Appearance
The difference between a successful gun drilling operation and a broken tool is often a 10% error in cutting speed — and the right number depends more on what you are drilling than how big the hole is.
Overview
Cutting speed and feed rate are the two primary variables that the operator controls in gun drilling and BTA drilling. Together they determine tool life, surface finish, chip form, and process stability.
For gun drilling specifically, parameters must balance three competing requirements:
- Chip formation — chips must be small enough to evacuate through the V-flute
- Tool temperature — cutting speed determines temperature at the cutting edge
- Productivity — higher speeds and feeds reduce cycle time
This article provides starting-point parameters organized by material group. These are recommended starting values — adjust based on chip form, tool wear, and surface finish results.
Calculating Spindle Speed
Spindle RPM is calculated from cutting speed using the standard formula:
RPM = (Vc × 1000) / (π × D)
Where:
- Vc = cutting speed in m/min
- D = drill diameter in mm
Pre-Calculated RPM by Diameter and Speed
| Drill Ø (mm) | Vc = 20 m/min | Vc = 40 m/min | Vc = 80 m/min | Vc = 120 m/min |
|---|---|---|---|---|
| 3 | 2,122 | 4,244 | 8,488 | 12,732 |
| 5 | 1,273 | 2,546 | 5,093 | 7,639 |
| 8 | 796 | 1,592 | 3,183 | 4,775 |
| 10 | 637 | 1,273 | 2,546 | 3,820 |
| 12 | 531 | 1,061 | 2,122 | 3,183 |
| 16 | 398 | 796 | 1,592 | 2,387 |
| 20 | 318 | 637 | 1,273 | 1,910 |
| 25 | 255 | 509 | 1,019 | 1,528 |
Carbon and Alloy Steels
Carbon and alloy steels are the most common workpiece materials for gun drilling. Parameters depend primarily on hardness.
| Material | Hardness (HB) | Vc (m/min) | Feed (mm/rev) | Notes |
|---|---|---|---|---|
| Low carbon (< 0.25% C) | < 180 | 60 – 80 | 0.020 – 0.050 | Stringy chips, use chip breaker |
| Medium carbon (1045, 1055) | 180 – 250 | 50 – 70 | 0.020 – 0.040 | Standard parameters |
| Alloy steel (4140, 4340) | 250 – 350 | 40 – 60 | 0.015 – 0.035 | Reduce speed as hardness increases |
| High alloy / tool steel | 300 – 400 | 30 – 50 | 0.010 – 0.025 | Low feed, high coolant pressure |
| Q&T steel (30–40 HRC) | 300 – 380 | 35 – 50 | 0.010 – 0.025 | Use coated carbide gun drills |
Feed Rate by Diameter for Carbon/Alloy Steel
| Drill Ø (mm) | Feed Range (mm/rev) | Typical Starting Point |
|---|---|---|
| 3 – 5 | 0.008 – 0.020 | 0.012 |
| 5 – 8 | 0.012 – 0.030 | 0.018 |
| 8 – 12 | 0.020 – 0.040 | 0.025 |
| 12 – 16 | 0.025 – 0.050 | 0.030 |
| 16 – 20 | 0.030 – 0.060 | 0.040 |
| 20 – 30 | 0.040 – 0.080 | 0.050 |
Chip color tells you if speed is correct
In steel gun drilling, chip color is an immediate diagnostic: straw or light blue chips indicate correct cutting temperature (600–700°C at the cutting zone). Dark blue or purple chips mean speed is too high. Silver chips mean speed is too low (risk of built-up edge). This rule applies to steel only — do not use it for stainless or aluminum.
Stainless Steels
Stainless steels require lower cutting speeds and careful feed management to avoid work hardening.
| Material | Condition | Vc (m/min) | Feed (mm/rev) | Critical Notes |
|---|---|---|---|---|
| Austenitic (304, 316) | Annealed | 20 – 40 | 0.010 – 0.030 | Never dwell — work hardens instantly |
| Ferritic (430) | Annealed | 30 – 50 | 0.015 – 0.035 | Less work hardening than austenitic |
| Martensitic (410, 420) | Annealed | 25 – 40 | 0.010 – 0.025 | Higher hardness range |
| Duplex (2205, 2507) | Annealed | 15 – 30 | 0.008 – 0.020 | Very low speeds, high pressure |
Stainless Steel Guidelines
- Feed must be continuous — stopping feed while the tool rotates causes work hardening that destroys the cutting edge
- Use sulfurized cutting oil for best lubricity and tool life
- Carbide grade: Use micrograin carbide with TiAlN coating for heat resistance
- Coolant pressure: Minimum 60 bar, preferably 80–120 bar for chip evacuation
Aluminum
Aluminum is the most productive material for gun drilling, allowing high speeds and feeds.
| Alloy Type | Vc (m/min) | Feed (mm/rev) | Notes |
|---|---|---|---|
| Wrought (6061, 7075) | 100 – 160 | 0.030 – 0.080 | High speeds, risk of BUE |
| Cast (A356, 319) | 80 – 120 | 0.020 – 0.060 | Lower speeds due to silicon content |
| High-silicon (> 12% Si) | 60 – 100 | 0.015 – 0.040 | Abrasive, use PCD or fine-grain carbide |
Aluminum Challenges
- Built-up edge (BUE) — aluminum cold-welds to the carbide cutting edge at low speeds. Maintain Vc above 100 m/min when possible
- Chip packing — stringy aluminum chips can jam the V-flute. Use polished flute gun drills with chip breakers
- Coolant: Kerosene-based or aluminum-specific cutting fluid. Water-soluble emulsion at 8–12% concentration
Titanium Alloys
Titanium's low thermal conductivity concentrates heat at the cutting edge, requiring lower speeds.
| Alloy | Condition | Vc (m/min) | Feed (mm/rev) | Notes |
|---|---|---|---|---|
| Ti-6Al-4V (Grade 5) | Annealed | 20 – 35 | 0.010 – 0.025 | Most common alloy |
| Ti-6Al-4V ELI | Annealed | 20 – 30 | 0.010 – 0.020 | Aerospace grade |
| CP Titanium (Grade 2) | Annealed | 25 – 40 | 0.015 – 0.030 | Gummy, risk of BUE |
| Ti-10V-2Fe-3Al | Aged | 15 – 25 | 0.008 – 0.015 | High strength, difficult |
Titanium Guidelines
- Keep feed constant — never let the tool dwell in titanium
- Use sharp cutting edges — dull tools generate excessive heat instantly
- High coolant pressure (80–120 bar) is essential for heat removal
- Avoid coolant interruption — thermal shock can crack the carbide tip
Titanium fires are a real risk
Titanium chips can ignite at high cutting temperatures, particularly at speeds above 40 m/min with inadequate coolant. Maintain coolant flow at all times. Never let titanium chips accumulate dry. If you see sparks at the cutting zone, stop the feed immediately and increase coolant pressure before resuming at reduced speed.
Heat-Resistant Superalloys (HRSA)
Inconel, Hastelloy, and similar nickel-based alloys are the most difficult materials for gun drilling.
| Alloy | Condition | Vc (m/min) | Feed (mm/rev) | Notes |
|---|---|---|---|---|
| Inconel 718 | Annealed | 12 – 20 | 0.005 – 0.015 | Most common, work hardens |
| Inconel 625 | Annealed | 15 – 25 | 0.008 – 0.018 | Less hardening than 718 |
| Hastelloy X | Solution treated | 10 – 18 | 0.005 – 0.012 | Very abrasive |
| Waspaloy | Aged | 8 – 15 | 0.004 – 0.010 | Extreme difficulty |
HRSA Guidelines
- Cutting speed is the primary limitation — do not exceed 20 m/min for Inconel 718
- Use TiAlN-coated carbide — coating provides thermal barrier
- Low feed prevents edge chipping HRSA chips are notch-hardening
- Coolant pressure 80–150 bar — necessary for chip evacuation
- Tool life will be 5–20% of steel — plan for frequent regrinds
Cast Iron
| Cast Iron Type | Vc (m/min) | Feed (mm/rev) | Notes |
|---|---|---|---|
| Gray iron (GG25) | 50 – 80 | 0.020 – 0.060 | Good chip formation, abrasive |
| Ductile iron (GGG40) | 40 – 70 | 0.015 – 0.045 | Nodular graphite, tougher |
| Malleable iron | 40 – 60 | 0.015 – 0.040 | Similar to ductile |
Cast iron produces short, discontinuous chips that evacuate easily. The primary wear mechanism is abrasion from graphite and carbide particles in the microstructure.
Coolant Parameters by Material
| Material | Pressure (bar) | Flow (L/min) | Coolant Type | Concentration |
|---|---|---|---|---|
| Carbon steel | 40 – 80 | 2 – 5 per mm Ø | Emulsion or oil | 8 – 12% |
| Alloy steel | 50 – 100 | 2 – 5 per mm Ø | Emulsion or oil | 10 – 12% |
| Stainless steel | 60 – 120 | 3 – 6 per mm Ø | Sulfurized oil preferred | N/A (neat oil) |
| Aluminum | 30 – 60 | 2 – 4 per mm Ø | Emulsion or kerosene | 8 – 10% |
| Titanium | 80 – 150 | 3 – 6 per mm Ø | Emulsion with EP additives | 10 – 15% |
| Inconel / HRSA | 80 – 150 | 3 – 6 per mm Ø | Sulfurized oil preferred | N/A (neat oil) |
| Cast iron | 30 – 50 | 2 – 4 per mm Ø | Emulsion | 8 – 10% |
Starting Point Selection Strategy
Rule 1: Start Low, Increase Gradually
Begin at 70% of the recommended cutting speed and 50% of the recommended feed. Increase speed first (in 10% steps) until chip color or tool temperature indicates the correct range, then increase feed until chip form is optimal.
Rule 2: Feed Determines Chip Form
In gun drilling, feed rate directly controls chip thickness. If chips are long and stringy, increase feed. If chips are powder-like or the tool chatters, decrease feed.
Rule 3: Speed Determines Tool Life
Tool life follows an exponential relationship with cutting speed. A 20% increase in speed reduces tool life by approximately 50%. For production operations, optimize for the speed that gives acceptable tool life at the required feed rate.
Summary
| Material | Vc (m/min) | Feed (mm/rev) | Coolant Pressure (bar) | Primary Challenge |
|---|---|---|---|---|
| Carbon steel | 40 – 80 | 0.015 – 0.060 | 40 – 80 | Chip control |
| Alloy steel | 30 – 60 | 0.010 – 0.050 | 50 – 100 | Tool wear at hardness |
| Stainless steel (austenitic) | 20 – 40 | 0.010 – 0.030 | 60 – 120 | Work hardening |
| Aluminum | 80 – 160 | 0.020 – 0.080 | 30 – 60 | Built-up edge |
| Titanium (Ti-6Al-4V) | 20 – 35 | 0.010 – 0.025 | 80 – 150 | Heat concentration |
| Inconel 718 | 12 – 20 | 0.005 – 0.015 | 80 – 150 | Low speed requirement |
| Cast iron | 40 – 80 | 0.015 – 0.060 | 30 – 50 | Abrasive wear |
FAQ
What is the correct cutting speed for gun drilling 1045 steel?
For 1045 steel (180–250 HB), start at Vc = 50–60 m/min with an uncoated carbide gun drill. With TiAlN-coated tools, increase to 60–70 m/min. Adjust based on chip color — straw to light blue indicates correct speed. Feed rate should be 0.020–0.040 mm/rev depending on diameter.
What happens if I run a gun drill too fast?
Excessive cutting speed causes: rapid flank wear and crater wear, dark blue or purple chips, poor surface finish (tearing or scoring), increased power consumption, and risk of brazing failure at the carbide tip joint. In extreme cases, the carbide tip detaches inside the hole.
What happens if feed rate is too low in gun drilling?
Too low a feed rate causes: thin chips that cannot evacuate properly, rubbing instead of cutting (work hardening on stainless), built-up edge on aluminum, poor surface finish, and reduced productivity. In gun drilling, feed must be high enough to produce chips thick enough for the coolant to transport.
What are the best cutting parameters for drilling Inconel 718?
For Inconel 718, use Vc = 12–18 m/min, feed = 0.008–0.015 mm/rev, coolant pressure > 80 bar with sulfurized oil, and TiAlN-coated micrograin carbide gun drills. Expect tool life of 5–20% compared to steel. Plan for regrinding after 20–50 holes depending on depth ratio.
How do I adjust parameters for deep holes (high L/D)?
For holes exceeding 50:1 depth ratio, reduce cutting speed by 10–15% and feed by 15–20%. At 100:1 L/D, reduce speed by 20–30% and feed by 25–35%. The reductions compensate for increased friction along the drill shank and reduced coolant effectiveness at depth.
Can I use the same parameters for BTA drilling as gun drilling?
No. BTA drilling uses higher feed rates (typically 0.10–0.25 mm/rev) and slightly lower cutting speeds than gun drilling in the same material. BTA's multi-edge design distributes the chip load across multiple inserts, allowing higher total feed. However, surface finish is generally not as fine as gun drilling in the same material.
Cutting parameters depend on machine rigidity, coolant system capability, tool geometry, and specific material properties. The values in this article are recommended starting points for production applications. Always verify with tool supplier recommendations for your specific tool and material combination. This article reflects industry knowledge as of 2026.