7 CNC Drilling Techniques to Boost Precision and Cut Costs

Once depth reaches three times the drill diameter, chip evacuation stops being a detail. Chips pack into the flutes, torque climbs, and the drill starts to wander or snap. Peck drilling breaks the cut into short feed strokes and retracts the tool so chips clear the hole. The retract also lets coolant reach the cutting edge instead of sitting at the entrance.

The peck depth matters more than the number of pecks. A common starting point is one diameter per peck for stainless and Inconel, and two to three diameters for aluminum. Full retract costs cycle time, so use chip-breaking retract for holes under 5:1 and full retract beyond that. Watch the chip shape on the first part. Fine powder means the feed is too low; long stringy chips mean the peck is too deep.

This technique earns its place on stainless, titanium, and nickel alloys where chip welding is a common failure mode. It is not the best choice for a Ø6 mm hole through 8 mm of aluminum plate. A straight feed with good coolant will finish that hole faster and just as accurately.

• 1
  Use it whenDepth-to-diameter is 3:1 or greater, or the material is gummy and prone to chip welding.
• 2
  Skip it whenThe hole is shallow and the drill has through-coolant capability.
• 3
  Typical cost driverExtra retract time versus the cost of one broken carbide drill.

High-speed drilling with chip breaking adds a small axial oscillation to the feed motion. The amplitude is usually 0.1–0.3 mm, fast enough that the drill never fully leaves the cut. Chips break into short segments instead of forming long ribbons that wrap around the tool and scratch the bore.

The gain shows up in two places. Tool life improves because chips leave the cutting zone before they can weld to the edge. Cycle time drops because the machine no longer needs a full retract for every peck. On aluminum and low-carbon steel, this can mean noticeably longer tool life and shorter cycle time than a plain G83 peck cycle.

Program it with a CAM path rather than a canned cycle. Trochoidal or sinusoidal motion gives you control over amplitude and frequency. A standard G73 or G83 does not. This is one of the CNC drilling techniques that boost throughput without touching spindle speed, which matters when the machine is already near its limit.

Through-tool coolant pushes fluid out of the drill tip at 70–200 bar, depending on diameter. The pressure lifts chips out of the flutes instead of relying on gravity and gravity-fed flood coolant. On horizontal holes and deep holes, that difference is the whole game.

The requirement is a drill with internal coolant channels and a spindle that supports high-pressure delivery. Not every machine in a shop has that. When it is available, through-tool coolant often removes the need for pecking in holes up to about 8:1, which cuts cycle time and reduces the chance of the drill rubbing on retract.

For materials like 17-4PH stainless or Inconel, coolant pressure also controls heat at the cutting edge. Heat is what kills the coating first. If your machine tops out at low pressure, keep the peck cycle and accept the extra time.

A spot drill creates a shallow cone that guides the tip of the following drill. Without it, a twist drill can walk on a curved surface or a rough cast skin, and the hole lands off position. The cost is a few seconds per hole. The return is fewer scrapped parts and less rework.

Spot depth should be just enough to cover the drill point angle. Extra depth wastes time and can leave a chamfer that interferes with a flat-bottom requirement. Match the spot angle to the drill angle, or use a spot that is slightly larger. For holes that need a tight position tolerance, spot drilling is not optional.

On a five-axis machine, spot, drill, and chamfer can run in the same setup with the same datum. That removes a re-fixturing step and keeps position error from stacking up across operations.

Tapping is faster for a single thread in a through hole with clearance at the bottom. Thread milling wins when the hole is blind, the material is hard, or the thread is large. A thread mill cuts with a helical path, so the tool diameter is smaller than the thread. That means less torque and a lower risk of tap breakage in titanium or hardened steel.

Thread milling also lets you adjust the fit by changing the cutter compensation offset. If a gauge shows the thread is tight, you make one offset change and rerun. With a tap, you scrap the part or chase the thread by hand.

The trade-off is cycle time. A thread mill takes longer per hole, and the tool costs more. For a high-volume part with a small through thread in aluminum, tapping is usually the right call. For a one-off housing with a deep blind thread in stainless, thread milling pays for itself.

Angled holes are the classic reason to move a part to a five-axis machine. Instead of building an angle fixture or repositioning the part three times, the rotary table tilts the workpiece and the drill enters normal to the surface. Position error from re-clamping disappears.

The second benefit is setup count. A part with holes on four faces can be drilled in one operation with one datum. That shortens the process, reduces the number of fixtures, and makes the first-article inspection simpler. For low-to-medium volume work, the setup saving often matters more than the cutting speed.

Five-axis drilling is not the answer for a flat plate with holes on one face. A three-axis machine with a good fixture will be cheaper and just as accurate. Use the rotary axes when the part geometry demands it, not because the machine is available.