CNC deep hole machining: why depth changes everything

• 1
  What counts as a deep hole
• 2
  Why deflection and chip evacuation set the limit
• 3
  Drilling, boring, and gundrilling compared
• 4
  How hole geometry changes the answer
• 5
  Material behavior in deep holes
• 6
  Which deep hole process fits which job

There is no universal number, but shops use the depth-to-diameter ratio (L/D) as the working measure. Below about 3:1, a standard twist drill behaves. From 5:1 to 10:1 you are in the range where peck drilling, through-spindle coolant, and a shorter flute length start to matter. Past 10:1, the drill body itself bends under cutting force, and the hole walks off center.

Depth matters because the tool is a cantilever. A drill clamped in a holder has one free end, and cutting force pushes that end sideways. Deflection grows with the cube of the unsupported length, so doubling the hole depth multiplies the bending by eight. A Ø6 mm drill at 30 mm depth is a different animal from the same drill at 120 mm.

Heat builds up too. Chips carry away most of the cutting heat, and in a deep hole they have a long way to travel. When chips pack into the flutes, the drill rubs instead of cuts. Rubbing raises temperature, temperature softens the edge, and the hole comes out oversize, tapered, or with a torn surface.

For the buyer, this means the drawing matters more than the material. A Ø10 mm hole through 20 mm of 6061 aluminum is routine work. The same hole through 200 mm of 17-4PH stainless is a process decision, not just a toolpath.

• 1
  L/D 1–3Standard twist drill, no peck needed
• 2
  L/D 5–10Peck cycles, through-coolant, rigid setup
• 3
  L/D 10+Gundrilling or BTA, dedicated process

Two physical problems run at the same time in a deep hole: the tool bends, and the chips have nowhere to go. Both get worse as the hole gets deeper, and they feed each other. A bent drill cuts unevenly on two flutes, which makes one chip thicker and one thinner, which pushes the drill further off axis.

Chip evacuation is the more common failure mode. In a shallow hole, gravity and coolant flush chips out of the flutes. In a deep hole, the flutes fill up. Once the flutes are packed, the drill has no cutting edge exposed. Spindle load rises, the drill squeals, and the edge breaks down.

Coolant pressure is the practical fix. Through-spindle coolant at 40–70 bar pushes chips back down the flutes and out of the hole. This is why gundrilling uses high-pressure oil or water-based coolant delivered through the tool shank, not from the outside.

The engineering consequence is simple. Hole depth drives tool choice, coolant delivery, and cycle time. It is not a tolerance call. A Ø4 mm hole at 60 mm depth may hold a looser tolerance than a Ø40 mm hole at 200 mm depth, because the small drill has less room for coolant and chips.

Three processes cover most deep holes, and they are not interchangeable. Twist drilling is fast and cheap, but it runs out of control past roughly 8:1. Boring follows a drilled hole to correct size and straightness, but the bar must be stiffer than the drill it follows. Gundrilling makes the hole in one pass with a single-lip cutter and high-pressure coolant.

Gundrilling is the process most people mean when they say cnc deep hole machining. A carbide or HSS head with one cutting edge cuts a hole that is straight to within a few thousandths over its length. The tool self-pilots on the hole wall, so deflection is controlled by the hole itself, not by the shank length.

Boring is what you do after a drill has already wandered. A boring bar with a single point removes the off-center material and brings the hole back to the spindle axis. It works well up to about 4:1 on the bar diameter. Past that, the bar chatters and the surface finish goes.

The selection is driven by the hole, not by the shop's preference. A cross-drilled oil gallery in a shaft is a gundrilling job. A bolt clearance hole through a flange is a drilling job. A bearing bore that needs a specific fit is a drilling plus boring job.

• 1
  Twist drillingFast, low cost, best under L/D 8
• 2
  GundrillingOne pass, straight, L/D 20–100+
• 3
  BoringCorrects size and straightness after drilling

A through hole is easier than a blind hole. In a through hole, coolant and chips exit the far side, so the drill never has to reverse the chip flow. A blind hole traps chips at the bottom and forces them back up the flutes, which is where most deep-hole problems start.

A stepped hole is harder than a straight one. Each diameter change is a new entry point for the tool and a new place for chips to collect. If the step is deep inside the part, the smaller drill has to reach through the larger bore, which means a long, thin tool with no support.

Cross holes and intersecting holes are the worst case. The drill breaks into an existing cavity, loses its piloting surface, and can grab. On a cross-drilled shaft, the drill often walks at the intersection. The fix is to drill the cross hole before the main bore, or to use a pilot bushing to guide the tool.

Wall thickness matters as much as hole size. A thin wall flexes under cutting force, so the drill cuts more on one side. This is why deep holes in thin-wall tubes are often machined with the tube supported on a mandrel or in a split bushing.

Aluminum is the friendly case. 6061 and 7075 cut fast and clear chips well, so L/D 10 is routine with good coolant. The risk is built-up edge on the drill edge, which makes the hole oversize. A polished flute and a sharp edge avoid it.

Stainless steel is the opposite. 304 and 316 work-harden as the drill rubs, so a dull edge makes the next pass harder than the last. Deep holes in 316L need a fresh edge, low surface speed, and steady feed. Stopping mid-hole is a bad habit because the edge rubs on restart.

Titanium and Inconel are the limit cases. Ti-6Al-4V conducts heat poorly, so the edge stays hot and the chip carries little away. Inconel is worse. Deep holes in these alloys are usually gundrilled with high-pressure coolant and a conservative feed, and the tool is often replaced before it is fully worn.

Plastics are their own problem. POM and PEEK expand with heat, so the hole closes on the drill. A deep hole in PEEK needs a sharp, polished tool, a fast retract, and often a reaming pass after the part cools. The hole you measure hot is not the hole you ship.