ISO 513 Material Groups (P, M, K, N, S, H) Explained

ISO 513 sorts the metals you cut into six groups, each with a colour code: P blue, M yellow, K red, N green, S orange, H grey. Every serious carbide grade is labelled with one or more of these letters, and catalogues quote cutting speeds per group. If you can read the group, you can read any insert catalogue in the world.

The six groups at a glance

Code Colour Workpiece materials Typical grades in our range
P Blue Carbon steel, alloy steel, free-cutting steel, cast steel AT210A, AC152P, AC052P, AC252P
M Yellow Austenitic and duplex stainless, cast stainless AP200U, AC200M, AC100M, AP301M
K Red Grey cast iron, nodular (ductile) iron, malleable iron AT202, AC102K, AC202K, AP251K
N Green Aluminium, copper, brass, bronze, non-metallics PD20, HS6120, HS7125, HS8115
S Orange Nickel and cobalt based superalloys, titanium, Inconel AP100S, AP351M, AP403M, AC200M
H Grey Hardened steel, chilled cast iron, hard surfacing PB30, PB60, AP151H, AP153H

Real cutting windows per group

The ranges below are not theory. They are the published manufacturer data of every insert in our catalogue, aggregated: 4526 cutting-data records across 586 insert models. “Typical” is the median of the manufacturer’s published window, which is where most shops actually run.

Group Cutting speed vc (m/min) Typical vc Feed fn (mm/rev) Depth of cut ap (mm)
P Steel 45 – 620 75 – 250 0.10 – 0.30 0.5 – 3.0
M Stainless 60 – 250 85 – 200 0.10 – 0.30 0.5 – 3.1
K Cast iron 50 – 490 95 – 400 0.10 – 0.40 0.7 – 3.5
N Non-ferrous 300 – 600 300 – 600 0.10 – 0.20 0.3 – 3.0
S Heat-resistant 20 – 200 30 – 90 0.10 – 0.30 0.6 – 3.2
H Hardened 90 – 180 120 – 180 0.03 – 0.30 shallow

Why the gaps are so wide

P40 steel can be cut at 620 m/min with a coated grade and a light finishing cut, while the same steel at 5 mm depth with a tough roughing grade runs at 80 m/min. The group code tells you the family, not the number. What actually sets the number is:

  • Depth of cut and feed. Heavy cuts need lower speed. This is the single biggest lever.
  • Grade and coating. CVD-coated grades tolerate more heat and run faster; PVD and uncoated fine-grain grades stay sharp at lower speed and are tougher.
  • Nose radius. A larger radius spreads heat and allows higher speed, but raises cutting forces and can chatter on slender parts.
  • Coolant. Continuous flood lets you push speed; dry or MQL usually means 10–30% less.
  • Machine and setup rigidity. A worn spindle or long overhang forces you down.

Group-by-group practical notes

P – Steel (the default case)

Steel is the most forgiving group. Chips should break into small “6” or “9” shapes, and the classic failure is crater wear on the rake face, which tells you the speed is too high or the grade too soft. If you see built-up edge at low speed, raise vc rather than lowering it. Start at the low end of the grade’s window and raise speed until flank wear reaches about 0.3 mm.

M – Stainless steel

Austenitic stainless (304, 316) work-hardens and has poor thermal conductivity, so heat stays in the tool. The rules: keep the tool in the cut continuously, never dwell, use a sharp positive geometry, and always cut below the work-hardened skin left by a previous pass. Typical vc is 85–200 m/min. Duplex and super-duplex grades drop to the lower half of that.

K – Cast iron

Grey cast iron breaks chips naturally and is easy on the tool, so speeds are high — 95–400 m/min is normal. The enemy is abrasive wear from sand inclusions and the casting skin; reduce speed on the first pass over a skin. Ductile (nodular) iron is tougher and needs about 20–30% less speed than grey. Dry cutting is standard and often preferable.

N – Aluminium and non-ferrous

Aluminium can be cut at 300–600 m/min, often faster, and the tooling problem is not wear at all — it is built-up edge and chip evacuation. Use a polished, sharp, positive insert with a large rake, use sharp nose radii, and do not use a grade with a coating designed for steel. Silicon content above about 7% in cast aluminium makes it abrasive and pushes you towards PCD.

S – Heat-resistant superalloys

Inconel, Waspaloy and titanium keep their strength at cutting temperature, so all the heat lands in the tool. Speed is low (30–90 m/min typical) and you must maintain a constant feed — never let the insert rub. Use a tough PVD grade and a positive geometry. Tool life is measured in minutes here, and the dominant failure is notch wear at the depth-of-cut line.

H – Hardened steel

Above roughly 45 HRC you stop cutting the conventional way and either use a dedicated hard-turning grade (PB30, PB60, AP151H, AP153H — 120–180 m/min) or CBN. Hard turning only works with a rigid setup, a negative geometry with a honed edge, and shallow depth of cut. It will not fix a weak machine.

How to use the group code when choosing an insert

  1. Identify the workpiece group — this narrows the grade immediately.
  2. Pick the geometry from the operation: roughing wants a strong edge (large nose radius, negative rake); finishing wants light cutting forces (small radius, positive rake).
  3. Read the manufacturer’s window for that specific grade and insert, not the group average.
  4. Start at 60–70% of the window, then raise speed in 10% steps while watching flank wear.

The group averages on this page are a starting point. For a specific insert, the per-model page lists the actual published cutting data for every SKU we stock.

Go deeper

Standards and further reading

The material group definitions used throughout this site follow ISO 513. The manufacturer links below are independent technical references.

Material group definitions follow ISO 513:2012. Cutting ranges are aggregated from the published data of the manufacturers we distribute.

Chat on WhatsApp