CNC Milling Machine: How It Cuts, and Where It Stops

• 1
  Key takeaways
• 2
  What a CNC milling machine actually does
• 3
  3-axis, 4-axis and 5-axis: which one your part needs
• 4
  Where the process gets hard: walls, depth and hardness
• 5
  What tolerance and surface finish you can expect
• 6
  Which materials mill well, and which fight back
• 7
  What drives the cost of a milled part
• 8
  Choosing an axis configuration

A CNC milling machine holds a block of material in a vise or fixture and moves a spinning cutter through it. The cutter has multiple teeth. Each tooth takes a small chip as it rotates into the work. The machine's controller reads G-code and drives the axes so the tool follows a path, leaving the shape you modeled.

That is different from turning, where the part spins and the tool stays put. Milling can produce pockets, slots, flats, ribs, threads and contoured surfaces on a part that starts as a solid billet. If your drawing shows a cavity that is not a surface of revolution, milling is usually the process that makes it.

The cut is not silent and not instant. A 12 mm carbide end mill running in 6061 aluminium might spin at 8,000 rpm with a feed of 2,000 mm/min, removing material at a steady rate. In 17-4PH stainless the same cutter drops to roughly 1,200 rpm and a much lighter feed. The controller does not care, but the tool and the spindle do.

• 1
  Material comes offNo mold, no pattern. The part is cut from solid stock.
• 2
  Paths come from CAMYour STEP file becomes tool paths and then G-code.
• 3
  Setup repeatsEach new face usually needs a new fixture or a new vise position.

A 3-axis mill moves X, Y and Z. The tool always points down, so it can only reach surfaces that face the spindle. Deep side pockets, undercuts and angled holes need the part to be flipped and re-fixtured. Every flip adds setup time and a small position error.

A 4-axis mill adds a rotary table, usually turning about X or Y. The part can be indexed to new faces without unclamping. This suits parts with features around a cylinder, such as a shaft with milled flats or a housing with radial ports. Our shop runs a Ø400 mm rotary table on these machines.

A 5-axis mill adds a second rotary axis, so the tool can tilt. That lets a stub cutter reach into a deep pocket with a short, stiff tool, and it lets the machine cut a contoured surface in one continuous pass. GreatLight runs 16 simultaneous 5-axis machining centers, 12 four-axis mills and 27 three-axis machines. The right choice is the cheapest one that reaches every feature.

• 1
  3-axisPrismatic parts, open faces, flat bottoms. Lowest cost per setup.
• 2
  4-axisFeatures around a bore or a cylindrical body; indexing instead of flipping.
• 3
  5-axisUndercuts, deep cavities, sculpted surfaces, tight true position across faces.

Tool deflection is the main enemy. A long, thin cutter bends under cutting force, and the wall it leaves is not where the program said. The rule of thumb is to keep the tool's length-to-diameter ratio below about 4:1 for finishing. Beyond that, you either accept a looser tolerance or pay for a 5-axis setup that uses a shorter tool.

Deep pockets are the same problem in another form. A pocket 5× deeper than the cutter diameter needs a long tool, which needs light passes, which takes time. If a pocket can be redesigned at 3× depth, the cost usually drops by a third or more. This is the kind of change a DFM review catches before the first chip.

Hardness changes everything. Aluminium 6061 and 6082 cut fast. 17-4PH, Inconel and tool steel cut slowly and wear the cutter, so the same part can take three or four times longer. Titanium TC4 (Ti-6Al-4V) also moves under heat, so finishing passes stay light and coolant flow matters.

• 1
  Thin floorsUnder 0.5 mm on aluminium, chatter shows up as a wavy finish.
• 2
  Sharp internal cornersA cutter has a radius. Cutters leave a corner radius equal to the tool.
• 3
  Hard materialsInconel and 17-4PH need slower speeds and more tool changes.

General milling holds ±0.05 mm without much effort. Tighten to ±0.01 mm and the shop starts measuring, controlling temperature and possibly adding a finishing pass. At ±0.005 mm, which is the limit GreatLight works to, the process needs stable fixturing and a final inspection step. Not every feature on a part needs that number.

Surface finish follows the same logic. As-machined surfaces land around Ra 1.6–3.2 μm. A finer finishing pass gets Ra 0.8–1.6 μm. Polishing or a dedicated finishing strategy can reach Ra 0.2–0.8 μm, but that adds time and hand work. If a sealing face needs Ra 0.8 μm, say so on the drawing. If a non-critical bracket is called out at Ra 0.2 μm, that is cost with no benefit.

Callouts should be per feature, not per part. Mark the datums, the fits and the sealing surfaces. Leave the rest at general tolerance. A drawing that demands ±0.005 mm everywhere and Ra 0.4 μm everywhere will be quoted high, and the shop will spend time on faces that never touch anything.

• 1
  General±0.05 mm and Ra 1.6–3.2 μm as machined.
• 2
  Controlled±0.01 mm with an in-process check.
• 3
  Fine±0.005 mm and Ra 0.8–1.6 μm on critical features only.

Aluminium is the easy case. Grades 6061, 6061-T6, 6082 and 7075 all cut cleanly and hold tight tolerances. 7075 is stronger but less corrosion resistant without a coating. 2024 machines well too, though it needs protection. If your part is a bracket, a housing or a heat sink, aluminium is usually the first choice.

Stainless grades behave differently. 303 is free-machining and kind to tools. 304 and 316L work-harden if the cutter rubs, so the feed has to stay aggressive enough to cut, not rub. 17-4PH in the H900 condition is hard and slow. For medical and food-contact parts, 316L is common, and we hold the finish that cleaning demands.

Steel, titanium and copper alloys each bring their own limits. 4140 and 4340 are tough and need rigid setups. Ti-6Al-4V has low thermal conductivity, so heat stays in the cut and coolant is essential. Copper and brass cut fast but can be gummy; beryllium copper is machinable but the dust needs control. Plastics like POM, PEEK and ABS mill easily, but they expand with heat, so a finishing pass at a stable temperature matters.

• 1
  Easy6061, 6082, 303 stainless, brass, POM.
• 2
  Moderate304, 316L, 4140, 7075, titanium TA2.
• 3
  Hard17-4PH, Inconel, tool steel, TC4.

Setup dominates small runs. If a part needs four faces machined, that is four setups, and each one costs time. A one-off bracket at 20 pieces will be quoted mostly on setup and programming. At 2,000 pieces the cycle time takes over and the setup is spread thin.

Material removal rate sets the middle of the cost curve. A part that is 90% air, like a thin frame with a few bosses, takes a lot of cutting time to free the shape. A compact part with a simple profile cuts fast. The buy-to-fly ratio, the weight of stock versus finished part, is a useful number to estimate this before quoting.

Secondary work adds up. Anodizing, plating, bead blasting and laser marking are separate steps with their own lead time. A tight tolerance on a coated part needs the coating thickness factored in. And if the drawing needs a CMM report per part, that inspection time is real cost, even when the part itself is simple.

• 1
  Number of setupsEach new face is time and a new chance for error.
• 2
  Stock removalMore air in the part means more cutting time.
• 3
  Finishing and inspectionCoating, polishing and reports are billed steps.