CNC Machine Bit Selection: A Working Checklist

• 1
  What decides a CNC machine bit before you open the catalog
• 2
  Carbide grade and coating: where the heat goes
• 3
  Flute count decides chip room and feed rate
• 4
  Feature geometry and setup rigidity set the real limit
• 5
  Practical pairings from aluminium to titanium
• 6
  Reading the wear pattern to correct the choice
• 7
  CNC machine bit selection by material and operation

A cutting tool is chosen by four inputs, not by brand. They are the workpiece material, the tool substrate and coating, the flute count and helix, and the operation with its target finish. Change one and the correct answer changes. Aluminium and stainless steel rarely share a cutter, and a roughing pass and a finishing pass rarely share one either.

Start with hardness and thermal conductivity. Aluminium conducts heat away fast, so the cutter stays cool and can run at high surface speed. Titanium and Inconel hold heat at the edge, so the same speed burns the tip in minutes. That single difference explains most of why the same geometry works in one material and fails in another.

Then look at the feature you are cutting. A deep pocket with a 4:1 depth-to-diameter ratio needs a different tool than a shallow face pass on the same part. A Ø6 mm cutter hanging 40 mm out of the holder will deflect, no matter how good the coating is. Rigidity of the setup sets the ceiling on what the bit can hold.

Finally, write down the tolerance and finish target. A ±0.005 mm bore and a Ra 0.8–1.6 μm wall are two separate problems. The first is about tool runout and machine repeatability. The second is about edge geometry and feed per tooth. Solving them with one tool usually costs more than splitting the job into roughing and finishing tools.

• 1
  Material firstHardness and heat transfer set the speed limit.
• 2
  Operation secondRoughing, semi-finish and finish need different edges.
• 3
  Rigidity thirdLong reach and thin walls cap the feed rate.
• 4
  Tolerance lastTight bores are a runout problem, not a coating problem.

Solid carbide covers most CNC milling and drilling under Ø20 mm. It holds an edge at high temperature far better than high-speed steel, and it resists the abrasive wear that comes with glass-filled plastics or cast aluminium. High-speed steel still has a place in low-volume drilling and in taps, where toughness beats hot hardness.

Coating choice follows the material. Uncoated polished carbide is the default for aluminium, because a rough coating traps chips and builds up edge material. Titanium aluminium nitride (TiAlN) handles steel and stainless at higher temperatures. Aluminium chromium nitride (AlCrN) suits hardened and high-alloy work. Diamond-like carbon helps in abrasive non-ferrous and composite work.

Geometry matters as much as the label on the box. A 45° helix clears chips quickly in aluminium. A 38° helix adds edge strength for steel. Variable helix and variable pitch break the harmonic chatter that shows up as a rippled floor in deep pockets. For finishing walls, a small corner radius distributes load and lengthens tool life.

Do not judge a cutter by coating color. Two tools with the same gold finish can differ by 30% in edge preparation, and edge preparation is what controls whether the tool chips on the first cut. Ask for the grade and the geometry, not the marketing name of the layer.

• 1
  AluminiumUncoated polished carbide, 2–3 flutes, 45° helix.
• 2
  Steel and stainlessTiAlN or AlCrN, 4–5 flutes, 38° helix.
• 3
  Titanium and InconelAlCrN or uncoated, sharp edge, conservative speed.
• 4
  Composites and plasticsDiamond-like carbon, low helix, sharp geometry.

Flute count is a trade. More flutes mean more teeth in the cut per revolution, so the feed rate rises for the same chip load per tooth. Fewer flutes leave bigger gullets, so chips clear without recutting. In soft, gummy aluminium, chip evacuation wins and 2 or 3 flutes are normal. In steel, more flutes win because the chip is short and breaks cleanly.

The rule of thumb: keep at least two flutes out of the cut at all times in a deep pocket. With a 4-flute cutter in a narrow slot, chip packing stalls the tool even at moderate feed. A 3-flute cutter with a polished flute face often cuts deeper and faster in 6061 than a 4-flute of the same diameter.

For finishing walls in 7075 or 17-4PH, a 5-flute or 6-flute cutter can raise the feed rate without losing surface quality, provided the machine has the spindle speed and the coolant reaches the edge. If coolant cannot reach the tip, more flutes simply means more heat trapped in the cut.

Drills follow the same logic. Two-flute drills remove chips from deep holes in aluminium. Three-flute and four-flute drills hold a straighter hole in steel, but they need through-spindle coolant once the depth passes 3× diameter. Without it, chip packing and drill wander show up together.

• 1
  2 flutesMaximum chip room, best for soft and gummy material.
• 2
  3 flutesBalanced choice for aluminium roughing and slotting.
• 3
  4–5 flutesHigher feed in steel and stainless, short chips.
• 4
  6+ flutesFinishing passes where chip load per tooth is small.

A tool that works on a Ø50 mm boss may fail in a 4 mm slot. The difference is engagement angle. In a full-width slot the cutter is buried in material and the radial load peaks on every pass. In a light side cut the same cutter sees a fraction of that load. This is why trochoidal paths let a small tool remove a large pocket at high feed.

Reach is the second constraint. Deflection scales with the cube of the overhang, so doubling the stick-out makes the tool eight times softer in bending. If a Ø6 mm cutter must reach 40 mm deep, expect to cut the feed and step-down by half, and to accept a slower cycle. A necked tool or a larger shank helps more than a coating change.

Thin walls are a third case. Below 1 mm wall thickness, the workpiece itself deflects away from the cutter. Spring passes and reduced radial engagement recover the dimension. On our 5-axis centers, we often rough with a 4-flute cutter and finish with a 3-flute at low engagement to hold wall straightness.

The holder is part of the system. A shrink-fit or hydraulic holder at 3× diameter runout under 0.005 mm keeps the edge load even between flutes. A worn collet chuck can add 0.02 mm runout, and one flute then does most of the cutting. That single flute wears first and the surface finish tells you which one it was.

• 1
  Deep pocketLimit step-down, use a necked tool, keep 2 flutes engaged.
• 2
  Thin wallLower radial engagement and add a spring pass.
• 3
  Long overhangCut feed and depth by half at 4:1 reach.
• 4
  Holder runoutKeep below 0.005 mm to share load across flutes.

For 6061, 6082 and 7075, a 3-flute uncoated carbide end mill with a 45° helix covers most roughing and semi-finishing. Run it at 300–500 m/min surface speed and 0.05–0.15 mm feed per tooth, depending on diameter. Add air blast or mist; flood coolant is optional but helps chip clearing in deep pockets.

For 304 and 316 stainless, switch to a 4-flute or 5-flute AlCrN-coated cutter at 80–150 m/min and 0.03–0.08 mm per tooth. Stainless work-hardens, so never let the tool rub. Keep the feed high enough to stay under the hardened layer, and never dwell in the cut. A light pass with a dull tool is worse than a heavier pass with a sharp one.

For 17-4PH and 4140, expect 60–120 m/min and a shallow step-down. Tool life drops fast past 200 m/min, and the failure mode is chipping rather than gradual wear. For TA2 and TC4 titanium, run 40–80 m/min, use plenty of coolant, and change the tool before the edge dulls. Titanium fires if the chip is recut, so chip evacuation is a safety issue, not just a quality one.

For POM, PEEK and ABS, use a 2-flute cutter with a sharp edge and a low helix. Plastics melt at the edge if the surface speed is too high, so keep 200–400 m/min and a generous chip load. For carbon fibre, use a diamond-coated cutter and expect the edge to dull by abrasion rather than heat.

• 1
  Aluminium 6061/70753 flutes, uncoated, 300–500 m/min.
• 2
  Stainless 304/3164–5 flutes, AlCrN, 80–150 m/min, no rubbing.
• 3
  Titanium TA2/TC4Sharp edge, 40–80 m/min, flood coolant.
• 4
  Plastics and composites2 flutes, sharp, diamond coating for CFRP.

The wear pattern tells you which variable was wrong. Uniform flank wear along the cutting edge is normal and expected; the tool simply reached end of life. Chipping at the corner means the feed per tooth was too high, the tool had runout, or the entry was too abrupt. Add a chamfer or a corner radius and reduce the feed by 20%.

Built-up edge in aluminium looks like a lump of welded material on the rake face. It comes from too low a surface speed or too little chip load, which lets the material smear instead of shear. Raise the speed or the feed, and switch to a polished uncoated tool if the coating is the culprit.

Thermal cracks that run perpendicular to the cutting edge come from interrupted cuts with too much coolant or too little. In face milling of cast iron or hardened steel, reducing coolant or switching to air blast usually fixes it. Notching at the depth-of-cut line points to work hardening in stainless; vary the axial depth between passes so the notch does not line up.

If the surface finish is poor but the tool looks fine, check the holder and the spindle first. Runout and vibration cause more finish problems than the cutter itself. Measure runout at the tool tip, not at the holder, and re-seat the tool before you change grades or coatings.

• 1
  Corner chippingLower feed per tooth 20%, add a corner radius.
• 2
  Built-up edgeRaise speed or feed; use uncoated polished carbide.
• 3
  Thermal cracksReduce coolant in interrupted cuts, check entry angle.
• 4
  Poor finish, good toolMeasure runout at the tip; re-seat the holder.