CNC Routing Aluminum: How the Cut Actually Works

• 1
  What Happens Where the Tool Meets the Metal
• 2
  Which Aluminum Alloys Route Well and Which Fight Back
• 3
  Routing vs Milling: When the Long Tool Wins
• 4
  Holding Thin Aluminum Without Bowing It
• 5
  What Tolerance CNC Routing Aluminum Can Actually Hold
• 6
  Router or Mill: Match the Part to the Machine

Aluminum is soft, gummy and a good conductor of heat. That combination sounds friendly, and it mostly is. A sharp carbide tool at 300 to 900 m/min surface speed will peel 6061 into a clean chip with little drama. The trouble starts when the chip does not leave. Aluminum melts at roughly 660 °C, and a chip that rubs twice against the same wall will weld itself to the edge. Once built-up edge forms, the surface tears and the tolerance walks.

The physical difference between routing and milling is the length and stiffness of the tool. A router spins a long, slender cutter over a large table. That geometry reaches across a 4,000 mm panel, but it also bends. Tool deflection rises with the cube of the stick-out length, so a cutter hanging 150 mm out of the collet is roughly 27 times softer than the same cutter at 50 mm. On aluminum that shows up as chatter marks and a wall that tapers.

Chip load per tooth is the number that matters most. For a 12 mm three-flute carbide cutter in 6061, a feed of 0.10 to 0.15 mm per tooth keeps the chip thick enough to carry heat away. Drop below 0.05 mm per tooth and the edge rubs instead of cuts. The chip gets thin, the heat stays in the part, and you get a smeared finish plus a burr that takes longer to remove than the cut itself.

Cooling matters, but not the way most people assume. Aluminum conducts heat away from the cut so quickly that flood coolant is often about chip evacuation, not temperature. A strong air blast plus a mist will clear a deep pocket better than a weak flood, because a flooded pocket fills with chips and recuts them. Re-cutting is the single most common cause of poor finish in aluminum routing.

• 1
  Keep the chip thick0.10–0.15 mm per tooth in 6061; never below 0.05 mm.
• 2
  Shorten the stick-outDeflection scales with the cube of tool length.
• 3
  Clear chips firstAir blast plus mist beats weak flood in deep pockets.

The 6xxx family is the default for routing. 6061 and 6061-T6 machine cleanly, hold a thread, weld well and anodize evenly. 6063 and 6082 behave close enough that a program written for one usually runs on the others with a small feed adjustment. If a part is mostly flat, has pockets and needs a good surface, 6061-T6 is the safe answer and usually the cheapest one.

2024 and 7075 are the high-strength choices. 7075-T6 reaches roughly 570 MPa yield, which is why it appears in aerospace brackets and racing suspension. It also cuts differently. The copper content that gives 7075 its strength makes the chip brittle and the tool wear faster. Expect shorter tool life and plan a finishing pass with a light radial depth, around 0.2 to 0.3 mm, to hit Ra 0.8–1.6 μm.

5052 and 5083 are the marine and sheet-metal grades. They bend and form well, resist salt water, and machine to a gummy finish. Routing them is possible but the surface rarely looks as good as 6061 without a finishing pass. If the drawing calls for a formed bracket in 5052, forming it first and routing the trim second usually beats routing a thick plate.

ADC12 is a die-casting alloy, not a wrought plate. It appears in routed work only when someone is machining a cast housing, and the porosity inside the casting changes everything. Interrupted cuts through a gas pocket will chip a small cutter. For castings, slower feed, a tougher carbide grade and a willingness to scrap the first part are the practical rules.

Hard-anodized or already-coated stock is a separate problem. The oxide layer is far harder than the aluminum under it, so the first pass cuts a hard skin and the second cuts soft metal. That transition chips edges. Machine the part, then anodize it, unless the drawing forces you the other way.

• 1
  6061-T6Default choice; clean chips, good anodizing, lowest risk.
• 2
  7075-T6High strength, brittle chips, shorter tool life; light finishing pass.
• 3
  5052 / 5083Formable and corrosion resistant; gummy finish without a final pass.
• 4
  ADC12Cast alloy; porosity causes interrupted cuts, so slow the feed.

A router earns its place on large, thin, flat parts. Think enclosure panels, chassis plates, heat-sink bases, drone frames, sign backs and fixture plates. When the part is longer than 1,000 mm and the wall thickness is under 6 mm, a moving gantry router with a vacuum table holds the work flat with almost no clamping distortion. A vertical mill would need tabs or a fixture that presses the part and bows it.

The second win is nesting. On a 2,500 × 1,250 mm sheet you can nest a dozen brackets and cut them from one program. That is a material and setup saving, not a precision saving. If the same brackets need a ±0.005 mm bore, route the profile and mill the bore in a second operation, or accept the router tolerance and design the bore as a clearance hole.

Milling wins on three-dimensional work. A 5-axis machining center with a Ø400 mm rotary table will cut an angled face, a contoured rib or a compound pocket in one setup. A 3-axis router cannot tilt the tool, so a drafted wall becomes a stepped wall or a separate fixture. When the part has more than two axes of contour, reach for the mill.

Rigidity is the dividing line. A router table is built to cover area; a mill is built to resist force. Deep pockets in thick plate, long overhangs and interrupted cuts all favor the mill. If you find yourself slowing the feed to stop the chatter, the machine is the wrong one for that feature, not the program.

• 1
  Route itLarge, thin, flat, nested parts; long profiles; sheet-based work.
• 2
  Mill it3D contours, deep pockets, tight bores, thick plate, angled faces.

Thin aluminum moves when you clamp it. A 3 mm 6061 panel pulled down with six clamps will bow between them, and once the clamps come off the part springs back. The cut that looked flat on the machine no longer is. Vacuum tables solve most of this because the load spreads across the whole face instead of six points.

When a vacuum table is not available, tabs and onionskin work. Leave 0.5 to 1.0 mm of material under the part and cut the profile in two passes. Cut the tabs last with a small cutter so the part does not shift when the last one goes. A 6 mm tab every 150 mm along the profile is usually enough for a 3 mm panel.

Thermal growth is the quiet problem. A 1,000 mm aluminum part grows about 0.023 mm per 1 °C. A cold morning shop and a warm afternoon shop are different machines as far as the part is concerned. If the tolerance is tight, let the stock sit in the shop overnight and measure it at the same temperature as the cut.

Vibration shows up before the dimension does. If the sound changes in a corner, stop and look. A part that rings during the cut will ring in the inspection report too, usually as a wall that is 0.03 mm thick on one end. Fixing the fixture is cheaper than re-cutting the part.

• 1
  Spread the loadVacuum over point clamps for anything under 6 mm thick.
• 2
  Tabs and onionskin6 mm tabs every 150 mm; leave 0.5–1.0 mm under the part.
• 3
  Let it soakAluminum grows about 0.023 mm per 1 °C per 1,000 mm.

Routers are not precision boring machines, and pretending otherwise costs money. On a well-maintained gantry router, a profile dimension of ±0.05 mm is realistic across a 1,000 mm part when the fixture is solid and the shop is temperature-stable. Hole positions in the same setup land around ±0.075 mm. Those are working numbers, not catalog numbers.

The reason is cumulative error. A long gantry has more travel to accumulate pitch error, thermal drift and deflection than a compact mill. Add tool wear on a long cut and the last feature on the part is cut with a different edge than the first. That is why routing aluminum suits profile work and clearance holes, and why a bearing bore belongs on a mill.

Where ±0.005 mm is needed, split the process. Route the blank to within 0.3 mm, then move to a 5-axis machining center for the critical bores, faces and threads. Two setups cost more than one, but they cost less than a scrapped batch. We quote both routes so the trade-off is visible before the chips fly.

Surface finish follows the same logic. A router with a sharp cutter and a light finishing pass reaches Ra 0.8–1.6 μm on a flat face. A finer Ra 0.2–0.8 μm finish is a milling or a polishing result. If the drawing calls for the finer band, plan the process around the finish, not around the machine that happens to be free.

• 1
  Realistic routing tolerance±0.05 mm profile, ±0.075 mm hole position on a 1,000 mm part.
• 2
  Split the processRough on the router, finish critical bores on a 5-axis mill.
• 3
  Finish bandRa 0.8–1.6 μm from routing; Ra 0.2–0.8 μm needs milling or polishing.