CNC processing: how computer-controlled cutting works

• 1
  What CNC processing actually does to metal
• 2
  Three-axis, four-axis, or five-axis CNC processing
• 3
  Geometry that justifies simultaneous five-axis work
• 4
  What ±0.005 mm means on a real part
• 5
  Surface roughness, burrs, and secondary operations
• 6
  When CNC processing is the wrong choice
• 7
  Choosing a machine type by part geometry

CNC processing is subtractive. A computer reads a toolpath and moves a spinning cutter through a solid block until the remaining material is the part. Nothing is formed or cast. The shape is whatever the tool can reach and the fixture can hold.

That single fact explains most of the design rules you will hear from a machine shop. Deep pockets, sharp internal corners, and thin unsupported walls are not forbidden because of policy. They are slow, or they chatter, or the tool breaks.

The machine itself is only part of the system. A CNC process includes the fixture, the tool holders, the coolant strategy, and the inspection plan. Change any one of those and the achievable tolerance moves with it.

Cutting data follows the material. Aluminum 6061 runs fast with high rake angles and generous coolant. Stainless 316 work-hardens if the feed is too light, so the cutter must stay engaged. Titanium Ti-6Al-4V conducts heat poorly, so most of the heat leaves with the chip and the tool needs lower surface speed.

A three-axis machine moves the table in X, Y, and Z while the spindle stays vertical. It is the fastest and cheapest way to cut a part whose features are reachable from a handful of orthogonal directions. Most brackets, plates, and housings never need anything else.

A four-axis machine adds rotation about one axis, usually A. The part turns while the tool cuts, so holes and slots can be placed around a cylinder without a second setup. This matters when concentricity between features on the same axis is tight.

Five-axis machining moves the tool in two rotary axes at once. The cutter can approach a face at an angle instead of straight down. That lets a short, rigid tool reach deep features, and it lets one setup cover faces that would otherwise need three or four.

The trade is programming time and machine cost. Five-axis toolpaths take longer to verify, and the machine is slower to set up. If a part can be made on three axes with two setups, that is usually the better route.

Impellers, turbine blades, and impeller-like rotors carry free-form surfaces that wrap around an axis. On three axes those surfaces need ball-end tools with long reach, which deflect and leave witness lines. Simultaneous five-axis keeps the tool normal to the surface and short.

Medical implants and instruments often combine an organic outer form with a machined mating feature. Cutting both in one setup removes the stack-up error you would get from re-fixturing. The same logic applies to aerospace structural parts with pockets on several faces.

Angled holes and undercut features are a common trigger. If a hole enters a face at 30°, a three-axis machine needs a tilted fixture or a second op. Five-axis simply tilts the head.

There is a limit. If the part is a flat plate with through holes, five-axis adds cost and no value. The geometry has to need the extra axes.

A tolerance is only meaningful with a datum. ±0.005 mm measured from a ground face on a rigid part is repeatable. The same number applied across a 400 mm weldment is not, because thermal drift alone can eat the budget.

Material stiffness sets the practical floor. Aluminum and brass hold tight tolerances well. Thin stainless walls deflect under cutting force and spring back after the tool passes, so the finished size differs from the programmed size.

Tool wear is the other slow variable. On a long run the cutter shrinks, and the last parts come out undersize unless the operator compensates or the tool is changed on a count. In-process monitoring catches this.

For most mating features, ±0.05 mm is enough and costs far less to hold. Reserve ±0.005 mm for bearing seats, spigots, and alignment features that actually need it. Tolerancing everything tight raises cost without improving function.

As-machined surfaces land around Ra 1.6–3.2 μm with a sharp cutter and stable setup. Pushing to Ra 0.8–1.6 μm needs a finishing pass with a smaller stepover, which adds cycle time. Ra 0.2–0.8 μm is a lapping or polishing operation, not a milling one.

Burrs form wherever the tool exits the material. They are a function of edge geometry and feed, not of machine quality. A chamfer or a radius on the drawing edge prevents most of them before they start.

Secondary operations change the part after machining. Anodizing builds a layer a few micrometers thick, which shifts dimensions on tight features. Hardcoat anodizing builds more. Mask or pre-size the feature if the tolerance is tight.

Laser marking needs a minimum character height of 1.5 mm to stay legible after finishing. Below that, characters fill in or fade.

CNC processing is a per-part cost with a low setup cost. That shape favors prototypes and low to mid volume. As quantity climbs, the cost per part stops falling because each part still consumes machine time.

Die casting and vacuum casting flip that curve. They carry a tooling cost up front and a low cost per part after that. Once the annual volume is high and the geometry is stable, casting wins.

Parts with a hollow internal cavity that no cutter can reach are a poor fit. So are parts where the material is cheaper to form than to cut away, such as large thin panels.

There is no minimum order quantity here, so one prototype and a 10,000-part run use the same route. The question is not whether CNC processing works. It is whether the volume has grown past the point where it is the cheapest way.