AISI 4140 and 4340 are the most widely used through-hardening alloy steels in mechanical engineering. Combined, they account for a substantial portion of deep hole drilling work in sectors ranging from oil and gas to aerospace, automotive, and heavy equipment. A 4140 or 4340 shaft, spindle, pin, or cylinder body requiring a deep hole is one of the most common jobs a deep hole drilling shop will encounter.
Despite their prevalence, these materials present distinct challenges in deep hole drilling. Their chromium-molybdenum chemistry provides good strength and toughness, but also generates higher cutting forces than carbon steels, requires careful coolant management, and demands specific parameter adjustments based on heat treatment condition. Furthermore, 4140 and 4340 behave differently from each other — 4340’s higher nickel content gives it superior toughness but significantly reduces machinability.
This guide provides comprehensive, manufacturer-sourced cutting data for deep hole drilling 4140 and 4340 alloy steel in all common heat treatment conditions, covering gun drilling and BTA methods.
Material Overview
AISI 4140 — Chromium-Molybdenum Steel
4140 is a low-alloy steel containing chromium and molybdenum as the primary alloying elements. It offers a good balance of strength, toughness, and wear resistance at moderate cost.
Chemical Composition (Weight %)
| Element | Range |
|---|---|
| Carbon | 0.38–0.43% |
| Manganese | 0.75–1.00% |
| Chromium | 0.80–1.10% |
| Molybdenum | 0.15–0.25% |
| Silicon | 0.15–0.35% |
Mechanical Properties by Condition
| Condition | Tensile Strength | Yield Strength | Elongation | Hardness |
|---|---|---|---|---|
| Annealed | 655 MPa (95 ksi) | 414 MPa (60 ksi) | 26% | 197 HB / 92 HRB |
| Quenched & Tempered (50 mm section) | 930 MPa (135 ksi) | 770 MPa (112 ksi) | 17% | 275 HB |
| Quenched & Tempered (Condition U) | 930–1080 MPa | ≥740 MPa | ≥12% | 269–331 HB |
| Prehardened (typical) | 850–1000 MPa | 650–850 MPa | 13–18% | 28–32 HRC (269–302 HB) |
| Hardened (max section) | — | — | — | Up to 38 HRC |
Standards: AISI 4140, ASTM A29, AMS 6349/6382, DIN 42CrMo4 (1.7225), BS 708M40, GB 42CrMo
Machinability Rating: 65% in annealed condition (relative to AISI 1112 = 100%), approximately 50% in prehardened condition.
AISI 4340 — Nickel-Chromium-Molybdenum Steel
4340 is a higher-alloy variant of 4140 with added nickel for significantly improved hardenability and toughness. It can achieve higher strength at larger cross-sections than 4140.
Chemical Composition (Weight %)
| Element | Range |
|---|---|
| Carbon | 0.38–0.43% |
| Manganese | 0.60–0.90% |
| Chromium | 0.70–0.90% |
| Molybdenum | 0.20–0.30% |
| Nickel | 1.65–2.00% |
| Silicon | 0.15–0.35% |
Mechanical Properties by Condition
| Condition | Tensile Strength | Yield Strength | Elongation | Hardness |
|---|---|---|---|---|
| Annealed | 745 MPa (108 ksi) | 470 MPa (68 ksi) | 22% | 217 HB |
| Quenched & Tempered (50 mm section) | 1030 MPa (150 ksi) | 830 MPa (120 ksi) | 14% | 290 HB |
| Quenched & Tempered (aircraft grade) | 1080–1280 MPa | ≥930 MPa | ≥10% | 36–45 HRC |
| High-strength condition | Up to 1960 MPa | Up to 1600 MPa | — | Up to 50 HRC |
Standards: AISI 4340, AMS 6414/6415, DIN 40NiCrMo6, BS 817M40
Machinability Rating: Approximately 50% in annealed condition, declining to 30–40% at higher hardnesses. 4340 is consistently rated as more difficult to machine than 4140 at equivalent hardness.
4140 vs 4340: Key Differences for Deep Hole Drilling
| Factor | 4140 | 4340 |
|---|---|---|
| Machinability | Good (65% annealed) | Moderate (50% annealed) |
| Maximum hardness after heat treatment | ~38 HRC | ~50 HRC |
| Hardenability | Medium — good in sections up to 50 mm | High — uniform hardness in sections up to 100 mm+ |
| Relative cutting speed | Baseline (recommended baseline) | Reduce by 15–25% at equivalent hardness |
| Chip formation | Generally favorable, good chip breaking | More ductile chips, harder to break |
| Work hardening tendency | Low to moderate | Moderate — more pronounced at higher cutting speeds |
| Best for | General machinery, shafts, gears, cost-sensitive applications | Aerospace landing gear, high-stress components, large cross-sections |
Recommended Speeds and Feeds for Gun Drilling
AISI 4140 — Gun Drilling with Carbide-Tipped Tools
The following values are from published technical data by Allied Machine & Engineering, adjusted for general deep hole drilling application. Speeds are in SFM (surface feet per minute) and feeds in IPR (inches per revolution). For metric conversion: multiply SFM by 0.3048 for m/min, IPR by 25.4 for mm/rev.
Carbide-Tipped Gun Drills — 4140 by Hardness
| Hardness (BHN) | Speed (SFM) | Feed (IPR) by Series (Diameter Range) |
|---|---|---|
| 125–175 BHN (annealed) | 420 | Y/Z (0.374–0.500“): 0.006; 0 (0.500–0.695“): 0.009; 1 (0.695–0.960“): 0.012; 2 (0.960–1.380“): 0.015; 3 (1.380–1.882“): 0.017 |
| 175–225 BHN | 390 | Y/Z: 0.005; 0: 0.009; 1: 0.012; 2: 0.015; 3: 0.017 |
| 225–275 BHN | 360 | Y/Z: 0.005; 0: 0.009; 1: 0.012; 2: 0.015; 3: 0.017 |
| 275–325 BHN (prehardened) | 340 | Y/Z: 0.004; 0: 0.009; 1: 0.012; 2: 0.015; 3: 0.015 |
| 325–375 BHN | 310 | Y/Z: 0.004; 0: 0.008; 1: 0.011; 2: 0.014; 3: 0.015 |
Series diameter ranges: Y/Z = 0.374–0.500“ (9.5–12.7 mm), Series 0 = 0.500–0.695“ (12.7–17.7 mm), Series 1 = 0.695–0.960“ (17.7–24.4 mm), Series 2 = 0.960–1.380“ (24.4–35.1 mm), Series 3 = 1.380–1.882“ (35.1–47.8 mm).
Carbide-Tipped Gun Drills — 4140 by Drill Diameter (125–225 BHN)
| Diameter (inch) | Diameter (mm) | Speed (SFM) | Feed (IPR) |
|---|---|---|---|
| 3/8“ | 9.5 | 175–195 | 0.004–0.006 |
| 1/2“ | 12.7 | 165–180 | 0.006–0.009 |
| 5/8“ | 15.9 | 105–140 | 0.009–0.012 |
| 3/4“ | 19.1 | 90–105 | 0.010–0.014 |
| 1“ | 25.4 | 70–100 | 0.012–0.016 |
| 1-1/4“ | 31.8 | 55–75 | 0.014–0.018 |
| 1-1/2“ | 38.1 | 50–70 | 0.016–0.020 |
AISI 4340 — Gun Drilling with Carbide-Tipped Tools
4340 requires reduced speeds compared to 4140 at the same hardness. The following data combines values from Allied Machine and Mitsubishi Carbide technical publications.
Carbide-Tipped Gun Drills — 4340 by Hardness
| Hardness (BHN) | Speed (SFM) | Feed (IPR) by Series (Diameter Range) |
|---|---|---|
| 225–300 BHN | 325–350 | Y/Z: 0.003–0.004; 0: 0.006–0.007; 1: 0.009–0.010; 2: 0.012–0.013; 3: 0.014–0.015 |
| 300–350 BHN | 300–325 | Y/Z: 0.003; 0: 0.006; 1: 0.009; 2: 0.012; 3: 0.014 |
| 350–400 BHN | 280–300 | Y/Z: 0.003; 0: 0.006; 1: 0.008; 2: 0.011; 3: 0.013 |
Carbide-Tipped Gun Drills — 4340 Small Diameters (Mitsubishi Data, 280–350 HB)
| Diameter | Speed (SFM) | Feed (IPR) |
|---|---|---|
| 1.0 mm (0.039“) | 65–100 | 0.0004–0.0011 |
| 1.6 mm (0.063“) | 65–100 | 0.0011–0.0030 |
| 2.0 mm (0.079“) | 130–180 | 0.0013–0.0037 |
| 2.5 mm (0.098“) | 130–180 | 0.0018–0.0047 |
Note that very small diameter gun drills operate at lower surface speeds due to the disproportionately high cutting edge temperatures at small diameters.
Recommended Speeds and Feeds for BTA Drilling
AISI 4140 — BTA / STS Drilling
BTA drilling allows higher penetration rates than gun drilling at equivalent diameters. The following data applies to single-tube (STS) BTA systems with carbide inserts.
BTA Drilling — 4140 by Hardness (Allied Machine T-A Series)
| Hardness (BHN) | Speed (SFM) | Feed (IPR) by Tube Size (Diameter Range) |
|---|---|---|
| 125–175 BHN (annealed) | 195–245 | 4–5 (0.374–0.500“): 0.004–0.006; 6–8 (0.500–0.695“): 0.007–0.009 |
| 175–225 BHN | 180–195 | 4–5: 0.004–0.006; 6–8: 0.007–0.009; 10 (0.695–0.960“): 0.009–0.011 |
| 225–275 BHN | 165–180 | 4–5: 0.004–0.005; 10: 0.008–0.010; 12–16 (0.960–1.380“): 0.011–0.013 |
| 275–325 BHN (prehardened) | 150–165 | 10: 0.008–0.010; 12–16: 0.011–0.013; 20–24 (1.380–1.882“): 0.013–0.015 |
| 325–375 BHN | 140–150 | 12–16: 0.010–0.012; 20–24: 0.012–0.014; 32 (2.000–2.500“): 0.014–0.016 |
BTA Drilling — 4140 (Quenched & Tempered, 280–320 HB)
Research on BTA drilling of quenched and tempered 4140 used the following parameters with carbide tooling:
- Cutting speed: 60–120 m/min (197–394 SFM)
- Feed rate: 0.150–0.300 mm/rev (0.006–0.012 IPR)
- Optimum parameters for surface finish: 90 m/min (295 SFM), 0.15 mm/rev (0.006 IPR)
- Higher speeds increase tool tip temperature, while higher feeds increase drilling torque
AISI 4340 — BTA Drilling
BTA Drilling — 4340 by Hardness
| Hardness (BHN) | Speed (SFM) | Feed (IPR) by Series |
|---|---|---|
| 225–300 BHN | 140–200 | Y/Z: 0.004–0.006; 0: 0.007–0.009; 1: 0.008–0.010; 2: 0.010–0.012; 3: 0.012–0.015 |
| 300–350 BHN | 120–180 | Y/Z: 0.004–0.005; 0: 0.007–0.008; 1: 0.008–0.009; 2: 0.009–0.011; 3: 0.011–0.014 |
| 350–400 BHN | 120–160 | Y/Z: 0.004; 0: 0.007; 1: 0.008; 2: 0.008–0.010; 3: 0.010–0.012 |
Real-World Case Study: 4340 Aerospace Landing Gear Component (BTA)
A documented application using Allied Machine’s BT-A drill on 4340 alloy steel for a landing gear component:
| Parameter | Value |
|---|---|
| Hole diameter | 2.050“ (52.1 mm) |
| Hole depth | 11.0“ (279 mm) |
| Spindle speed | 125 RPM |
| Feed rate | 0.006 IPR (0.152 mm/rev) |
| Penetration rate | 0.75 IPM (19 mm/min) |
| Cycle time | 1 min 20 sec |
| Tool life | 43 holes per insert edge |
| Coolant | 60 GPM oil |
Speeds and Feeds for Conventional (Twist) Drilling
For applications where deep holes are drilled using extended-length twist drills or where deep hole drilling is preceded by a pilot hole operation, the following general guidelines apply.
4140 — Conventional Carbide Drilling
| Hardness | Speed | Feed (IPR) |
|---|---|---|
| ≤ 375 BHN | 170–390 SFM | 1/8“: 0.003–0.006; 1/4“: 0.004–0.008; 3/8“: 0.006–0.012; 1/2“: 0.007–0.015 |
4340 — Conventional Carbide Drilling
| Hardness | Speed | Feed (IPR) |
|---|---|---|
| ≤ 350 HB | 150–200 SFM | 1/8“: 0.003; 1/4“: 0.004; 1/2“: 0.008 |
| 280–350 HB | 65–180 SFM (small diameters: 65–100) | Small diameters (1–2.5 mm): 0.0004–0.0047 IPR |
Coolant Pressure and Flow Requirements
Effective chip evacuation is essential in deep hole drilling of alloy steels. The chips produced by 4140 and 4340 are more cohesive than those from cast iron or free-machining steels, placing greater demands on the coolant system.
Recommended Coolant Parameters for Gun Drilling 4140
| Drill Diameter | Pressure (PSI) | Flow Rate (GPM) |
|---|---|---|
| 3/8“ – 1/2“ (9.5–12.7 mm) | 165–175 | 2.4–2.5 |
| 33/64“ – 11/16“ (13–17.5 mm) | 85–100 | 2.6–2.9 |
| 23/32“ – 1“ (18–25.4 mm) | 90–100 | 4.1–4.4 |
| 1“ – 1-3/8“ (25.4–35 mm) | 70–75 | 6–8 |
| 1-13/32“ – 1-7/8“ (36–47.6 mm) | 70–75 | 12–15 |
Values from Allied Machine for 4140 steel (carbide inserts). HSS tools require slightly lower pressure and flow.
BTA Drilling Coolant Requirements
BTA systems require higher pressure than gun drilling at equivalent diameters due to the more restrictive chip evacuation path through the tube interior. For alloy steels, increase coolant pressure by approximately 20–30% over the values recommended for gun drilling at the same diameter.
For material in the 300–400 BHN range, a documented military study on gun drilling 4140 (at 35–39 HRC) used a pump pressure of 190 PSI with a soluble oil coolant mixture at 10:1 water-to-oil ratio, powered by a 10 HP pump with a 180-gallon reservoir.
Coolant Type Recommendations
For deep hole drilling of 4140 and 4340 alloy steel:
- Annealed to 300 BHN: High-performance emulsion at 6–8% concentration, or low-viscosity cutting oil (10–20 cSt at 40°C). Emulsions provide adequate lubrication and better cooling; oils provide better lubricity and longer tool life.
- 300–375 BHN (prehardened): Low-viscosity cutting oil is preferred. The higher cutting forces require maximum lubrication at the cutting interface. If using water-based coolant, increase concentration to 8–10% and verify EP additive content.
- Above 375 BHN: Straight cutting oil only. Water-based coolants lack sufficient lubricity for the extreme pressures at the cutting edge in hardened material.
Tool Selection
Carbide Grade
For deep hole drilling 4140 and 4340, use carbide grades with the following characteristics:
- Substrate: Fine to medium grain tungsten carbide (6–10% cobalt)
- Coating: TiAlN or AlTiN (best high-temperature hardness for alloy steel)
- Edge preparation: Honed edge (0.02–0.05 mm radius) to prevent micro-chipping at entry
- Coolant hole: Single or dual internal coolant holes, sized for the diameter
Gun Drill Head Profile
For 4140 and 4340 alloy steel, the following gun drill head profiles are recommended:
- Profile G (Universal) — Standard choice for 4140 in annealed through prehardened condition. Provides good chip formation and stable burnishing.
- Profile E — Recommended for 4340 and higher-strength alloy steels. Eliminates tool sticking in the hole after the outer corner dulls. Suitable for accurate straightness requirements.
- Profile C — Use for 4340 in hardened condition (above 35 HRC). Provides increased back taper and larger coolant gaps to accommodate the more difficult chip evacuation from high-strength materials.
BTA Drill Head
For BTA drilling of 4140/4340:
- Brazed carbide heads for diameters under 20 mm
- Indexable insert heads for diameters 20 mm and above
- For 4340 at hardness above 300 BHN, use insert grades with increased edge toughness (less brittle than grades optimized for cast iron or aluminum)
Depth Adjustment Factors
The following adjustment factors from Allied Machine apply when drilling depths exceed 7× diameter:
| Drilling Condition | Speed Factor | Feed Factor |
|---|---|---|
| Standard depth (< 7×D) | 1.0 | 1.0 |
| 7×D to 12×D | 0.9 | 1.0 |
| 12×D to 20×D | 0.8 | 0.9 |
| 20×D to 30×D | 0.7 | 0.8 |
| Over 30×D | 0.6 | 0.7 |
Additionally, for extended-length tool holders (gun drills with long shanks):
| Holder Length | Speed Factor | Feed Factor |
|---|---|---|
| Standard | 1.0 | 1.0 |
| Extended | 0.9 | 1.0 |
| Long | 0.85 | 0.95 |
| XL | 0.8 | 0.9 |
| 3XL | 0.7 | 0.8 |
Deep Hole Drilling Procedure
The following step-by-step procedure is recommended for deep hole drilling of alloy steels with carbide gun drills or BTA tools.
Pilot Hole Requirements
A properly prepared pilot hole is critical for deep hole drilling accuracy in alloy steel. The pilot hole serves to guide the tool and prevent the chisel edge from walking at entry.
- Depth: Minimum 1×D, recommended 2×D for L/D ratios above 30:1
- Diameter: 0.0005–0.001“ (0.013–0.025 mm) larger than the gun drill diameter
- Point angle: The pilot drill should have a point angle greater than the deep hole drill to prevent the deep drill’s center from contacting the pilot bottom first
Entry Procedure
- Drill pilot hole at 100% recommended speed and feed
- Feed the deep hole drill to within 1.5 mm of the pilot hole bottom at maximum 50 RPM and 300 mm/min feed with coolant OFF
- Drill 1×D past the pilot hole bottom at 50% speed and 75% feed (allow 1-second dwell before feed start)
- Resume 100% speed and feed for the remainder of the hole
Running the Hole
- No peck cycle — pecking is not recommended with carbide deep hole drills. The interrupted cutting edge contact during re-entry causes micro-chipping.
- Continuous feed — maintain constant feed throughout. Do not stop the feed while the tool is cutting.
- Monitor chip form — check that chips are small and well-broken. Long stringy chips indicate that feed may be too low or chip breaker geometry needs adjustment.
Breakout and Retract
- Through holes: Reduce speed by 50% and feed by 25% before breakout. Do not break out more than 3 mm past full diameter.
- Retract: Reduce speed to maximum 50 RPM before retracting, with coolant OFF.
Surface Finish and Dimensional Accuracy
Deep hole drilling of 4140 and 4340 can achieve the following specifications:
| Parameter | Achievable Range |
|---|---|
| Surface finish (Ra) | 0.4–1.6 µm (gun drilling); 0.3–0.8 µm (BTA with optimized parameters) |
| Diameter tolerance | IT7–IT9 |
| Straightness | 0.5 mm per meter (gun drilling); varies with depth and setup for BTA |
Surface finish is influenced most strongly by feed rate and tool condition. Increasing spindle speed at a given feed rate improves surface finish. Tool wear degrades surface finish progressively — if Ra values begin to rise, inspect the cutting edge before continuing.
For material in the quenched and tempered condition (280–320 HB), research shows that feed rate has the greatest influence on surface roughness, followed by cutting speed. The interaction between speed and feed is significant — simply reducing feed without adjusting speed may not achieve the expected improvement.
Common Problems in Alloy Steel Deep Hole Drilling
Work Hardening
Symptom: Cutting forces increase progressively through the hole; tool begins to squeal or chatter; subsequent passes or tapping operations become difficult or impossible.
Cause: 4140 and particularly 4340 work harden when cutting conditions allow rubbing instead of clean shearing. This occurs most commonly at low feed rates, dull tools, or insufficient coolant pressure.
Solution:
- Maintain minimum feed rate of 0.003 IPR (0.075 mm/rev) for carbide tools — never dwell while the tool is in the cut
- Use sharp tools and replace at the first sign of dulling
- Ensure adequate coolant pressure and flow (refer to the coolant tables above)
- If work hardening has occurred, the hardened skin must be removed with a grinding operation before drilling can resume
Chip Breaking Difficulties
Symptom: Long stringy chips that wrap around the tool, chip packing in the flute or evacuation tube, torque spikes.
Cause: 4340’s higher toughness produces more ductile chips that resist breaking. Incorrect feed rate or chip breaker geometry for the material condition.
Solution:
- Increase feed rate incrementally until chips break into short segments (6–12 mm length is ideal)
- Verify chip breaker geometry is appropriate for alloy steel (some indexable inserts offer alloy-steel-specific chip breaker designs)
- If chips remain stringy at maximum recommended feed, consult the tool manufacturer for a chip breaker modification
- For BTA drilling, check that the chip former in the drill head has not been ground too deep in previous regrinds
Tool Wear at Guide Pads
Symptom: Oversized holes, poor surface finish, visible wear on the guide pad carbide.
Cause: Alloy steel generates higher cutting forces than carbon steels, placing greater load on the guide pads. The combination of high pressure and abrasive carbides in the steel accelerates pad wear.
Solution:
- Use coolant with proper EP additive content
- Verify that guide pad material grade matches the application (some manufacturers offer tougher grades for steel drilling)
- Monitor hole size trends — a gradual increase in diameter indicates pad wear
- For BTA tools, consider pad replacement or head disposal when diameter exceeds tolerance midpoint
Center Drift / Straightness Deviation
Symptom: Hole exits off-center; straightness measurement exceeds specification.
Cause: Inconsistent apex offset after tool regrinding is a known cause of straightness deviation in gun drilling. Research on gun drilling of nickel alloys confirms that inconsistent apex offset between regrinds leads to unbalanced cutting forces and hole deviation. The same principle applies to alloy steels.
Solution:
- Verify tool regrinding quality — lip height difference must be within 0.02 mm
- Check that the tool regrinding maintains consistent apex offset from one regrind to the next
- Ensure the pilot hole is correctly sized and aligned
- Whip guide positioning should be checked for correct spacing
Heat Treatment and Material Condition
The heat treatment condition of 4140 and 4340 has a larger effect on deep hole drilling parameters than almost any other variable. Using parameters intended for annealed material on a hardened workpiece will destroy the tool. Conversely, using conservative hardened-material parameters on annealed material wastes productive capacity.
Practical Guidelines by Condition
Annealed (197–241 HB) Use the upper end of the speed and feed ranges. Chip formation is generally favorable. Standard carbide grades with TiAlN coating perform well.
Prehardened (269–331 HB, typical 28–32 HRC) Reduce speeds by 15–25% from annealed values. Feeds should be reduced by approximately 10%. Use TiAlN-coated carbide exclusively. This is the most common condition for deep hole drilling of 4140.
Hardened (35–45 HRC) Reduce speeds by 40–50% from annealed values. Use feeds at the lower end of the recommended range. Consider CBN or ceramic tooling for the hardest conditions. Coolant pressure at the upper end of the recommended range. This condition is more common for 4340 than 4140, as 4340 can achieve higher hardness.
Machining Before vs After Heat Treatment
For deep holes in alloy steel components:
- Drill rough, heat treat, finish bore — This sequence produces the best geometric accuracy. The hole is drilled slightly undersize, then heat treated to final hardness, then finished with a BTA single-pass boring tool or precision reamer. The heat treatment step may cause distortion that is corrected in the finishing operation.
- Drill after heat treatment (prehardened stock) — Avoids the secondary finishing operation. Prehardened 4140 (28–32 HRC) is widely available and can be deep-hole drilled with carbide tooling at economical rates. For 4340 above 35 HRC, drilling becomes significantly more difficult and the rough-then-heat-treat-then-finish sequence is strongly recommended.
Summary
Deep hole drilling of 4140 and 4340 alloy steel is a routine operation in many shops, but achieving consistent results requires careful parameter selection based on the specific material condition:
- 4140 — The more machinable of the two alloys. Start with speeds of 300–420 SFM for carbide gun drills in annealed condition. Reduce to 150–340 SFM for prehardened material.
- 4340 — Requires 15–25% lower speeds than 4140 at equivalent hardness. Use Profile E or C gun drill head geometry for better chip control.
- Coolant — Use low-viscosity oil for high-pressure applications, or emulsion at 6–10% concentration. Maintain 165–190 PSI minimum pressure for diameters under 1/2“.
- Heat treatment condition is the most significant variable. Adjust parameters according to the hardness, not the grade name.
For related reading, see the Speeds and Feeds for Deep Hole Drilling Reference Tables, the Material Machinability Ratings for Deep Hole Drilling, and the Deep Hole Drilling Troubleshooting Guide.