Problems to Be Careful When Drilling Materials That Are Difficult to Cut

• 1
  Common problems to be careful when drilling: symptom, cause, fix
• 2
  Why these alloys behave so differently from mild steel
• 3
  Drill geometry and grade for hard-to-cut stock
• 4
  Coolant and chip evacuation decide the outcome
• 5
  Hole accuracy, straightness and finish
• 6
  What we check before a difficult drilling job runs
• 7
  Step by step: drilling a tough alloy without wrecking the tool

The problems to be careful when drilling start with the material, not the machine. Austenitic stainless, titanium and nickel alloys keep their strength at the temperature where mild steel has already gone soft. That means the cutting edge never gets an easy ride. All the heat that would normally leave with the chip stays near the edge and the hole wall.

Nickel alloys such as Inconel are the worst case. Thermal conductivity is roughly a third of steel, so heat concentrates in a very small zone. Titanium adds a second problem: it reacts with most tool coatings and with air at high temperature, so the chip tends to gall and weld instead of sliding.

There is also a chemical side. Titanium and stainless both work harden when the tool rubs instead of cutting. The surface under the edge gets harder than the parent metal, and the next revolution of the flute meets that harder skin. Drill a hole with a dull edge and the second pass is cutting something noticeably tougher than the first.

The practical point is that these materials punish light passes. A machinist trained on 6061 aluminium often backs off the feed when the drill sounds unhappy. On stainless that makes things worse. Rubbing creates heat, heat creates hardening, and hardening breaks the edge.

• 1
  Low conductivityHeat stays in the edge and the workpiece, not the chip.
• 2
  Work hardeningRubbing raises surface hardness above the base metal.
• 3
  GallingTitanium and stainless tend to weld to the cutting edge.
• 4
  SpringbackThese alloys push back on the drill and raise cutting force.

For stainless 303, 304, 316 and 17-4PH, a solid carbide drill with an AlTiN or TiAlN coating is the normal choice. The coating keeps the heat off the carbide. For 304 and 316, look for a 140° point and a thicker web. A 118° point with a thin web flexes and chips at the corners.

Titanium TC4 (Ti-6Al-4V) prefers a sharp, uncoated or lightly coated carbide grade. TiAlN can react with titanium at high edge temperature. Keep the cutting speed low, around 30–45 m/min, and never let the drill dwell in the cut. A dwell in titanium is a spot weld.

For Inconel, cobalt HSS or fine-grain carbide with a 135–140° point and a strong negative rake works better than a general-purpose geometry. The edge needs mass. Thin, sharp geometries fail quickly in nickel alloys because the corner cannot take the load.

Coatings are not decoration. They matter most where the material is gummy. On 316L, an uncoated drill will show built-up edge within a few holes. On aluminium 6061, the opposite is true: a high-polish uncoated drill with a steep helix clears chips best, and a rough coating drags.

• 1
  StainlessSolid carbide, AlTiN, 140° point, web thickness 0.25–0.3 × Ø.
• 2
  TitaniumSharp carbide, low speed, no dwell, high-pressure coolant.
• 3
  InconelCobalt HSS or fine-grain carbide, 135–140°, strong corner.
• 4
  AluminiumUncoated high-polish, 40–45° helix, fast and open flutes.

In stainless and nickel alloys, coolant does two jobs. It lowers edge temperature, and it flushes chips out of the flute. If chips stay in the hole, they get re-cut, which doubles the heat and triples the load on the drill. Through-tool coolant at 40–70 bar is the reliable answer for holes deeper than 3 × Ø.

Flood coolant aimed from one side is not enough for deep holes. It cools the outside of the drill but does not reach the tip. A peck cycle is the fallback when through-tool is not available. Peck every 0.5–1 × Ø with a full retract, and let the spindle keep turning so the chip clears.

Chip form tells you whether the parameters are right. Stainless should produce short, curled chips with a slight silver-grey colour. Long stringy chips mean the feed is too low. Blue or black chips mean the speed is too high or the coolant is not reaching the edge.

In titanium, the risk is different. Fine powdery chips look harmless but pack the flute and cause heat. A light peck with good pressure clears them. If you see a bright white spark, stop. That is titanium burning at the edge, and the hole is already damaged.

• 1
  Through-tool40–70 bar for holes deeper than 3 × Ø.
• 2
  Peck cycleEvery 0.5–1 × Ø with full retract when through-tool is not available.
• 3
  Chip colourSilver-grey is good, blue or black means back off.
• 4
  Titanium sparksStop immediately, re-check speed and coolant.

Difficult materials also push back on the tool. Cutting force is higher, so any weakness in the setup shows up as oversize holes, tapered walls or a drill that walks on entry. A spot drill with a 90° or 120° point removes the walk and gives the main drill a true start.

Runout is the quiet killer. On a carbide drill, total indicated runout above 0.02 mm loads one flute more than the other. In stainless that flute work hardens first, then chips. Check the holder and collet before blaming the drill. A worn collet can add 0.03 mm of runout on its own.

Depth-to-diameter ratio sets the practical limit. Beyond 5 × Ø, chip evacuation and drill deflection both get harder. Beyond 10 × Ø, you are in gun-drilling territory and a standard twist drill will not hold straightness without a pilot and a guide bushing.

Finish follows the same logic. A sharp edge and steady feed give Ra 0.8–1.6 μm in stainless. A dull edge or a dwell leaves a torn, hardened wall that is hard to ream and hard to tap. On a reamed hole, leave 0.1–0.2 mm for the reamer. On a tapped hole, keep the drilled hole 0.05 mm over the nominal tap size so the tap cuts instead of rubbing.

• 1
  Spot first90° or 120° spot drill removes entry walk.
• 2
  Runout limitKeep TIR under 0.02 mm on carbide drills.
• 3
  Depth ratioPlan a pilot or gun drill beyond 10 × Ø.
• 4
  Reaming stockLeave 0.1–0.2 mm for the reamer.

On our 127 CNC machines, drilling these alloys is a normal part of the week. Inconel and titanium parts run on the 5-axis centers where the setup is rigid and the coolant pressure is high. Stainless production runs often go on the mill-turn centers so the hole is drilled and turned in one setup.

The first check is material condition. 304 and 316 arrive in different hardness states, and a batch that is 30 HB harder will change the feed. We check the certificate and, when needed, cut a test hole. On 17-4PH we confirm whether it is in the solution-treated or aged condition before choosing parameters.

The second check is the drill itself. New drills get a runout reading in the holder. Worn drills are measured at the corner, not the margin. A corner wear land over 0.15 mm is the point where stainless starts to work harden, so that drill goes for regrinding.

The third check is the hole. We inspect diameter, roundness and wall finish on a sample before the batch runs. With ±0.005 mm tolerance on finished parts, a drilled hole that is 0.03 mm oversize will not clean up in a light reaming pass. Catching that on the first part is much cheaper than catching it on the last.

• 1
  Material stateConfirm hardness and heat treatment before setting feed.
• 2
  Drill runoutMeasure in the holder, not on the bench.
• 3
  Corner wearRegrind when the wear land passes 0.15 mm.
• 4
  First-part checkVerify diameter and finish before the batch runs.