CNC Processing Materials: How to Match Alloy to Part

• 1
  What Machinability Actually Measures in CNC Processing Materials
• 2
  Aluminium Alloys: The Default for Most Housings
• 3
  Stainless and Steel: Where Tolerances Get Expensive
• 4
  Titanium, Copper, and Other Difficult Grades
• 5
  Plastics: Tolerance Is a Moving Target
• 6
  How to Read a Material Callout on a Drawing
• 7
  CNC Processing Materials Compared

Machinability is not one number. It is a shorthand for four separate behaviors that show up at the cutting edge: how easily the material forms a breakable chip, how much heat the tool absorbs, how much the surface work-hardens, and how far the part moves once the clamps come off. A material that scores well on the first two can still fail on the last one.

Take 304 stainless. It cuts with long, stringy chips that wrap around the tool and pull heat into the insert. The same alloy work-hardens under a dull edge, so a second pass over the same surface often cuts harder than the first. That is why 303, with its sulfur addition, machines roughly twice as fast as 304 despite similar strength.

Aluminium 6061-T6 sits at the opposite end. Chips break cleanly, cutting forces stay low, and the material dissipates heat fast enough that carbide tool life is measured in hours, not minutes. The penalty is stiffness: thin walls in 6061 deflect under a 0.5 mm depth of cut, and that deflection shows up as taper, not as a surface finish problem.

Hardness alone predicts very little. Annealed 4140 at 28 HRC machines reasonably well, while the same alloy at 45 HRC needs reduced feed, smaller radial engagement, and a rigid setup. Two parts with the same alloy name can behave like different materials depending on heat treatment and stock condition.

• 1
  Chip formBreaks short = easier automation
• 2
  Heat pathWhere the heat goes decides tool life
• 3
  Work hardeningAffects second-pass cutting load
• 4
  Residual stressDecides whether the part moves after unclamping

6061-T6 covers a large share of machined enclosures, brackets, and manifolds. Its yield strength around 276 MPa is enough for structural housings, and it anodizes predictably to Ra 0.8–1.6 μm before coating. If a part needs a clean cosmetic face and moderate load, 6061 is the safe starting point.

7075-T6 raises strength to roughly 503 MPa and is common in aerospace ribs and fittings. It machines well but costs more and anodizes to a slightly darker, less uniform tone than 6061. Choose it when the strength-to-weight ratio drives the design, not when the part merely needs to look good.

2024-T4 cuts cleanly and takes threads well, though its copper content makes it less corrosion resistant without cladding or coating. 5052 and 5083 bend and weld better than they cut, so they usually belong in sheet metal work rather than CNC turning. ADC12 covers die-cast housings where a casting plus light finishing beats machining from solid.

Watch for thin floors. A 1.0 mm aluminium floor will chatter at 12,000 rpm unless the tool path keeps constant radial engagement. Roughing with a 6 mm carbide end mill and finishing with a 3 mm tool at light depth usually holds ±0.005 mm on wall thickness.

Stainless grades split into two practical groups. The 303, 304, 316, and 316L family covers fluid handling, food equipment, and general corrosion resistance. The 17-4PH and 440C group covers higher strength and wear: 17-4PH in the H900 condition reaches roughly 1,310 MPa, and 440C hardens to around 58 HRC for wear surfaces.

Free-machining 303 is the cheapest stainless to cut, but its sulfur content lowers corrosion resistance and weldability. If the part will be welded or exposed to chlorides, move to 304 or 316L and accept slower cutting with more coolant. That trade is usually decided by the service environment, not by the machine shop.

Carbon and alloy steels behave predictably once hardness is known. 1018 and 1045 are common for shafts and fixtures. 4130, 4140, and 4340 enter when fatigue life or impact strength matters, and A36 stays in weldments and base plates. Tool steel appears in dies and wear inserts, usually hardened after machining.

The hard part is not cutting these steels. It is holding size after heat treatment. A 4140 shaft that measures correctly in the soft state can move 0.02–0.05 mm per 100 mm through quench and temper. Leave grinding stock, or specify a stress-relief step before finishing.

• 1
  303 / 304 / 316LCorrosion first, speed second
• 2
  17-4PHStrength with moderate corrosion resistance
• 3
  4140 / 4340Fatigue and impact, plan for post-HT movement
• 4
  440CWear surfaces, machine before hardening

Titanium TC4, also written Ti-6Al-4V, has a thermal conductivity near 7 W/m·K, roughly a tenth of aluminium. Heat stays in the cut zone, so the cutting edge reaches temperatures that dull carbide quickly. Low surface speed, high feed per tooth, and flood coolant keep tool life usable. Never let the tool rub.

Inconel behaves worse. It work-hardens fast and holds strength at temperatures that soften the insert. Light radial engagement, sharp edges, and rigid toolholding matter more than spindle speed. These parts also carry higher residual stress, so a finishing pass after roughing and a stress-relief cycle help hold flatness.

Copper and brass sit at the easy end. C36000 free-cutting brass machines faster than any steel on this page. C101 and C110 copper cut cleanly but gum up on the tool if rake angles are too small, and beryllium copper needs dust control because the fines are a health hazard.

Magnesium AZ31B and AZ91D cut fast with excellent surface finish, but the chips are flammable. Dry machining with proper chip evacuation and no accumulated fines is standard practice. If your shop cannot control that, the part should be cut elsewhere.

Plastics are not metals with a different cutting speed. Their thermal expansion is five to ten times higher, so a POM or PP part measured at 20 °C will not measure the same at 40 °C. Quote drawings should state the measurement temperature if the tolerance is tight.

POM and PA machine well and hold ±0.05 mm on stable geometry. ABS and PMMA are softer and prone to edge burrs, so sharp tools and climb milling reduce cleanup. PEEK holds strength at high temperature but costs far more and needs slower speeds to avoid melting at the edge.

Carbon fibre reinforced plastics cut cleanly only with diamond-coated tooling. Standard carbide wears in minutes, and delamination at the exit face appears when feed is too high. Support the back side of the laminate or use a backing plate.

HDPE and PP are low cost and chemically resistant, but they flex under clamping. Holding ±0.005 mm on a 200 mm PP part is unrealistic. Loosen the tolerance, or switch to a stiffer material if the function allows it.

• 1
  POM / PABest dimensional stability among common plastics
• 2
  PEEKHigh temperature service, high cost
• 3
  CFRPDiamond tooling, backed exit face
• 4
  PP / HDPEChemical resistance, poor stiffness

A callout like 6061-T6 tells the machinist the alloy and temper, but not the stock form, grain direction, or which faces are datum. Those three items decide whether the finished part meets the drawing as easily as the alloy choice does.

Grain direction matters on thin ribs and long shafts. A part cut from extruded bar can bow after material is removed from one side only. Specify the stock form, or allow the shop to choose plate versus bar based on symmetry.

Temper also sets the finishing plan. Anodized 7075 looks different from anodized 6061, and hardcoat anodizing on 2024 can fail on copper-rich phases if the surface prep is wrong. If cosmetics matter, name the alloy and the finish together.

Finally, state the inspection basis. A ±0.005 mm callout with no datum scheme and no measurement temperature gives the inspector nothing to work with. Add datum targets and a note on where the part is measured.