Material Hardness: What It Tells a CNC Engineer

• 1
  What material hardness actually measures
• 2
  Rockwell, Brinell, and Vickers: picking the right scale
• 3
  How material hardness changes the cutting process
• 4
  Surface hardness and core toughness together
• 5
  Writing hardness on a drawing without ambiguity
• 6
  Typical hardness ranges for common CNC alloys
• 7
  Which hardness test fits which job
• 8
  Hardness versus toughness: where the limit sits

Material hardness is a material's resistance to localized plastic deformation. A hard indenter is pressed into a surface under a known load, and the resulting dent is measured. That is the whole test. It says nothing directly about tensile strength, fatigue life, or impact resistance, though it correlates loosely with some of them in specific alloy families.

The dent geometry defines the scale. A diamond cone gives you Rockwell C. A hardened steel ball gives you Rockwell B or Brinell. A square-based diamond pyramid gives you Vickers. Same physical idea, three different numbers, no universal conversion that holds across every alloy.

This is why a drawing that says only "hardness 55" is incomplete. Fifty-five on which scale? Measured where on the part? At what depth below the surface? A carburized case at 58 HRC with a 0.4 mm effective depth behaves nothing like through-hardened 58 HRC stock.

For machining, the number you care about is the one at the depth the tool engages. A soft core under a hard skin cuts very differently from a uniformly hard bar.

Rockwell is fast and needs no optical measurement, so it dominates production floors. Rockwell C (150 kgf, diamond cone) covers hardened steels, roughly 20 to 70 HRC. Rockwell B (100 kgf, 1/16 in ball) covers soft steels, brass, and aluminum, roughly 20 to 100 HRB. The two scales do not overlap, and quoting one when the drawing means the other is a classic shop error.

Brinell uses a 10 mm ball, usually at 3,000 kgf for steel or 500 kgf for softer metals. The large impression averages out local variation, which is why foundries and casting suppliers still use it. The downside is a visible dent. You cannot Brinell-test a finished sealing face.

Vickers uses a pyramid and a microscope. It works on the widest range of materials, and because the loads can be tiny (10 gf to 1 kgf), it is the standard choice for case depth profiles, weld heat-affected zones, and thin coatings. A microhardness traverse is how you prove a nitrided layer is 0.25 mm deep rather than 0.15 mm.

Leeb and ultrasonic rebound testers are portable. They are useful for sorting incoming stock and for field checks on large parts. Treat their readings as screening values, not as acceptance data, unless you have a correlation curve built against a bench test for that exact alloy.

Below roughly 30 HRC, carbide tools cut most steels comfortably. Feed rates stay high, tool life is long, and the main constraint is chip evacuation. This is the range where 6061-T6 aluminum, 303 stainless, and 1018 steel live, and where a 3-axis or 4-axis setup handles most work.

Between 30 and 45 HRC, cutting forces rise and heat concentrates at the edge. You drop surface speed, increase feed per tooth to keep the edge engaged, and expect shorter tool life. Rigid setups matter more than tool grade at this point. Chatter shows up first on thin walls and long overhangs.

Above 45 HRC, you are in hard milling territory. Either use CBN or coated carbide with a negative rake and accept lower material removal rates, or anneal the part, machine it soft, and harden it afterward. The second route is usually cheaper for complex geometry, because hardened stock at 55 HRC grinds tooling budgets fast.

Very soft materials have their own problem. Annealed aluminum and pure copper gum up flutes, build up an edge, and leave a torn finish. Hardness below 20 HRB is often harder to machine cleanly than 35 HRC steel, just for different reasons.

• 1
  Under 30 HRCCarbide, high speeds, standard geometry.
• 2
  30-45 HRCReduce speed, increase feed per tooth, check rigidity.
• 3
  Over 45 HRCHard mill with CBN, or machine soft and heat treat after.
• 4
  Under 20 HRBWatch built-up edge and chip welding, use sharp positive rake.

Most wear parts do not want uniform hardness. They want a hard skin and a tough core. Carburizing a 1018 or 8620 gear to 58-62 HRC over a 0.3-0.8 mm case gives you abrasion resistance at the flank and impact resistance at the root. Through-hardening the same gear to 58 HRC would crack on the first overload.

The number that matters on the drawing is effective case depth, not total case depth. Effective depth is measured to the point where hardness drops to 50 HRC, or 550 HV, depending on the standard your customer uses. Two suppliers quoting "0.5 mm case" can deliver parts that differ by 40 percent in effective depth.

Nitriding produces a thinner, harder layer, typically 0.1-0.3 mm at 60-70 HRC equivalent, with almost no distortion because the process runs around 500-550 °C and needs no quench. It suits finished parts where you cannot grind after treatment: valve stems, extrusion screws, injection mold cores.

Induction hardening is the fast option for a localized band, such as a shaft journal or a spline. Depth control is looser than carburizing, but cycle time is seconds rather than hours. For a 40 mm shaft journal, 2-4 mm depth at 55-60 HRC is a routine spec.

State the scale and the range, not a single value. "58-62 HRC" tells the heat treater and the inspector the same thing. "60 HRC" invites argument over a 0.5-point miss that has no engineering consequence.

State the location. A hardness callout on the title block applies to the whole part unless you say otherwise. If only the raceway needs 58 HRC, mark that zone and give the core a separate softer spec, for example 30-38 HRC.

State the test method and the conversion basis. If the part is small or thin, Rockwell C may not be valid because the anvil effect distorts the reading. Vickers with a defined load is the honest choice there. If you accept converted values, name the conversion table.

Finally, say what happens at the boundary. Is a reading one point below the low limit a reject, or a re-test? Deciding that before the parts arrive saves a lot of back-and-forth, especially on small lots where rework means re-heat-treating the whole batch.

Aluminum 6061-T6 sits around 95 HRB, or 60 HV. It machines fast and finishes well with carbide. 7075-T6 is harder at roughly 150 HB, which improves strength but slightly increases tool wear and reduces the mirror finish you get from 6061.

Stainless 303 is the free-machining grade, around 200 HB in the annealed condition. 304 and 316 work-harden quickly, so light cuts and constant feed matter more than raw hardness. 17-4PH in the H900 condition reaches about 44 HRC and is a common choice for shafts that need corrosion resistance and strength together.

Steel 4140 in the normalized state is around 25-30 HRC and cuts cleanly. Quenched and tempered to 40 HRC it is still machinable with coated carbide if you keep the setup rigid. Tool steel like D2 arrives annealed at roughly 20 HRC and only reaches 58-62 HRC after hardening.

Titanium Ti-6Al-4V measures around 36 HRC, but it cuts like something much harder because of low thermal conductivity and high chemical reactivity. Hardness alone would badly understate the difficulty. Inconel 718 sits near 40 HRC and is worse still. In these alloys, tool life is governed by heat and chemistry, not by the indentation number.