Understand the Basics of CNC Drilling Machines

• 1
  What the machine actually moves
• 2
  Drill geometry and what it does to the hole
• 3
  Peck drilling, chip breaking, and depth control
• 4
  Tolerance, position, and surface finish you can hold
• 5
  How material grade changes the setup
• 6
  Choosing a holemaking method

A CNC drilling machine is a two-and-a-half-axis tool at heart. The spindle carries the drill on the Z axis, the table positions the part in X and Y, and the controller ties those moves to a program. Everything else on the machine exists to keep those three motions accurate under load.

The cutting happens at the tip. Flutes only lift chips out of the hole. If the drill cannot clear chips, the flutes rub, heat climbs, and the hole grows oversize. Chip evacuation is the constraint that shapes most drilling decisions, not spindle power.

Positioning accuracy and hole accuracy are different numbers. A machine may repeat to ±0.005 mm at the spindle taper and still cut a hole 0.05 mm oversize because of drill grind, runout, or workpiece deflection. Buyers who treat the two as one number get surprised at first article inspection.

So the basics of CNC drilling start with the kinematics, not the tool catalog. Know which axis holds the depth, which axis holds position, and where the compliance sits in the loop. That framing explains almost every drilling problem you will meet on the floor.

• 1
  Z axisDepth and feed rate, set by the program
• 2
  X and YHole pattern position on the table
• 3
  Fourth axisRotary table for holes on a bolt circle

A standard twist drill is not a precision boring tool. Its point angle, typically 118° or 140°, leaves a conical bottom that no flat-bottom feature can hide. The chisel edge at the center does not cut so much as push, which is why a drill walks on a smooth surface unless you spot it first.

Lip height mismatch between the two cutting edges is the usual cause of a hole that comes out oversize. A few thousandths of an inch of asymmetry doubles the radial force and pushes the drill off line. Regrinding on a proper fixture keeps that mismatch small. Hand grinding on a bench wheel does not.

Point angle changes the thrust load. A 118° point is a general-purpose compromise. A 140° point is stiffer and suits harder steels, but it increases thrust and can bow thin plates. A 90° point is for plastics and sheet, where you want the tip to break through cleanly.

Coating matters less than geometry for hole size. Titanium nitride and similar coatings extend tool life in abrasive or gummy materials. They will not fix a drill that was ground wrong or is running 30 percent too fast for the material.

• 1
  Spot drill firstStops walk on curved or scaled surfaces
• 2
  118° pointGeneral purpose in steel and aluminum
• 3
  140° pointStiffer, higher thrust, harder alloys
• 4
  90° pointPlastics and thin sheet

Peck drilling retracts the tool at set intervals so chips can leave the hole. The controller handles this with a canned cycle, so the program stays short. The tradeoff is time. Every retract adds a rapid move that cuts no metal.

For soft aluminum, a single plunge often beats pecking. Chips are long and curl out of the flutes on their own. Peck too often and you rub the cutting edges against work-hardened material, which shortens tool life for no gain in hole quality.

Deep holes behave differently. Past roughly three times the diameter, chip packing becomes the limiting factor. Use a peck depth near one diameter, or switch to through-coolant tooling if the machine has it. High-pressure coolant changes the depth-to-diameter ceiling more than any feed change will.

Breakout is the other depth question. As the drill exits, thrust drops and the last material can tear or burr. Backing the feed to about half rate over the final millimeter reduces exit burrs on ductile materials without adding much cycle time.

• 1
  Soft aluminumSingle plunge, long chips clear on their own
• 2
  Past 3×DPeck near one diameter per retract
• 3
  Exit zoneHalve feed near breakout to limit burrs

Hole diameter from a twist drill lands around IT10 to IT12 unless you ream or bore. In inch terms that is a few thousandths either way, which is fine for clearance holes and not fine for bearing seats. Position can be tighter than diameter, because the machine positions the spindle, not the cutting edge.

When a drawing calls for a precise bore, the drill is a roughing step. Drill undersize, then ream or circular interpolate with an end mill. On our 5-axis centers we typically interpolate bores to hold ±0.005 mm and Ra 0.8–1.6 μm without a dedicated reamer.

Surface finish inside a drilled hole depends on feed per revolution. Heavy feed leaves a spiral that seals poorly against an O-ring. Light feed burns the edge in stainless. There is a window, and it moves with the material grade and the coolant.

Remember that the hole is only as good as the surface it starts on. A cast or scalped surface puts the drill on a slope, and the hole follows the slope. Face the entry surface flat, or spot it, before you expect a straight hole.

• 1
  As-drilledIT10 to IT12, clearance applications
• 2
  ReamedTighter diameter, still needs a pilot
• 3
  Interpolated±0.005 mm and Ra 0.8–1.6 μm on 5-axis

Aluminum 6061 drills fast and leaves a built-up edge if the feed is too light. Run it at a surface speed in the hundreds of meters per minute and keep the feed high enough to form a real chip. 7075 and 2024 are stronger and slightly less forgiving on tool wear but drill the same way.

Austenitic stainless, 304 and 316, work-hardens the moment the edge rubs. Any dwell in the cut raises the local hardness and the next pass cuts worse. Keep a constant feed, use sharp tooling, and never let the drill sit spinning in one spot.

Titanium TC4 (Ti-6Al-4V) is worse on heat. It conducts poorly, so the heat stays at the edge. Reduce surface speed, flood the cut, and accept shorter tool life. Inconel follows the same logic with a narrower window.

Plastics and composites need geometry changes, not speed changes. A 90° point, a slow helix, and a backing plate to stop delamination on exit. On carbon fibre we back the feed right down at breakout, or the last plies lift.

• 1
  6061 aluminumHigh speed, firm feed, long chips
• 2
  304 / 316 stainlessNo dwell, constant feed, sharp edge
• 3
  Ti-6Al-4VLower speed, heavy coolant
• 4
  Carbon fibreBacking plate, slow exit feed