Precision Metal CNC Milling Guide

• 1
  How a milling cutter removes metal
• 2
  Where ±0.005 mm is realistic, and where it is not
• 3
  How the alloy changes the cut
• 4
  What 3-axis, 4-axis and 5-axis each buy you
• 5
  What to check before you release a file for quote
• 6
  Choosing the machine and the alloy for the part

Milling is subtractive. A spindle spins a multi-tooth cutter, the machine moves that cutter along a programmed path, and each tooth shears a chip off the workpiece. Nothing about the part comes from a mold or a die, so geometry is limited by tool reach rather than by draft angles. That is the single most useful thing to remember when you compare milling against casting or forging.

Every tooth takes a chip of a certain thickness, called feed per tooth. Set it too low and the tool rubs instead of cutting, which work-hardens stainless and burns the edge. Set it too high and the flute packs, the tool deflects, and the wall you wanted at 2 mm comes out at 2.4 mm. Cutting speed and feed sit in a window, and the window is narrow on titanium and wide on 6061 aluminium.

Heat goes two places: into the chip and into the tool. On aluminium most of it leaves with the chip, which is why 6061 can run at high spindle speeds with no coolant flood. On Inconel and Ti-6Al-4V the heat stays near the edge, so speeds drop and coolant matters more. If a shop quotes titanium at aluminium cutting speeds, the tool life math was never done.

Rigidity decides accuracy more than the control does. A 27 kW spindle on a light fixture will chatter before a modest spindle on a rigid tombstone setup. Tool overhang is the usual culprit. Keep it under 4× diameter for finishing passes and the same program will hold a tighter band without any change to the code.

A CNC mill does not know what tolerance you need. It executes a path. The tolerance you get is the sum of machine positioning, tool deflection, thermal growth, and how the part was held. That is why two shops can run the same file and deliver parts that measure differently.

±0.005 mm is our standard achievable band on metal parts, roughly ±0.0002 in. It is a shop-floor number, not a marketing number. It assumes the feature is reachable, the wall is stiff enough, and the datum is defined on the drawing. Move any of those and the band widens.

Feature size drives the answer. A Ø6 mm bore in 6061 held in a vise hits ±0.005 mm all day. The same bore 90 mm deep in 316 stainless is a different job: the boring bar deflects, chips evacuate poorly, and you should expect ±0.02 mm or a second operation. Deep holes and thin walls are where tight tolerances get expensive.

Thermal drift is real. A spindle running for two hours grows, and a 500 mm aluminium part grows about 0.012 mm per 1 °C of temperature change. Shops that hold tight bands on long parts either control the room or finish-cut in the morning before the machines warm up. Ask which one applies to your order.

Surface finish and tolerance are separate purchases. Ra 0.8–1.6 μm is a normal machined finish. Ra 0.2–0.8 μm needs a finer stepover, a sharper tool, and often a separate finishing pass, so it costs more time. Buying Ra 0.4 μm on a mounting face that sits against a gasket is money spent for nothing.

GD&T callouts are only as good as the datum scheme. If a position tolerance references a datum that cannot be fixtured, the inspector and the machinist will read the part differently. Fix the datum before you argue about the number.

Aluminium is the easy case. 6061-T6 machines fast, holds a good finish, and takes anodizing well. 7075 is stronger but more prone to stress movement after heavy stock removal, so rough it, let it rest, then finish. If a bracket needs stiffness more than weight, 7075 is the pick; if it needs corrosion resistance and weldability, stay with 6061.

Stainless splits into free-machining and not. 303 cuts cleanly and is the default for shafts and fittings. 304 and 316 are tougher, work-harden quickly, and punish a light feed. 17-4PH gives high strength after aging, but the heat treat step adds days and can move dimensions, so leave grinding stock if the tolerance is tight.

Steel covers a wide range. 1018 and 1045 are straightforward. 4140 and 4340 need more rigid setups and lower speeds, and 4130 is common for aerospace tube and fittings. Tool steel is machinable in the annealed state only; plan the hardening sequence before you release the drawing.

Titanium and nickel alloys are where quotes diverge. Ti-6Al-4V cuts at roughly a quarter of the speed of aluminium, and Inconel is slower still. Both generate heat at the edge, both need rigid tooling, and both eat inserts. A part that takes 20 minutes in 6061 can take two hours in Inconel. That is not a shop padding the price.

Copper and brass machine easily but move. C36000 brass is the free-cutting grade and holds fine detail. Beryllium copper machines well and conducts heat, but the dust needs control, so expect a shop to handle it as a controlled process. Plastics behave differently again: POM and PEEK cut cleanly, ABS and PP tend to smear, and carbon fibre wears tools fast.

Three-axis milling moves X, Y and Z. One setup reaches one face. Prismatic parts, plates, housings with open pockets, and anything you can hold flat are three-axis work. It is the cheapest way to remove metal and the easiest to inspect, because everything is referenced to one face.

Four-axis adds rotation about one axis, usually A. A Ø400 mm rotary table lets the spindle reach four sides of a part without a re-clamp. Shafts with flats, cross-drilled holes, and parts with features on multiple faces around a single axis all fit here. Fewer setups means fewer datum shifts, which is often worth more than the machine rate.

Five-axis simultaneous moves the tool along a path that tilts as it goes. That is what makes impellers, turbine blades, deep cavities with undercuts, and contoured surfaces machinable in one setup. It also lets a short, stiff tool reach a deep feature by tilting instead of hanging out. The gain is not just capability, it is rigidity.

Five-axis is not automatically more accurate. It is more expensive per hour and it needs a programmer who understands collision checking. Put simple prismatic work on a three-axis machine and save the five-axis capacity for geometry that genuinely needs it. A shop that quotes everything on five-axis is either busy or not thinking about your cost.

Setup count is the hidden variable. Every re-clamp adds a datum shift and a chance for error. If your drawing has features on five faces and a ±0.01 mm relationship between two of them, one five-axis setup will beat three three-axis setups on both accuracy and total cost.

Tolerance is not free. A blanket ±0.005 mm title-block callout on a 300 mm aluminium weldment is not achievable without a controlled process, and a shop that accepts it silently will either charge for it or miss it. Mark the features that matter and let the rest run at general tolerance.

Look at every internal corner. A cutter is round, so a square internal corner needs either a relief, a broached feature, or EDM. Designers who draw a true sharp internal corner force the shop into a second process. Add a corner radius at least equal to the tool radius you expect.

Depth-to-diameter matters on every hole. Past roughly 4× diameter in aluminium or 3× in stainless, chip evacuation and tool deflection start to bite. If you need a deep, tight bore, expect a drill-and-ream sequence or a wire EDM operation, and price it accordingly.

Threads, engraving and marking have minimum sizes. Laser marking needs a character height of at least 1.5 mm to stay legible after finishing. Fine cosmetic text on a curved surface often comes out blotchy on anodized parts. Put the marking on a flat or a gentle curve.

Finally, say what the part does. A machinist who knows a face is a sealing surface will hold it to a tighter flatness and think about burrs. A note costs nothing and prevents a scrapped run.