30-Second Summary: Cutting parameters = material group × bore diameter × depth coefficient. First, find the recommended Vc and feed in the tables below, then multiply by the depth correction factor based on L/D. Separate tables are provided for gundrilling and BTA drilling, as their operating parameters differ significantly.
Gundrill Recommended Cutting Speed Vc (m/min)
| Material Group | Hardness HB | Carbide-Tipped Vc | Solid Carbide Vc |
|---|---|---|---|
| Non-alloy steel <0.25%C | ~125 | 120-180 | 100-140 |
| Non-alloy steel ≥0.25%C | ~190 | 100-150 | 90-120 |
| Low-alloy steel (annealed) | ~200 | 60-80 | 60-70 |
| High-alloy steel, tool steel | ~200 | 60-80 | 60-70 |
| Hardened steel | ~325 | 40-60 | 30-50 |
| Ferritic/Martensitic stainless steel | — | 40-80 | 40-50 |
| Austenitic/Duplex stainless steel | — | 30-60 | 30-40 |
| Gray cast iron | — | 70-100 | 60-90 |
| Aluminum alloy (wrought) | — | 80-160 | 100-200 |
| Aluminum alloy (cast, high Si) | — | 60-120 | 80-140 |
| Copper alloy / Brass | — | 80-150 | 80-140 |
| Bronze (high-tensile) | — | 50-90 | 50-80 |
| Nickel-based superalloy (Inconel) | — | 15-30 | 10-20 |
| Titanium alloy (Ti-6Al-4V) | — | 20-40 | 15-30 |
| Magnesium alloy | — | 100-200 | 100-200 |
| Thermoplastics / Composites | — | 40-100 | — |
Gundrill Feed Rate Reference (mm/rev)
| Material | D=3mm | D=5mm | D=10mm | D=20mm | D=30mm |
|---|---|---|---|---|---|
| Low-carbon steel | 0.005-0.010 | 0.010-0.020 | 0.020-0.040 | 0.050-0.080 | 0.100-0.160 |
| Alloy steel (annealed) | 0.005-0.010 | 0.010-0.020 | 0.020-0.040 | 0.050-0.080 | 0.100-0.140 |
| Alloy steel (hardened) | 0.004-0.008 | 0.008-0.018 | 0.015-0.030 | 0.040-0.070 | 0.080-0.120 |
| Stainless steel (austenitic) | 0.004-0.008 | 0.008-0.015 | 0.020-0.030 | 0.050-0.070 | 0.100-0.150 |
| Cast iron (gray/ductile) | 0.006-0.012 | 0.012-0.025 | 0.030-0.050 | 0.070-0.120 | 0.150-0.220 |
| Aluminum alloy | 0.020-0.040 | 0.040-0.080 | 0.070-0.130 | 0.150-0.280 | 0.300-0.500 |
| Copper alloy / Brass | 0.015-0.030 | 0.030-0.060 | 0.050-0.100 | 0.100-0.200 | 0.200-0.400 |
| Titanium alloy | 0.003-0.006 | 0.006-0.012 | 0.010-0.025 | 0.030-0.060 | 0.060-0.100 |
| Nickel superalloy | 0.002-0.005 | 0.005-0.010 | 0.008-0.020 | 0.020-0.050 | 0.040-0.080 |
BTA Drilling Feed Rate Reference (mm/rev)
BTA feed rates are typically 3-10x higher than gundrilling for the same diameter. Use these values as starting points for BTA/STS systems.
| Material | D=20mm | D=50mm | D=100mm |
|---|---|---|---|
| Low-carbon steel | 0.08-0.18 | 0.20-0.40 | 0.30-0.60 |
| Alloy steel (annealed) | 0.06-0.15 | 0.15-0.35 | 0.25-0.50 |
| Alloy steel (hardened) | 0.05-0.12 | 0.12-0.28 | 0.20-0.40 |
| Stainless steel | 0.05-0.12 | 0.12-0.30 | 0.20-0.45 |
| Aluminum alloy | 0.15-0.30 | 0.30-0.60 | 0.50-0.90 |
| Cast iron | 0.10-0.25 | 0.25-0.50 | 0.40-0.75 |
| Titanium alloy | 0.03-0.08 | 0.08-0.18 | 0.12-0.28 |
L/D Depth Correction Factors
As hole depth increases, both cutting speed and feed rate must be reduced to compensate for reduced rigidity, chip evacuation difficulty, and coolant pressure drop along the bore. The table below shows correction factors for both speed and feed.
| L/D Ratio | 3D | 5D | 8D | 10D | 15D | 20D | 30D | 50D | 75D | 100D |
|---|---|---|---|---|---|---|---|---|---|---|
| Speed factor Klv | 1.00 | 0.85 | 0.70 | 0.60 | 0.50 | 0.40 | 0.35 | 0.28 | 0.22 | 0.18 |
| Feed factor Klf | 1.00 | 0.80 | 0.60 | 0.50 | 0.40 | 0.35 | 0.30 | 0.25 | 0.20 | 0.16 |
How to use: Find the base Vc and feed from the tables above for your material and diameter, then multiply both by the correction factor for your L/D ratio. For L/D values between table entries, interpolate linearly.
Worked example:
Part: Gundrilling 4140 alloy steel, annealed, 15 mm diameter × 450 mm deep (L/D = 30:1)
Base Vc: 70 m/min (mid-range for alloy steel)
Base feed: 0.030 mm/rev (mid-range for 15 mm, interpolated between 10mm and 20mm)
Correction at L/D = 30: Klv = 0.35, Klf = 0.30
Adjusted Vc: 70 × 0.35 = 24.5 m/min
Adjusted feed: 0.030 × 0.30 = 0.009 mm/rev
Spindle speed: 24.5 × 1000 / (π × 15) = 520 RPM
Feed rate: 520 × 0.009 = 4.7 mm/min
Machining time: 450 / 4.7 = 96 minutes
Speed and Feed Rate Calculation
Spindle speed n (RPM) = Vc × 1000 / (π × D)
Feed rate Vf (mm/min) = n × f (f = feed mm/rev)
Machining time T (min) = L / Vf (L = hole depth mm)
Material removal rate Q (cm³/min) = Vf × π × D² / 4000
Break-Through and Entry Recommendations
- Entry: Start at 80% of target feed for the first 2-3 mm of cut, then ramp to full feed
- Break-through: Reduce feed by 50% over the last 2-3 mm to prevent exit burrs and edge chipping
- Retraction: Reduce speed to ≤50 RPM before retracting; maintain coolant flow during retraction to flush remaining chips
⚠️ Important: The above are recommended starting values. Actual parameters should prioritize tool manufacturer recommendations and be confirmed through trial cuts. For new workpiece materials, start from the lower limit and optimize incrementally. Chip shape observation during the first 10-20 seconds of cut is the best real-time indicator of parameter suitability.