Drilling Machine Basics: How Holes Get Made

• 1
  What happens at the drill point
• 2
  Feed, speed and depth decide the result
• 3
  Where drilling stops and milling starts
• 4
  What the material does to the process
• 5
  Drill, bore or mill: which process fits

A CNC drilling machine rotates a cutting tool on a vertical or horizontal spindle and feeds it into the workpiece along a programmed axis. The motion is simple: spindle rotation, Z-axis feed, and a table that positions the part. A controller drives all three from a program, so the same hole lands in the same place on part one and part ten thousand.

The cutting action is different from milling. A drill has two cutting edges at the tip and two flutes along the body. It cuts on the point, not on the side. That geometry makes drilling fast and cheap, but it also limits what the process can hold: hole straightness depends on how well the point self-centers, and hole size depends on how much the drill wanders.

Most twist drills run a 118° or 135° point angle. The 118° point is general purpose and pushes harder into the material. The 135° point is flatter, self-centers better and suits stainless, titanium and other tough alloys. Point angle also changes the chip: a flatter point makes a thinner, wider chip that clears the flutes more easily.

Because the drill cuts only at the tip, side loads build up along the flutes. Any runout in the holder is copied into the hole. A holder with 0.02 mm runout will cut a hole that is oversized and out of round, no matter how good the machine is. That is why toolholding is part of the process, not an accessory.

Surface speed and feed per revolution are the two dials that matter most. In aluminum 6061, a high-speed steel drill runs around 60–90 m/min, and a carbide drill runs 150–250 m/min. In 304 stainless, drop to roughly 15–25 m/min for HSS and 60–90 m/min for carbide. Too much speed burns the point; too little speed work-hardens stainless and rubs the edge dull.

Feed per revolution sets chip thickness. A Ø6 mm drill in aluminum wants roughly 0.10–0.15 mm/rev. The same drill in stainless wants 0.05–0.10 mm/rev with more coolant. If the feed is too light, the edge rubs instead of cuts, and the drill work-hardens the bottom of the hole. If the feed is too heavy, the drill deflects and the hole drifts off position.

Depth changes everything past about three times the diameter. A drill has a length-to-diameter ratio, and long drills bend. At 3:1 the hole is usually fine with a stub or jobber drill. At 5:1 you want a parabolic flute and a peck cycle. Past 10:1 the process needs a gun drill or a dedicated deep-hole cycle, because chip evacuation, not cutting, becomes the limit.

Peck depth is a practical control. A common starting point is one diameter of peck per cycle, then reduce to half a diameter as the hole deepens and chip packing starts. Through-spindle coolant changes this: with high-pressure coolant you can often drill in one pass because the chips are pushed out the flutes instead of packing at the bottom.

Drilling makes a round hole on a straight axis. It cannot make a square pocket, a slot with a flat bottom, or a hole whose axis is at an angle to the surface without a secondary setup. It also cannot hold a tight diameter tolerance on its own. A twist drill typically holds ±0.05 mm to ±0.10 mm on diameter in a rigid setup, which is far looser than the ±0.005 mm our machines can hold on a bored or milled feature.

Hole position is a different story. On a rigid machine with a good fixture, drilling holds position within ±0.05 mm without much effort, and a spot drill can tighten that. If a print calls for ±0.02 mm position and a reamed fit, the sequence is spot drill, drill undersize, then bore or ream to size. That is normal practice, not a workaround.

Roughly 90% of drilled holes are functional, not precision fits. Bolt clearance, cable pass-through, vent holes and dowel pilots usually need position control and a clean exit, not a tight diameter. Spending a boring cycle on those holes adds cost and lead time for nothing.

The exception is a hole that has to seal or locate. Hydraulic ports, bearing bores and dowel holes need roundness, straightness and a controlled surface finish. Those get a reamer or a boring head, and the drill is only the first step.

Aluminum is the easy case. Chips are soft, heat leaves with the chip, and 6061 or 7075 drills cleanly at high speed. The main risks are built-up edge on the cutting edge and long stringy chips wrapping the tool. A polished flute and a higher feed break the chip.

Stainless 303 and 304 behave differently. The material work-hardens under the cutting edge, so any dwell or light feed creates a hard skin that dulls the next pass. Sharp tools, positive feed and a flood of coolant are the fix. 316 and 17-4PH are harder again and usually call for carbide and a peck cycle.

Titanium TC4 (Ti-6Al-4V) has low thermal conductivity, so heat stays in the tool edge instead of leaving with the chip. Surface speed drops to roughly 30–50 m/min with carbide, feed stays positive, and coolant must reach the point. Inconel is worse: 15–25 m/min, rigid setup, and a tool change before the edge rubs.

Plastics are the opposite problem. POM and ABS cut fast but melt and grab if the drill rubs. Use a sharp drill with a steep helix, a light feed and air blast rather than flood coolant. PMMA cracks at the exit, so a backing plate or a pilot point helps. Carbon fibre needs a diamond-coated drill and dust extraction, because the abrasive fibre eats HSS in a few holes.