Aluminum CNC machining: an accurate solution

Aluminum is soft, light and cuts fast, which is why so much CNC work lands on it. That same softness is the problem. A free-machining alloy like 6061-T6 holds a wall thickness well and finishes clean. A gummy alloy like 5052 will push away from the cutter, smear at the edge and spring back after the vise opens. The drawing may allow the same tolerance for both, but only one of them will repeat it across 500 parts.

Pick the alloy for the feature, not for the price list. If you have thin ribs, deep pockets or a flatness callout under 0.05 mm, 6061-T6 or 6082-T6 gives you the best chance. If you need wear resistance, 7075 machines to a good finish but moves more after heat treat, so leave stock and plan a second op. 2024 cuts clean and is strong, yet it corrodes without anodizing or primer.

Small changes in silicon and copper content swing the chip formation. That is why two blocks of the same series can behave differently. Tell us the temper and the supplier if the part is thin. We will run a test cut before the full batch.

Most shops can hit ±0.05 mm all day. The hard part starts around ±0.01 mm. Below that, the machine is rarely the limit. The setup is. A part held in a vise on two parallels will bow when the jaws tighten. A thin floor will lift in the middle. A deep pocket will chatter and leave a taper.

Five-axis work removes some of this because the tool reaches the feature in one setup. On a 16-station five-axis cell, we can cut five faces plus a compound angle without re-clamping. Every re-clamp adds position error, so fewer setups means tighter results. That matters most on parts with holes that must line up across two sides.

Thermal drift is the quiet one. Aluminum expands roughly 23 μm per meter per °C. A 3,000 mm rail that warms 5 °C between roughing and finishing grows about 0.35 mm before the cutter touches it. On a ±0.005 mm callout, that is the whole budget. We rough in the morning, let the part rest, then finish after the temperature settles.

Tool runout and cutter wear also count. A 6 mm end mill with 0.02 mm runout will cut a slot 0.04 mm wide. Change the collet, not the program. We log tool life per material and replace before the finish pass, not after a bad reading.

A machined part is the right answer for prototypes, low volume, tight tolerance and features that cannot be molded. It is the wrong answer when the part is a simple shell with no critical dimension. Deep-drawn sheet or die casting will cost less at 20,000 pieces and hold the tolerance the drawing actually needs.

Very thin, large panels are another mismatch. A 1,500 mm cover with a 0.5 mm wall will chatter and distort no matter how it is clamped. Rolled or formed sheet keeps its shape. Machining it just adds cost and stress.

High-volume simple brackets are a third case. If the tolerance is ±0.2 mm and the shape is flat, stamping wins. Send the drawing anyway. We will tell you when another process is cheaper, because a bad fit costs more than a lost order.

For the rest, aluminum remains the practical choice. It cuts three to four times faster than stainless, tool wear is low, and the chip is easy to clear. That speed is what makes accurate aluminum CNC machining affordable at prototype quantity.

The common grades split into three groups. 6061-T6 and 6082-T6 are the general-purpose picks: good strength, clean chips, stable after machining. 7075-T6 is stronger but moves more and is harder on tools. 2024-T4 cuts well and is used in aerospace, but needs coating for corrosion.

Casting alloys such as ADC12 are for die casting, not for hogging out of plate. If you need a machined casting, tell us and we will quote the casting plus the finish passes, because the skin is harder than the core.

Anodizing adds 5–25 μm per surface depending on type. That changes a fit. If a bore must stay at Ø10.000 mm after hardcoat, machine it undersize and let the coating bring it back. We mark those dimensions on the traveler so the operator does not miss them.

Bead blasting and tumbling round edges and remove tool marks. They do not fix a tolerance. Keep finish and tolerance as separate requirements on the drawing. When both sit on the same callout, the shop has to guess which one you care about.