Appearance
Cutting parameters for deep hole drilling are not the same as for conventional drilling. The chip evacuation constraint — not tool life — is usually the limiting factor. Starting parameters should be conservative enough to ensure reliable chip evacuation, then optimized upward based on observed chip formation and tool wear.
This article provides cutting speed and feed recommendations for deep hole drilling organized by material, drilling method, and tool diameter. Use these tables as starting points and adjust based on your specific conditions.
Fundamental Formulas
Cutting Speed to RPM
Imperial: RPM = (SFM × 12) / (π × Dia) or RPM = (SFM × 3.82) / Dia
Metric: RPM = (Vc × 1000) / (π × Dia)Where Dia is the drill diameter (inches or mm), SFM is surface feet per minute, and Vc is cutting speed in m/min.
Feed Rate
Imperial: IPM = IPR × RPM
Metric: mm/min = mm/rev × RPMWhere IPM is inches per minute, IPR is inches per revolution.
Material Removal Rate
Imperial: MRR (in³/min) = (D × IPR × SFM × 12) / π
Metric: MRR (cm³/min) = (D × f × Vc × 1000) / 4Where D is drill diameter, f is feed per revolution, and MRR is material removal rate.
Quick approximation for BTA drilling: Material removal rate (in³/min) ≈ 0.26 × D × IPR × SFM. Multiply by 0.0164 to convert to cm³/min.
Cutting Speed Recommendations
Gun Drilling — Cutting Speed by Material
| ISO | Material Group | Condition | Hardness (HB) | Vc (m/min) | SFM |
|---|---|---|---|---|---|
| P | Low-carbon steel (< 0.25% C) | Annealed | 125 | 180–200 | 590–655 |
| P | Carbon steel (≥ 0.25% C) | Annealed | 190 | 160–180 | 525–590 |
| P | Medium-carbon steel (< 0.55% C) | Q&T | 250 | 130–160 | 425–525 |
| P | High-carbon steel (≥ 0.55% C) | Annealed | 220 | 110–140 | 360–460 |
| P | High-carbon steel | Q&T (1,000 N/mm²) | 300 | 70–90 | 230–295 |
| P | Low-alloy steel | Annealed | 200 | 100–120 | 330–395 |
| P | Low-alloy steel | Q&T (1,200 N/mm²) | 350 | 40–70 | 130–230 |
| P | High-alloy / tool steel | Annealed | 200 | 50–90 | 165–295 |
| P | High-alloy / tool steel | Q&T (1,100 N/mm²) | 325 | 40–80 | 130–260 |
| M | Stainless steel (austenitic) | Annealed | 180 | 50–100 | 165–330 |
| M | Stainless steel (ferritic/martensitic) | Annealed | 200 | 60–110 | 195–360 |
| K | Gray cast iron | Ferritic/pearlitic | 180 | 80–120 | 260–395 |
| K | Nodular/ductile cast iron | Ferritic | 160 | 90–180 | 295–590 |
| N | Aluminum (wrought) | — | 60 | 160–220 | 525–720 |
| N | Aluminum (cast, ≤ 12% Si) | — | 75 | 90–160 | 295–525 |
| N | Copper alloys / brass | Free-cutting | 110 | 90–120 | 295–395 |
| S | High-temp alloys (Fe-based) | Annealed | 200 | 30–50 | 100–165 |
| S | High-temp alloys (Ni-based, Inconel) | Annealed | 250 | 20–40 | 65–130 |
| S | Titanium alloys | Annealed | 400 | 30–50 | 100–165 |
Important: These are starting ranges for gun drilling with carbide-tipped tools. Use the lower end of the range for smaller diameters, deeper holes, or less rigid setups. Use the higher end for larger diameters, shallow holes, and rigid setups.
BTA Drilling — Cutting Speed by Material
| ISO | Material Group | Condition | Hardness (HB) | Vc (m/min) | SFM |
|---|---|---|---|---|---|
| P | Low-carbon steel (< 0.25% C) | Annealed | 125 | 120–200 | 395–655 |
| P | Carbon steel (≥ 0.25% C) | Annealed | 190 | 110–180 | 360–590 |
| P | Medium-carbon steel | Q&T | 250 | 90–160 | 295–525 |
| P | Low-alloy steel | Annealed | 200 | 70–130 | 230–425 |
| P | Low-alloy steel | Q&T | 300 | 55–100 | 180–330 |
| P | Tool steel | Annealed | 200 | 50–90 | 165–295 |
| M | Stainless steel (austenitic) | Annealed | 180 | 30–70 | 100–230 |
| M | Stainless steel (ferritic/martensitic) | Annealed | 200 | 40–80 | 130–260 |
| K | Gray cast iron | — | 180 | 80–140 | 260–460 |
| K | Nodular/ductile cast iron | — | 160 | 90–150 | 295–490 |
| N | Aluminum (wrought) | — | 60 | 150–220 | 490–720 |
| N | Aluminum (cast, ≤ 12% Si) | — | 75 | 100–150 | 330–490 |
| N | Copper alloys / brass | — | 110 | 80–120 | 260–395 |
Note on BTA speeds: BTA cutting speeds are typically 10–20% lower than gun drilling speeds for the same material because BTA drill heads have multiple cutting edges generating more heat and requiring more aggressive chip evacuation.
Feed Rate Recommendations
Gun Drilling Feed by Tool Insert Size
Gun drill feed rates are primarily determined by the insert size, not the drill diameter:
| Insert Size | Minimum Feed (mm/rev) | Maximum Feed (mm/rev) | Typical (mm/rev) |
|---|---|---|---|
| 06–07 | 0.02 | 0.10 | 0.06 |
| 08–09 | 0.04 | 0.16 | 0.10 |
| 10–11 | 0.06 | 0.18 | 0.12 |
| 12–13 | 0.08 | 0.22 | 0.14 |
| 14–16 | 0.10 | 0.28 | 0.18 |
Gun Drilling Feed by Material
| Material Group | Feed Range (mm/rev) | Feed Range (IPR) |
|---|---|---|
| Low-carbon steel | 0.04–0.18 | 0.0016–0.0071 |
| Alloy steel (annealed) | 0.04–0.14 | 0.0016–0.0055 |
| Alloy steel (hardened) | 0.03–0.10 | 0.0012–0.0039 |
| Stainless steel (austenitic) | 0.02–0.08 | 0.0008–0.0031 |
| Stainless steel (ferritic) | 0.03–0.10 | 0.0012–0.0039 |
| Cast iron | 0.04–0.20 | 0.0016–0.0079 |
| Aluminum | 0.03–0.16 | 0.0012–0.0063 |
| Brass / bronze | 0.04–0.18 | 0.0016–0.0071 |
| Titanium alloys | 0.02–0.08 | 0.0008–0.0031 |
| High-temp alloys | 0.02–0.06 | 0.0008–0.0024 |
BTA Drilling Feed by Diameter
BTA feed rates are typically specified by drill diameter range:
| Drill Diameter | Feed Range (mm/rev) | Feed Range (IPR) |
|---|---|---|
| 20–30 mm (0.79–1.18 in) | 0.04–0.12 | 0.0016–0.0047 |
| 30–50 mm (1.18–1.97 in) | 0.06–0.16 | 0.0024–0.0063 |
| 50–80 mm (1.97–3.15 in) | 0.08–0.20 | 0.0031–0.0079 |
| 80–120 mm (3.15–4.72 in) | 0.10–0.25 | 0.0039–0.0098 |
| 120–200 mm (4.72–7.87 in) | 0.12–0.30 | 0.0047–0.0118 |
| 200–300 mm (7.87–11.81 in) | 0.15–0.35 | 0.0059–0.0138 |
BTA Drilling Feed by Material
| Material Group | Feed Range (mm/rev) | Notes |
|---|---|---|
| Low-carbon steel | 0.08–0.30 | Higher end for larger diameters |
| Alloy steel (annealed) | 0.06–0.20 | Reduce for higher hardness |
| Alloy steel (hardened) | 0.04–0.12 | Use lower end |
| Stainless steel | 0.04–0.14 | Lower end for austenitic |
| Cast iron | 0.06–0.35 | Higher feeds possible |
| Aluminum | 0.06–0.25 | Chip breaker critical |
Correction Factors
Depth Correction
As hole depth increases, both speed and feed must be reduced to account for increasing friction, reduced coolant effectiveness, and tool deflection:
| L/D Ratio | Speed Factor | Feed Factor |
|---|---|---|
| < 5:1 | 1.0 | 1.0 |
| 5:1–10:1 | 0.9 | 0.9 |
| 10:1–20:1 | 0.8 | 0.8 |
| 20:1–50:1 | 0.7 | 0.7 |
| 50:1–100:1 | 0.6 | 0.6 |
| > 100:1 | 0.5 | 0.5 |
Example: For a gun drilling operation in low-carbon steel at 20:1 L/D ratio, start at 180 m/min × 0.8 = 144 m/min and 0.10 mm/rev × 0.8 = 0.08 mm/rev.
Hardness Correction
When workpiece hardness differs from the standard range, adjust cutting speed:
| Hardness (HB) | Speed Factor |
|---|---|
| < 150 | 1.2 |
| 150–250 | 1.0 (baseline) |
| 250–350 | 0.8 |
| 350–450 | 0.6 |
| > 450 | 0.4 |
Coolant Pressure Correction
If coolant pressure at the tool is below the recommended range, reduce parameters:
| Coolant Condition | Speed Factor | Feed Factor |
|---|---|---|
| Above recommended pressure | 1.0 | 1.0 |
| At recommended pressure | 1.0 | 1.0 |
| 20% below recommended | 0.9 | 0.85 |
| 40% below recommended | 0.8 | 0.7 |
| Below 50% of recommended | Do not drill | Do not drill |
Machine Rigidity Correction
| Machine Condition | Speed Factor | Feed Factor |
|---|---|---|
| New, rigid machine | 1.0 | 1.0 |
| Well-maintained machine | 0.95 | 0.95 |
| Older machine with some wear | 0.85 | 0.85 |
| Machine with alignment issues | Do not use | Do not use |
Calculation Examples
Example 1: Gun Drilling 10 mm Hole in Low-Carbon Steel
Given:
- Material: Low-carbon steel (annealed, 125 HB)
- Drill diameter: 10 mm (0.394 in)
- Target depth: 200 mm (L/D = 20:1)
- Insert size: 10
Step 1 — Select base speed: From the gun drilling table: Vc = 180–200 m/min. Start at 180 m/min.
Step 2 — Select base feed: From the feed table for insert size 10: 0.06–0.18 mm/rev. Start at 0.10 mm/rev.
Step 3 — Apply depth correction: L/D = 20:1. Factor = 0.8. Adjusted speed: 180 × 0.8 = 144 m/min Adjusted feed: 0.10 × 0.8 = 0.08 mm/rev
Step 4 — Calculate RPM: RPM = (144 × 1000) / (π × 10) = 4,583 RPM
Step 5 — Calculate feed rate: mm/min = 0.08 × 4,583 = 367 mm/min
Starting parameters: 4,580 RPM, 0.08 mm/rev, 367 mm/min
Example 2: BTA Drilling 50 mm Hole in Medium-Carbon Steel
Given:
- Material: Medium-carbon steel (Q&T, 250 HB)
- Drill diameter: 50 mm (1.97 in)
- Target depth: 1,000 mm (L/D = 20:1)
Step 1 — Select base speed: From the BTA table: Vc = 90–160 m/min for medium-carbon steel Q&T. Start at 120 m/min.
Step 2 — Select base feed: From the BTA diameter table for 30–50 mm: 0.06–0.16 mm/rev. Start at 0.12 mm/rev.
Step 3 — Apply depth correction: L/D = 20:1. Factor = 0.8. Adjusted speed: 120 × 0.8 = 96 m/min Adjusted feed: 0.12 × 0.8 = 0.096 mm/rev
Step 4 — Calculate RPM: RPM = (96 × 1000) / (π × 50) = 611 RPM
Step 5 — Calculate feed rate: mm/min = 0.096 × 611 = 59 mm/min
Starting parameters: 610 RPM, 0.10 mm/rev, 59 mm/min
Penetration Rate Comparison
Typical penetration rates achievable in production (for reference):
| Material | Gun Drilling (10 mm) | BTA Drilling (50 mm) | BTA Drilling (100 mm) |
|---|---|---|---|
| Low-carbon steel | 200–400 mm/min | 50–80 mm/min | 30–60 mm/min |
| Alloy steel (annealed) | 150–300 mm/min | 40–70 mm/min | 25–50 mm/min |
| Stainless steel | 80–150 mm/min | 25–50 mm/min | 15–35 mm/min |
| Cast iron | 250–500 mm/min | 60–100 mm/min | 40–80 mm/min |
| Aluminum | 300–600 mm/min | 70–120 mm/min | 50–90 mm/min |
| Titanium | 40–80 mm/min | 15–30 mm/min | 10–20 mm/min |
Note: These are typical ranges for production drilling. Actual penetration rates depend on machine rigidity, coolant system capability, and surface finish requirements.
Troubleshooting Parameter Selection
Signs Parameters Need Adjustment
| Observation | Probable Cause | Adjustment |
|---|---|---|
| Chip packing | Feed too high or speed too low for chip breaking | Increase speed, reduce feed, or adjust chip breaker |
| Stringy chips | Feed too low — chip breaker not engaging | Increase feed |
| Powder chips (dust) | Feed too low or tool rubbing | Increase feed |
| Tool wear excessive | Speed too high | Reduce speed by 15–20% |
| Edge chipping | Feed too high or interrupted cut | Reduce feed at cross-holes |
| Poor surface finish | Feed too high or speed too low | Reduce feed or increase speed |
| Chatter marks | Speed in resonant range or feed too high | Change speed by 20%, reduce feed |
| Bore oversize | Speed too high relative to feed | Reduce speed or increase feed |
| Bore undersize | Tool wear or speed too low | Increase speed, replace tool |
Parameter Adjustment Guidelines
| Parameter | Effect on Chip Evacuation | Effect on Tool Life | Effect on Surface Finish |
|---|---|---|---|
| Increase speed | Improves chip breaking | Reduces tool life | Improves finish |
| Decrease speed | May cause stringy chips | Extends tool life | May degrade finish |
| Increase feed | Increases chip load, may cause packing | Reduces tool life | Degrades finish |
| Decrease feed | May cause stringy chips | Extends tool life | Improves finish |
Critical rule: Change only one parameter at a time. Change by 10–15% increments. Document the result before making the next adjustment. This is the only reliable way to optimize deep hole drilling parameters.
Safety Margins for Starting Parameters
When starting a new application, apply these safety margins to the table values:
| Condition | Speed Safety Factor | Feed Safety Factor |
|---|---|---|
| Known material, known tool | 0.9 | 0.85 |
| New material, known tool | 0.8 | 0.75 |
| Known material, new tool design | 0.75 | 0.7 |
| New material, new tool | 0.65 | 0.6 |
| Unknown coolant condition | 0.8 | 0.75 |
Summary Table
| Aspect | Key Information |
|---|---|
| Gun drilling cutting speed range | 20–220 m/min (65–720 SFM) depending on material |
| BTA drilling cutting speed range | 30–220 m/min (100–720 SFM) depending on material |
| Gun drilling feed range | 0.02–0.28 mm/rev depending on insert size and material |
| BTA drilling feed range | 0.04–0.35 mm/rev depending on diameter and material |
| Depth correction | Reduce speed and feed by 50% at L/D > 100:1 |
| Hardness correction | Reduce speed by 20% per 100 HB above 250 HB |
| RPM formula | RPM = (Vc × 1000) / (π × Dia) for metric |
| Feed rate formula | mm/min = mm/rev × RPM |
| Starting strategy | Use lower end of range, increase parameters based on chip formation |
| Change rule | Change one parameter at a time, 10–15% increments |
FAQ
What cutting speed should I use for gun drilling stainless steel?
For austenitic stainless steel (304, 316), start at 50–80 m/min (165–260 SFM) for carbide-tipped gun drills. Use the lower end for smaller diameters or deeper holes. For ferritic and martensitic stainless (410, 430), start at 60–100 m/min (195–330 SFM). Stainless steel produces tough, stringy chips that challenge chip evacuation, so chip breaker geometry is critical — use a chip breaker specifically designed for ISO M materials. Feed rates should start at 0.03–0.08 mm/rev.
How do I calculate RPM for a deep hole drilling operation?
Use the formula: RPM = (Vc × 1000) / (π × Drill Diameter in mm) for metric, or RPM = (SFM × 3.82) / Drill Diameter in inches for imperial. For example, to gun drill a 10 mm hole in low-carbon steel at 180 m/min: RPM = (180 × 1000) / (π × 10) = 4,583 RPM. Then calculate the feed rate: mm/min = feed per revolution × RPM = 0.08 × 4,583 = 367 mm/min.
What is the correct feed rate for BTA drilling a 100 mm hole in carbon steel?
For a 100 mm diameter BTA drill in medium-carbon steel, start with a feed rate of 0.15–0.25 mm/rev (the 80–120 mm diameter range in the BTA table). Apply the depth correction based on your hole depth. The cutting speed should be 90–140 m/min depending on material condition. Starting parameters: approximately 380 RPM (using the middle of the speed range) and 0.18 mm/rev feed, giving a penetration rate of approximately 68 mm/min.
How do deep hole cutting parameters differ from conventional drilling?
Deep hole drilling parameters are typically 40–60% of conventional drilling parameters for the same material and diameter. The reduction is necessary because: (1) chip evacuation is more difficult and must be managed continuously, (2) coolant must travel much farther to reach the cutting zone, (3) the tool is more slender and prone to deflection and vibration, and (4) heat builds up along the entire bore length. Conventional drilling feeds and speeds should never be used as starting points for deep hole drilling.
When should I reduce cutting speed for deep hole drilling?
Reduce cutting speed when: tool life is shorter than expected (excessive flank wear), chip packing occurs at the current speed/feed combination, the L/D ratio exceeds 20:1, workpiece hardness is above 300 HB, coolant pressure at the tool is below specification, machine rigidity is compromised by age or condition, or when drilling difficult materials (titanium, high-temp alloys, work-hardening stainless steels). Reduce speed in 10–15% increments and evaluate the effect on chip formation and tool wear.