CNC Material Guide

• 1
  What Machinability Actually Means in a CNC Material Guide
• 2
  Aluminum Alloys: The Usual Starting Point
• 3
  Stainless, Carbon and Alloy Steel: Where Tolerances Get Harder
• 4
  Titanium, Copper Alloys and Engineering Plastics
• 5
  How Part Geometry Pushes You Toward a Material
• 6
  CNC Material Guide: Machinability and Typical Use

Machinability is not one number. It is a summary of four things happening at the cutting edge: how much heat the chip carries away, how much the tool rubs, how the material work-hardens, and how the chip breaks. A material with high thermal conductivity pulls heat out of the shear zone and into the part and the fixture, which keeps the edge cooler but pushes thermal growth into your dimensions.

Alloy and temper move these four factors more than most designers expect. 6061-T6 machines cleanly because the magnesium-silicon precipitate is fine and the chip is brittle enough to break at moderate feeds. Switch to 6061-O and the same cutter smears instead of shears. Switch to 7075-T6 and the chip breaks easily but the cutting forces are higher because the yield strength is roughly double.

Hardness alone does not predict the result either. Annealed 304 stainless is softer than 4140 pre-hardened, yet it machines worse. The austenitic structure work-hardens under the tool, so a light finishing pass on a dull insert raises the surface hardness exactly where you wanted a clean cut.

This is why we ask for the drawing, the alloy and the temper before quoting cycle time. A CNC material guide that only lists alloy names leaves out the half that decides the number.

• 1
  Chip formationBrittle chips break and clear; gummy chips wrap the tool and raise temperature.
• 2
  Thermal conductivityHigh conductivity cools the edge but moves heat into the workpiece.
• 3
  Work hardeningAustenitic stainless and titanium harden under a rubbing tool.
• 4
  AbrasionHard second phases wear the edge and shorten tool life.

Aluminum is the default for machined prototypes and enclosures because it cuts fast and holds tight tolerance without drama. 6061-T6 covers most brackets, housings and fixture plates. It welds, anodizes predictably and takes Ra 0.8–1.6 μm off a normal finishing pass. If your part needs stiffness more than weight savings, 7075-T6 gives roughly twice the yield strength and machines nearly as well.

2024 is stronger in fatigue but contains copper, which makes it less corrosion resistant and harder to anodize for appearance. Use it where fatigue life drives the design and you can specify a protective coating. 5052 and 5083 are the forming grades, chosen for sheet parts that get bent; they machine softer and tend to leave a torn edge on a sheared face.

ADC12 is a die casting alloy, not a wrought one. It appears in our list because we also run die casting, but its porosity and silicon content make it a poor choice for tight-tolerance machined features. If a part is cast then machined, expect to leave 0.5–1.0 mm of stock and accept the surface the casting provides.

One practical note on temper. T6 gives the strength everyone quotes, but if a part will be bent after machining, a T4 or O condition bends without cracking. Specify the temper on the drawing, not just the alloy.

• 1
  6061-T6General purpose: brackets, plates, housings, prototypes.
• 2
  7075-T6High strength, aerospace and racing components.
• 3
  2024Fatigue-critical parts; needs corrosion protection.
• 4
  5052 / 5083Formed sheet, low-strength panels and covers.

Free-machining 303 is the easy stainless. Sulfur additions break the chip and it turns and mills like a mild steel, which is why it shows up in shafts, fittings and bushings. The trade-off is corrosion resistance and weldability: 303 does not weld well and it is not the grade for a marine or medical environment.

304 and 316 are the corrosion grades. They work-harden, so your finishing pass has to cut under the hardened layer, not rub on it. Keep radial engagement high enough to stay in the cut and never let the tool dwell. 17-4PH (SUS630) is a precipitation-hardening stainless that can be machined in the solution-treated condition and then aged to high strength; it is common in medical and aerospace work where both corrosion resistance and strength matter.

Carbon and alloy steels follow the hardness rule. 1018 and 1045 are straightforward. 4140 and 4340 at higher hardness need carbide and a rigid setup; pre-hardened 4140 around 30 HRC is still routine for us, but above roughly 40 HRC you should expect slower cycle times and shorter tool life, and the part may need grinding after heat treatment.

Tool steel is the extreme case. If the final hardness is above 50 HRC, plan for the part to be machined soft, heat treated, then finished by grinding or EDM. Machining the hardened part directly is possible but rarely economical.

• 1
  303Shafts, bushings, fittings; not for welding.
• 2
  304 / 316LCorrosion resistance; expect work hardening.
• 3
  17-4PHAge-hardening stainless for medical and aerospace.
• 4
  4140 / 4340High-load parts; slow down above 40 HRC.

Titanium TC4 (Ti-6Al-4V) has a low thermal conductivity, so heat stays in the cut instead of leaving with the chip. Use sharp tools, generous coolant and moderate surface speed; a worn edge rubs and hardens the surface. TA1 and TA2 are commercially pure grades, softer and easier to machine, used where corrosion resistance matters more than strength.

Copper and brass machine easily but move. C36000 free-cutting brass gives short chips and good finish. C101 and C110 copper are gummy and need sharp tools and high rake. Beryllium copper machines well and conducts heat, but the dust requires controlled handling, so tell us if the part is beryllium copper before we plan the operation.

Engineering plastics behave differently from metal. POM and PA hold tolerance well and cut cleanly. PEEK keeps stiffness at high temperature but is abrasive and expensive, so tool wear shows up in the cost. ABS and PC machine easily but have low stiffness, which means thin walls deflect from clamping pressure, not from the cutter.

Carbon fibre reinforced plastic is the awkward one. It is abrasive, the dust is a health hazard, and delamination can start at a drilled hole. Plan for diamond-coated tooling and sealed edges.

• 1
  TC4Heat stays in the cut; use sharp edges and coolant.
• 2
  C36000Free-cutting brass, short chips, good finish.
• 3
  PEEKAbrasive and costly; wear shows in cycle time.
• 4
  Carbon fibreDiamond tooling; delamination risk at holes.

Thin walls are the most common reason a material choice gets reconsidered. Aluminum at 1.0 mm wall thickness deflects under clamping and cutting force, so the part springs back and the dimension drifts. A stiffer material or a change to the setup can fix it, but a softer material usually makes it worse.

Deep pockets and long tools are the second constraint. A tool with a 4:1 length-to-diameter ratio is stable; at 8:1 you should expect chatter and reduced depth of cut. If the material is also gummy, chatter marks get worse because the chip does not clear. This is where a five-axis setup earns its cost, since a rotary table lets the tool reach the feature from a better angle instead of hanging out of the holder.

Holes are worth planning separately. Deep holes in stainless and titanium need peck cycles and good chip evacuation. A 10 mm hole through 60 mm of 316L is a different job from the same hole in 6061.

Finally, surface finish drives material as much as shape. Ra 0.2–0.8 μm is achievable on aluminum and brass with a fine finishing pass. On soft plastics the same target may require polishing after machining.

• 1
  Thin wallsBelow 1 mm in aluminum, expect deflection and setup changes.
• 2
  Deep pocketsAbove 4:1 tool ratio, reduce depth of cut.
• 3
  Deep holesStainless and titanium need peck cycles.
• 4
  FinishRa 0.2–0.8 μm is routine on aluminum, harder on plastics.