Metal CNC Milling Guide

• 1
  How a milling cutter actually removes metal
• 2
  3-axis, 4-axis, and 5-axis: what each one buys you
• 3
  What ±0.005 mm really requires from the part
• 4
  Surface finish: what Ra values mean on the shop floor
• 5
  When metal CNC milling is the wrong process
• 6
  Five DFM checks that cut cost before the first chip
• 7
  Choosing an axis configuration by part geometry

In metal CNC milling, a multi-flute cutter spins at a set spindle speed while the workpiece or the tool moves along programmed axes. Each tooth takes a small chip. The chip thickness is set by feed per tooth, not by the feed rate you type into the controller. That distinction matters when a tool starts chipping or burning.

Cutting speed is surface speed at the tool edge, measured in m/min. It depends on the material and the tool coating. Aluminum 6061 runs fast, often 300–500 m/min with carbide. Ti-6Al-4V runs slow, 40–60 m/min, because titanium conducts heat poorly and the edge overheats. Stainless 316 sits between, around 120–180 m/min.

Chip evacuation is the hidden constraint. A deep pocket in 7075 may look easy on the drawing, but if chips recut under the tool, the finish degrades and the edge wears fast. Air blast, through-spindle coolant, or a roughing strategy with a larger radial step all solve it. The choice is a process decision, not a machine setting.

• 1
  Feed per toothSets chip load; too low rubs, too high breaks edges.
• 2
  Surface speedMaterial-driven; titanium runs roughly 8× slower than aluminum.
• 3
  Radial and axial depthBalance to keep tool deflection predictable.

A 3-axis mill moves X, Y, and Z. The tool always points down. That is enough for plates, brackets, and housings where all features are reachable from one direction. It is the cheapest setup and often the fastest, because fewer axes mean fewer repositioning moves.

A 4-axis mill adds rotation around one axis, usually A. This lets you machine features on multiple faces of a cylindrical or prismatic part without unclamping. Shafts, flanges, and parts with radial holes fit here. The limit is that the tool still approaches from a single plane relative to the part.

A 5-axis mill adds two rotary axes, so the tool can tilt and the table can rotate. Simultaneous 5-axis motion lets a short, stiff cutter reach deep pockets, undercut walls, and complex contours in one setup. For impellers, medical implants, and aerospace structural parts, this is the difference between one operation and five.

The trade-off is programming time and inspection load. Five-axis toolpaths need verification, and the machine costs more per hour. If a part can be made in two 3-axis setups with a simple fixture, that is usually the better route.

• 1
  3-axisFlat parts, simple pockets, lowest cost per hour.
• 2
  4-axisCylindrical parts, radial features, one clamping.
• 3
  5-axisComplex contours, undercuts, fewer setups.

Tolerance is not a single number you attach to a drawing. It is a chain: machine positioning, tool wear, thermal drift, fixturing, and inspection uncertainty. A ±0.005 mm callout is achievable, but only when the part geometry cooperates. Thin walls, long unsupported sections, and deep small holes all push against it.

Wall thickness matters more than most designers expect. Below about 0.8 mm in aluminum, the cutter pushes the wall instead of cutting it. You can still hold the dimension, but the surface will show chatter and the next part may differ. Adding a rib or increasing the wall to 1.2 mm often costs less than holding a tight tolerance on a flimsy feature.

Datums drive everything. If the drawing calls a tight tolerance on a hole but the datum is a rough cast surface, the inspector cannot reproduce the measurement. Define datums on machined faces. That single change removes most disputes at first article.

For parts that need ±0.005 mm, we inspect 100% before shipment and can provide reports on request. Raw material check, in-process monitoring, and final inspection are standard steps, not add-ons.

• 1
  Minimum wallAbout 0.8 mm in aluminum, more in stainless.
• 2
  Datum choiceUse machined faces, not cast or rough surfaces.
• 3
  InspectionTight tolerance means 100% check, not sampling.

Ra is the arithmetic average roughness of the profile. It is a single number that hides a lot. A face can read Ra 0.8 μm and still show visible tool marks if the feed marks are regular. Visual acceptance and Ra acceptance are different checks.

As-machined finish sits around Ra 1.6–3.2 μm. This is fine for brackets, fixtures, and internal parts where only fit matters. High-finish milling reaches Ra 0.8–1.6 μm with a finishing pass, sharper tool, and lighter chip load. Fine finish, Ra 0.2–0.8 μm, usually needs a dedicated finishing operation or a secondary process.

The fastest way to a better finish is often not more milling. Bead blasting, tumbling, or polishing can bring a milled surface to a cosmetic standard at lower cost than chasing Ra with the cutter. For sealing faces or bearing bores, though, the geometry matters and you should finish by milling or grinding.

Anodizing, plating, and powder coating change the surface too. Hardcoat anodizing adds roughly 25–50 μm per side, which moves a tight bore. Tell the shop which surfaces are functional before finishing starts.

• 1
  As-machinedRa 1.6–3.2 μm, functional fit surfaces.
• 2
  High finishRa 0.8–1.6 μm, sealing and sliding faces.
• 3
  Finishing adds materialHardcoat anodize moves dimensions by tens of microns.

Milling is subtractive, so the tool needs room to enter and exit. A closed internal channel with no access cannot be milled. If the channel is essential, the part becomes two pieces joined later, or the process changes to casting or 3D printing.

Very high volumes change the math. At 10,000+ parts, die casting or injection molding usually beats milling on unit cost, even after tooling. Milling still wins for prototypes, low volumes, and parts where the design is not frozen.

Hardened tool steel above about 45 HRC is difficult to mill in the finished state. The usual route is to mill soft, then heat treat, then grind or EDM the critical features. Trying to mill the hardened part directly costs more in tooling than it saves in steps.

Material choice also constrains geometry. Inconel and titanium cut slowly and wear tools fast. A design that is easy in 6061 may be impractical in Ti-6Al-4V if it has thin fins or deep slots. Ask for a DFM review before you commit the design.

• 1
  No tool accessClosed internal channels cannot be milled.
• 2
  High volumeAbove roughly 10,000 parts, casting or molding wins.
• 3
  Hardened steelMill soft, heat treat, then grind or EDM.

Corner radii should match standard cutter sizes. A 6 mm internal corner needs a 6 mm or smaller cutter, which is slower and less stiff than a 12 mm cutter. If you can open the radius to 6 mm, do it. If the design needs 2 mm, expect a longer cycle and a higher price.

Pocket depth relative to cutter diameter drives deflection. A rule of thumb: keep depth under 4× the cutter diameter for roughing, and under 2× for finishing where finish matters. Deeper pockets need a smaller step-down and more passes.

Threads and holes should be specified with standard sizes. A #10-32 or M6 thread is quick. A custom pitch requires a special tap or single-point threading, which adds setup time. Hole depth also matters: a blind hole deeper than 3× diameter is hard to tap cleanly.

Text and logos on a milled face need a minimum character height of 1.5 mm for laser marking, and more if you want the mark to read after anodizing. Engraved text with a small cutter is slow, so keep it shallow and simple.

Finally, define the finish on the surfaces that matter only. Specifying a cosmetic finish on every face adds cost with no function. Mark the sealing, sliding, and mating surfaces, and leave the rest as-machined.

• 1
  Corner radiusMatch to standard cutter sizes where possible.
• 2
  Depth ratioKeep roughing depth under 4× cutter diameter.
• 3
  Marking heightMinimum 1.5 mm character height for laser marking.