UK CNC Aluminum Processing Guide

• 1
  Why aluminum behaves differently at the spindle
• 2
  Alloy grades and what each one buys you
• 3
  Tooling, speeds, and the numbers that hold tolerance
• 4
  Fixturing and how parts actually move
• 5
  Finishes and what they change about the part
• 6
  When CNC aluminum processing is the wrong choice
• 7
  What drives cost in a UK CNC aluminum processing quote
• 8
  How to brief a shop so the first part is right
• 9
  Aluminum grade selection at a glance

Aluminum cuts fast. That is the whole attraction and the whole problem. A 6061 block will take a 10 mm depth of cut at 12,000 rpm without blinking, while the same cutter in 304 stainless would fail in seconds. The material removes heat quickly, so chips carry most of the thermal load away from the part.

The flip side is that aluminum is soft and springy. Young's modulus sits around 69 GPa, roughly a third of steel, so thin walls deflect under cutting force instead of resisting it. A wall under 1 mm on a 6061 bracket will move during roughing and spring back after the tool passes. The finished dimension then drifts.

Built-up edge is the second trap. Aluminum galls on the cutting edge at low surface speed, so the tool starts smearing instead of shearing. The result is a torn surface and a size that wanders. Sharp, polished carbide and cutting fluid solve most of it. So does running faster than instinct suggests.

This is the baseline for any UK CNC aluminum processing decision. If you understand heat path, stiffness, and chip evacuation, the rest of the choices follow. Alloy, tool, fixture, and finish are consequences of those three.

• 1
  Heat goes into the chipDry or near-dry cutting works when the tool and speed are right.
• 2
  Stiffness sets wall limitsThin walls need support, not more passes.
• 3
  Built-up edge kills finishRa climbs fast once the edge starts smearing.

Most aluminum parts land on 6061-T6. It welds, anodizes, machines cleanly, and holds ±0.005 mm on a stable setup. If a drawing says "aluminum, no further spec", that is what you should quote. 6082 is the European near-equivalent and is common in UK supply chains; it has slightly higher strength and similar machining behavior.

2024 machines beautifully and takes a better finish than 6061, but its copper content makes it corrode in damp air. It is a controlled-material grade, usually for aerospace. If you do not have a corrosion allowance or a coating step planned, 2024 is the wrong pick.

7075 is the strong one, around 500 MPa yield in T6. It also machines well, but it costs more and it does not weld. Use it when the part is a stressed bracket, a jig, or a thin ribbed structure where 6061 would bend. For a simple enclosure, the extra strength does nothing.

5052 and 5083 are the formable marine grades. They bend and resist salt water, but they are gummy at the spindle and hard to hold to tight tolerance. If the part is a bent panel, they win on the press brake. If it is a milled block, they lose. Material choice and process choice are the same decision.

• 1
  6061-T6Default for milled and turned parts; anodizes well.
• 2
  6082-T6Common in the UK; close to 6061 in behavior.
• 3
  7075-T6High strength for stressed, thin-walled parts.
• 4
  5052 / 5083Formable and corrosion-resistant, gummy to mill.

Aluminum is cut with two or three flute carbide end mills, polished and usually uncoated. Coatings help on 7075 and on long runs, but a thick AlTiN layer can dull the edge radius and encourage built-up edge on soft stock. High helix angles of 40 to 45 degrees clear chips faster and reduce recutting.

Surface speed for 6061 sits between 300 and 600 m/min with carbide. Feed per tooth runs 0.05 to 0.15 mm depending on cutter diameter. For a 10 mm three-flute tool, a spindle of 12,000 to 16,000 rpm and a feed of 2,000 to 4,000 mm/min is a normal roughing window. Flood coolant or high-pressure air both work; the choice is chip evacuation, not cooling.

Tolerance is where the machine and the setup matter more than the alloy. Our 5-axis centers hold ±0.005 mm on features that are reachable in one setup. Move a feature to a second operation and datum shift eats part of that budget. Design for one setup where you can.

Finish values are predictable. As-machined aluminum lands at Ra 1.6–3.2 μm. A finer stepover and a sharp tool reach Ra 0.8–1.6 μm. Below Ra 0.8 μm you are polishing, not cutting, and the cost curve bends upward.

• 1
  2–3 flute carbidePolished, 40–45° helix for chip clearance.
• 2
  300–600 m/minSurface speed window for 6061-T6.
• 3
  One setup, one datumKeeps ±0.005 mm achievable.
• 4
  Ra 0.8–1.6 μmReachable with a fine stepover, no polishing.

A part is only as accurate as the fixture holding it. Aluminum's low stiffness means cutting force pushes the workpiece away from the tool, and the workpiece pushes back when the tool leaves. On a thin rib that movement can be 0.05 mm or more, which is ten times the tolerance we quote.

The fix is support, not patience. Add sacrificial tabs, use a soft jaw machined to the part profile, or leave a thick web that gets removed in a finishing pass. Vacuum chucks work for flat plates. Low-melt fixturing wax works for awkward thin sections. Both keep the part still while the tool works.

Thermal drift is the quieter problem. A 500 mm aluminum plate grows about 0.012 mm per degree Celsius. If the shop warms up ten degrees between roughing and finishing, the part moves more than the tolerance. Rough in the morning, finish after the machine has settled, and measure at 20 °C.

For UK buyers sending work overseas, this is the part that gets lost in translation. Ask how the part is held, not just what machine cuts it. The fixture answer tells you whether ±0.005 mm is real or a number on a datasheet.

• 1
  Soft jaws and tabsSupport thin walls instead of chasing them.
• 2
  Vacuum and waxGood for flat plates and thin sections.
• 3
  Warm-up matters0.012 mm per 500 mm per °C on aluminum.

Anodizing is the default finish on machined aluminum. Type II clear adds 5 to 25 μm per surface and builds outward, so a Ø10.00 mm shaft becomes Ø10.01 to Ø10.05 mm after coating. If the drawing has a tight bore, mask it or specify the pre-anodize dimension. Hardcoat Type III is thicker and harder, and it builds more.

Colour anodizing and hardcoat both change dimensions. Conductive anodizing keeps the surface electrically live, which matters for chassis and grounding plates. Electroless nickel adds a uniform layer and holds tight tolerance better than anodize, but it changes the colour to a dull grey.

Bead blasting gives a matte, uniform look and hides tool marks. It also rounds edges slightly, so a sharp cosmetic edge should be specified before blasting, not after. Brushing leaves a directional grain and is common on front panels. Polishing reaches the lowest Ra but is a manual step and costs accordingly.

Laser marking is the last step, and minimum character height is 1.5 mm. Anything smaller fills in or becomes unreadable, especially on a blasted surface. Plan the marking on the drawing before the finish, not after.

• 1
  Type II anodizeBuilds 5–25 μm per surface; mask tight bores.
• 2
  Hardcoat Type IIIHarder and thicker; more dimensional shift.
• 3
  Electroless nickelUniform layer, good for tight tolerance.
• 4
  Laser markingMinimum 1.5 mm character height.

CNC wins on tolerance, material properties, and one-off geometry. It loses on hollow internal volumes, on parts with complex internal cooling channels, and on very large thin shells. If the geometry is a lattice or an internal manifold, no cutter reaches it.

Die casting makes sense above roughly 5,000 identical parts where wall thickness is 2 mm or more and tolerance can sit at ±0.1 mm. Tooling cost is the barrier, not the piece price. Below that volume, the amortization never works.

3D printing in aluminum is viable for prototypes and for geometries that cannot be machined, but surface finish is rough and porosity varies. It is a fit for a manifold or a lightweight bracket, not for a sealing face or a bearing bore.

Sheet metal takes over when the part is a flat or bent panel under 6 mm thick. Bending and laser cutting beat milling on both cost and speed for an enclosure side. If your part is a 2 mm plate with holes and a few bends, the CNC quote will look strange because the process is wrong.

• 1
  CNC for tolerance±0.005 mm, dense material, one-off geometry.
• 2
  Casting above 5,000 partsWall ≥2 mm, tolerance ≥±0.1 mm.
• 3
  Printing for internal geometryRough finish, porosity varies.
• 4
  Sheet metal for panelsUnder 6 mm thick, flat or bent.

Material is rarely the largest line. On a 200 g 6061 part, the stock costs a few pounds. The machine time and setup dominate. A part that needs three operations on three machines costs more than a part that runs in one 5-axis setup, even if the second part uses more metal.

Setup time is the hidden multiplier. A one-off prototype pays the full setup. A run of 500 amortizes it to almost nothing. This is why the piece price drops sharply between quantity one and quantity fifty, and then flattens.

Tolerance drives cost because it drives inspection and slower cutting. Opening a bore from ±0.02 mm to ±0.05 mm can cut cycle time noticeably and reduce scrap. If a feature does not need the tight callout, loosen it. Engineers who do this get better quotes.

Finish is the third lever. Anodizing adds a per-part cost and a handling step. Bead blasting adds another. Laser marking adds another. Each is cheap on its own and expensive when stacked on a low-volume run. We quote these as separate lines so you can see the trade.

• 1
  Setup dominates at low volumeA one-off pays the full fixture and program cost.
• 2
  Tolerance is a cost leverLoosening from ±0.02 to ±0.05 mm cuts cycle time.
• 3
  Finishes stackAnodize, blast, and marking each add a step.

Send a 3D model and a 2D drawing with the critical dimensions called out. The model defines geometry. The drawing defines what matters. If only a model exists, say which bores and faces are functional, because the shop will otherwise assume everything is critical and price accordingly.

State the alloy, the finish, and the quantity. If the alloy is open, say so. If the finish is open, say so. Ambiguity at the brief stage turns into a rework conversation later.

Mark the datum. A drawing with a clear datum scheme lets the shop build one fixture and hold the tolerance. A drawing without one forces the shop to guess, and guessing is where ±0.005 mm quietly becomes ±0.05 mm.

Mention the end use. A bracket that sits inside a machine and a bracket that is the visible face of a product have different finishing priorities. That single sentence changes the quote and the result.

• 1
  Model plus drawingGeometry from the model, intent from the drawing.
• 2
  Call out critical featuresOtherwise everything gets priced as critical.
• 3
  State alloy and finishOr accept the shop's default and risk rework.
• 4
  Name the end useIt changes finish and inspection priorities.