Appearance
In conventional drilling, you can compensate for incorrect parameters by pecking, by using a stubby drill, or by ignoring chip form and simply extracting the tool to clear the flutes. None of these options exist in deep hole drilling. The parameters you choose are the only control you have over chip formation, tool temperature, and hole quality — and once the tool is past 10× diameter, you cannot intervene. Parameter selection is not a recommendation; it is the process.
Why Parameter Selection Differs for Deep Hole Drilling
Deep hole drilling is defined by a depth-to-diameter ratio exceeding 10:1. In practice, production gun drilling and BTA drilling routinely operate at 50:1 to 250:1. At these ratios, three constraints dominate:
| Constraint | Effect on Parameters |
|---|---|
| Chip evacuation path length | Chips must travel the full hole length without packing — feed rate must be high enough to break chips, but low enough to avoid chip volume overload |
| Coolant pressure drop | Pressure at the cutting edge is always lower than at the pump — the pressure drop increases with hole depth and limits the usable speed range |
| Column buckling | Feed force must not exceed the buckling limit of the drill tube — this sets an absolute upper bound on feed rate for a given L/D ratio |
Cutting Speed Selection
General Ranges by Drilling Method
| Method | Typical Cutting Speed Range |
|---|---|
| Gun drilling (carbide) | 70–160 m/min |
| Gun drilling (HSS) | 35–70 m/min |
| BTA drilling | 20–120 m/min |
| BTA with chipbreaker inserts | 50–140 m/min |
Cutting Speed by Material Group
| Material | Hardness (HB) | Cutting Speed Vc (m/min) |
|---|---|---|
| Low-carbon steel (< 0.25% C) | 125 | 80–140 |
| Alloy steel (< 0.55% C), Q&T | 250 | 50–100 |
| Tool steel, annealed | 200 | 50–100 |
| Stainless steel (austenitic) | 180 | 50–100 |
| Grey cast iron (ferritic/pearlitic) | 180 | 80–140 |
| Nodular cast iron (pearlitic) | 250 | 80–140 |
| Aluminium (wrought) | 60 | 100–200 |
| Brass and bronze | 90 | 100–200 |
| Titanium alloys | 300–400 | 8–25 |
Key principle: Harder materials require lower cutting speeds. The penalty for excessive speed is not gradual wear acceleration but thermal cracking of the carbide tip — a sudden, catastrophic failure that usually destroys both tool and workpiece.
Spindle Speed Calculation
Once cutting speed is selected, spindle speed is calculated from:
n = (1000 × Vc) / (π × D)Where:
- n = spindle speed (RPM)
- Vc = cutting speed (m/min)
- D = drill diameter (mm)
Example: For a 12 mm gun drill running at 90 m/min in alloy steel:
n = (1000 × 90) / (π × 12) = 2387 RPM| Drill Diameter | Vc = 80 m/min | Vc = 120 m/min | Vc = 160 m/min |
|---|---|---|---|
| 5 mm | 5093 RPM | 7640 RPM | 10186 RPM |
| 10 mm | 2546 RPM | 3820 RPM | 5093 RPM |
| 20 mm | 1273 RPM | 1910 RPM | 2546 RPM |
| 40 mm | 637 RPM | 955 RPM | 1273 RPM |
Tip: Most deep hole drilling machines have a maximum spindle speed limit that becomes the binding constraint for small diameters. If the calculated RPM exceeds the machine limit, reduce Vc — do not attempt to run at reduced RPM without reducing Vc, as the resulting speed will be too low for proper chip formation.
Feed Rate Selection
Feed Rate by Diameter and Material (mm/rev)
| Diameter Range (mm) | Brass | Aluminium | Carbon/Alloy Steel | Cast Iron |
|---|---|---|---|---|
| 1.9–2.49 | 0.003–0.015 | 0.002–0.012 | 0.003–0.007 | 0.005–0.019 |
| 5.0–5.99 | 0.010–0.069 | 0.010–0.109 | 0.016–0.026 | 0.018–0.068 |
| 10.0–11.99 | 0.020–0.139 | 0.025–0.174 | 0.030–0.049 | 0.050–0.120 |
| 20.0–23.99 | 0.040–0.249 | 0.060–0.254 | 0.060–0.107 | 0.106–0.207 |
| 32.0–39.99 | 0.064–0.380 | 0.096–0.455 | 0.085–0.154 | 0.160–0.245 |
| 40–50 | 0.072–0.399 | 0.105–0.488 | 0.091–0.169 | 0.180–0.254 |
BTA Feed Rate by Insert Type (ISCAR TRI-DEEP)
| Material Group | Feed fn (mm/rev) for Ø 16–18 mm | Feed fn (mm/rev) for Ø 18–40 mm |
|---|---|---|
| P (steel) | 0.025–0.10 | 0.025–0.13 |
| M (stainless) | 0.025–0.05 | 0.025–0.05 |
| K (cast iron) | 0.025–0.15 | 0.05–0.18 |
| N (non-ferrous) | 0.025–0.15 | 0.025–0.15 |
Feed Speed (Penetration Rate)
Feed speed (the rate at which the drill penetrates the workpiece) is calculated from feed per revolution and spindle speed:
Vf = fn × nWhere:
- Vf = feed speed (mm/min)
- fn = feed per revolution (mm/rev)
- n = spindle speed (RPM)
Example: A 12 mm drill at 2387 RPM with fn = 0.040 mm/rev:
Vf = 0.040 × 2387 = 95.5 mm/minWarning: Feed speed (Vf) is what the machine operator sets, but feed per revolution (fn) is the parameter that determines chip thickness and chip breakage. When adjusting parameters on the machine, always think in terms of fn, not Vf. If you increase spindle speed and keep Vf constant, fn drops — and chip breakage becomes unreliable.
Coolant Parameters
Pressure Requirements
| Method | Diameter Range | Coolant Pressure |
|---|---|---|
| Gun drilling | 1.4–6 mm | 70–200 bar (1000–3000 PSI) |
| Gun drilling | 6–19 mm | 50–140 bar (700–2000 PSI) |
| Gun drilling | > 19 mm | 35–100 bar (500–1400 PSI) |
| BTA drilling | 18–40 mm | 20–70 bar |
| BTA drilling | 40–100 mm | 10–50 bar |
Flow Rate Requirements
| Drill Diameter | Minimum Flow Rate |
|---|---|
| 5 mm | 8 L/min |
| 10 mm | 30 L/min |
| 20 mm | 100 L/min |
| 40 mm | 250 L/min |
| 60 mm | 400 L/min |
Coolant Pressure Drop
Coolant pressure at the cutting edge is always lower than at the pump. The pressure drop increases with:
- Hole depth — longer holes create more flow resistance
- Smaller clearance — the annular gap between drill tube and bore wall determines flow restriction
- Higher coolant viscosity — oil-based coolants have higher pressure drop than emulsions
Rule of thumb: If the coolant pressure gauge shows a 10% or greater drop from the starting pressure for the same flow rate, suspect chip blockage or internal erosion of the drill tube.
Tip: Install a pressure gauge at the coolant inlet of the machine spindle, not just at the pump. The difference between pump pressure and spindle pressure tells you the pressure losses in the coolant feed system. A sudden increase in this differential indicates a blockage; a gradual decrease over weeks indicates internal erosion or seal wear.
Feed Rate and Chip Formation
Research by Thil et al. (2013) on BTA drilling chip formation established that feed rate is the dominant parameter controlling chip morphology:
| Feed Rate | Chip Type | Evacuation Reliability | Surface Finish |
|---|---|---|---|
| < 0.06 mm/rev | Long spiral chips | Poor — high clogging risk | Excellent |
| 0.08–0.12 mm/rev | Curved and short spiral | Moderate — occasional jamming | Good |
| 0.12–0.18 mm/rev | C-shaped and short chips | Excellent | Acceptable |
| > 0.20 mm/rev | Fragment chips | Good | Poor — feed marks visible |
Why Feed Rate Controls Chip Breakage
Chip breakage in deep hole drilling depends on the chip curl radius and the bending strain imparted by the chipbreaker. A higher feed rate produces a thicker chip, which:
- Increases the bending strain at the chipbreaker
- Reduces the chip curl radius
- Causes the chip to fracture into short segments before it can form a long spiral
This relationship is well-established for both BTA and gun drilling. Cutting speed, by contrast, has a relatively minor effect on chip morphology — it primarily affects tool wear rate and cutting temperature.
Optimal Parameters from Published Research
| Workpiece Material | Optimal Vc | Optimal fn | Observed Chip Form |
|---|---|---|---|
| 42CrMo steel (Zheng et al., 2023) | 27.6 m/min | 0.18 mm/rev | C-shaped chips |
| 18MND5 steel (Thil et al., 2013) | 60–80 m/min | 0.10–0.16 mm/rev | Short spiral chips |
| TA10 titanium alloy | 8–12 m/min | 0.08–0.12 mm/rev | Short curved chips |
Material-Specific Parameter Strategies
Steels (Carbon and Alloy)
| Hardness | Strategy |
|---|---|
| < 200 HB | High Vc (80–140 m/min), moderate fn (0.05–0.12 mm/rev). Chip control is the priority — use the higher end of the fn range |
| 200–350 HB | Moderate Vc (50–90 m/min), moderate fn (0.06–0.14 mm/rev). Watch for built-up edge at lower speeds |
| > 350 HB | Low Vc (20–40 m/min), low fn (0.03–0.08 mm/rev). Tool wear is the limiting factor |
Stainless Steels
Austenitic stainless steels work-harden rapidly. The parameter strategy must:
- Use sufficient fn (> 0.04 mm/rev) to ensure the cutting edge passes below the work-hardened layer from the previous revolution
- Keep Vc moderate (50–80 m/min) to control heat generation
- Ensure coolant pressure is at the upper end of the recommended range
Never allow the feed rate to drop below 0.03 mm/rev in stainless steel — rubbing rather than cutting will work-harden the surface to the point where the next cut fractures the edge.
Cast Irons
Cast irons produce short, naturally broken chips. This relaxes the chip-control constraint and allows:
- Higher feed rates (up to 0.25 mm/rev for larger diameters)
- Moderate cutting speeds (70–140 m/min)
- Lower coolant pressure requirements
The primary concern in cast iron is abrasive wear from free graphite and carbide particles in the microstructure. Monitor flank wear (VB) more frequently than with steel.
Aluminium and Non-Ferrous
Aluminium alloys permit aggressive parameters but require attention to:
- Built-up edge formation at low speeds (below 60 m/min)
- Chip packing — although aluminium chips are short, they can weld together under pressure
- Coolant filtration — aluminium fines can clog coolant passages
Machine Constraints
Spindle Power
The net power required for deep hole drilling is:
Pnet = (D × fn × Vc × kc) / (4 × 60,000)Where:
- Pnet = net power (kW)
- D = drill diameter (mm)
- fn = feed per revolution (mm)
- Vc = cutting speed (m/min)
- kc = specific cutting force (N/mm²)
| Material | Specific Cutting Force kc (N/mm²) |
|---|---|
| Low-carbon steel | 1800–2200 |
| Alloy steel | 2200–2800 |
| Stainless steel | 2400–3000 |
| Cast iron | 1200–1800 |
| Aluminium | 700–900 |
Example: 20 mm BTA drill in alloy steel (kc = 2500), Vc = 80 m/min, fn = 0.10 mm/rev:
Pnet = (20 × 0.10 × 80 × 2500) / 240000 = 1.67 kWFeed Force and Column Buckling
The maximum feed force must not exceed the column buckling limit of the drill tube. For a tube of given diameter and wall thickness, the buckling load decreases with the square of the L/D ratio — at 100:1, the critical load is only 1% of what it is at 10:1.
| L/D Ratio | Approximate Maximum Feed Force (50 mm tube) |
|---|---|
| 10:1 | 50 kN |
| 50:1 | 8 kN |
| 100:1 | 2 kN |
| 150:1 | 0.9 kN |
Warning: If the machine is capable of applying more feed force than the tube can sustain in compression, the tube will buckle — not gradually but catastrophically. Most BTA machines are fitted with a feed force limiter. Verify it is set below the tube buckling limit before starting production. For gun drilling at high L/D ratios, the feed force is usually well below the buckling limit, but the drill can still bend elastically, causing hole deviation.
Starting Parameters vs Production Parameters
Parameter Ramp Strategy
Deep hole drilling should never start at full production parameters. The standard approach:
| Phase | Duration | Speed | Feed | Coolant |
|---|---|---|---|---|
| 1 — Guide entry | First 2× diameter | 50% of target | 30% of target | Full pressure |
| 2 — Stabilisation | 2× to 10× diameter | 80% of target | 70% of target | Full pressure |
| 3 — Production | 10× diameter onward | 100% | 100% | Full pressure |
Reasoning: During guide entry, the drill is supported only by the guide bush and has not yet established full bearing contact with the bore wall. The reduced parameters prevent deflection during this critical phase. Once the drill has penetrated 10× diameter, the bore wall provides full support and parameters can be increased.
Parameter Adjustment Based on Chip Form
| Observed Chip Form | Required Adjustment |
|---|---|
| Long continuous spiral | Increase fn (feed per revolution) |
| Powder or dust chips | Decrease fn (cutting edge is overloaded) |
| Chips welded or discoloured | Decrease Vc or increase coolant pressure |
| Ribbon chips with burns | Decrease Vc (thermal damage occurring) |
| Short C-shaped chips (target) | No adjustment needed |
| Inconsistent chip form (mix of types) | Check coolant pressure and flow stability |
Troubleshooting Parameter-Related Problems
| Problem | Most Likely Parameter Cause | Corrective Action |
|---|---|---|
| Chip clogging | fn too low for the diameter — chips are long spirals that cannot evacuate | Increase fn by 20–30% to promote chip breakage |
| Poor surface finish | fn too high, or Vc too low | Reduce fn by 15% or increase Vc by 10% — test which gives the better result |
| Oversize hole | Vc too high causing whipping, or fn too low causing rubbing | Reduce Vc by 15%, verify guide bush fit |
| Tool wear accelerating | Vc too high for the material grade | Reduce Vc by 20%, check coolant concentration |
| Built-up edge | Vc too low (< 40 m/min for steel) or coolant insufficient | Increase Vc or increase coolant pressure |
| Rifling marks on bore wall | fn too high, causing vibration at the cutting edge | Reduce fn by 10–15% |
| Spindle power exceeding limit | Vc, fn, or depth of cut exceeding machine capacity | Reduce fn first (it has the greatest effect on power) |
| Coolant pressure drop | Chip blockage in tube or worn coolant seals | Stop feed, retract tool, inspect for blockage |
| Hole deviation | fn too low (drill is rubbing, not cutting), or Vc incorrect for the material | Verify fn is above the minimum for the diameter |
FAQ
What is the difference between parameter selection for gun drilling vs BTA drilling?
Gun drilling typically uses higher cutting speeds (70–160 m/min) and lower feed rates (0.008–0.050 mm/rev). BTA drilling uses lower speeds (20–120 m/min) and higher feed rates (0.03–0.25 mm/rev). The difference reflects the fundamentally different chip evacuation systems: gun drills evacuate chips externally through a V-shaped flute, while BTA systems evacuate chips internally through the drill tube centre, allowing higher chip volume.
How do I calculate spindle RPM for deep hole drilling?
RPM = (1000 × Vc) / (π × D), where Vc is the cutting speed in m/min and D is the drill diameter in mm. For a 10 mm drill at 90 m/min: RPM = (1000 × 90) / (3.14159 × 10) = 2865 RPM.
What is the most important parameter for chip control?
Feed per revolution (fn) is the dominant parameter controlling chip breakage. Research consistently shows that feed rate has a greater effect on chip morphology than cutting speed. Higher feed rates produce thicker chips that break into short C-shaped segments. If chips are too long, increase fn; if chips are too fragmented or powdery, decrease fn.
What coolant pressure is needed for gun drilling?
Small-diameter gun drilling (under 6 mm) typically requires 70–200 bar (1000–3000 PSI). Larger diameters reduce the pressure requirement — a 20 mm gun drill typically runs at 50–100 bar. Minimum pressure for any gun drilling operation is 50 bar; below this, chip evacuation becomes unreliable.
How does hole depth affect parameter selection?
Deeper holes increase coolant pressure drop, chip evacuation distance, and column buckling risk. As hole depth increases, the pressure available at the cutting edge decreases, and the feed force must be limited to prevent tube buckling. For very deep holes (L/D > 100:1), coolant pressure at the pump may need to be increased to compensate for the pressure drop, and feed rate may need to be reduced to stay within the buckling limit.
What parameters should I use for stainless steel deep hole drilling?
For austenitic stainless steel: Vc = 50–80 m/min, fn = 0.04–0.08 mm/rev (never below 0.03 mm/rev to avoid work hardening). Coolant pressure at the upper end of the recommended range. Use the chipbreaker version of the drill if available — stainless steel produces tough chips that are harder to break.
How do I know if my parameters are correct?
The primary indicator is chip form. Short C-shaped or short spiral chips that evacuate consistently indicate correct parameters. Secondary indicators: stable spindle power (within 10% of calculated), good surface finish (within specification), and no abnormal tool wear. If chip form is correct, the parameters are in the right window regardless of whether they match published tables.
Should I start at full production parameters?
No. Use a parameter ramp strategy: start at 50% speed and 30% feed for the first 2× diameter (guide entry), increase to 80% speed and 70% feed from 2× to 10× diameter, and only go to 100% parameters after the drill is fully stabilised in the bore.
How does feed rate affect tool life in deep hole drilling?
Feed rate affects tool life differently by context. Higher feed rates increase mechanical load and can accelerate flank wear. However, very low feed rates can be more damaging — they cause rubbing rather than cutting, generate excessive heat, and can lead to work hardening in stainless steels. The optimum feed rate is the lowest one that produces reliable chip breakage, not the lowest possible feed rate.
What is the specific cutting force and how do I use it?
Specific cutting force (kc) is a material property that relates the cutting cross-section to the required cutting force. It is used to calculate net power: Pnet = (D × fn × Vc × kc) / 240000. Typical values: low-carbon steel 1800–2200 N/mm², alloy steel 2200–2800 N/mm², stainless steel 2400–3000 N/mm², aluminium 700–900 N/mm². Use the power calculation to verify that the selected parameters are within the machine's capacity.
Conclusion
Machining parameter selection for deep hole drilling is constrained by three interdependent limits: chip evacuation (feed rate must be high enough to break chips), coolant pressure (must be sufficient at the cutting edge, not just at the pump), and column buckling (feed force must not exceed the tube's critical load). Within these constraints, feed per revolution is the primary parameter — it determines chip morphology, which determines process reliability. Cutting speed is selected for tool life and surface finish. Coolant pressure and flow must be verified at the cutting edge, not assumed from the pump rating. The correct approach is to start conservatively (reduced speed and feed for the first 10× diameter), observe chip form, and adjust parameters based on what the chips reveal. A parameter table is a starting point, not a prescription — the chips tell you whether the settings are correct.