Appearance
A speed and feed chart for deep hole drilling is not a substitute for process development — it is a starting point. Every deep hole job differs in machine condition, tool geometry, coolant system capability, and workpiece setup. Use these values as initial settings and adjust based on actual chip shape, surface finish, and tool wear.
Gun Drilling Speeds and Feeds
Recommended Starting Parameters
| Material | Hardness (HB) | Cutting Speed (m/min) | Feed (mm/rev) | Coolant Pressure (bar) |
|---|---|---|---|---|
| Low-carbon steel (1018) | 100–180 | 80–120 | 0.02–0.06 | 60–100 |
| Medium-carbon steel (1045) | 180–250 | 60–90 | 0.02–0.05 | 80–120 |
| Alloy steel (4140) annealed | 200–280 | 55–80 | 0.02–0.05 | 80–120 |
| Alloy steel (4340) hardened | 280–350 | 35–50 | 0.015–0.04 | 100–150 |
| Tool steel (H13) annealed | 200–280 | 40–60 | 0.015–0.04 | 100–150 |
| Stainless steel (304) | 150–250 | 35–55 | 0.015–0.04 | 100–140 |
| Stainless steel (416) | 250–350 | 30–45 | 0.015–0.04 | 100–140 |
| Aluminum (6061) | 50–150 | 120–200 | 0.03–0.10 | 30–60 |
| Aluminum (cast, high Si) | 80–150 | 100–160 | 0.03–0.08 | 40–70 |
| Brass (free-machining) | 80–180 | 100–200 | 0.04–0.12 | 20–50 |
| Bronze (high-strength) | 150–250 | 35–55 | 0.02–0.05 | 40–70 |
| Cast iron (gray) | 150–250 | 40–70 | 0.03–0.08 | 30–70 |
| Cast iron (ductile) | 200–300 | 35–55 | 0.02–0.06 | 40–80 |
| Titanium (Ti-6Al-4V) | 300–400 | 15–25 | 0.01–0.03 | 120–180 |
| Inconel 718 | 350–500 | 10–18 | 0.008–0.02 | 150–200 |
Tip: For gun drilling, feed rate affects surface finish more than speed does. If surface finish is critical, use the lower end of the feed range. If tool life is the priority, use the lower end of the speed range.
BTA Drilling Speeds and Feeds
Recommended Starting Parameters
| Material | Hardness (HB) | Cutting Speed (m/min) | Feed (mm/rev) | Coolant Pressure (bar) |
|---|---|---|---|---|
| Low-carbon steel (1018) | 100–180 | 90–120 | 0.08–0.20 | 10–20 |
| Medium-carbon steel (1045) | 180–250 | 70–100 | 0.06–0.16 | 12–20 |
| Alloy steel (4140) annealed | 200–280 | 60–90 | 0.06–0.14 | 12–20 |
| Alloy steel (4340) hardened | 280–350 | 40–60 | 0.04–0.10 | 15–25 |
| Stainless steel (304) | 150–250 | 40–65 | 0.04–0.10 | 15–25 |
| Aluminum (6061) | 50–150 | 150–300 | 0.10–0.30 | 8–15 |
| Cast iron (gray) | 150–250 | 50–80 | 0.08–0.20 | 8–15 |
| Cast iron (ductile) | 200–300 | 40–60 | 0.06–0.16 | 10–15 |
| Titanium (Ti-6Al-4V) | 300–400 | 15–30 | 0.03–0.08 | 15–25 |
| Inconel 718 | 350–500 | 10–20 | 0.02–0.06 | 15–25 |
RPM and Feed Rate Calculation
Formulas
| Calculation | Formula | Example |
|---|---|---|
| RPM | (Vc × 1000) / (π × D) | For 10 mm drill, Vc=80 m/min: RPM = (80 × 1000) / (π × 10) = 2,546 RPM |
| Feed rate (mm/min) | RPM × feed/rev | At 2,546 RPM, 0.04 mm/rev: Feed = 2,546 × 0.04 = 102 mm/min |
| Cutting time (min) | Depth / feed rate | For 500 mm depth at 102 mm/min: Time = 500 / 102 = 4.9 min |
Quick RPM Reference Table
| Drill Dia. (mm) | 20 m/min | 40 m/min | 60 m/min | 80 m/min | 100 m/min | 150 m/min |
|---|---|---|---|---|---|---|
| 3 | 2,122 | 4,244 | 6,366 | 8,488 | 10,610 | 15,915 |
| 5 | 1,273 | 2,546 | 3,820 | 5,093 | 6,366 | 9,549 |
| 8 | 796 | 1,591 | 2,387 | 3,183 | 3,979 | 5,968 |
| 10 | 637 | 1,273 | 1,910 | 2,546 | 3,183 | 4,775 |
| 15 | 424 | 849 | 1,273 | 1,697 | 2,122 | 3,183 |
| 20 | 318 | 637 | 955 | 1,273 | 1,591 | 2,387 |
| 25 | 255 | 509 | 764 | 1,019 | 1,273 | 1,910 |
| 30 | 212 | 424 | 637 | 849 | 1,061 | 1,591 |
| 40 | 159 | 318 | 477 | 637 | 796 | 1,194 |
| 50 | 127 | 255 | 382 | 509 | 637 | 955 |
Correction Factors
Depth-to-Diameter Ratio Correction
| Depth-to-Diameter Ratio | Speed Factor | Feed Factor | Coolant Pressure Factor |
|---|---|---|---|
| Up to 10:1 | 1.0 | 1.0 | 1.0 |
| 10:1 to 30:1 | 0.95 | 0.90 | 1.2 |
| 30:1 to 50:1 | 0.90 | 0.85 | 1.4 |
| 50:1 to 100:1 | 0.85 | 0.80 | 1.6 |
| Over 100:1 | 0.80 | 0.75 | 2.0 |
Machine Condition Correction
| Machine Condition | Speed Factor | Feed Factor |
|---|---|---|
| New or well-maintained | 1.0 | 1.0 |
| Moderate wear (5+ years old) | 0.95 | 0.90 |
| Significant wear (10+ years) | 0.90 | 0.85 |
| Questionable coolant system | 0.85 | 0.80 |
Coolant Type Correction
| Coolant Type | Speed Factor | Feed Factor |
|---|---|---|
| Water-based emulsion (8–12%) | 1.0 | 1.0 |
| Oil-based (neat oil) | 1.1 | 1.1 |
| Synthetic coolant | 0.95 | 1.0 |
| Minimum quantity lubrication | 0.70 | 0.60 |
CNC Programming Examples
Gun Drilling Cycle (Fanuc-Style)
(10 mm gun drill in 1045 steel)
(Dia = 10 mm, Vc = 80 m/min, f = 0.04 mm/rev)
(Depth = 300 mm)
#1 = 2546 (RPM = 80*1000/(PI*10))
#2 = 102 (Feed mm/min = 2546*0.04)
#3 = 300 (Depth)
G00 X0 Y0 Z5
M03 S#1
M08 (Coolant on)
G01 Z-#3 F#2 (Drill to depth)
G04 P1 (Dwell to clear chips)
G00 Z5 (Rapid retract)
M09
M05BTA Drilling Cycle (Fanuc-Style)
(50 mm BTA drill in 4140 steel)
(Dia = 50 mm, Vc = 70 m/min, f = 0.12 mm/rev)
(Depth = 500 mm)
#1 = 445 (RPM = 70*1000/(PI*50))
#2 = 53 (Feed mm/min = 445*0.12)
#3 = 500 (Depth)
G00 X0 Y0 Z5
M03 S#1
M08 (Coolant on)
G01 Z-#3 F#2 (Drill to depth)
G04 P3 (Dwell 3 sec for chip clearance)
G00 Z5 (Rapid retract)
M09
M05Quick Diagnosis: Parameter Adjustment
Symptom-Based Guide
| Symptom | Likely Parameter Issue | Adjustment |
|---|---|---|
| Rapid flank wear | Speed too high | Reduce speed 10–15% |
| Edge chipping | Feed too high | Reduce feed 10–15% |
| Built-up edge | Speed too low | Increase speed 15–20% |
| Stringy chips | Feed too low | Increase feed 15–25% |
| Poor surface finish | Feed too high | Reduce feed 10–20% |
| High spindle load | Feed too high | Reduce feed 10% first |
| Vibration or chatter | Speed too high | Reduce speed 10% |
| Tool burning | Speed too high or coolant low | Reduce speed, check coolant |
| Oversize hole | Feed too high or runout | Reduce feed, check runout |
FAQ
What cutting speed should I use for gun drilling 4140 steel?
For 4140 alloy steel in the annealed condition (200–280 HB), use a cutting speed of 55–80 m/min and a feed rate of 0.02–0.05 mm/rev. Start at 60 m/min and 0.03 mm/rev, then adjust based on chip shape and tool wear. Coolant pressure should be 80–120 bar.
How do I calculate RPM from cutting speed in deep hole drilling?
RPM = (cutting speed in m/min × 1000) / (π × drill diameter in mm). For example, a 10 mm drill at 80 m/min: RPM = (80 × 1000) / (π × 10) = 2,546 RPM.
Does depth-to-diameter ratio affect speed and feed?
Yes. As the depth-to-diameter ratio increases, reduce speed and feed to compensate for reduced coolant effectiveness and increased tool deflection. At 50:1 ratio, reduce speed by 10% and feed by 15%. At 100:1, reduce speed by 20% and feed by 25%. Increase coolant pressure to compensate.
What is the difference between gun drilling and BTA speeds?
BTA drilling typically uses 10–20% higher cutting speeds and 2–3× higher feed rates than gun drilling for the same material. BTA uses lower coolant pressure but higher flow. The parameters differ because BTA uses indexable inserts compared to gun drilling's brazed carbide.
Where should I start when drilling a material for the first time?
Start at the lower end of the cutting speed range and the middle of the feed range. Drill one hole, inspect the chip shape (target: C-shaped chips), check surface finish, and listen for chatter. If chips are C-shaped and surface finish is acceptable, increase speed by 10% and drill another test hole. Repeat until chip shape or finish degrades, then back off to the previous good parameter.
Use this chart as a starting point, not a final specification. Every machine, tool, and workpiece combination is different. Optimize parameters based on the chips you see, not the chart you read. This article reflects industry practice as of 2026.