CNC Milling Basic Guide: How Material Becomes a Part

• 1
  What actually happens at the cutting edge
• 2
  Axes, travels and what each configuration buys you
• 3
  From CAD model to inspected part
• 4
  Where milling stops being the right process
• 5
  Holding tolerance and finish in production
• 6
  Material behavior you should expect on the floor
• 7
  Choosing the machine configuration for your part

Milling is subtractive. A spindle spins a multi-flute cutter, the machine moves the workpiece or the tool along programmed paths, and each flute shears off a chip. The CAM program decides feed per tooth, spindle speed, stepover and depth of cut. Get those four numbers wrong and you get chatter, tool wear or a scrapped part.

The chip carries the heat. If chips are thin, blue and powdery, the cutter is rubbing instead of cutting. If they are thick and silver, the load is healthy. On aluminium 6061 we typically run 3-flute carbide at 8,000–12,000 rpm and 0.05–0.15 mm per tooth. On 304 stainless the surface speed drops hard, often to 80–120 m/min, and coolant becomes mandatory.

Climb milling is the default on modern machines. The cutter tooth enters at maximum chip thickness and exits at zero, which pushes the material into the workpiece instead of lifting it. That gives better surface finish and longer tool life on rigid setups. Conventional milling still has a place on castings with hard scale, where the tool would otherwise bite into an abrasive skin.

• 1
  Chip loadFeed per tooth sets the real cutting load; too low work-hardens stainless.
• 2
  Radial engagementBelow 10% of cutter diameter keeps heat low in deep pockets.
• 3
  RigidityShortest possible tool stick-out beats any feeds-and-speeds trick.

A 3-axis mill moves X, Y and Z. It cuts everything reachable from one direction, which covers most plates, housings and brackets. The limit shows up as soon as a part has undercuts, angled holes or features on five faces. Then you either add setups or move to a machine that tilts the tool.

A 4-axis mill adds rotation around one axis, usually A. That lets you index the part between operations without re-fixturing, so concentric features stay concentric. Shafts, manifolds and parts with radial hole patterns sit here.

A 5-axis machine adds a second rotary axis, so the tool can approach from almost any direction. Two things improve at once: you can machine complex geometry in a single setup, and you can keep the tool short and stiff by tilting into corners. GreatLight runs 16 simultaneous 5-axis centers and 12 four-axis mills alongside 27 three-axis machines, which means we route the part to the cheapest machine that can still hold the tolerance.

• 1
  3-axisPlates, covers, simple pockets. Lowest cost per hour.
• 2
  4-axisCylindrical parts and radial features without re-chucking.
• 3
  5-axisUndercuts, deep cavities, blisks, and hard-to-reach faces.

The workflow is linear and each stage can break the next one. Design intent goes into a CAD model. CAM turns that into toolpaths and G-code with chosen tools, stock and workholding. The operator sets the origin, loads the program and proves it out, often on a scrap blank or in single block. Then the part is cut, deburred and measured.

Tolerances should reflect function, not habit. A ±0.005 mm callout on every dimension triples inspection time and adds cost with no benefit. Reserve tight tolerance for mating surfaces, bores and datums. A bolt clearance hole at ±0.2 mm works fine and machines faster.

Every removed feature leaves a witness. Datum selection at the drawing stage decides how the part will be held and probed, so a good drawing names the same A-B-C datums the machinist will use. When drawing and setup disagree, the inspector finds out first, and that is the expensive way to learn.

Milling removes material, so deep narrow pockets are slow and tool breakage is real. Below a certain corner radius the cutter simply will not fit. If the radius is smaller than about 1 mm and the pocket is more than five diameters deep, expect long cycle times or a wire EDM operation on the side.

Thin walls deflect. A 0.5 mm wall on a 100 mm aluminium part will move under cutting pressure no matter how sharp the tool is. If the design needs that wall, plan on light finishing passes and possibly a support fixture, which is a cost you should know about before releasing the drawing.

For high volumes of a single geometry, casting or forging followed by light machining usually wins. For one-off parts, hard materials or features that must be geometrically exact, milling wins. The crossover sits somewhere in the low thousands of parts, and it depends on shape complexity more than on part count alone.

• 1
  Tight internal cornersTool radius sets the floor; under 1 mm gets slow.
• 2
  Thin unsupported wallsBelow 0.8 mm on metal, chatter and deflection dominate.
• 3
  Very high volumeDie casting or forging plus finish milling usually costs less.

Tolerance is a system, not a number. Spindle runout, thermal growth, fixturing and tool wear all move the part. A machine rated at ±0.005 mm only delivers that when the setup is stable and the room is temperature-controlled. On long runs we check the first article, then monitor at intervals, because a worn Ø6 mm end mill will drift before it breaks.

Surface finish follows the same logic. As-machined aluminium usually lands at Ra 1.6–3.2 μm. A finishing pass with a sharp tool and small stepover gets you to Ra 0.8–1.6 μm. Below Ra 0.8 μm you are into polishing or a specific finishing strategy, and the cost curve turns steep.

Inspection closes the loop. We check raw material certificates on arrival, monitor in process, and inspect 100% before shipment, with reports available on request. For regulated work, the paperwork that matters is traceability, not just the measurement.

• 1
  First articleConfirms the setup before the run commits.
• 2
  Tool life trackingReplacement scheduled by cut time, not by failure.
• 3
  CertificatesISO 9001, IATF 16949, ISO 13485 and ISO 27001 cover different programs.

Aluminium is the default for prototypes and many production parts. 6061 and 7075 cut fast, hold tight tolerance and anodize well. 7075 gives higher strength but is less weldable and slightly more prone to stress movement after heavy material removal.

Stainless 304 and 316 work-harden if the cutter rubs. The fix is a positive feed per tooth and no dwelling in the cut. 17-4PH machines well in the solution-treated condition and is common for medical and aerospace parts that need corrosion resistance plus strength.

Titanium Ti-6Al-4V and Inconel sit at the hard end. They conduct heat poorly, so the cutting edge runs hot and tool life drops fast. Feed rates come down, coolant flow goes up, and cycle time becomes a real cost line. If a design can use 17-4PH or 4140 instead, the part gets cheaper without losing much.

• 1
  PlasticsPOM and PEEK machine cleanly; ABS can melt at the cutter.
• 2
  Brass and copperFree-cutting, good for electrical contacts and fittings.
• 3
  MagnesiumMachines fast but needs chip handling controls.