Appearance
A job shop receives an urgent order for 200 deep-drilled holes in 316L stainless steel. The drawing specifies 12 mm diameter, 480 mm depth, surface finish Ra 1.6 µm. The operator sets parameters based on experience with 4140 steel: speed 60 m/min, feed 0.020 mm/rev, coolant pressure 50 bar. The first hole takes eight minutes. The surface finish measures Ra 3.2 µm. The tool shows visible edge wear after three holes. The operator calls the tool supplier, who provides a stainless-specific parameter set: speed 45 m/min, feed 0.008 mm/rev, coolant pressure 80 bar. The next hole takes 12 minutes — 50% longer cycle time. But the surface finish is Ra 1.2 µm, the tool shows no measurable edge wear after 20 holes, and the hole diameter is within 0.01 mm of nominal. The original parameters were optimized for productivity in steel. The corrected parameters are optimized for the material. The difference is not in the machine, the tool, or the coolant chemistry — it is entirely in the numbers entered into the CNC program.
The Three Interdependent Variables
Deep hole drilling has three primary parameters that interact to determine hole quality, tool life, and productivity:
Cutting speed (Vc): The surface speed at which the cutting edge passes the workpiece, expressed in meters per minute. Determines the thermal load on the cutting edge and the material removal rate.
Feed rate (f): The axial advance per revolution of the drill, expressed in millimeters per revolution. Determines chip thickness, surface finish, and cutting forces.
Coolant pressure and flow: The hydraulic conditions at the cutting edge that control chip evacuation, cooling, and lubrication.
These three variables cannot be optimized independently. Increasing cutting speed generates more heat, which requires higher coolant flow. Increasing feed rate produces thicker chips, which requires higher coolant pressure for evacuation. The optimum parameter set is the combination that produces acceptable chip shape, surface finish, tool life, and cycle time for a specific material and hole geometry.
Cutting Speed by Material
Cutting speed in deep hole drilling is limited by the thermal tolerance of the cutting edge. Exceeding the maximum speed for a given material causes rapid flank wear, crater wear, or edge chipping.
Gun Drilling — Recommended Cutting Speeds
| Material | Hardness (HB) | Cutting Speed (m/min) |
|---|---|---|
| Low-carbon steel (1010, 1020) | ≤ 180 | 70 – 100 |
| Alloy steel (4140, 4340) annealed | 180 – 280 | 50 – 80 |
| Alloy steel quenched and tempered | 280 – 350 | 40 – 60 |
| Tool steel | 200 – 300 | 30 – 50 |
| Stainless steel (304, 316) | ≤ 200 | 30 – 50 |
| Stainless (17-4 PH, 15-5 PH) | 300 – 400 | 20 – 35 |
| Gray cast iron | 180 – 250 | 60 – 90 |
| Ductile cast iron | 200 – 300 | 50 – 80 |
| Aluminum (6061, 7075) | 60 – 100 | 80 – 160 |
| Brass and bronze | 80 – 150 | 80 – 150 |
| Titanium (Ti6Al4V) | 300 – 400 | 15 – 30 |
| Inconel and nickel alloys | 250 – 400 | 15 – 25 |
| Hardened steel (40 – 60 HRC) | 400 – 600 | 15 – 25 |
These values assume carbide-tipped gun drills with adequate coolant pressure. For HSS gun drills, reduce speeds by approximately 50%.
BTA Drilling — Recommended Cutting Speeds
BTA drilling operates at higher speeds than gun drilling for equivalent diameters because the internal chip evacuation provides better cooling at the cutting edge.
| Material | Cutting Speed (m/min) |
|---|---|
| Low-carbon steel | 80 – 140 |
| Alloy steel (quenched and tempered) | 60 – 100 |
| Stainless steel | 50 – 80 |
| Gray cast iron | 80 – 120 |
| Aluminum | 100 – 200 |
| Titanium | 20 – 40 |
Speed Selection Strategy
Within the recommended range, start at the lower third and increase based on chip appearance and tool wear:
- If chips are short and well-broken with no visible edge chipping after 10 holes, increase speed by 10%.
- If chips show discoloration (blue or brown tint) or the cutting edge displays crater wear, reduce speed by 15%.
- If tool life is the priority, run at the lower end of the recommended range. For maximum productivity with acceptable tool life, run at the upper end.
Feed Rate by Material and Diameter
Feed rate in deep hole drilling must be high enough to produce a chip thickness that breaks naturally but low enough to maintain the required surface finish.
Feed Rate Formula
The feed rate is selected as a function of the drill diameter and the material. A general starting point is:
f = 0.001 × D × K
Where f is feed in mm/rev, D is drill diameter in mm, and K is a material factor:
| Material | K Factor |
|---|---|
| Low-carbon steel | 1.0 – 1.5 |
| Alloy steel | 0.8 – 1.2 |
| Stainless steel | 0.5 – 0.8 |
| Cast iron | 1.5 – 2.0 |
| Aluminum | 1.5 – 2.5 |
| Titanium | 0.4 – 0.6 |
For a 12 mm drill in low-carbon steel: f = 0.001 × 12 × 1.2 = 0.014 mm/rev.
Gun Drilling Feed Rate by Diameter — Steel
| Drill Diameter (mm) | Feed Range (mm/rev) | Starting Point (mm/rev) |
|---|---|---|
| 3 – 4 | 0.005 – 0.015 | 0.008 |
| 5 – 6 | 0.010 – 0.025 | 0.015 |
| 8 – 10 | 0.015 – 0.035 | 0.020 |
| 12 – 16 | 0.020 – 0.050 | 0.025 |
| 18 – 25 | 0.030 – 0.080 | 0.040 |
| 30 – 40 | 0.050 – 0.120 | 0.070 |
For aluminum, multiply these values by 1.5–2.0. For stainless steel or titanium, multiply by 0.5–0.7.
BTA Drilling Feed Rate
BTA drilling feed rates are significantly higher than gun drilling for the same diameter:
| Drill Diameter (mm) | Steel Feed (mm/rev) |
|---|---|
| 16 – 25 | 0.08 – 0.20 |
| 25 – 40 | 0.12 – 0.30 |
| 40 – 65 | 0.15 – 0.40 |
| 65 – 100 | 0.20 – 0.50 |
Feed Rate and Chip Shape
The most reliable indicator of correct feed rate is chip shape:
| Chip Shape | Indication | Action |
|---|---|---|
| Short conical or "sixes and nines" | Correct feed | Maintain |
| Long stringy chips | Feed too low | Increase feed by 20% |
| Needle-like fragments | Feed too high or dull edge | Reduce feed or regrind tool |
| Powder or dust | Feed too high for material | Reduce feed by 30% |
| Discolored chips | Excessive speed or low coolant | Adjust speed or pressure |
TIP
Adjust only one parameter at a time when optimizing. If the chip shape is correct but surface finish is marginal, adjust feed rate first. If tool wear is excessive, adjust cutting speed first. Changing both simultaneously makes it impossible to identify which change produced the result.
Coolant Pressure and Flow
Coolant pressure and flow are not secondary parameters in deep hole drilling — they are as critical as speed and feed. Inadequate coolant conditions make correct speed and feed settings irrelevant.
Coolant Pressure by Drill Diameter
| Drill Diameter (mm) | Gun Drilling Pressure (bar) | BTA Drilling Pressure (bar) |
|---|---|---|
| 2 – 4 | 100 – 150 | — |
| 4 – 8 | 60 – 100 | — |
| 8 – 14 | 40 – 70 | 30 – 80 |
| 14 – 25 | 30 – 60 | 25 – 60 |
| 25 – 40 | 20 – 40 | 20 – 50 |
| 40 – 65 | — | 15 – 40 |
| 65 – 100 | — | 10 – 30 |
These pressures must be measured at the drill shank — not at the pump. A pressure gauge installed at the pump can read 20–40% higher than the pressure actually reaching the cutting edge.
Material-Specific Coolant Requirements
| Material | Pressure Requirement | Notes |
|---|---|---|
| Low-carbon steel | Standard range | Standard EP oils sufficient |
| Alloy steel | Upper end of range | Sulfurized EP oils recommended |
| Stainless steel | Upper end + 10% | High pressure prevents work-hardening |
| Aluminum | Lower end | Higher flow more important than pressure |
| Titanium | Upper end + 20% | Coolant critical — never stop feed |
| Cast iron | Lower end | Can be drilled dry in some cases |
Flow Rate Requirements
Coolant velocity at the cutting edge must be sufficient to transport chips out of the hole. The minimum velocity for effective chip transport is 8–12 m/s depending on drill diameter.
The flow rate Q (L/min) required to achieve velocity V (m/s) in a drill of diameter D (mm) with coolant hole area A (mm²) is:
Q = (V × A × 60) / 1000
For a typical gun drill with coolant hole area equal to approximately 10% of the drill cross-section, the flow rate at 10 m/s velocity is:
| Drill Diameter (mm) | Minimum Flow Rate (L/min) |
|---|---|
| 6 | 15 |
| 10 | 30 |
| 16 | 60 |
| 25 | 120 |
| 40 | 200 |
Coolant Temperature
Coolant temperature should be maintained at 20–30°C with variation of no more than ±5°C during production. Coolant temperature affects viscosity, which directly impacts the pressure delivered to the drill tip. A 10°C temperature rise reduces oil viscosity by approximately 40%, requiring pump speed adjustment to maintain consistent pressure.
Optimizing for Surface Finish
Surface finish in deep hole drilling is controlled primarily by feed rate and tool condition. The theoretical surface roughness generated by a single-point cutting edge is:
Ra = f² / (32 × r)
Where f is feed in mm/rev and r is the nose radius in mm. For a typical gun drill with 0.4 mm nose radius:
| Target Ra (µm) | Maximum Feed (mm/rev) |
|---|---|
| 0.8 | 0.010 |
| 1.6 | 0.015 |
| 3.2 | 0.020 |
To improve surface finish:
Reduce feed rate — This is the most direct method. However, reducing feed below 0.005 mm/rev can produce chip shapes that are too thin to break, causing chip wrapping and flute clogging.
Increase cutting speed — Within the material's recommended range, higher speeds produce better surface finish by reducing built-up edge formation.
Increase coolant pressure — Higher pressure at the cutting edge improves lubrication at the guide pad contact surfaces, reducing friction marks on the hole wall.
Check tool condition — A worn cutting edge or chipped guide pad degrades surface finish immediately. If surface finish degrades over a production run, the tool is approaching the end of its regrind interval.
Optimizing for Tool Life
Tool life in deep hole drilling is determined primarily by cutting speed and coolant conditions.
Cutting Speed and Tool Life
The relationship between cutting speed and tool life follows the Taylor tool life equation:
V × Tⁿ = C
Where V is cutting speed, T is tool life, n is the tool life exponent (typically 0.15–0.25 for carbide), and C is a constant. This means a 20% reduction in cutting speed approximately doubles tool life. Conversely, a 20% increase in cutting speed reduces tool life by approximately 50%.
Feed Rate and Tool Life
Feed rate has a smaller effect on tool life than cutting speed in deep hole drilling. A 20% reduction in feed increases tool life by approximately 20–30%. However, reducing feed too much produces thin chips that do not carry away heat effectively, which can actually reduce tool life.
Coolant and Tool Life
Inadequate coolant pressure accelerates tool wear by:
- Allowing chips to recirculate past the cutting edge
- Reducing lubrication at the guide pad contact surfaces
- Failing to remove heat from the cutting zone
A 20 bar pressure drop below the minimum requirement for a given diameter reduces tool life by approximately 40–60%.
Practical Tool Life Targets
| Material | Holes per Regrind (Gun Drill) | Holes per Edge (BTA Indexable) |
|---|---|---|
| Low-carbon steel | 200 – 500 | 80 – 150 |
| Alloy steel (4140) | 80 – 200 | 50 – 100 |
| Stainless steel | 30 – 80 | 20 – 50 |
| Aluminum | 500 – 2000 | 100 – 300 |
| Titanium | 15 – 40 | 10 – 25 |
Balancing Productivity and Quality
The optimum parameter set is rarely the maximum possible feed rate or the longest possible tool life. It is the combination that achieves the required hole quality at the lowest cost per hole.
Cost Per Hole Calculation
Cost per hole includes:
- Machine time cost (cycle time × machine hourly rate)
- Tool cost per hole (tool purchase or regrind cost divided by holes per regrind)
- Coolant cost (negligible per hole for production volumes)
- Inspection cost (higher if process capability is marginal)
For a typical deep hole drilling operation with a machine rate of €80/hour, tool cost of €50 per regrind, and 100 holes per regrind:
- Reducing cycle time by 20% saves €16 per hour in machine cost
- Reducing tool life by 50% adds €0.50 per hole in tool cost
The crossover point where faster feeds become uneconomical due to tool cost depends on the specific values. For most production deep hole drilling, feeding at 80–90% of the maximum recommended rate and running the tool to 80% of its maximum regrind interval produces the lowest cost per hole.
Parameter Adjustment Sequence
When setting up a new deep hole drilling job:
Set coolant pressure to the recommended value for the drill diameter and material. This is the foundation parameter — correct coolant enables everything else.
Set cutting speed at the low end of the recommended range for the material. Run 10 holes and inspect for edge wear.
Set feed rate at the middle of the recommended range for the diameter. Examine chip shape. Adjust feed up or down until chip shape is acceptable.
Adjust speed upward in 10% increments. At each step, run 10 holes and check surface finish and edge condition. Stop when surface finish target is met or edge wear becomes visible.
Adjust feed upward in 10% increments if cycle time reduction is needed. Stop when surface finish degrades below target or chip shape becomes unacceptable.
FAQ
What is the most important parameter in deep hole drilling?
Coolant pressure is the foundation parameter. Without adequate coolant pressure and flow, the correct speed and feed cannot produce a quality hole. Insufficient coolant causes chip packing, tool breakage, and poor surface finish regardless of the speed and feed selected.
How do I calculate RPM from cutting speed?
RPM = (Vc × 1000) / (π × D), where Vc is cutting speed in m/min and D is drill diameter in mm. For 50 m/min in a 10 mm drill: RPM = (50 × 1000) / (π × 10) = 1591 RPM.
What feed rate should I use for a 6 mm gun drill in stainless steel?
Start at 0.008–0.012 mm/rev at a cutting speed of 30–40 m/min with coolant pressure of 80–100 bar. The feed should be at the lower end of the range until chip shape is verified.
Why does my tool wear rapidly even at recommended speeds?
Check coolant pressure at the drill shank. A 30% pressure drop from pump to tool is common and can reduce tool life by 50% or more. Also verify coolant temperature — oil above 40°C loses viscosity and lubricity.
How do I balance surface finish and productivity?
Reduce feed rate to achieve the required surface finish, then increase cutting speed (within the material's range) to recover productivity. The higher speed generates more heat but the increased material removal rate compensates for the lower feed.
What is the maximum depth-to-diameter ratio for gun drilling?
Standard gun drills can achieve 100:1 depth-to-diameter ratios with correct parameters. Ratios up to 200:1 are possible with optimized parameters, whip guides, and counter-rotation.
Can I increase feed rate on a BTA drill without affecting hole quality?
BTA drills can run at 5–7 times the feed rate of gun drills at equivalent diameters. The feed rate for BTA is limited by chip evacuation capacity and machine power, not by surface finish requirements.
How does chip shape indicate correct parameters?
Short conical or "C-shaped" chips indicate correct feed and speed. Long stringy chips indicate feed too low. Discolored chips indicate excessive speed or inadequate coolant. Powder or dust indicates severe tool wear or incorrect geometry.
What coolant pressure is needed for small diameter gun drills?
For drills under 4 mm diameter, minimum 100 bar (1450 psi) at the drill shank. Pressures of 120–150 bar are common for 2–3 mm drills. The small coolant hole creates significant pressure drop that must be accounted for at the pump.
How often should I adjust parameters for a running job?
Parameters should remain stable once optimized. Adjust only when material batch changes, tool supplier changes, or coolant conditions change. A stable process with documented parameters produces more consistent results than continuous adjustment.
Summary
Deep hole drilling parameters form an interdependent system where coolant pressure, cutting speed, and feed rate must be matched to the material, diameter, and depth requirement.
The selection sequence should always be:
Coolant first — Set pressure and flow to the requirements of the drill diameter and material. Measure at the drill shank, not the pump. Verify temperature stability.
Speed second — Start at the lower third of the recommended range for the material. Adjust upward based on edge wear observation. A 20% speed reduction doubles tool life.
Feed third — Start at the middle of the recommended range for the diameter. Adjust based on chip shape. Feed rate determines surface finish directly.
Balance last — Once the hole meets quality requirements, adjust for productivity by incrementally increasing speed and feed. Stop when quality degrades or tool life becomes uneconomical.
The most reliable indicator of correct parameter selection is chip shape. A consistent flow of short, conical chips across the full drilling cycle confirms that all three parameters — coolant, speed, and feed — are correctly balanced. Change one parameter at a time, document the results, and build a site-specific parameter database that captures what works for your materials, machines, and tools.