Deep Hole Drilling Techniques on CNC Machines

• 1
  Key takeaways
• 2
  What counts as deep hole drilling on a CNC
• 3
  Gun drilling: the precision standard for deep holes
• 4
  BTA and ejector drilling for higher removal rates
• 5
  CNC peck drilling: when it works and when it does not
• 6
  Tooling, speeds and feeds that survive deep cuts
• 7
  Coolant, chip evacuation and machine requirements
• 8
  Step by step: setting up a deep hole job
• 9
  Comparing deep hole drilling techniques on CNC
• 10
  Coolant and cutting data by method

A hole is deep when its depth passes roughly 5 times its diameter, written as L/D > 5. That ratio, not the absolute depth, is what changes the process. A Ø6 mm hole 40 mm deep is the same problem as a Ø60 mm hole 400 mm deep.

Three things degrade as L/D climbs. Chip evacuation gets harder because the flutes fill before the chips reach the surface. Tool deflection grows, so the drill walks off axis. Cutting heat has less time to leave with the chip, so the edge runs hotter. Past L/D 10, these effects decide the result. Past L/D 20, a special process is mandatory.

On a CNC machine the difficulty is not opening the hole. It is holding diameter tolerance, straightness and surface finish at the same time. A hole can be on size at the entry and 0.4 mm off center at the bottom. That is a scrap part, not a drilling problem you can fix later.

The practical targets for deep work are a diameter tolerance around ±0.05 mm for standard jobs and tighter when the drawing demands it, plus a finish between Ra 0.4 and Ra 1.6 μm for gun-drilled holes. Anything looser usually means a shorter hole or a different method.

Gun drilling uses a single-flute or two-flute tool with internal coolant holes and a V-shaped shank that supports the tool along the bore. Coolant enters through the shank and pushes chips out along the V groove. It covers L/D from 10 to 100 and is the method to choose when straightness and finish come first.

Typical results are straightness within 0.1 mm per 100 mm, diameter tolerance near ±0.012 mm under good conditions and a finish of Ra 0.4–1.6 μm. The price is speed. Feed rates sit at 0.005–0.05 mm/rev, so a Ø10 mm hole 300 mm deep takes a long cut.

Coolant pressure is not a suggestion here. Gun drilling needs 3–10 MPa and 10–40 L/min to flush the chip and cool the edge. Neat oil carries chips better than water-soluble coolant and gives better lubrication on the guide pads. If your machine tops out at 2 MPa, plan for a different method.

Use gun drilling for hydraulic bores, fuel injector bodies, mold cooling channels and medical shafts. Skip it for large diameters above about 40 mm, where BTA removes metal far faster, and for short holes where a standard drill is already on size.

BTA systems use a hollow boring bar with coolant fed from outside and chips evacuated through the inside of the bar. The chip never touches the finished wall, so the bore stays clean. Removal rates run 3 to 5 times faster than gun drilling, and the method covers diameters from 20 mm up to 300 mm.

Typical cutting data in steel is 60–120 m/min with feeds of 0.05–0.2 mm/rev. Coolant volume is the limit, not pressure: BTA needs 1–3 MPa but 100–400 L/min. That means a large tank, a high-flow pump and filtration down to 10–20 μm so fines do not score the bore.

Straightness is looser than gun drilling, often around 0.5 mm per 100 mm, and the entry needs a pilot hole or a bushing to start the cut. Surface finish lands at Ra 1.6–3.2 μm. On a lathe, the workpiece usually rotates while the bar stays still.

Ejector drilling sits between the two. It uses a double tube, so coolant flows down the outer gap and returns with the chips through the inner tube. It needs less volume than BTA and works well on machining centers where a rotating tool is simpler than a rotating workpiece. Use it for diameters around 18–65 mm when you want BTA speed on a mill.

Peck drilling is the default because every CNC has the cycle. G83 retracts the tool fully to clear chips, G73 breaks the chip without a full retract. With a standard drill, the reliable range is L/D up to 5. Push to 8 and the cycle still works if you shorten the peck and keep the tool sharp.

Between L/D 8 and 15, a parabolic flute drill with through-coolant can hold the job. Two conditions matter: coolant pressure above 2 MPa at the tool, and peck depth kept below 1×D. Many shops try to reach 15×D with a standard jobber drill and 1 MPa of coolant. That is where drills break.

Beyond L/D 15, peck drilling starts to fight itself. The repeated retract polishes the wall and opens a bell-mouth at the entry. Each re-entry can chip the cutting edge, and the drill drifts because nothing guides it. Tool breakage in a deep hole is the worst outcome: you lose the part and the job stalls while you fish out carbide.

The method is wrong when the hole must be straight, when the wall finish is specified tighter than Ra 1.6 μm, or when the diameter tolerance is under ±0.05 mm at depth. Use it for clearance holes, tapped holes and cross-drillings where position matters more than axis.

Tool material sets the speed window. Solid carbide suits gun drilling and small peck cycles because it holds the edge at high temperature. High-speed steel is still useful on tough, low-speed jobs and on older machines with limited rpm. BTA heads use indexable carbide inserts.

Coating choice follows the workpiece. TiAlN for steel and cast iron, TiCN for aluminum, and diamond-like carbon for non-ferrous metals and composites. The wrong coating causes built-up edge on aluminum or rapid wear on stainless.

Speed ranges are broad because the material matters more than the method. HSS runs 30–80 m/min. Carbide in steel runs 80–200 m/min. Feed per revolution should sit between 0.5% and 2% of the drill diameter, so a Ø10 mm drill feeds 0.05–0.2 mm/rev. Under-feeding work-hardens stainless and rubs the edge; over-feeding overloads a small gun drill.

Guide pads and bushings do the steering. A carbide guide bushing at the entry keeps the tool on axis for the first few diameters, which is where most drift starts. Replace worn pads before they open the hole. On our own deep hole work we hold ±0.005 mm on the machines and inspect 100% before shipment.

Coolant does three jobs at once: it carries chips out, cools the edge and lubricates the guide pads. When any one of those fails, the hole goes out of tolerance. Pressure and flow must be checked at the tool, not at the pump, because fittings and long hoses eat the difference.

Filtration is the quiet variable. A 20 μm filter keeps fines out of the bore on gun drilling and BTA work. Above 50 μm, recirculated chips act like lapping compound on the wall and the finish drops a full grade. Change filter elements on schedule, not on failure.

The machine has to resist the axial force. Thrust on a large BTA cut reaches several kN, so fixtures need positive stops and enough clamp area. Gun drilling on a lathe usually needs a guide bushing and a pilot hole or a spot with a 90° included angle so the tool enters squarely.

For long parts, a rotating workpiece with a stationary bar keeps the bore straight because the bar stays supported. On a machining center, a rotating tool in a rigid holder with high-pressure through-spindle coolant is the practical route. Our 127 CNC machines include 16 simultaneous 5-axis centers and mill-turn platforms with travels up to 4,000 mm, so long shafts and deep bores can be held in one setup.