CNC Milling Cutter Guide

• 1
  What happens at the cutting edge
• 2
  Flute count, helix, and core diameter
• 3
  Why coating choice follows material, not habit
• 4
  Runout and holder choice decide the real tolerance
• 5
  When five-axis removes the second setup
• 6
  Matching the cutter to the material
• 7
  Cutter geometry by feature and material

A milling cutter does not shear metal the way scissors do. Each tooth takes a short, thick chip, then leaves the cut and air-cools before the next tooth arrives. That interrupted contact is why milling tools fail differently from turning tools. The load is cyclic, so the edge sees impact as well as abrasion.

Feed per tooth sets chip thickness. Too thin and the edge rubs instead of cutting, which work-hardens stainless and burns the flank. Too thick and the tooth chips. A practical starting range for carbide in 6061 aluminium is 0.05–0.15 mm per tooth; in 4140 steel, 0.03–0.08 mm.

Radial and axial depth of cut decide how much of the flute is engaged. A 50 percent radial stepover with a shallow axial pass spreads heat into the chip rather than the tool. That is the usual fix when a cutter squeals on a light finishing pass.

Heat leaves with the chip. If the chip looks blue or gray, the edge is running too hot for the material, and the coating is already losing its job.

More flutes means more teeth in the cut per revolution, so feed rate climbs. Fewer flutes means a deeper chip gullet, so the tool can clear material in aluminium without packing the flutes. That single trade-off explains most cutter selection.

A 2-flute cutter is the default for aluminium and plastics. A 4-flute cutter is the general-purpose choice for steel. A 6-flute or higher tool is for finishing and for light radial engagement, where the extra teeth carry the load and surface finish improves.

Helix angle controls the direction the chip is pushed and how much axial force the tool generates. A 30° helix on steel is common. A 45° helix on aluminium lifts the chip and reduces chatter. A variable helix breaks the harmonic that causes a single tone to build into a full chatter mark.

Core diameter is the hidden variable. A tool with a thick core resists deflection and cuts more accurately, but it has less room for chips. On deep pockets, a thin-core tool with a large gullet wins even though it deflects more.

Uncoated carbide is still correct for aluminium in many shops. The polished surface keeps the chip from welding to the edge. A coating with high aluminium content, such as AlTiN, can drag on aluminium and build up edge material.

TiAlN and AlTiN work on steel and stainless because they form an oxide layer at the temperatures the cut generates. That layer slows diffusion wear. Drawback: they need speed to reach that temperature, so running them slowly wastes the coating's benefit.

DLC and diamond coatings suit non-ferrous work and composites. Carbon fibre and graphite are abrasive, and these coatings are the reason a cutter survives a full panel rather than one pass.

Tool life is not linear with speed. Doubling surface speed can halve life or worse, depending on the material. Write the cutting parameters down for each combination you run, not just the ones that work.

Runout is the amount the cutting edge wobbles off the spindle centerline. A cutter with 0.01 mm runout cuts one tooth deeper than the rest. The load is uneven, and the tool wears out on one side first. Finished size wanders with it.

Check runout at the tip of the tool, not at the holder face. For a finishing cutter, keep total indicated runout under 0.005 mm. That figure matters more than the tool's catalog tolerance, because the machine, holder, and tool stack together.

A hydraulic or shrink-fit holder runs truer and stiffer than a collet chuck at long reach. On a Ø6 mm end mill reaching 60 mm deep, a collet holder will chatter where a shrink-fit holder will not.

Tool overhang is the main lever on stiffness. Deflection rises with the cube of the length, so cutting overhang in half reduces it roughly eight-fold. If a cutter sings, pull it back before changing the feed.

A three-axis machine reaches only along one tool axis. Features on the side of a part need a re-fixture, and every re-fixture adds error and time. A five-axis machine tilts the tool and the table so the cutter stays normal to the surface.

Keeping the cutter normal to a curved surface keeps the effective chip load even across the path. On a ball-nose tool, working off-axis also moves the contact point off the tool center, where surface speed is zero. That is why five-axis finishing looks better and cuts cooler.

The tilt is not free. A tilted tool in a deep pocket will collide with the wall, so a short, stiff cutter is mandatory. Setup and programming take longer, and the work envelope is smaller than on a three-axis machine.

The gain is real on parts with angled faces, ports, or a feature on more than one side. A bracket with two machined faces and a bolt hole at 45° is a good fit. A flat plate with a pocket is not; three-axis does it faster and cheaper.

Aluminium 6061 cuts fast and wants a 2-flute or 3-flute cutter with polished flutes. 7075 behaves differently: it is stronger and more abrasive, and a coated 3-flute tool at moderate speed keeps the finish clean.

Stainless 304 and 316 work-harden under a rubbing edge. Use a 4-flute or 5-flute cutter, keep the chip load up, and never dwell. A light pass that rubs will harden the surface and dull the next tooth faster.

Titanium Ti-6Al-4V and Inconel 718 hold heat at the edge. Cut with flood or high-pressure coolant, a sharp edge, and a lower surface speed than you would use on steel. Tool life is short by nature, so plan for it.

Plastics and composites behave differently again. POM and PEEK cut cleanly with a sharp 2-flute tool and high rake. Carbon fibre needs a diamond-coated cutter and a dust extraction plan, because the dust is abrasive and a health hazard.