CNC Drilling Steps: 7 Moves That Protect Hole Precision

• 1
  Key takeaways
• 2
  Spot the hole and pick the right drill geometry
• 3
  Set speeds, feeds and peck depth around the drill
• 4
  Hold the part and the tool steady
• 5
  Finish the hole, then verify it mid-run
• 6
  The seven CNC drilling steps in order
• 7
  Drilling method versus achievable result

Every CNC drilling steps sequence starts before the drill touches metal. Spot with a 90° or 120° spot drill, 0.3 to 0.5 mm deep, at roughly 60 to 70% of the drilling speed. That shallow cone gives the twist drill a true entry angle. Without it, a standard 118° point wanders on curved or inclined surfaces, and the hole walks 0.05 to 0.15 mm off position before the full diameter is cut.

Match the point angle to the material. A 118° point suits 6061 and most stainless. A 140° point is stiffer and works better in 304 or 316 where the edge tends to rub. For Inconel or Ti-6Al-4V, use a split-point or thinned web with a 135° to 140° angle. That geometry pulls the chisel edge into the cut rather than pushing material sideways.

Web thinning matters most on small holes. Under Ø3 mm, a heavy web doubles the thrust force and pushes the drill off center. Ask for a thinned web and a polished flute when you order tooling. The cost is small next to scrapped parts.

Do not spot on a rough cast skin or a plasma-cut edge. Face it first, or expect the spot to follow the surface instead of removing it.

• 1
  Spot depth0.3 to 0.5 mm. Deeper than 1 mm just wears the spot tool.
• 2
  Point angle118° for aluminum, 135° to 140° for stainless, titanium and nickel alloys.
• 3
  Surface prepFace rough or scaly stock before spotting.

Surface speed drives edge life more than anything else in the CNC drilling steps list. In 6061, run 90 to 120 m/min. In 304 and 316, drop to 15 to 25 m/min. Titanium sits around 10 to 15 m/min, and Inconel lower still. If the chips come off blue or the drill squeals on entry, the surface speed is too high, not the feed.

Feed per revolution controls chip thickness. A common starting value is 0.05 to 0.10 mm/rev per 3 mm of drill diameter, then adjust by chip shape. You want short comma-shaped chips in steel and 6-9 chips in aluminum. Fine powder means the feed is too low and the edge is rubbing. Long stringy chips mean the feed is too high or the flute is not clearing.

Peck depth follows hole diameter. On Ø3 mm and under, peck at roughly 1×D. On Ø6 mm and up, 2 to 3×D per peck is usually enough. Deep holes past 5×D benefit from a full retract, not just a chip break, so coolant reaches the tip. On a 4,000 mm maximum processing size part with many holes, a consistent peck plan beats a clever one.

Coolant must reach the cutting edge. Through-spindle coolant is the cleanest answer on holes deeper than 3×D. Flood coolant alone often misses the tip on horizontal setups.

• 1
  Aluminum 606190 to 120 m/min, 0.10 to 0.20 mm/rev.
• 2
  Stainless 304 and 31615 to 25 m/min, 0.05 to 0.10 mm/rev.
• 3
  Titanium and Inconel10 to 15 m/min or lower, light feed, rigid setup.

Rigidity is where most precision is won or lost. Keep the drill overhang under 5×D where you can. Every extra 10 mm of stick-out bends the tool a little more, and that bend shows up as hole taper. On a Ø8 mm drill, a 60 mm overhang instead of 40 mm can add 0.03 mm of taper across a 30 mm deep hole.

Clamp close to the hole. If the part lifts or rings during the cut, the drill is telling you the fixture is soft. Plates bolted only at the corners will flex in the middle, and the hole comes out oversize at the top. Add a support or move the clamps inward.

Spin the tool, not the part, for off-center holes on a plate. On a mill-turn center or a lathe, drilling on the axis is fine, but an off-axis hole on a rotating part tends to ride the surface.

Check runout on the holder and the drill together. Total indicated runout above 0.02 mm will open the hole and shorten tool life. Clean the taper, seat the collet properly, and re-check before the first cut.

• 1
  OverhangKeep under 5×D. Reduce it before you change any speed or feed.
• 2
  RunoutHold under 0.02 mm at the drill tip.
• 3
  ClampingSupport the part directly under the hole whenever possible.

A drilled hole is not a finished hole unless the drawing says so. Drilling holds roughly H11 to H12 on diameter, and position depends on the spot and the fixture. If the tolerance is tighter than ±0.05 mm, plan a reamer, a boring pass, or a helical interpolation with a small end mill. Reaming removes 0.1 to 0.2 mm of stock and needs a straight, round pilot hole first.

Deburr both ends. Burrs at the exit change the effective diameter where a pin or a dowel seats. On cross-drilled holes, a burr inside the main bore is worse than the one you can see, so deburr before you measure.

Verify with the right tool. A pin gauge checks size but not position. A CMM or a bore gauge with a dial indicator catches roundness and taper. Check the first part, then every 10 to 20 parts depending on tool wear rate, and always after a tool change.

Log what you see. Drill wear, chip color, and coolant flow tell you when to index the tool before the hole drifts out of tolerance.

• 1
  Reaming stock0.1 to 0.2 mm on diameter for a clean finish.
• 2
  Deburr firstMeasure after deburring, not before.
• 3
  FrequencyFirst article, then every 10 to 20 parts, and after every tool change.