CNC Milling Drill Guide

• 1
  How a drill cuts compared with a milling cutter
• 2
  Point angle, helix, and what each one changes
• 3
  Tool material and coating for the alloy in front of you
• 4
  Speed, feed, and peck depth that hold a hole size
• 5
  Depth-to-diameter limits and when drilling stops working
• 6
  Design rules that keep a drilled hole cheap
• 7
  Drill, interpolate, or bore: which method for which hole

A twist drill removes material with two cutting lips at the tip and a chisel edge at the very center. That chisel edge does not cut cleanly. It pushes and scrapes, which is why a drilled hole starts with a wandering center and ends with a ragged exit burr. The flutes only lift chips out of the hole; they do not control the wall.

An end mill works differently. The side of the tool cuts, so the wall of the hole is generated by a rotating cylinder rather than by a point. The cutting force points sideways, which means the tool deflects sideways too. That is the trade: a mill gives you a better wall and a true position, but it needs a rigid setup and a smaller stepdown.

This single difference explains most of what follows. Drilling is fast and cheap for the first pass. Milling is slower but holds position and surface finish. A good process plan uses each for the job it does best.

• 1
  Drilling forceMostly axial, pushing the tool into the part.
• 2
  Milling forceMostly radial, bending the tool away from the wall.
• 3
  Chisel edgeThe dead zone at the drill tip that walks off center.

Point angle sets how the drill enters the material. A 118° point is the general-purpose choice for steel and aluminium. A 135° or 140° point is flatter and stiffer, so it resists walking and suits hard alloys and stainless. A 90° point is for sheet and for spotting, where you want a shallow cone and no breakthrough surprise.

Helix angle controls chip evacuation. A standard 30° helix works for most steel. A high helix of 40–45° lifts chips faster and is common in aluminium, where the material is gummy and the flutes can pack. A low helix of 15–20° is stronger and used in brass and in hard materials where the cutting edge needs support behind it.

Web thickness matters more than most drawings suggest. A thick web is strong but the chisel edge is long, so the drill pushes harder and walks more. Web thinning shortens that dead zone. On holes smaller than 3 mm, thinning is often the difference between a straight hole and a broken drill.

• 1
  118° pointGeneral steel and aluminium, low feed pressure.
• 2
  140° pointStainless and hard alloys, less walking.
• 3
  High helixAluminium and soft plastics, better chip lift.
• 4
  Web thinningSmall holes, reduces thrust at the tip.

Uncoated high-speed steel is cheap and sharp, and it still has a place in plastics and soft aluminium. It wears fast in anything abrasive. Cobalt HSS holds an edge longer at higher temperature and is a reasonable middle option for stainless on a manual or light CNC machine.

Solid carbide is the default for production. It is stiffer, so it deflects less and holds size in a deep hole. It also tolerates the surface speeds that make cycle time short. The trade is brittleness: carbide dislikes interrupted cuts and any runout above roughly 0.02 mm.

Coatings change the friction at the cutting edge. TiN is general purpose. TiAlN is the workhorse for steel and stainless because it survives high temperature. DLC is for aluminium and copper alloys, where built-up edge ruins the wall. On aluminium, a polished uncoated carbide drill often beats a coated one, because the coating itself can grab the soft material.

• 1
  HSSPlastics, soft aluminium, low volume.
• 2
  Cobalt HSSStainless on lighter machines.
• 3
  TiAlN carbideSteel, stainless, high-temperature cutting.
• 4
  DLC or polishedAluminium and copper, fights built-up edge.

Surface speed is the first number to set. In 6061 aluminium, carbide runs comfortably at 200–300 m/min. In 304 stainless, drop to 40–80 m/min. In mild steel, 80–120 m/min. These are starting points, not limits; the machine, the coolant, and the hole depth all move them.

Feed per revolution sets the chip thickness. Too light a feed rubs the edge and work-hardens stainless. Too heavy a feed overloads a small drill. A usable rule is 0.02–0.05 mm per revolution for drills under 3 mm, and 0.08–0.20 mm per revolution for 6–12 mm drills in steel.

Peck depth controls chip clearing. For holes deeper than three times the diameter, peck in increments of one diameter or less. In aluminium you can often peck at two diameters. In stainless, stay at 0.5–1 diameter and keep the coolant aimed at the tip, because the chip will not break on its own.

Runout is the quiet killer. If the drill is not concentric with the spindle within about 0.02 mm, one lip does more work than the other, the hole grows, and the drill breaks early. Check the holder before you blame the tool.

• 1
  Aluminium 6061200–300 m/min, high helix, air or mist.
• 2
  304 stainless40–80 m/min, 0.5–1 D pecks, flood coolant.
• 3
  Mild steel80–120 m/min, 1 D pecks, TiAlN.
• 4
  Runout limitKeep below about 0.02 mm TIR.

A standard twist drill is practical up to about 4 times the diameter in a CNC mill. Beyond that, chip evacuation and coolant reach both fail, and the hole starts to drift. At 8 times the diameter you are in gun-drilling territory, where a single-flute tool with through-coolant is the only reliable way.

Hole position is the second limit. A drilled hole on a mill typically lands within 0.05–0.10 mm of nominal, because the chisel edge walks at entry. If the drawing calls for ±0.025 mm position, drill undersize and then interpolate with an end mill, or bore it.

Wall straightness is the third limit. Drills tend to produce a slightly lobed or tapered wall, and the exit burr caps the hole. For a bore that must seal, or a hole that takes a dowel pin, drilling alone is rarely enough.

• 1
  Up to 4 DStandard twist drill, normal peck cycle.
• 2
  4 D to 8 DCarbide drill with through-coolant, tight peck.
• 3
  Beyond 8 DGun drilling or a dedicated deep-hole process.

Keep the hole depth under 4 times the diameter where you can. If a design needs a deep passage, split it: drill from both ends, or add a cross hole so the chips have somewhere to go. A blind hole that traps chips will cost more than a through hole every time.

Standardize diameters. A shop with a drill index full of odd sizes spends setup time hunting for tools. If a hole does not need a specific size, pick from the common set and let the machinist run it without a tool change.

Leave a flat entry. A drill entering a curved or angled surface walks. Add a spot face, or have the shop spot-drill first. On castings and forgings, this one step prevents more scrap than any parameter change.

Call out the tolerance you need, not a tighter one. A hole at ±0.1 mm and a hole at ±0.005 mm look the same on a drawing but are different processes. Reaming or boring adds a step, a tool, and inspection time.

• 1
  Depth under 4 DStandard drilling, no special tooling.
• 2
  Common diametersFewer tool changes, faster cycle.
• 3
  Flat entrySpot face curved surfaces before drilling.
• 4
  Honest toleranceOnly tighten what the function requires.