The CNC drilling machine has the following main functions

• 1
  Position control: the axis function behind every hole
• 2
  Hole making: drilling, pecking and the chip problem
• 3
  Reaming, tapping and spot facing: the finishing functions
• 4
  What the control adds, and where drilling stops working
• 5
  CNC drilling machine main functions at a glance

On a CNC drilling machine, the computer controls the movement trajectory of the drill, its rotation speed and its feed speed. That is the whole idea. The spindle turns the tool; the axes move the tool or the table to the programmed coordinate; the Z axis decides how deep the tip travels. Every other function on this page is built on top of that loop.

Position accuracy comes from the machine, not the program. A machine with a Ø400 mm rotary table and ground ball screws holds a hole-to-hole tolerance well inside ±0.005 mm on a stable setup. A worn machine will not, no matter how clean the G-code looks. This is the first thing to check when holes drift on a part you have run for years.

The control also owns rapid positioning between holes. On a plate with 200 holes, rapid moves are most of the cycle time, not the cutting. A control that plans the tool path well cuts seconds per part without touching a single feed rate. That is why the same drill and the same program can run 20% faster on a newer controller.

Depth control is the part engineers underestimate. The tip of a 118° drill is not the flat bottom of the hole. If the drawing calls a 12 mm deep hole and the program commands Z-12.0 mm at the tip, the usable cylindrical depth is shallower. Add half the drill diameter times 0.3 for a 118° point, or program to the shoulder directly.

Axes also carry the work offset. One fixture, six parts, six offsets. When a fixture is re-clamped after maintenance, the offsets must be re-probed. Most position errors blamed on backlash are actually stale offsets. Re-probe first, then look at the machine.

• 1
  Spindle speedSet by surface speed and drill diameter, not by habit.
• 2
  Feed ratePer revolution (mm/rev), so it scales with rpm.
• 3
  DepthCounts the drill point, not just the cylindrical section.

The core function is making a hole to size and position. A standard twist drill does this in one pass when the depth-to-diameter ratio stays under about 4:1 and the material makes a broken chip. Aluminum 6061 and 6082 cut clean at 60–120 m/min surface speed with a feed of 0.10–0.25 mm/rev. Below that, the drill rubs and work-hardens the wall.

Once the ratio passes 4:1, chips stop leaving the flutes on their own. Peck drilling is the answer: the control retracts the tool at set intervals to clear the chip. Typical peck depth is one diameter for steel, up to two diameters for aluminum. Retract amount is usually 0.5–1.0 mm above the last depth to avoid re-cutting the same chip.

Deep holes change the numbers. At 8:1 and deeper, feed drops to 50–70% of the shallow value, and through-spindle coolant becomes the difference between a good hole and a broken drill. A 6 mm drill at 10:1 depth in 304 stainless will snap on the first peck without high-pressure coolant. That is not a programming mistake; it is a setup limit.

Chip shape tells you whether the function is working. Long stringy chips in steel mean the feed is too light. Fine powder in aluminum means the speed is too high or the drill is dull. Blue chips in carbon steel mean heat is going into the part, not the chip. Adjust feed before you adjust speed.

• 1
  4:1 or shallowerSingle pass is usually fine with good chip evacuation.
• 2
  4:1 to 8:1Peck drilling, one diameter per peck in steel.
• 3
  Deeper than 8:1Reduce feed, add through-coolant, expect a slower cycle.

Drilling rarely holds a tight bore. The drill wanders, and the hole comes out 0.05–0.15 mm oversize on a typical job. Reaming fixes that. A reamer removes 0.1–0.3 mm of radial stock and holds H7 fit with a finish around Ra 0.8–1.6 μm. Leave less than 0.05 mm and the reamer rubs; leave more than 0.4 mm and the flutes load up.

Reaming also needs a straight entry. If the drilled hole is off-axis by more than 0.05 mm, the reamer follows the error instead of correcting it. Spot drilling before the drill, or boring before the reamer, is how you get a true bore. This is the step people skip, then blame the reamer.

Tapping is the third function. On a CNC drilling machine with rigid tapping, the spindle reverses in sync with the feed, so thread depth repeatability is good. In aluminum, a form tap gives a stronger thread than a cut tap and makes no chips. In 304 stainless, use a cut tap with a spiral flute and a tapping fluid; form tapping there needs more torque than small machines have.

Spot facing is the last common function: a flat seat for a bolt head or washer on a curved or rough surface. It uses a piloted counterbore or an end mill plunged to a set depth. Depth tolerance matters here, because a spot face that is too deep leaves too little material under the head. Keep it within ±0.05 mm of the drawing.

These functions share one requirement: the tool must enter on the same centerline. Every operation after drilling inherits the drill's position error. If the drilled hole is off by 0.08 mm, the reamed and tapped features are off by 0.08 mm too.

• 1
  Reaming stock0.1–0.3 mm on diameter for H7 fits.
• 2
  TappingRigid tapping holds depth; form taps suit aluminum.
• 3
  Spot facingHold depth within ±0.05 mm of the drawing.

Modern controls add canned cycles: G81 for a plain hole, G83 for peck drilling, G84 for tapping, G85 for boring. These are not extra machine functions; they are stored motion patterns that save programming time and reduce typos. A G83 cycle with a 3 mm peck and 1 mm retract does the same thing a hand-written loop does, with fewer lines to debug.

Chip breaking is the function most tied to the control. Some controls oscillate the Z axis a few hundredths of a millimeter to break the chip without a full retract. That works well in aluminum and brass. In gummy materials like 316L or Inconel, it is unreliable and full peck retracts are safer. Match the strategy to the material, not to the control's default.

Drilling has real limits. It cannot hold a bore tolerance tighter than about ±0.02 mm, cannot produce a square corner, and cannot cut a slot. If the feature needs a flat bottom, an internal corner or a true diameter, the part needs milling or boring instead. A hole is a starting point, not a finished feature.

The other limit is the tool itself. A drill pushes material, so it creates a burr on exit. On a through hole in ductile material, plan a deburring pass or accept a burr of 0.05–0.1 mm. On a cross hole, the drill deflects as it breaks into the intersecting bore. That is where you see a bell-mouth, and it is a geometry problem, not a feed problem.

When a part has more holes than pockets, drilling is the fast path. When a part has deep pockets, tight corners and a few holes, a mill with helical interpolation does the whole job in one setup and drilling becomes a subroutine inside it.

• 1
  Canned cyclesG81, G83, G84, G85 cover most hole work.
• 2
  Chip breakingWorks in aluminum and brass, not in 316L or Inconel.
• 3
  Known limitsNo tight bores, no square corners, no slots.