Holes Machining Tool Design: How Geometry, Coolant and Cycle Choice Decide Hole Quality

• 1
  What actually happens when a holes machining tool enters metal
• 2
  Point angle, helix and coating: three choices that change the hole
• 3
  Coolant delivery decides how deep you can go
• 4
  Where a drilled hole stops being accurate enough
• 5
  Common hole defects and what causes them
• 6
  Hole type vs. tool and process choice

A drill removes material with two cutting edges that share the load. The chisel edge at the center does not cut cleanly. It pushes material aside and creates a dead zone where speed drops to zero. That is why the first few millimeters of a drilled hole tend to wander, and why the drill tip geometry matters more than most drawings suggest.

As the tool advances, the margin (the narrow cylindrical land behind the cutting edge) rubs the hole wall. This rubbing stabilizes the drill but also generates heat and can smear soft materials like aluminium. The flute then has to evacuate chips fast enough that they do not pack against the wall and push the drill off axis.

The result is a hole that is rarely a perfect cylinder. It usually has a slight bell mouth at entry, a taper along the depth, and a lobed cross-section. For a bolt clearance hole this is fine. For a hydraulic spool bore it is not. Knowing which one you are making decides the tool and the cycle.

• 1
  Chisel edgeLow cutting speed zone; the main source of wander on entry.
• 2
  MarginRubbing contact that guides the drill and adds friction heat.
• 3
  FluteChip path; if it clogs, hole straightness suffers first.

Point angle sets how the drill enters and how the thrust load spreads. A 118° point is the general-purpose standard. A 140° point is stiffer and better for hard steels and for drilling into angled or curved surfaces. A 90° point is used when you need a flat-bottomed hole or a short chamfer at entry.

Helix angle controls chip evacuation. Slow helix (around 15–20°) is for brass and short-chipping materials where you want the chip to break small. Fast helix (35–45°) pulls chips out of deep holes in aluminium and low-carbon steel. If you run a fast helix in brass, the drill will grab and pull itself into the part.

Coatings change tool life, not hole size. TiN and TiAlN raise the temperature ceiling and reduce built-up edge on steel. Uncoated or polished tools are often better on aluminium because the coating itself can become a chip trap. On stainless steel, a TiAlN coating plus a heavier web reduces work hardening at the cutting edge.

• 1
  118° pointGeneral purpose, low thrust, most materials.
• 2
  140° pointHarder materials and interrupted entry surfaces.
• 3
  35–45° helixDeep holes in aluminium and ductile steel.
• 4
  15–20° helixBrass, bronze, short-chip plastics.

Coolant does two jobs: it removes heat and it flushes chips. In a hole deeper than about 3× diameter, chip evacuation becomes the limiting factor, not tool strength. Flood coolant often cannot reach the cutting edge at depth because the drill body blocks the path.

Through-spindle coolant, pushed out through holes in the drill, solves this. It flushes chips back along the flutes and keeps the cutting edges at a stable temperature. Deep-hole drilling with through-coolant tools can run at 20–30× diameter without a peck cycle in the right material.

Without through-coolant, you rely on peck drilling. Each peck retracts the tool to break the chip and let coolant in. The cost is cycle time and a small risk of re-entry marks on the wall. For holes under 3× diameter, a single peck or none at all is usually enough.

• 1
  Shallow holes (≤3× D)Flood coolant is normally sufficient.
• 2
  Medium holes (3–10× D)Use peck cycles or through-coolant.
• 3
  Deep holes (>10× D)Through-coolant or gun drilling; flood will not clear chips.

A standard twist drill typically holds H12 to H13 diameter tolerance and a position within about ±0.1 mm on a rigid setup. That is enough for clearance holes, tapped holes before threading, and most vent or drain features. It is not enough for a bearing seat or a dowel pin hole.

To improve diameter and finish, the usual path is drill, then ream. Reaming removes 0.1–0.3 mm of material and produces a rounder, straighter hole with a finish around Ra 0.8–1.6 μm. It does not correct position error, so the drilled hole must already be in the right place.

When position matters as much as size, the hole is often milled with an end mill or interpolated with a helical path. This lets the machine control the center location directly. A bored hole on a boring head or a 5-axis interpolation can reach ±0.005 mm and a finish of Ra 0.2–0.8 μm in the right material.

• 1
  Drill onlyH12–H13, position about ±0.1 mm; clearance and tapped holes.
• 2
  Drill + reamH7–H8, Ra 0.8–1.6 μm; dowel and pin holes.
• 3
  Bore or interpolate±0.005 mm, Ra 0.2–0.8 μm; bearing seats and spool bores.

Oversize holes usually come from drill runout, an unbalanced setup, or a point that has been sharpened asymmetrically. If one cutting lip is longer than the other, the drill cuts on one side and the hole grows. Check the drill in a holder with a dial indicator before blaming the machine.

Bell-mouth entry and exit burrs are mechanical, not random. A drill that is not guided by a spot or pilot hole will wobble at entry. A part that is not supported under the exit will push the last few millimeters of material outward instead of cutting it cleanly. Support the exit with a backing plate or reduce feed near breakthrough.

Tapered or bowed holes point to chip packing or a drill that is too flexible for the depth. Increase coolant pressure, shorten the peck depth, or step up to a carbide drill with a heavier core. On deep holes in stainless steel, work hardening at the entry of each peck can also bend the drill, so keep each peck engaged and avoid dwelling.

• 1
  OversizeRunout, uneven lips, or too little pilot guidance.
• 2
  BurrsUnsupported exit or feed too high at breakthrough.
• 3
  Bowed holeChip packing or insufficient tool stiffness for depth.