What Do CNC Machines Do?

• 1
  What do CNC machines do, in five points
• 2
  What do CNC machines do with a CAD file?
• 3
  Subtractive manufacturing: what actually happens at the cut
• 4
  What do 3-axis, 4-axis and 5-axis CNC machines do differently?
• 5
  Turning, grinding and cutting: the other jobs CNC does
• 6
  Where CNC machining stops working
• 7
  What the tolerance and finish numbers mean on the shop floor
• 8
  From drawing to finished part: step by step
• 9
  Which CNC setup fits your part?

A CNC machine does not see a drawing. It sees coordinates. The CAD model is imported into CAM software, where a programmer picks the tool, the stepover, the feed and the depth of cut. The output is G-code: a list of positions the tool must reach, plus spindle speeds, coolant commands and tool changes.

The controller reads that list and drives servo motors on each axis. A ball screw turns, a linear guide slides, and the spindle arrives at X, Y and Z within a few micrometres of the commanded point. The cutting tool then takes a chip of metal. Repeat that a few thousand times per second of contact and the block becomes a part.

The important part is the feedback loop. Linear scales or rotary encoders report the actual position back to the controller, which corrects for backlash, thermal drift and cutting force. That closed loop is why CNC holds repeatability that a manual operator cannot match across an eight-hour shift.

• 1
  CADThe part geometry, including tolerances and surface callouts.
• 2
  CAMToolpath strategy, cutter selection, feeds and speeds.
• 3
  G-codeMachine-readable motion and logic commands.
• 4
  Servo motionClosed-loop positioning of spindle and axes.

Every CNC operation removes material. There is no forming, no layer stacking and no mold. A solid block of aluminium, stainless or titanium goes in, and the finished geometry comes out minus the chips. That is the whole premise of subtractive manufacturing.

At the cutting edge, three things happen at once. The tool shears the metal, heat builds up in the chip and the workpiece, and the tool wears. The machinist controls the balance with surface speed, feed per tooth and coolant. Aluminum 6061 cuts at 300–600 m/min with good coolant flow. Titanium TC4 runs at 30–60 m/min and needs heavy coolant or it work-hardens at the cut.

Chip evacuation matters as much as the cut itself. Deep pockets trap chips, which recut and wreck the surface finish. CAM programmers use trochoidal paths and air blast to clear pockets. On a 4,000 mm gantry part, chip clearance alone can decide the cycle time.

The reward for all this is freedom of geometry. Undercuts, thin ribs, internal bores and face profiles are all just toolpath problems. Nothing needs a mold or a die.

A 3-axis machine moves the tool in X, Y and Z only. The workpiece stays put. This suits prismatic parts: brackets, plates, housings and manifolds where every feature is reachable from one direction. A typical 3-axis envelope here runs 500 × 500 × 450 mm. Roughly 27 of these machines sit in our shop because most parts never need more.

A 4-axis machine adds a rotary table, usually Ø400 mm. The part turns about one axis while the tool cuts. That opens wrapped features: slots around a cylinder, cross-holes, and cam profiles. It is the efficient choice for shaft-like parts that would otherwise need two or three setups.

A 5-axis machine tilts the tool as well as the table. The cutter can approach a surface at the ideal angle instead of straight down. Deep cavities, impellers, turbine blades and organic shapes become reachable in one setup. We run 16 simultaneous 5-axis centers for exactly this reason: fewer setups, shorter cycle, and no re-fixturing error between operations.

The trade-off is real. Five-axis programming takes longer, the machine is more expensive per hour, and rigid workholding is harder to design. If your part is a flat plate with holes, 5-axis adds cost without adding value.

Milling is the most common answer to what do CNC machines do, but the same control logic drives other processes. A CNC lathe spins the workpiece and moves a single-point tool along it. That is the right call for round parts: shafts, bushings, fittings and connectors. Mill-turn centers combine both, so a part can be turned and then milled without leaving the spindle.

CNC grinding uses an abrasive wheel for tight tolerance and fine finish. When a bore needs Ra 0.2–0.8 μm or a fit that holds ±0.005 mm over a long length, grinding usually follows milling. CNC wire EDM cuts hardened steel with a thin wire and no cutting force, which suits sharp internal corners and thin features that would deflect under a cutter.

CNC cutting covers routers, waterjets and plasma for sheet and plate. These are subtractive too, just with a different energy source. For a 2 mm aluminum panel, a router is cheaper than milling. For 20 mm stainless, waterjet avoids the heat-affected zone.

The common thread is the same: a program defines the path, a servo follows it, and material is removed. The physics of each process decides which one fits the part.

CNC is not universal. It struggles with a few specific conditions, and knowing them early saves a redesign later. Thin walls are the classic problem. Below roughly 0.5 mm in aluminum or 0.8 mm in steel, cutting force deflects the wall and the tool chatters. You can hold the dimension, but not always the flatness.

Deep holes are the second limit. A drill that is more than 10 times its diameter deep tends to wander. Gun drilling helps, but cost rises fast and straightness is still not guaranteed to the same tolerance as a bored hole.

Hardness is the third. Above roughly 45 HRC, carbide struggles and the part usually moves to EDM or grinding. Above 60 HRC, wire EDM is the only practical subtractive route.

Finally, geometry that is not reachable is not machinable. A closed internal cavity with no tool entry is a casting or 3D printing job, not a CNC job. If a feature cannot be reached by a tool of reasonable length-to-diameter ratio, the drawing needs to change.

• 1
  Thin wallsDeflection and chatter below about 0.5 mm in aluminum.
• 2
  Deep holesDrill wander past 10× diameter; gun drilling adds cost.
• 3
  Hard materialAbove 45 HRC, grinding or EDM is usually better.
• 4
  Unreachable cavitiesNo tool entry means casting or additive, not milling.

A tolerance callout is not free. ±0.005 mm on a 50 mm aluminum part is a normal day. The same callout on a 400 mm steel frame is a different job, because thermal expansion alone moves the part more than that between morning and afternoon. Steel grows about 12 μm per metre per degree Celsius. A 4 °C shop swing eats the whole band.

Surface finish follows the same logic. Ra 1.6–3.2 μm is as-machined and usually needs no extra step. Ra 0.8–1.6 μm needs a finishing pass with a sharp tool and light depth of cut. Ra 0.2–0.8 μm usually means grinding or a fine finishing cycle with reduced feed. Each step adds time.

Datums decide whether the tolerance is even measurable. If the drawing calls ±0.005 mm but names a datum that is not accessible during setup, the inspection setup becomes ambiguous. Good drawings tie critical tolerances to datums the machine can actually touch.

Material choice moves the ceiling too. Aluminum 6061 and 7075 machine cleanly to tight tolerance. Inconel and titanium hold the dimension but punish the tool, so cycle time and cost rise sharply. 17-4PH stainless sits in between and machines well in the H1150 condition.