ドリル切削条件（回転数・送り）完全ガイド
Mastering holemaking requires balancing tangential cutting velocity (SFM or $V_c$) with axial penetration rate ($f_n$ or IPR). Correct parameters guarantee predictable tool life, precise hole diameters, and chip evacuation without work hardening.
1. The Four Core Parameters of Drilling
Unlike milling where cutters encounter air between teeth, a drill remains continuously engaged inside a confined cylindrical cavity. Every calculation revolves around four interrelated variables:
The peripheral speed at the drill's outer edge as it shears material. Dictated by workpiece hardness and tool substrate metallurgy.
Rotational frequency of the machine spindle. Calculated from cutting speed and drill diameter: RPM = (SFM × 3.82) / D.
The axial distance the drill penetrates in one full 360° rotation. Governs un-deformed chip thickness and cutting thrust force.
The programmed Z-axis downward feed velocity: Vf = RPM × fn. This is the rate entered into CNC G-code (F-word).
2. Tool Substrates & Advanced Coatings
The maximum permissible surface speed is governed primarily by drill substrate thermal hardness:
| Drill Substrate | Relative Speed | Toughness vs Wear | Best Application |
|---|---|---|---|
| High-Speed Steel (HSS M2) | 1.0× (Baseline) | Extremely tough, resists chatter | Manual drill press, deep holes, interrupted cuts |
| Cobalt HSS (M42 / 8% Co) | 1.3× - 1.5× | High red hardness up to 600°C | Stainless steels, inconel, titanium, tough alloys |
| Solid Carbide (Micrograin) | 2.5× - 4.5× | Superior hardness, brittle if chattering | Rigid CNC machining centers, mass production |
| TiN Coated (Titanium Nitride) | +25% over uncoated | Low friction coefficient (0.4) | General steels, reduces built-up edge |
| AlTiN / TiAlN Coated | +50% - 100% | Forms aluminum oxide armor at 800°C | High-speed dry drilling, tool steel, stainless |
3. Recommended Feed per Revolution (fn / IPR)
A common failure mode is under-feeding a drill. Light feeding rubs the cutting lips against the material rather than shearing a clean chip. This induces rapid friction hardening, particularly in 300-series stainless steels.
| Drill Diameter Range | HSS Feed (mm/rev) | HSS Feed (IPR) | Carbide Feed (mm/rev) | Carbide Feed (IPR) |
|---|---|---|---|---|
| 1.0 - 3.0 mm (1/16" - 1/8") | 0.02 - 0.05 | 0.0008 - 0.0020 | 0.04 - 0.08 | 0.0015 - 0.0030 |
| 3.0 - 6.0 mm (1/8" - 1/4") | 0.05 - 0.10 | 0.0020 - 0.0040 | 0.08 - 0.15 | 0.0030 - 0.0060 |
| 6.0 - 12.0 mm (1/4" - 1/2") | 0.10 - 0.20 | 0.0040 - 0.0080 | 0.15 - 0.25 | 0.0060 - 0.0100 |
| 12.0 - 25.0 mm (1/2" - 1") | 0.20 - 0.35 | 0.0080 - 0.0140 | 0.25 - 0.40 | 0.0100 - 0.0160 |
4. Troubleshooting Drill Failure Modes
Cause: Excessive spindle RPM (cutting speed too high) or lack of coolant at depth.
Solution: Reduce RPM by 20–30%, check coolant concentration.
Cause: Excessive feed rate, chip packing in flutes, or bottoming out without dwell.
Solution: Reduce IPR/feed, initiate peck drilling cycle (G83).
Cause: Speed too low or cutting dry in ductile materials (e.g. 6061 aluminum).
Solution: Increase cutting speed, use high-lubricity coolant or polished flutes.
Cause: Asymmetric drill point grinding, excessive runout (TIR), or lack of spotting.
Solution: Spot drill first, verify collet runout < 0.0005" (0.012 mm).
Ready to Calculate Your Parameters?
Use our full speed and feed calculator to test any drill size, material hardness, and machine RPM limit.