CNC Machine Work: 7 Steps From CAM File to Finished Part

• 1
  Key takeaways
• 2
  What CNC Machine Work Actually Does to Metal
• 3
  The Parts of a CNC Machine and What Each One Controls
• 4
  How CNC Machine Work Changes With 3, 4 and 5 Axes
• 5
  Fixtures, Datums and the Mistakes That Move a Dimension
• 6
  Feeds, Speeds and Finishing Passes That Hold Tolerance
• 7
  How CNC Machine Work, Step by Step
• 8
  Axis Count vs Part Geometry

CNC machine work is subtractive. A solid block, bar or casting goes in, and a rotating cutter removes material until the shape matches the CAD model. The controller does not see a drawing. It reads G-code: one block per movement, each with a target coordinate, a feed rate and a spindle speed. Everything the operator does is aimed at making those coordinates land on the part, not in the air.

The cutting edge removes metal by shearing it. That shearing generates heat, and heat is the enemy of a tight dimension. A 12 mm carbide end mill in 6061-T6 aluminium running at 8,000 rpm and 2,400 mm/min will pull heat away with the chip when the chip load is right. Drop the feed and the same cutter rubs instead of cuts. The edge dulls, the surface tears, and the dimension drifts.

Accuracy comes from three places: the machine geometry, the fixture, and the tool. A machine that holds ±0.005 mm on a warm spindle will not hold it on a part that moves in the vise. On aluminium we usually plan around Ra 0.8–1.6 μm from a finishing pass, then decide whether a finer Ra 0.2–0.8 μm pass is worth the extra cycle time.

Subtractive work has a boundary. Deep pockets narrower than 4× the tool diameter, sharp internal corners, and features that need a tool to reach under a lip all raise cost or become impossible. If you cannot see the cutter reaching the feature in your head, run a toolpath simulation before you release the drawing.

The frame and linear guides set the ceiling on accuracy. Cast iron or polymer concrete absorbs vibration; linear rails keep the axis straight over travel. A machine with 750 × 1,150 × 550 mm of travel behaves differently at the edge of the envelope than at the center, so keep critical tolerances near the middle of the table when you can.

The spindle holds the tool and turns it. Speed range, runout and thermal growth all show up in the part. A spindle that grows 10 μm over an hour will move a bore dimension by the same amount. For finishing runs we let the spindle idle up to temperature first, then touch off the tool.

The tool changer and the tool holders decide how many setups you can chain without stopping. A 24-station magazine lets a job run roughing, drilling, tapping and finishing in one program. Each tool added to the program is one more chance for a length offset to be wrong. Offline tool presetting removes that risk.

The controller reads the program and closes the position loop. Modern controls also handle look-ahead: they slow the feed before a tight corner so the tool does not overshoot. A program written with a constant feed through every corner will cut the corner and scrap a mating face. Adaptive feed control is worth turning on for hard materials.

A 3-axis mill moves X, Y and Z. The tool always points straight down, so every face you machine must face the spindle. A part with features on five sides needs five setups, and each setup re-introduces the same errors: zeroing, clamping distortion, and chip re-cutting. For flat plates and simple housings, 3-axis is still the fastest and cheapest route.

A 4-axis machine adds one rotary axis, usually A around the X axis. That lets you machine a shaft, a cylinder or a part on four sides without re-fixturing. A Ø400 mm rotary table covers most shaft work we see. The trade-off is that the rotary axis takes table space and adds a rotation error you must calibrate.

A 5-axis machine adds two rotary axes, so the tool can approach from almost any direction. The value is not the extra directions by themselves. It is that you can cut a compound angle, a deep pocket wall or an undercut feature in one setup. Fewer setups means fewer datum shifts, which is where most tolerance stacks come from.

Five axes are not free. Programming takes longer, the post-processor must be correct for that exact machine, and simulation is mandatory. For a part that is flat with a few holes, 5-axis adds cost with no gain. For a turbine blade, an impeller or a medical implant with curved surfaces, it is the only practical route.

Pick the datum before you pick the fixture. If the drawing locates a bore from a machined face, that face should be the first surface cut and the one you clamp against later. When the datum is a raw casting surface, the tolerance has to absorb the casting variation. Say so on the drawing instead of leaving it to the shop.

Clamping force bends thin parts. A 3 mm aluminium wall will deflect under a vise and spring back after unclamping, so the cut looks correct on the machine and wrong on the bench. Use soft jaws machined to the part profile, lower the clamp pressure, and take a light finishing pass after stress relief if the part is long.

Tool length and diameter offsets are the quiet source of scrap. A single wrong offset moves every feature cut by that tool. Prove the offsets on a scrap block or a test coupon before the first good part. On a 5-axis job, also check the rotary center point; a center that is off by 0.05 mm shows up as a step on a blended surface.

Chip evacuation decides whether the second part matches the first. Aluminium chips that pack into a pocket re-cut and damage the finish. Air blast or through-spindle coolant fixes most of it. In deep pockets, program a peck or a helical entry instead of a straight plunge, and give the chip a path out.

Start from chip load, not spindle speed. For aluminium with a 10–12 mm carbide end mill, a chip load of 0.05–0.1 mm per tooth is a normal roughing range. Multiply by the tooth count and the rpm to get the feed. If the machine cannot reach that feed, reduce the rpm instead of starving the cutter.

Roughing removes most of the volume and leaves stock for finishing. Leave 0.3–0.5 mm on walls and floors for the finishing pass. That pass should run at a higher surface speed and a smaller chip load so the tool leaves a consistent Ra 0.8–1.6 μm. Then decide whether a separate fine pass at Ra 0.2–0.8 μm is needed for a seal or a bearing seat.

Stainless and titanium behave differently. 316L work-hardens, so a cut that rubs is worse than a cut that is too aggressive. Keep the tool engaged, use a heavier chip load and plenty of coolant, and never let the cutter dwell in the cut. Ti-6Al-4V needs lower surface speed, sharp edges and rigid workholding, and it will show every vibration in the finish.

Measure while the part is still on the machine when the tolerance is tight. A bore that measures Ø20.005 mm at 20 °C may not measure the same after it cools in the inspection room. Note the temperature at inspection on the report, especially for parts with a ±0.005 mm callout.