Manufacturing processesReading time 12 min

How to pick a cutter, and when to change it

Tooling is the only thing in machining that gets consumed, and the thing most often treated as “just buy the same one again”.

⌀

01Materials: hardness against toughness

Material	Hardness	Toughness	Typical use
High-speed steel	Low	High	Low speed, interrupted cuts, form tools
Powder metallurgy HSS	Medium-low	High	Broaches, hobs
Carbide	High	Medium	The vast majority of milling and turning
Cermet	High	Medium-low	Finish turning steel, excellent surface
Ceramic	Very high	Low	High-speed turning of cast iron and heat-resistant alloys
CBN	Very high	Low	Hardened steel above HRC 45
PCD	Very high	Low	Aluminium, copper, composites (never steel)

Further down the list means harder and faster but less tolerant of shock. PCD cannot machine steel, the carbon diffuses.

02Coatings: layers of function

Coating	Colour	Temperature	Good at
TiN	Gold	About 600 °C	General purpose, cheap
TiCN	Blue-grey	About 400 °C	Wear resistant; suits stainless and cast iron
TiAlN / AlTiN	Purple-black	Above 800 °C	High-speed dry cutting, hard materials
AlCrN	Grey-blue	Above 1000 °C	Heat-resistant alloys, stable at temperature
DLC	Black	Low	Aluminium, copper and other gummy materials; prevents built-up edge
Uncoated (polished flute)	—	—	Aluminium alloys; a sharp edge that does not load up

TiAlN forms an alumina layer at temperature, so it actually wears better the hotter it gets, which is why it suits dry cutting.

03Flutes: productivity, chip evacuation and rigidity

Two flutes. The most chip room; suits aluminium, deep slots and full-engagement slotting.
Three flutes. The usual compromise for high-speed aluminium work.
Four flutes. The general choice for steel; balanced rigidity and productivity.
Five or more. Finishing and high-speed machining at light radial depth: faster feed at the same speed, but little chip room and no deep slotting.

Flute count affects the feed rate at a given spindle speed (Vf = fz × z × n). Double the flutes at the same fz and the feed doubles, provided the chips can get out and the machine can push it.

04Hole making: three methods and their places

Method	Achievable accuracy	Depth	Notes
Drill	IT11 ～ IT13	3 to 5 D typically	Poor positional accuracy; needs a spot drill or centre drill
Gun drill / deep-hole drill	IT9 ～ IT10	Beyond 10 D	Through coolant, excellent straightness
Reamer	IT7 ～ IT8	Shallow holes	Corrects size only, never position
Boring bar	IT6 ～ IT7	Depends on the bar	Corrects position and roundness; single-point and adjustable
Helical interpolation	IT8 ～ IT9	Depends on tool length	One tool covers many diameters; suits low-volume, high-mix

A reamer follows the existing hole, so positional accuracy has to be guaranteed by the previous operation.

05When to change the tool

Tool wear takes several forms, and each points at a different problem.

Wear pattern	Appearance	Cause	What to do
Flank wear VB	A flat worn below the edge	Normal wear	Change at a set VB, usually 0.2 to 0.3 mm
Crater wear	A hollow in the rake face	Chip friction, diffusion wear	Reduce Vc, change coating
Chipping	A piece missing from the edge	Impact, chip packing	Reduce fz, improve chip evacuation, choose a tougher grade
Built-up edge	Material welded to the edge	Speed too low, gummy material	Raise Vc, use DLC or a sharper edge
Thermal cracking	Cracks perpendicular to the edge	Alternating heating and cooling in interrupted cuts	Cut dry or supply coolant steadily, never intermittently

The wear pattern tells you more than the hours. It tells you which parameter is wrong.