CNC Drills Selection: A Working Guide for Engineers

• 1
  Key takeaways
• 2
  Drill type at a glance
• 3
  Point angle, flute count and web thickness
• 4
  Matching the drill to the workpiece
• 5
  Coolant, chip evacuation and peck cycles
• 6
  Hole tolerance, finish and reaming
• 7
  What to check before you place the order
• 8
  Step by step: choosing a drill for a new job

Point angle sets where the cutting edge first touches the material. A 118° point is the general-purpose default for carbon steel and aluminium. Move to 135° or 140° when the material work-hardens, because the wider point puts more of the edge in contact and reduces the chance of rubbing. Plastics and thin sheet behave differently again: a 90° point cuts cleaner and reduces breakout on the exit side.

Flute count controls chip room. Two flutes give the largest chip channel and work well in aluminium and deep holes. Three flutes are a compromise for steel. Five or more flutes raise feed rates in hard materials but leave little space for chips, so they suit shallow holes with good coolant. If you see packed flutes, the count is wrong for the depth, not the speed.

Web thickness is the metal between the flutes at the tip. A thick web makes the drill stiff but needs a split-point grind to cut at all. Thin-web drills self-center better in soft material but deflect more in deep holes. For holes deeper than 5× diameter, a thicker web and a split point are usually worth the extra cost.

Drill length is a stiffness decision. Jobber length is fine to about 4× diameter. Beyond that, use a screw-machine or stub drill for the first pass and step up. Every extra 10 mm of flute length adds deflection you cannot remove with feed and speed changes.

• 1
  118° pointGeneral steel, aluminium, low-volume work.
• 2
  140° pointStainless, titanium, Inconel, abrasive alloys.
• 3
  90° pointPlastics, composites, thin sheet, clean exit.
• 4
  Split pointReduces thrust, improves location on hard material.

Aluminium 6061 and 7075 cut fast with uncoated or ZrN-coated carbide. High helix and polished flutes clear the soft chip. Watch for built-up edge on 6061; if the hole starts to smear, raise speed and check coolant flow rather than changing the drill. Aluminium 7075 is harder and benefits from a sharper edge and slightly lower feed per revolution.

Stainless 303, 304 and 316 work-harden under a dull edge. Use cobalt or carbide with a 135° to 140° point, keep the feed per revolution up so the edge always bites, and never let the drill dwell. 316L is the worst of the three for this. If you hear a squeal, the drill is rubbing, and the next pass will be harder.

Titanium Ti-6Al-4V and Inconel need low surface speed, high feed per revolution and generous coolant. Carbide with AlTiN or AlCrN coating is the usual starting point. Heat goes into the tool in these alloys, so tool life is short and predictable. Budget for regrind or replacement every few hundred holes.

Plastics and composites are not soft metals. POM and PEEK need sharp, polished flutes and a slow feed to avoid melting. Carbon fibre delaminates if you push too hard at the exit, so back up the part with a sacrificial plate. ABS and PC are more forgiving but still show a poor hole if the drill is dull.

• 1
  AluminiumUncoated or ZrN carbide, high helix, fast.
• 2
  StainlessCobalt or carbide, 140° point, no dwell.
• 3
  Titanium / InconelAlTiN or AlCrN carbide, low speed, high feed.
• 4
  Plastics / CFRPSharp polished flutes, backing plate at exit.

Chip evacuation is the limit on hole depth. Without through-spindle coolant, keep the depth-to-diameter ratio under 3 and peck every 0.5× diameter. With through-coolant, you can push to 8× diameter or more depending on the drill and material. Flood coolant helps but does not reach the tip in a deep hole, so do not treat it as equivalent.

Peck depth is not a fixed number. In aluminium, a full-diameter peck works because chips are light. In stainless and titanium, peck at 0.5× to 1× diameter so the chip breaks before it packs. If the peck is too deep, the drill re-cuts chips, which is the fastest way to burn an edge.

MQL and air blast work for aluminium and some plastics. They fail in stainless and titanium because the heat stays in the tool. If your shop runs MQL only, choose carbide with a heat-resistant coating and accept shorter tool life, or move the deep holes to a machine with through-coolant.

Chip color tells you what happened. Silver or straw chips mean the speed is reasonable. Blue or black chips mean the edge is running too hot, and the next hole will be oversize. Stop and check the drill before the tolerance drifts.

• 1
  No through-coolantDepth under 3× diameter, peck at 0.5× diameter.
• 2
  Through-coolantDepth to 8× diameter, fewer pecks, better finish.
• 3
  MQLAluminium and plastics only; not for titanium.

A drilled hole is rarely the finished hole. A standard twist drill holds about ±0.05 mm on diameter in good conditions, and more in deep holes or gummy material. If the drawing calls for ±0.005 mm, plan a reamer or a boring pass. Drilling is for stock removal, not for the final size.

Reaming removes 0.1 to 0.3 mm of material and follows the drilled hole. It improves roundness and finish but will not correct position. If the hole is in the wrong place, reaming makes a round hole in the wrong place. Fix location with a spot drill and a rigid setup before you ream.

Surface finish depends on feed per revolution more than speed. A slower feed per revolution gives a finer finish but rubs the edge. In stainless, that trade is not worth it. In aluminium and brass, it often is. Typical drilled finish lands around Ra 1.6–3.2 μm, and reaming can reach Ra 0.8–1.6 μm.

Breakout at the exit is a separate problem. Support the far side of the part, reduce feed for the last few millimeters, or use a 90° point in sheet and plastics. A clean exit is a setup decision, not a drill catalog decision.

• 1
  Drill onlyAbout ±0.05 mm on diameter in good conditions.
• 2
  Drill + ream0.1–0.3 mm stock, better roundness and finish.
• 3
  Tight callout±0.005 mm needs reaming or boring, not drilling.

Ask how the shop sets tool length and runout. A drill held in a worn collet cuts oversize no matter how good the tool is. Shops running 127 high-precision CNC machines usually have a presetter and a runout target under 0.02 mm. If the answer is vague, the hole tolerance will be vague too.

Ask about regrind. A reground drill loses coating at the point and cuts differently from a new one. Some shops track drill life by hole count, others by time. Either works if it is written down. Without records, the tenthousandth hole is a guess.

Certifications matter when the part is regulated. ISO 9001:2015 covers general quality, IATF 16949:2016 covers automotive, ISO 13485:2016 covers medical, and ISO 27001:2022 covers data handling. If your drawing needs a material cert and an inspection report, confirm both are available before the job starts.

Lead time and quantity shape the tooling choice. For one prototype, a shop may hand-drill or use a general-purpose carbide drill. For a 10,000-part run, a custom step drill or a form tool pays for itself. Ask how the quote changes between the two, and whether the shop will run the first article before the full batch.

• 1
  RunoutAsk for the target, not just the machine brand.
• 2
  Regrind recordsHole count or time, written down per tool.
• 3
  CertificatesMatch the certificate to the industry, not the website.
• 4
  First articleConfirm inspection before the full run starts.