CNC Aluminum Parts Machining: How Aluminum Behaves on a Machine

• 1
  Why aluminum machines fast, and where the process slows down
• 2
  Choosing an alloy before the drawing is released
• 3
  3-axis, 4-axis, or 5-axis: picking the right setup
• 4
  What ±0.005 mm really costs on an aluminum part
• 5
  Wall thickness, radii, and features that cut cleanly
• 6
  Matching alloy and setup to the part

Aluminum cuts at high surface speed because it is soft and carries heat away from the edge quickly. On a 6061-T6 block, a 12 mm carbide end mill can run at 300–500 m/min surface speed and 0.1–0.2 mm per tooth feed. Chips evacuate well with air blast or through-spindle coolant, so cycle times stay short and tool life is long.

The catch is built-up edge. Pure aluminum galls and welds to the cutting edge under light feed, which smears the surface and shifts dimensions. Higher silicon grades such as ADC12 and castings with hard inclusions wear tools faster. Both problems are solved with the right coating and a feed rate that keeps the edge cutting rather than rubbing.

Thermal expansion matters more than most shops admit. Aluminum grows about 23 μm per meter per degree Celsius. A part held at ±0.005 mm over 300 mm needs roughly ±0.7 °C of temperature control between roughing and final inspection, or the measurement means nothing. We rough, rest, then finish on the same setup where the geometry allows it.

Thin walls behave differently again. Below 1 mm wall thickness, cutting force deflects the part away from the cutter, and the finished wall springs back oversize or chatters. The fix is usually support, not a slower spindle. Leave a web, machine in two passes, or move the part to a fixture that backs the wall.

• 1
  Good chip evacuationAir blast or through-coolant keeps 6061 running at 300–500 m/min.
• 2
  Built-up edgeLight feed on soft alloy smears the surface; increase feed per tooth.
• 3
  Thermal drift23 μm per meter per °C; control shop temperature on tight parts.

Most machined aluminum parts ship in 6061-T6. It welds, anodizes cleanly, holds tolerance well, and costs less than the high-strength grades. If the drawing does not name an alloy, this is the default we quote. Yield strength sits around 275 MPa, which covers brackets, housings, and most fixture work.

7075-T6 is the choice when strength per weight matters. Yield strength reaches roughly 505 MPa, close to some steels, so aerospace ribs and racing components use it. It machines well but does not weld with practical results and anodizes to a darker, less uniform color. It also costs more and takes longer to source.

2024-T351 has good fatigue resistance and is common in aircraft structure, though its corrosion resistance is poor without cladding or coating. 5052 and 5083 are marine and sheet-friendly grades with excellent corrosion resistance but lower strength. 6082 sits close to 6061 and is common in Europe.

Cast alloys such as ADC12 are for die-cast blanks that get finish-machined. They contain silicon and porosity, so expect more tool wear and a slightly rougher as-machined surface. Fine finishes on castings need a light skim cut after the skin is removed.

• 1
  6061-T6Default for housings, brackets, and general machined parts.
• 2
  7075-T6High strength, aerospace and racing; no practical welding.
• 3
  5052 / 5083Best corrosion resistance, lower strength, sheet work.
• 4
  ADC12Die-cast blanks; more tool wear, rougher surface.

A 3-axis mill cuts from one direction. It is the cheapest and fastest option when every feature is reachable from the top, or when the part can be flipped onto a second setup. Flat plates, pockets, and drilled hole patterns rarely need more.

A 4-axis mill adds a rotary table, so the part indexes around one axis. This suits cylindrical parts with cross-drilled holes, or long parts with features on several faces. One setup replaces three, which cuts position error between operations.

A 5-axis center tilts the tool or the table, so undercuts, angled faces, and deep cavities are cut in a single setup. The benefit is not speed. It is that every feature shares one datum, so hole-to-hole position stays consistent. Complex housings and impellers are the usual candidates.

The limit is stiffness. A tilted tool has less support than an upright one, so deep pockets at steep angles chatter. We keep tool length short, use a stub or reduced-neck cutter, and accept a slightly lower material removal rate. If the geometry allows, a 3-axis rough followed by a 5-axis finish often beats a full 5-axis cycle.

• 1
  3-axisCheapest and fastest when all features face one way.
• 2
  4-axisRotary indexing for cross holes and multi-face parts.
• 3
  5-axisUndercuts and angled faces in one setup, one datum.

Tolerance drives cycle time, inspection time, and scrap rate. General machined features hold ±0.1 mm comfortably. Tighten to ±0.05 mm and we add in-process checks. At ±0.005 mm, the part needs temperature-controlled finishing, a dedicated fixture, and full inspection before shipment.

Not every dimension needs the same tolerance. A common mistake is a title block calling out ±0.01 mm on a drawing where the only critical dimension is a bearing bore. Restricting the tight tolerance to the three or four features that matter keeps cost down without affecting function.

Surface finish is separate from dimensional tolerance. As-machined aluminum lands around Ra 1.6–3.2 μm. A high-quality finish reaches Ra 0.8–1.6 μm, and a fine finish with a polished cutter and light finishing pass reaches Ra 0.2–0.8 μm. Finer than that usually means a secondary process, not a cutting change.

Anodizing changes dimensions. Type II clear anodizing grows roughly 5–10 μm per surface, hardcoat can add more than 25 μm. Threads and bores that mate with other parts need masking or a pre-machined allowance, otherwise the assembly binds.

• 1
  Tolerance drives cost±0.1 mm general, ±0.005 mm needs temperature control.
• 2
  Call out only what mattersTight tolerance on three features, not the whole drawing.
• 3
  Anodizing grows the part5–10 μm Type II, over 25 μm hardcoat; mask threads.

Aluminum deflects under cutting load, so wall thickness sets the floor on what is practical. Walls of 1.5 mm and thicker machine reliably. Between 1 mm and 1.5 mm, support and a lighter finishing pass keep the part in tolerance. Below 1 mm, expect chatter and distortion unless the geometry is short and well supported.

Internal corners need a radius at least as large as the cutter. A 6 mm end mill leaves a 3 mm corner radius. If the drawing calls for a sharp internal corner, the shop has to burn it with EDM or leave it oversized. Adding corner radii to the model saves a process and money.

Threads below M2 and holes below 1 mm diameter are possible but fragile. Deep holes need a length-to-diameter ratio under 10:1 for reliable drilling on aluminum, and deep pockets need clearance for the cutter shank, not just the tip. Check that the tool can reach the floor without rubbing the wall.

Sharp external edges are a handling risk and a finishing problem. A 0.3–0.5 mm chamfer or edge break removes burrs, protects the anodized layer, and gives the part a cleaner look. It also reduces the chance of a nick during packing.

• 1
  Wall thickness1.5 mm and up is reliable; under 1 mm needs support.
• 2
  Corner radiusMatch or exceed the cutter radius, typically 3 mm.
• 3
  Edge break0.3–0.5 mm chamfer removes burrs and protects coating.