CNC Drilling Program: How Holes Actually Get Made

• 1
  What a CNC drilling program controls
• 2
  Tool choice and hole quality
• 3
  How material changes the numbers
• 4
  Fixturing, runout and hole position
• 5
  Where drilling stops being the right answer
• 6
  Matching the drilling method to the hole

Every hole in a part needs four decisions before the spindle turns: where the tool goes in X and Y, how fast it feeds down Z, how fast it spins, and how deep it goes. A CNC drilling program is simply those decisions written in G-code and grouped by tool. G81 covers a plain hole. G83 adds a peck cycle, retracting the tool in steps so chips clear instead of packing around the flutes. G84 handles rigid tapping. The choice of cycle, not the coordinate list, decides whether the hole comes out clean.

Position comes from the drawing, but the reference matters. Hole coordinates are usually called from a datum edge or a bore, not from the raw stock corner. If the datum is wrong in the program, every hole shifts by the same amount and the part is scrap. Setup sheets should state the datum, the work offset, and the stock allowance in one place. That single sheet is what a machinist trusts at the machine.

Feed and speed follow the tool and the material. A 6 mm high-speed steel drill in 6061 aluminium runs near 3,000 rpm and 0.15 mm per revolution. The same drill in 4140 steel drops to roughly 800 rpm and 0.08 mm per revolution. Holes deeper than about three times the diameter need either a peck cycle or a through-coolant drill, otherwise chips jam, the drill rubs, and the hole grows oversize.

Depth is where most small programs fail. A blind hole called 10 mm deep must include the drill point. A 118° point adds about 0.3 × diameter of cone below the flat depth, so a 6 mm drill cutting to a 10 mm flat is programmed closer to 11.8 mm. Add clearance for chips and the number moves again. Read the callout on the drawing before you write the Z value.

• 1
  Drilling cyclesG81, G83 and G84 cover the common hole types
• 2
  DatumState it once on the setup sheet, not per operation
• 3
  Peck depthRoughly one diameter per peck in steel
• 4
  Point allowanceAdd 0.3 × diameter for a 118° drill point

The drill sets the ceiling on hole quality. A standard twist drill leaves a hole 0.05 to 0.15 mm oversize and rarely holds a tight position, because the point wanders on entry. A spot drill or a stub drill first fixes the start point. For holes that carry a pin or a bolt shank, we spot, drill undersize, then ream to size. Reaming holds ±0.01 mm or better in most steels and aluminium.

Coating changes tool life more than geometry for production runs. TiN and TiAlN coatings let a drill run faster in steel and stainless without burning the edge. Through-coolant drills push chips out of deep holes and let one tool finish a hole that would otherwise need three pecks. In 17-4PH or Inconel, coolant through the tool is often the difference between a stable process and a broken drill.

Carbide drills cut faster and hold size better than high-speed steel, but they are brittle. A slight runout or a hard spot can chip the corner. For a short run in soft material, high-speed steel is cheaper and more forgiving. For thousands of holes in aluminium or cast iron, carbide pays back through cycle time. Pick by run length and material, not by habit.

Hole finish follows the same logic. As-machined drilling lands around Ra 1.6–3.2 μm. A reamed hole reaches Ra 0.8–1.6 μm. If the drawing asks for Ra 0.2–0.8 μm inside a bore, drilling is only a pre-step and the finishing cut belongs to a boring head or a reamer with a controlled feed.

• 1
  Spot firstStops the drill walking on a curved or angled surface
• 2
  Ream for fitsHolds ±0.01 mm on pin and dowel holes
• 3
  Through-coolantBest for depth over 3 × diameter in steel

Aluminium drills fast and forgiving. 6061 and 7075 both cut cleanly at high spindle speed, but 7075 work-hardens if the feed is too light, so keep the chip load up. Cast aluminium like ADC12 can have porosity that pulls the drill off line. A spot drill and a slightly heavier feed usually fix it. Deep holes in aluminium clear chips well with air blast, no coolant needed.

Steel needs more control. 1018 and 1045 drill predictably with high-speed steel and flood coolant. 4140 and 4340 at higher hardness push you toward carbide or coated tools, lower surface speed, and a peck cycle for anything past two diameters. Work-hardening grades like 17-4PH can harden under a rubbing drill, so a dull tool is worse than no tool. Change the drill before it rubs.

Stainless is where peck drilling earns its keep. 304 and 316 work-harden at the surface, so the drill must cut, not slide. Keep feed per revolution steady, use a sharp coated drill, and peck at about half a diameter in deep holes. 316L behaves similarly. Titanium TC4 and Inconel 718 go further: low surface speed, generous coolant, and a rigid setup. A drill that chatters in Inconel will not last a single hole.

Plastics and composites follow different rules. POM and ABS cut cleanly but melt if the speed is too high. PEEK tolerates more heat but costs more, so tool life matters. Carbon fibre needs carbide and sharp edges to avoid delamination at the exit. In all of these, feed rate controls the finish more than spindle speed.

• 1
  AluminiumHigh speed, heavy chip load, no peck needed
• 2
  SteelPeck past two diameters, watch work hardening
• 3
  StainlessSharp tool, steady feed, half-diameter pecks
• 4
  CompositesBacking plate at exit stops delamination

A perfect CNC drilling program still fails on a loose setup. The vise or fixture must hold the part against the cutting force, which pushes down and sideways. Thin plates bow under a drill unless supported underneath. We use parallels or a dedicated nest for thin parts, and check the setup with an indicator before running the first hole.

Runout is the quiet killer. A drill with 0.03 mm of runout cuts a hole larger than its nominal size and wears on one flute. Check the holder, the collet and the drill shank. A shrink-fit or hydraulic holder holds runout under 0.01 mm. An ER collet is fine if it is clean and torqued correctly. On a five-axis machine, the same rule applies after every tool change.

Position accuracy depends on the machine, the tool and the thermal state. A warm spindle drifts, so long runs need a warm-up cycle. Probing on the machine catches a shifted work offset before the whole batch is cut. For parts with many holes, we drill the critical ones first, measure, then adjust the offset if needed.

On a five-axis machining center, a CNC drilling program can reach holes on five faces in one setup. That removes the re-fixturing error that comes from moving a part between a drill press and a mill. The trade-off is that a five-axis cycle costs more per hour, so it only pays when the part has angled holes or tight true-position callouts.

• 1
  Support thin platesUse a nest or backing plate under the hole
• 2
  Check runoutKeep it under 0.01 mm for tight holes
• 3
  Probe on machineCatches a shifted offset before the batch

Drilling makes round holes. If the feature is a slot, a pocket or a square opening, a drill is only the entry move, and an end mill does the real work. Writing a drilling cycle for a slot wastes time and leaves a poor floor. Match the tool to the geometry, not to the machine's default list.

Very tight true position is another boundary. A drilled hole typically holds ±0.05 to ±0.1 mm position in a good setup. If the drawing calls for ±0.02 mm between holes, plan to drill undersize and bore or ream. Trying to hold that by tweaking the drilling cycle alone usually fails on the second shift.

Depth-to-diameter ratio sets a hard limit too. Past about 10 × diameter, chip evacuation and drill wander dominate. Gun drilling or a specialist deep-hole process takes over. It is not a matter of a longer peck; the tool itself is too flexible at that length.

Finally, surface finish inside the hole. Drilling leaves a helical feed mark. If the bore seals against a shaft or holds an O-ring, that mark leaks. Reaming or boring fixes it. Do not ask a drilling cycle to deliver a sealing surface.

• 1
  Slots and pocketsUse an end mill, not a drill cycle
• 2
  Tight positionDrill undersize, then bore or ream
• 3
  Over 10 × ØMove to gun drilling or a deep-hole process
• 4
  Sealing boresReam or bore for a leak-free surface