CNC aluminum milling essentials
Aluminum cuts fast and looks simple on paper. The hard part is holding tolerance across a full batch. This page covers the machining behavior that decides whether your part comes back at ±0.005 mm or drifts out of spec. Written for design engineers and sourcing teams who need to judge a milling quote, not just accept it.
In this article
- 1
- 2
- 3
- 4
- 5
- 6
CNC aluminum milling essentials start with the alloy
Aluminum is not one material. 6061-T6 machines cleanly and holds a good surface, which is why it carries most bracket, plate and housing work. 7075 is roughly twice the strength but grabs the tool and chips less predictably. 2024 machines well yet corrodes faster without protection. The alloy you pick sets the tool, the speed and the fixture before anyone writes a program.
Silicon content matters more than most drawings admit. ADC12 die-cast stock runs abrasive, so carbide tools wear on the flank and finish dulls after a few hundred parts. Wrought grades like 6082 and 6063 cut freely. Tell the shop which grade you intend, or ask for a substitution note. A swap from 6061 to 7075 changes feed rates, tool life and sometimes the fixture entirely.
Temper also moves the result. 6061-T6 is stable and predictable. Annealed 6061 machines gummier, produces long stringy chips and tends to smear on light finishing passes. If a part needs both strength and a fine surface, rough it in T6 and leave 0.3–0.5 mm for a finishing pass rather than cutting the whole part in one go.
Heat treatment after milling is a separate risk. Thin walls relax when the part goes through solution treatment and aging, and flatness can move 0.1 mm or more. Where flatness matters, rough machine, stress relieve, then finish. That sequence costs a day but saves a scrapped batch.
Tool geometry and coating decide chip evacuation
Aluminum is soft, sticky and a good conductor of heat. A sharp edge with high rake lifts the chip instead of rubbing it. Two-flute and three-flute end mills in uncoated or ZrN-coated carbide work for most pockets because they clear chips quickly. Four flutes and above raise cutting forces on deep walls where the tool has little support.
Helix angle is the trade-off. A 45° helix pulls chips out of a deep slot but adds axial force. A 30° helix is steadier for finishing vertical walls. For thin floors, drop to a smaller step-down and a shorter flute length rather than pushing the same tool harder.
Coating is not automatically better. TiAlN and AlTiN run hot and suit steel; on aluminum they can encourage built-up edge on softer tempers. Polished uncoated carbide and diamond-like coatings work better on high-silicon stock. Ask what the shop runs before assuming a premium coating helps.
Chip evacuation is where most aluminum milling jobs fail quietly. Recutting a chip doubles the load on the edge and leaves marks on the wall. Air blast plus through-spindle coolant beats flood alone on deep cavities. If a tool sounds like it is grinding rather than cutting, the chips are staying in the cut.
Speeds, feeds and radial engagement in practice
Aluminum tolerates high surface speed. A 10 mm carbide end mill commonly runs 300–500 m/min in 6061, which puts spindle speed well above 10,000 rpm on smaller tools. The limit is usually the machine, not the material. Rigid spindles hold that speed; light benchtop spindles do not.
Feed per tooth is where surface finish is won or lost. A 0.05–0.12 mm chip load per tooth gives a clean cut in 6061. Too light a chip load rubs the edge and work-hardens the surface, and the next pass cuts through a harder skin. That is the usual cause of a finish that looks torn on a light spring pass.
Radial engagement controls tool life more than speed does. Trochoidal paths that keep radial engagement near 10–15% of the cutter diameter let you run deeper axial cuts without stalling. The same part with a 50% radial step-down heats the tool and forces slower feed.
Axial depth follows the tool. A cutter with a 3× diameter length of cut can take 1× diameter axial depth at reduced radial engagement. Push past 4× and chatter appears, especially in thin webs. When in doubt, reduce radial engagement first and keep the chipload steady.
Workholding, setup count and tolerance stack-up
Every additional setup adds error. A part machined on three sides needs three datum transfers, and each transfer can move the zero by 0.01 mm or more. Five-axis machining keeps more features in one setup, which is why complex housings often come off a five-axis center at tighter tolerance than the same part run on three separate three-axis operations.
Thin walls deflect under cutting force. A 1 mm wall in 6061 will push away from a 10 mm cutter unless the part is supported. Options include leaving sacrificial ribs, backing the wall with machinable wax, or cutting both sides of the wall in a finishing pass with light radial engagement. Support is cheaper than a scrapped part.
Vacuum fixtures and soft jaws suit plate work. For high-volume runs, a dedicated fixture with hardened locating pins holds repeatability better than clamps that move with torque. Where a part needs flatness under 0.05 mm, check that the fixture does not warp the blank when clamped.
Setup also affects lead time. A part that needs four setups and custom fixturing takes longer to first article than a part that fits a standard vise. If you have flexibility on geometry, a design that can be machined from two sides often cuts both cost and risk.
Surface finish, deburring and inspection choices
As-machined aluminum sits around Ra 1.6–3.2 μm. A controlled finishing pass with a sharp tool, steady chipload and good coolant reaches Ra 0.8–1.6 μm, and a light polishing pass can push toward Ra 0.2–0.8 μm on flat and cylindrical faces. Deeper pockets and complex 3D surfaces are harder to bring down uniformly.
Deburring is not cosmetic. A 0.1 mm burr on a mating face becomes a gap or a stress riser. Hand deburring works for prototypes; vibratory tumbling and abrasive flow suit production runs where every edge needs the same treatment. Specify which edges matter and which can stay sharp.
Anodizing changes dimensions. Type II clear anodizing typically adds 5–10 μm per surface, and hardcoat can add 25–50 μm. On a ±0.005 mm bore that matters. Mask critical diameters or plan the pre-anodize size so the finished part lands in tolerance.
Inspection closes the loop. CMM reports on critical features, plus a first article report, show whether the process held. For aluminum parts with tight flatness or true position, ask for the report before the run ships. GreatLight inspects 100% of parts before shipment and can supply reports on request.
When each aluminum milling approach fits
Match the part to the process before you request a quote.
| Situation | Recommended approach | Watch out for |
|---|---|---|
| Simple plate, 2 sides, ±0.05 mm | 3-axis mill, soft jaws | Setup drift on re-clamp |
| Housing with 4+ faces | 5-axis, one setup | Fixture access to all faces |
| Thin wall under 1.5 mm | Light radial pass, extra support | Wall deflection and chatter |
| High-silicon ADC12 stock | Polished carbide, slower speed | Flank wear and dull finish |
| Bore needing anodize | Mask or pre-size for coating | 5–50 μm growth per surface |
| 10,000+ part run | Dedicated fixture, hard stops | Fixture wear over time |
Pick the process, then the tolerance
If the part is mostly flat with a few pockets, a 3-axis setup in 6061-T6 is the cheaper, faster route. If it has features on four or more faces, tight bores or thin walls, put it on a five-axis center in one setup and accept the higher hourly rate. Choose the setup count first; tolerance and finish follow from it.
Common questions on aluminum milling
What tolerance can aluminum milling realistically hold?
On a rigid machine with a controlled setup, ±0.005 mm is achievable on critical features such as bores and mating faces. General dimensions across a part often sit at ±0.02 to ±0.05 mm because thermal movement and setup transfer add up.
Tighter than ±0.005 mm needs temperature control, in-process probing and a part that is stiff enough not to move when it is unclamped.
Is 6061 or 7075 better for milling?
6061-T6 is the default. It machines cleanly, welds, anodizes well and costs less. Choose 7075 when you need yield strength near 500 MPa or better fatigue performance.
7075 is less forgiving. It chips harder, wears tools faster and is more prone to stress corrosion. If the part does not need the strength, 6061 will usually give a better surface and a lower price.
Why does my aluminum part come back with a torn surface?
Torn or smeared surfaces usually mean the chip load is too light on the finishing pass, so the edge rubs instead of cutting. Built-up edge on the tool does the same thing.
Check feed per tooth first, then the coating. On softer tempers, a polished uncoated tool often leaves a better finish than a coated one running too slowly.
How much does anodizing change a dimension?
Type II clear anodizing adds roughly 5–10 μm per surface. Hardcoat can add 25–50 μm and is less uniform on sharp edges and inside corners.
On a bore with a ±0.005 mm tolerance, specify masking or size the pre-anodize diameter smaller. State the finished requirement on the drawing so the shop can plan the sequence.
When should a part move from 3-axis to 5-axis?
Move when features sit on four or more faces, when the part is too large or awkward to re-fixture, or when tolerance stack-up across multiple setups is the main risk.
Five-axis has a higher hourly rate but removes setups. On complex housings, the total cost is often lower because fixturing and re-datum time disappear.
Can thin aluminum walls be milled without distortion?
Yes, with support. Leave sacrificial ribs, back the wall with machinable wax or take light radial finishing passes on both sides of the wall.
A wall under 1 mm in 6061 will still deflect under normal cutting force. Design flexibility on wall thickness saves more cost than any tooling trick.
Send the drawing, get a milling plan
We review your aluminum part, flag the setup and tolerance risks, and return a quote with free DFM analysis within 12 hours.
12-hour quote100% inspectionNo minimum order
More machining notes
We publish setup notes, tooling trials and inspection data from the factory floor.
