Here are the cutting parameters I use as starting points for deep hole drilling. These are starting points — adjust based on the specific material, machine, and tooling. I’ve collected these numbers over years of setup work, and they save me a lot of trial and error.
Cutting Speed Selection by Material
Cutting speed is the first parameter I set. It directly affects tool life and hole quality. Run too fast and the tool edge breaks down. Run too slow and you risk work hardening and poor chip formation.
The table below shows the surface speed ranges I use for gun drilling. All values are in meters per minute (multiply by 3.28 for SFM). I pick the middle of the range for an initial pass.
| Material | Cutting Speed (m/min) | Typical SFM |
|---|---|---|
| Low-carbon steel (1018, 1020) | 100-140 | 330-460 |
| Alloy steel (4140, 4340) | 60-90 | 200-300 |
| Tool steel (D2, H13) | 45-70 | 150-230 |
| Stainless steel (304, 316) | 50-75 | 165-245 |
| Aluminum (6061, 7075) | 120-200 | 395-655 |
| Cast iron (gray, ductile) | 60-100 | 200-330 |
| Titanium (6Al-4V) | 25-45 | 80-150 |
| Superalloys (Inconel, Hastelloy, Waspaloy) | 15-30 | 50-100 |
That’s eight material families. For superalloys especially, I stay conservative — a 0.1 mm wear flat on the tool is enough to scrap the hole. Also refer to my gun drilling speeds and feeds reference for notes on specific alloys.
Feed Rate by Diameter
Feed rate controls chip thickness. In deep hole drilling, chip evacuation is the bottleneck. If the chip is too thick it jams in the flute. Too thin and it won’t break, leading to a packed chip string.
I choose feed rate based on tool diameter and process type. The table covers my usual ranges.
| Diameter Range | Gun Drilling (mm/rev) | BTA Drilling (mm/rev) |
|---|---|---|
| Under 6 mm | 0.008-0.025 | Not typical |
| 6-12 mm | 0.015-0.040 | Not typical |
| 12-25 mm | 0.020-0.060 | 0.06-0.12 |
| 25-50 mm | 0.030-0.080 | 0.08-0.15 |
| 50-100 mm | Not typical | 0.10-0.20 |
| Over 100 mm | Not typical | 0.12-0.25 |
Inside these ranges, I bias toward the higher feed on softer materials and toward the lower feed on tough or stringy materials.
Coolant Pressure by Diameter and Material
Coolant does three jobs: flush chips, lubricate the cut, and remove heat. The pressure I run depends on the hole diameter, the material, and the L/D ratio.
Here is my coolant pressure table for gun drilling.
| Diameter | Low-Pressure Range | High-Pressure Range | Notes |
|---|---|---|---|
| Under 6 mm | 100 bar (1450 psi) | 200 bar (2900 psi) | Small drills need high pressure |
| 6-15 mm | 70 bar (1000 psi) | 140 bar (2000 psi) | Standard range |
| 15-30 mm | 55 bar (800 psi) | 100 bar (1450 psi) | Lower pressure works here |
| 30-50 mm | 40 bar (600 psi) | 70 bar (1000 psi) | BTA may need 200-400 psi only |
Material also matters. For titanium I run toward the high-pressure side because the chips are long and stringy. For cast iron I can drop 20% below the standard range because the chips are short and brittle and flush easily.
For BTA drilling, the coolant path is different — through the tube annulus, not the drill shank. My BTA coolant pressures are typically 200-500 psi (14-35 bar) regardless of diameter, with higher pressure at the small end.
The Speed-Feed-Coolant Triangle
These three parameters are interdependent. I think of them as a triangle.
- Higher speed generates more heat, which requires more coolant volume to remove.
- Higher feed produces thicker chips, which need more coolant pressure to evacuate.
- If I push speed up, I often drop feed slightly and bump coolant pressure 10%.
- If I push feed up, I drop speed slightly to keep chip load manageable.
When one leg of the triangle changes, the other two need attention. I never adjust speed alone without checking coolant flow.
Adjusting for L/D Ratio
L/D ratio — the ratio of hole depth to hole diameter — is the defining constraint in deep hole drilling. My starting parameters assume an L/D up to 30:1. Beyond that, everything changes.
Here is the reduction rule I follow:
- L/D 30:1 to 40:1 → reduce cutting speed by 10%, reduce feed by 10%
- L/D 40:1 to 50:1 → reduce cutting speed by 20%, reduce feed by 15%
- L/D 50:1 to 80:1 → reduce cutting speed by 30%, reduce feed by 20%
- L/D 80:1 to 120:1 → reduce cutting speed by 40%, reduce feed by 25%
- Over 120:1 → reduce cutting speed by 50% or more, reduce feed by 30%
A rule of thumb: reduce speed and feed by roughly 10-20% for every additional 10:1 L/D beyond 30:1. This accounts for the increasing friction, heat buildup, and chip evacuation distance. I also increase coolant pressure 10-15% at each step past 30:1 to help push chips the full length of the hole.
My Parameter Setup Workflow
Here is the exact sequence I follow when setting up a new job.
Step 1 — Identify material. I look up the cutting speed range from the material table above. For an unknown alloy I start conservative at 60 m/min and watch the chips.
Step 2 — Calculate RPM. Once I know the cutting speed, I hit the RPM calculation guide to convert surface speed to spindle speed. The formula is always: RPM = (Vc x 1000) / (pi x D), where Vc is cutting speed in m/min and D is tool diameter in mm.
Step 3 — Select feed rate. I pick a feed rate from the diameter table. I start at the middle of the range.
Step 4 — Set coolant pressure. I look up the recommended pressure for the hole diameter. If the material is tough or stringy, I go high. If the L/D is past 30:1, I add 15%.
Step 5 — Check the triangle. I run the three numbers through the interdependency check. If I am running high speed with high L/D I make sure coolant pressure is on the high end too.
Step 6 — First test. I drill a short pilot start, then check chip formation. Good chips are short, broken, and uniform — comma shapes or half-moons. Bad chips are long ribbons or dust.
Step 7 — Adjust. If chips are long and stringy I increase feed or decrease speed. If the tool squeals I drop feed first. If the hole finish is poor I check RPM and coolant pressure.
Step 8 — Lock in. Once chips look right and finish is acceptable I record the parameters for the job card.
Key Takeaways
- Start with material selection to determine cutting speed, then calculate RPM from speed and diameter.
- Feed rate depends on diameter and process — thicker tools can handle higher feed, but chip evacuation is the real limit.
- Coolant pressure must be matched to diameter, material, and L/D ratio — there is no universal setting.
- The speed-feed-coolant triangle means you cannot change one parameter without checking the other two.
- For every 10:1 L/D beyond 30:1, reduce speed and feed by roughly 10-20% and increase coolant pressure by 10-15%.
- Always test the first hole and adjust based on chip shape and sound. The numbers on the page are starting points, not gospel.