cause. Running too fast generates heat that softens the cutting edge — permanently, because HSS loses its heat treatment above about 600°F. Running too slow isn't catastrophic, but it's inefficient and can cause built-up edge in certain materials. The numbers are not complicated, but most shops either don't know them or don't apply them consistently.
Here are the correct surface footage ranges for HSS drilling across common materials, the formula to convert them to RPM, and the feed rates that go with them.
The Fundamental Formula
Cutting speed for drilling is measured in surface feet per minute (SFM) — the speed at which the cutting edge moves through the material. SFM is constant regardless of drill diameter; the RPM you set changes to achieve the same SFM with different size drills.
The 3.82 constant is 12 ÷ π rounded. Some machinists use 4 for quick mental math — it's close enough for most shop calculations. The important thing is getting into the right ballpark, not hitting an exact number.
SFM Reference Table for HSS Drills
| Material | SFM Range (HSS) | Cutting Fluid | Notes |
|---|---|---|---|
| Mild steel (1018, A36) | 80–100 SFM | Sulfurized or soluble oil | General baseline. Err toward lower end without flood coolant. |
| Medium carbon steel (1040, 1045) | 60–80 SFM | Sulfurized cutting oil | Higher carbon = more heat. Reduce speed accordingly. |
| Alloy steel (4140, 4340 annealed) | 40–60 SFM | Sulfurized cutting oil, heavy application | Tougher, more heat-generating. Keep speed conservative. |
| Stainless 304/316 | 30–50 SFM | Sulfurized cutting oil — do not drill dry | Work-hardens. Slow, constant feed, no dwelling or stopping mid-hole. |
| Cast iron (gray) | 50–80 SFM | Dry | No coolant — thermal shock risk. Graphite self-lubricates. |
| Aluminum (6061, 7075) | 200–300 SFM | Light oil, kerosene, or WD-40 | High speed, polished flutes preferred, watch for chip welding. |
| Copper | 150–200 SFM | Light oil | Gummy material. Maintain constant feed; don't pause mid-hole. |
| Brass | 200–300 SFM | None or light oil | Fast and dry. Ensure zero-rake geometry to prevent self-feeding. |
| Plastic (acrylic, nylon) | 100–200 SFM | Compressed air or dry | Sharp bits only. Acrylic: no coolant, risk of crazing. |
Quick RPM Reference — Mild Steel at 80 SFM
For mild steel drilling at 80 SFM, here are pre-calculated RPMs by common drill size:
| Drill Diameter | RPM at 80 SFM | RPM at 60 SFM (stainless) |
|---|---|---|
| 1/8" (0.125") | 2,445 | 1,833 |
| 3/16" (0.1875") | 1,630 | 1,222 |
| 1/4" (0.250") | 1,222 | 917 |
| 5/16" (0.3125") | 978 | 733 |
| 3/8" (0.375") | 815 | 611 |
| 1/2" (0.500") | 611 | 458 |
| 5/8" (0.625") | 489 | 367 |
| 3/4" (0.750") | 407 | 305 |
| 1" (1.000") | 306 | 229 |
Feed Rate — The Other Half of the Equation
Feed rate is how fast the drill advances axially into the material, measured in inches per revolution (IPR) or inches per minute (IPM). Feed rate matters almost as much as speed for drill life and hole quality.
Too light a feed and the drill rubs rather than cuts — the edge heats up without actually removing material efficiently, and work hardening accelerates in materials like stainless. Too heavy a feed and the drill breaks.
General IPR guidelines for HSS jobber drills in steel:
- Under 1/8" diameter: 0.001–0.002 IPR (very light — small drills break easily)
- 1/8" to 1/4": 0.002–0.004 IPR
- 1/4" to 1/2": 0.004–0.008 IPR
- 1/2" to 1": 0.008–0.015 IPR
- Over 1": 0.015–0.025 IPR
These ranges go down for harder materials (stainless, alloy steel) and up for softer ones (aluminum, brass). The practical signal is chip formation: in steel, you want tight curled chips. In aluminum, short broken chips. If chips are stringy and long, feed is likely too light. If the machine is struggling and chips are discolored, speed is too high or feed too heavy.
Why This Matters for Drill Life
A bit run at 200 SFM in mild steel — roughly double the recommended speed — will dull in a fraction of the holes it would otherwise drill. The heat generated at the cutting zone is not linear with speed; it rises faster. And once the steel at the cutting edge reaches its tempering temperature, the hardness is gone permanently — no amount of resharpening recovers that bit to its original performance potential.
Correct speed is the simplest, highest-leverage thing a shop can do to extend drill life. A sharp bit at correct speed with appropriate cutting fluid will drill many times more holes per regrind cycle than the same bit pushed too fast and dry.
Running correct speeds helps — but HSS drill bits still wear out. MachinistPost resharpens HSS drills by mail from anywhere in the US, restoring geometry on a WinsloMatic grinder. Back to you sharp within the week.
Send Your Bits