CNC metal cutting: the future of metal parts, explained

• 1
  What CNC metal cutting actually removes
• 2
  Where ±0.005 mm holds and where it does not
• 3
  Axis count and the parts it changes
• 4
  Fixtures, workholding, and the first-article check
• 5
  When CNC metal cutting is the wrong choice
• 6
  Process choice by part and volume

CNC metal cutting is subtractive. A cutter with a defined edge turns against the workpiece and lifts a chip off it. The program controls where the edge goes, how fast it turns, and how fast it feeds. Nothing is formed or added, so the starting block must already contain the part.

Three variables decide the cut: surface speed, feed per tooth, and depth of cut. In aluminium 6061 a 12 mm three-flute end mill might run at 8,000 rpm and 0.08 mm per tooth. In 17-4PH stainless the same cutter drops to around 1,200 rpm. Get the speed wrong and the edge rubs instead of cutting, which work-hardens the surface and kills the next pass.

The chip carries the heat. Most of the energy from the cut leaves with it. That is why coolant matters less for cooling the part than for clearing chips and stopping them from being re-cut. Re-cut chips dull an edge fast and leave a poor finish.

Every pass leaves marks. A roughing pass leaves visible steps. A finishing pass with a smaller radial stepover and a sharper edge brings the surface toward Ra 1.6 μm. Below that, you are usually grinding, lapping, or polishing, not cutting.

• 1
  RoughingHeavy depth of cut, large stepover, fast removal
• 2
  FinishingSmall stepover, high speed, surface and tolerance

A tolerance is a promise about a feature, not about a machine. On a rigid setup with a short tool and a stable material, ±0.005 mm is routine. On a thin wall, a long boring bar, or a deep pocket, it is not. The cut pushes the part away from the edge, and the springback shows up in the measurement.

Thermal drift is the quiet variable. A spindle warms up over the first hour and grows a few microns. On a ±0.005 mm feature, that matters. We run warm-up cycles and hold critical dimensions for checking after the machine has settled, not on the first article off a cold spindle.

Material behaviour sets the floor. Aluminium 6061 and 7075 cut clean and hold tight. Titanium Ti-6Al-4V deflects more and generates heat at the edge, so the same nominal tolerance needs a gentler cut and more passes. Inconel is harder again.

If a drawing calls for ±0.005 mm on a 300 mm unsupported span, the answer is usually a design change, not a bigger machine. Add a rib, shorten the span, or accept a looser tolerance where the function allows it.

A three-axis machine moves the cutter in X, Y, and Z. It is fast and stiff, and it handles prismatic parts well: plates, brackets, housings with features reachable from one side. If your part is a block with holes and pockets, three axes is the efficient answer.

A fourth axis adds rotation about one axis. That lets the machine cut around a cylinder, index to several faces, or run a continuous contour on a shaft. Mill-turn centers combine this with turning, so a part that needs both a turned diameter and milled flats can finish in one setup.

Five-axis machining adds two more rotations. The tool can tilt to reach undercut faces, drill at an angle, and keep the cutter normal to a curved surface. The gain is not just reach. A shorter, stiffer tool cuts better, and one setup removes the stacked error of moving a part between fixtures.

The trade is programming and setup time. A five-axis job needs a solid model, a verified post-processor, and a proven fixture. For a simple plate, that overhead buys nothing. For an impeller or a medical implant with compound angles, it is the only practical route.

Workholding decides whether the cut is accurate. Every clamp point is a place the part can move, and every unsupported span is a place it can ring. A well-supported part cuts quietly and measures consistently. A part held on two corners tells you so in the sound.

Soft jaws machined to the part profile spread the load and reduce distortion on thin walls. Vacuum plates suit thin flat parts that cannot take clamp pressure. For a long shaft, a steady rest or a tailstock is not optional.

The first article is measured against the drawing, then the setup is locked. In-process checks catch drift before it becomes a batch of scrap. We inspect 100% of parts before shipment and supply reports on request, including raw material certificates and dimensional data.

If a feature fails on the first article, the fix is usually in the setup or the tool, not in the program. Chasing it with offsets hides the cause and returns later in the run.

Subtractive cutting wins when the part is one-off, complex, tight, or made of a material that cannot be cast or moulded at low volume. It loses when the shape is simple and the quantity is high. A bracket that can be stamped will always be cheaper stamped at 50,000 pieces.

Deep internal cavities with no tool access cannot be cut. A part with a closed internal channel needs casting, additive, or a split design that is assembled. No axis count solves a feature the tool cannot reach.

Very thin walls are a limit too. Below roughly 0.5 mm in aluminium, the cutting force deflects the wall and chatter starts. You can cut it, but the tolerance has to loosen and the pass has to be gentle.

Material cost can decide it. Titanium and Inconel are expensive per kilogram, and a subtractive process turns most of that block into chips. Near-net forming plus a finishing cut can save a lot on a large part.