How to Machine Aluminium on CNC

• 1
  Key takeaways
• 2
  Before the first cut: alloy and stock
• 3
  Tool selection for aluminium
• 4
  Speeds, feeds and chip load
• 5
  Workholding, coolant and finishing
• 6
  Step by step: machining an aluminium part
• 7
  Which aluminium alloy for which job

Start with the alloy, because it decides everything downstream. 6061-T6 is the workhorse for machined aluminium. It cuts cleanly, takes anodizing evenly and holds ±0.005 mm on well-supported features. 6082 is close behind and common in Europe. 2024 and 7075 are stronger but gummier and more prone to stress movement after heavy stock removal.

Use 7075 when you need high strength in a thin section, such as a bracket or a fixture body. Accept that you may need a roughing pass, a stress-relief pause, then a finishing pass. 5052 and 5083 bend and weld well but machine to a softer, stickier chip, so they suit formed parts more than tight-tolerance machined ones. ADC12 covers die-cast blanks that only need secondary machining.

Stock form changes the setup. Plate is the usual choice for flat parts and stays flattest when you remove material evenly from both faces. Extrusion is cheap for long straight parts but carries internal stress, so it can bow after the skin is cut. Castings and forgings need a first cut that removes skin without pulling the part out of shape.

Leave 0.3–0.5 mm of radial stock for finishing on most aluminium parts. On thin floors that number should drop to 0.15–0.25 mm, because a heavy finishing pass deflects the floor and leaves a visible step. If the drawing allows, remove internal pockets from both sides so the neutral axis stays near the middle of the plate.

• 1
  6061-T6 / 6082General parts, housings, brackets, heat sinks.
• 2
  2024 / 7075High-strength, thin-section, aerospace-style parts.
• 3
  5052 / 5083Formed and welded parts, marine and enclosure work.
• 4
  ADC12Die-cast blanks needing secondary machining.

Aluminium cuts fast, but it also sticks to cutting edges. That single fact drives tool choice. Use two or three flute end mills for roughing and finishing in aluminium. Three flutes give a better surface on side walls; two flutes leave more room for chip evacuation in deep pockets. Avoid four-flute tools unless the operation is light and the coolant flow is strong.

Helix angle should sit between 35 and 45 degrees. A higher helix lifts chips out of the cut and reduces recutting, which is the main cause of chatter and poor wall finish. Positive rake angles lower cutting forces, so small machines and long reach tools survive the cut. Polished flutes and an uncoated or ZrN-coated surface work well. TiAlN is a poor match for aluminium; it tends to grab the material.

Reach is a quiet killer. A tool with a 3:1 length-to-diameter ratio can be pushed hard. At 6:1, deflection becomes the limiting factor, not spindle speed. At 10:1, plan on light radial engagement and a separate finishing pass. If a deep pocket needs a long tool, rough it with the longest rigid tool that fits, then finish with a smaller stepover at reduced feed.

For drilling, use 118° or 130° point angles with polished flutes and a split point. Peck drilling is rarely needed in aluminium unless the hole is deeper than 5× diameter. For reaming and boring, single-point boring heads give straightness that a reamer cannot on interrupted cuts. Chamfer tools should be sharp; a dull chamfer tool smears aluminium instead of cutting it.

• 1
  2–3 flutes, 35–45° helixStandard geometry for aluminium milling.
• 2
  Positive rake, polished flutesLower forces, less built-up edge.
• 3
  Keep L:D under 6:1 where possibleDeflection grows fast past that ratio.

Working out how to machine aluminium on CNC starts with chip load, not spindle speed. Pick a chip per tooth first, then let the spindle and feed follow. For a 6 mm three-flute end mill in 6061, 0.05–0.08 mm per tooth is a reasonable roughing target. For a 12 mm tool, 0.10–0.15 mm per tooth. Too light a chip load rubs the edge and work-hardens the surface, which makes the next pass worse.

Surface speed for aluminium with carbide runs 300–600 m/min in roughing and 500–900 m/min in finishing. These figures assume good chip evacuation. In a deep pocket with a long tool, cut them by 30–40 percent. For high-speed-steel tooling, stay near 150–250 m/min. If the chips come off blue or the part is hot to touch, the speed is too high or the feed is too low.

Aluminium chips should look like small commas or short curls, silver and warm, not hot. Long stringy chips mean the feed is too low. Fine dust means the tool is rubbing. Dark or welded chips mean built-up edge is forming, so reduce speed or increase feed per tooth, and check the flute polish.

Radial engagement is the other lever. On a 12 mm tool, a 6 mm radial stepdown (50 percent) with a full axial depth works for rigid setups. On thin walls and long reaches, drop radial engagement to 10–25 percent and raise the feed per tooth to keep the chip thick. This is the single most useful trick when a wall starts to ring.

For finishing passes, use 0.2–0.5 mm radial stepover, full depth where the tool can take it, and a feed around 0.03–0.06 mm per tooth. That combination gives Ra 0.8–1.6 μm on side walls in 6061 without a separate polish. When the drawing calls for Ra 0.2–0.8 μm, plan a dedicated finishing pass with a fresh tool and a light spring pass.

• 1
  Chip load firstChoose mm per tooth, then set spindle and feed.
• 2
  Silver short curlsCorrect. Long strings or dust mean the numbers are wrong.
• 3
  Reduce radial, keep chip thickUse this on thin walls and long reach tools.

Aluminium is soft, so fixtures can leave marks and setups can move the part. Clamp on a surface that will be machined later, or use soft jaws and sacrificial stock. For thin plates, support the whole underside with a dedicated fixture or vacuum plate. A part that is only held at four corners will bow between them during a heavy cut and spring back when released.

Coolant choice is simple. Dry machining with a strong air blast handles most aluminium jobs and avoids the mess. Mist coolant helps on deep pockets, deep holes and anything with a long cycle time. Flood coolant is useful when the machine has good filtration and the part has many fine features. Water-based coolant should be kept at the recommended concentration; weak mix causes staining on 2024 and 7075.

Deburr as you go. Aluminium burrs are soft but stubborn, and a burr left on a mating face becomes a leak path or a seating error. Use a chamfer pass on every edge the customer touches, and hand-deburr internal cross-holes with a scraper or a rotary burr. A light bead blast hides tool marks but also rounds sharp edges, so mask edges that must stay crisp.

Finishing affects the tolerance you can promise. Anodizing builds 5–25 μm per surface depending on the process. Clear anodize is the thinnest, hardcoat the thickest. If a bore must stay within ±0.005 mm after anodizing, mask it or machine it undersize by the coating thickness and let the plater bring it back. Threads should be masked or chased after coating. Laser marking needs at least 1.5 mm character height to stay readable.

Inspection closes the loop. Check critical dimensions after the finishing operation, not before, because coating and stress relief move parts. For production runs we inspect 100 percent before shipment and can supply reports on request.

• 1
  Support the whole partVacuum plates and soft jaws beat corner clamps.
• 2
  Air blast for most jobsMist on deep features, flood when filtration allows.
• 3
  Measure after finishingAnodizing shifts fits by 5–25 μm per surface.