Aluminum Plate CNC Processing: Step-by-Step Guide

The choice of alloy comes before the toolpath. 6061-T6 is the default for brackets, housings, manifolds and fixture plates because it machines cleanly, welds, anodizes, and holds a stable price. Its yield strength sits near 276 MPa, which is enough for most structural work but not for highly loaded airframe parts.

6082-T6 behaves close to 6061 with slightly higher strength and better corrosion resistance. It is common on European drawings and works well for load-bearing frames and transport hardware. 7075-T6 reaches roughly 503 MPa yield, so it suits high-stress parts such as wing fittings and racing suspension arms where weight matters more than cost.

Temperature matters as much as grade. T6 plate arrives stress-relieved from the mill, but sawing and heavy roughing still release internal stress. A 7075 plate cut from the center of a thick billet can move 0.2 mm or more after the first pass. If your part has a flatness callout under 0.1 mm, plan a stress-relief step or choose a cast tooling plate instead.

• 1
  6061-T6General machining, anodizing, moderate loads. Best cost-to-strength balance.
• 2
  6082-T6Slightly stronger than 6061, good corrosion resistance, common in EU drawings.
• 3
  7075-T6High strength, poor weldability, higher cost. Use where weight is critical.
• 4
  Cast tooling plateLow internal stress, good for large flat fixture plates and vacuum tables.

Plate thickness is normally bought 1–3 mm oversize on each face. That allowance absorbs saw marks, surface bow and the material removed during the first facing cut. Cutting a 20 mm finished part from 20 mm stock leaves no room to clean up both faces, and it forces the operator to chase a bowed surface across the whole program.

Fixturing decides whether the part stays accurate under load. A thin 300 × 300 mm plate clamped only at the corners will lift in the middle as the cutter pushes down. We use vacuum chucks for flat plates above roughly 200 mm, soft jaws for small parts, and a Ø400 mm rotary table when features sit on multiple faces.

For long parts we work inside a 4,000 × 400 × 150 mm travel envelope. Anything longer than that needs a different setup, usually a spliced design or a weldment. Bring that up early, because a redesign after the first article is expensive.

Roughing removes 60–80% of the stock with a large-diameter end mill. Depth of cut and feed are set high enough to keep the tool cutting rather than rubbing, which is the main cause of built-up edge on aluminum. We leave 0.3–0.5 mm of radial stock for the finishing passes.

Semi-finishing brings walls and pockets close to size. Thin walls below 2 mm are the hard case: cutting force pushes them away from the tool, so the wall springs back after the pass and finishes oversize. The fix is to leave more stock, take lighter radial cuts, and support the wall with a sacrificial rib where the geometry allows.

Finishing sets the final dimension and surface. A sharp, polished carbide cutter at high spindle speed gives Ra 0.8–1.6 μm on 6061 without any secondary operation. Tighter face tolerances, down to ±0.005 mm on a well-supported part, are possible but they need temperature control and a stable setup, so reserve them for the features that actually need it.

Holes are drilled after the main faces are true, not before. That way the hole axis references a machined surface instead of a rough saw cut. For a pattern that must match a mating part, drill and ream in the same setup, or use a boring head if the position tolerance is tight.

Threads in aluminum pull out easily. A 6 mm thread in 6061 needs at least 1.5× diameter of engagement, so roughly 9 mm of full thread. Deeper than 2.5× diameter adds little strength and raises the risk of a broken tap. Rolled threads are stronger than cut threads in this material and leave no chips in the hole.

Features on a second or third face are where 5-axis work pays off. One setup on a simultaneous 5-axis center avoids re-datuming the part four times, which removes both the handling time and the stacked positional error. On a simple plate with one face of work, a 3-axis machine is faster and cheaper.

A machined plate is never finished when the spindle stops. Burrs on edges, hole rims and pocket floors have to come off before anodizing, or the coating builds over them and the edge looks uneven. Bead blasting, tumbling and hand deburring are all in scope, and the choice depends on whether you want a uniform matte look or a crisp machined edge.

If the part needs color, hardcoat or a conductive coating, say so at quote time. Anodizing adds roughly 0.005–0.025 mm of build-up per surface, which matters on a close-tolerance bore. Hardcoat is thicker and harder, and it can change a sliding fit. Masking is possible but adds labor.

Inspection runs alongside production, not only at the end. We check incoming plate for grade and flatness, monitor critical dimensions during the run, and inspect 100% of parts before shipment. Reports with measured values are available on request. For a first article, ask for a dimensional report against the drawing's datum scheme.

• 1
  Deburr before coatingBurrs trapped under anodize leave visible ridges and uneven color.
• 2
  Anodize build-up0.005–0.025 mm per surface. Account for it on tight bores.
• 3
  Laser markingMinimum character height 1.5 mm for a legible mark.
• 4
  First articleRequest a dimensional report against the drawing datums.

Not every aluminum part should start as plate. If the geometry is a thin shell with uniform wall, deep ribs and no tight tolerance, die casting or vacuum casting will be cheaper at volume. Plate machining wins when quantities are low, when the part is large, or when the design is still changing.

A part that removes more than about 70% of the billet as chips is usually a casting or forging candidate. The machining time and material cost both scale with that removed volume, and neither drops much at higher quantities. It is worth a cost comparison before committing to a 10,000-piece plate order.

Sheet metal is another alternative for flat parts under roughly 3 mm thick with simple bends. If the part is a flat bracket with a few holes, laser cutting plus forming beats milling on both price and lead time. Plate CNC processing makes sense once you need thickness, pockets, or tolerances that forming cannot hold.