CNC drilling machine: key functions and how each one shapes your holes

• 1
  Spindle rotation and the cutting speed it sets
• 2
  Feed motion: how the drill actually enters the material
• 3
  Axis positioning and hole location accuracy
• 4
  Peck cycles, chip evacuation and coolant
• 5
  Where drilling stops and boring or milling starts
• 6
  Which hole-making function matches the tolerance

Every CNC drilling machine starts with one motion: the spindle turns the tool at a programmed speed. Surface speed at the drill's outer corner is what wears the margin, so the number that matters is not rpm but m/min at the diameter you are cutting. A Ø5 mm drill at 3,000 rpm runs at roughly 47 m/min. The same rpm on a Ø20 mm drill runs at 188 m/min, which is too hot for mild steel but fine for aluminium.

Speed alone does not make a hole. The spindle has to hold its speed under load. If rpm drops when the drill enters the workpiece, the chip thins, the edge rubs, and you get work hardening in stainless or a bell-mouthed entry in aluminium. Spindle stiffness and drive torque are what keep the programmed number honest.

On our 5-axis and 3-axis centers, spindle speeds run from a few hundred rpm for large insert drills up to 15,000 rpm for small solid carbide. The practical rule: pick surface speed from the material, then check the machine can hold it at that diameter before you commit to a cycle time.

One of the most overlooked CNC drilling machine key functions is thermal stability. A spindle that has run for two hours at 12,000 rpm is longer than a cold one. Warm-up routines of 10 to 15 minutes keep the first holes and the last holes in the same position.

• 1
  Aluminium 6061150–300 m/min with carbide, uncoated or ZrN
• 2
  Mild steel 101880–120 m/min with TiAlN-coated carbide
• 3
  Stainless 30440–70 m/min, generous coolant, sharp edge
• 4
  Ti-6Al-4V25–45 m/min, low surface speed, high pressure coolant

Feed is the second half of the CNC drilling machine key functions. The spindle turns; the axis pushes. Feed rate is programmed in mm/min, but the number that controls chip formation is feed per revolution, usually written fz or fn. A Ø8 mm drill at 0.15 mm/rev removes 1.2 mm² of chip area per revolution, and that is what sets the load on the edge.

Thin chips cause more trouble than thick ones. Below about 0.05 mm/rev on steel, the edge rubs instead of cuts. Heat builds at the corner, the drill dulls, and hole diameter drifts oversize because the margin has worn. On aluminium, too light a feed lets the material smear and the chip welds to the flute.

The entry is where most holes go wrong. A standard 118° twist drill walking on a flat or angled surface will bend before it bites. Spot drilling with a 90° or 120° spot gives the drill a cone to sit in. On curved or cast surfaces, use a flat-bottom spot or interpolate a shallow pocket first.

Exit matters too. As the drill breaks through, the thrust drops suddenly and the drill can grab. Support the back side with a sacrifice plate or reduce feed for the last 1–2 mm. On thin walls, this is the difference between a clean hole and a torn edge.

• 1
  Spot firstØ2–5 mm spot, depth no more than the point length
• 2
  Peck when deepDepth over 3× diameter needs chip evacuation
• 3
  Reduce on exitDrop feed 30–50% for the final 1–2 mm

A drilling machine is only as good as its positioning. The X, Y and Z axes move the tool or the table to the programmed coordinate, and any error there shows up directly as hole location error. Ball screw pitch error, thermal growth, and backlash all land in the same place: your hole is off.

Positioning accuracy and repeatability are different numbers. Accuracy is how close the first hole is to the drawing. Repeatability is how close hole 400 is to hole 1. For a fixture plate with 200 holes, repeatability matters more. A machine that repeats within ±0.005 mm but sits 0.02 mm off nominal can be offset in the control. A machine that wanders cannot.

Clamping moves parts. A vise tightened on one side lifts the other. Thin plates bow when you clamp them, and the bow springs back after you release, leaving the hole out of square. Check flatness after clamping, not before.

Reference edges and probing close the loop. On our machines we touch off the datum with a probe, then drill. That removes fixture variation from the stack. For a part with a ±0.025 mm hole-to-edge tolerance, probing before cutting is cheaper than scrapping after.

• 1
  Probe the datumTouch off stock or a machined edge, not the vise jaw
• 2
  Check after clampingMeasure flatness with the part held, not loose
• 3
  Warm up firstRun the spindle 10–15 minutes before tight-tolerance work

Deep holes fail for one reason: chips cannot get out. The CNC drilling machine key functions around chip removal are the peck cycle and the coolant system. A G83-style peck retracts the drill to the clearance plane every few millimeters so the flutes clear. Full retract costs cycle time but saves tools.

Peck depth depends on the material and the flute. Aluminium with polished flutes can go 1× diameter per peck. Stainless and titanium usually want 0.5× diameter or less. If you hear the drill squeal on the retract, the chips are packing. Shorten the peck.

Through-spindle coolant changes the limit. At 70 bar, coolant reaches the drill tip and pushes chips back up the flute. Holes of 10× diameter and deeper become routine in steel and titanium. Without high pressure, the same hole needs many more pecks and a lot more time.

Coolant also controls diameter. Steel grows as it heats. A hole drilled dry at 80 m/min can finish 0.02 mm smaller than the same hole flooded, simply because the workpiece was cooler. For tight bores, drill wet and measure at room temperature, not immediately after the cut.

• 1
  Peck depthAluminium 1× D, steel 0.5× D, titanium 0.3–0.5× D
• 2
  Clearance plane0.5–1 mm above the surface, or R plane in the control
• 3
  High pressure70 bar through-spindle for holes over 8× D
• 4
  Chip colorSilver chips are right; blue or grey means too much heat

Drilling produces a hole. It does not produce a precise one. A twist drill typically holds H12 to H13 on diameter, which is roughly +0.1 to +0.3 mm on a Ø10 mm hole. If your drawing says Ø10 H7, you drill undersize and bore or ream to size.

Reaming is the middle option. A reamer removes 0.1–0.3 mm of material and holds H7 to H8 with a good surface, often Ra 0.8–1.6 μm. It follows the drilled hole, so it cannot fix location. If the drilled hole is off-center, the reamed hole is off-center too.

Boring fixes both. A single-point boring head corrects location and size in one pass, and it can hold ±0.005 mm on diameter with the right setup. Boring is slower and needs a rigid setup, so it goes where the tolerance justifies it: bearing bores, hydraulic manifolds, seal seats.

Interpolation on a 3-axis mill is the fourth path. A smaller end mill circles the hole to size, which is useful for odd diameters and for holes that need a flat bottom. It is not a substitute for boring when roundness and straightness matter, because tool deflection leaves a slight lobed profile.

• 1
  Drill onlyH12–H13, for clearance and tapped holes
• 2
  Drill and reamH7–H8, good finish, location follows the drill
• 3
  Drill and bore±0.005 mm on diameter, corrects location
• 4
  InterpolateOdd sizes and flat bottoms, roundness less certain