How Does CNC Machining Work?

• 1
  Key takeaways
• 2
  How does CNC machining work: the cutting loop
• 3
  From CAD model to G-code
• 4
  Which machine does which job
• 5
  When CNC machining is the wrong choice
• 6
  How accuracy is held across a batch
• 7
  Step by step: running a CNC job
• 8
  CNC machining compared with other processes

CNC stands for computer numerical control. A controller reads a program of coordinates and moves the machine axes to those points. The cutter spins at a set speed while the table or spindle moves along X, Y and Z. Material leaves the workpiece as chips, so the final shape is whatever the tool path leaves behind.

The loop is simple to describe and fussy to run. A cutter has a diameter, a helix angle and a number of flutes. Each flute takes a bite of material called the chip load. If the chip load is too small, the tool rubs and work-hardens the surface. If it is too large, the tool deflects or breaks. The sweet spot depends on material, tool material and how rigidly the part is held.

Cutting speed is the surface speed of the tool edge, usually written in m/min. Feed rate is how fast the tool moves through the material, in mm/min. These two numbers, plus depth of cut and stepover, define the cut. For aluminium 6061 on a carbide end mill, a common range is 200–500 m/min surface speed with a feed per tooth of 0.05–0.15 mm. For 304 stainless, drop to 60–120 m/min and 0.03–0.08 mm per tooth.

Heat is the quiet constraint. Most of it leaves with the chip, which is why chip evacuation matters so much in deep pockets. Flood coolant, air blast or through-tool coolant all work, but the wrong choice for the material can cause thermal cracking or poor finish. Titanium and Inconel need low surface speeds and steady coolant, or the edge fails early.

• 1
  Climb millingThe cutter tooth enters at maximum chip thickness. Standard for CNC work because it reduces rubbing and improves finish.
• 2
  Conventional millingThe tooth enters at minimum thickness. Used mainly on older machines with backlash or on cast skin surfaces.
• 3
  Roughing vs finishingRoughing removes volume fast with larger stepovers; finishing uses small stepovers and higher speed for size and finish.

The process starts with a 3D model. STEP and IGES are the safest neutral formats for machining; native files from SolidWorks, Creo or NX are also fine. Send the model with a 2D drawing that carries tolerances, datums and surface finish callouts. A model alone does not say which face is the datum or where the ±0.05 mm applies.

The CAM programmer imports the model, chooses a stock size and defines the work coordinate system. Tools are selected from the shop library. The programmer then generates roughing, semi-finishing and finishing passes. Simulation runs before anything is cut. This is where a clash, a too-long tool or a missing fixture is caught for free.

Post-processing converts the tool paths into G-code for a specific controller. Fanuc, Siemens, Heidenhain and Haas all read G-code, but the canned cycles and tool change macros differ. A correct post-processor is not optional. A wrong one produces a program that looks fine on screen and alarms out on the machine.

For simple 2.5D parts, a programmer can write the code by hand. For contoured surfaces, impellers or mold cavities, CAM is the only practical route. Once the program is proven, it is stored with the setup sheet so repeat orders run from the same file.

• 1
  Model checkLook for open surfaces, zero-thickness walls and features smaller than the smallest available cutter.
• 2
  Stock allowanceLeave 0.3–0.5 mm on finishing surfaces for aluminium, 0.2–0.3 mm for steel.
• 3
  SimulationRun the full program with fixture and tool holder geometry, not just the tool path.

A 3-axis mill moves the table in X and Y and the spindle in Z. It handles plates, brackets, housings and any part where features sit on accessible faces. It is the most economical choice and should be the default unless the geometry says otherwise. Our shop runs 27 three-axis machines for exactly this reason.

A 4-axis mill adds a rotary axis, usually around X. That lets the part rotate while the tool cuts, so holes on four sides can be drilled in one setup. It is a good fit for shafts with cross holes, valve bodies and long parts that would otherwise need three or four re-fixturings.

A 5-axis machine adds a second rotary axis. Simultaneous 5-axis motion lets the cutter stay normal to a curved surface, which is how impellers, turbine blades and complex medical instruments are made. It also lets a short, stiff tool reach features that a long 3-axis tool could not. We run 16 simultaneous 5-axis machining centers, including a Ø400 mm rotary table for round parts.

Mill-turn centers combine turning and milling in one machine. A part like a hydraulic manifold can be turned to diameter, then milled and drilled without losing concentricity. That removes a setup and a re-clamping error. Our 16 mill-turn centers cover parts up to 4,000 mm in the largest configuration.

• 1
  3-axisFlat or prismatic parts, one face at a time. Lowest cost per part.
• 2
  4-axisCylindrical or box parts with features on multiple sides. One rotary setup.
• 3
  5-axisContoured surfaces, deep cavities and tight angular tolerances.
• 4
  Mill-turnRound parts with off-axis holes or milled flats. Fewer setups, better concentricity.

CNC is subtractive, so every feature needs tool access. A deep pocket with a sharp internal corner cannot be milled with a round cutter. Either the corner gets a radius, the part gets split, or the feature goes to EDM. Deep holes with a high depth-to-diameter ratio, say 10:1 or more, need special drills and peck cycles, and the hole may drift.

Undercuts are another limit. If a feature is wider below the surface than at the surface, a standard end mill cannot reach it. A T-slot cutter or a custom form tool can, but the setup gets expensive. For one-off parts, redesigning the feature is usually cheaper than buying a tool.

Volume matters too. CNC is efficient from one piece to a few thousand. Above that, die casting, investment casting or injection molding usually wins on unit cost. We run die casting and vacuum casting alongside machining, so a program can start as a machined prototype and move to a cast production part with the same drawing datums.

Finally, consider material behavior. Some plastics machine cleanly with sharp, polished tools; others gum up and need high speed and air blast. Carbon fiber and glass-filled resins wear carbide quickly, so tool life, not cycle time, becomes the cost driver.

• 1
  Internal corner radiusMinimum radius equals the cutter radius. Smaller radius means a smaller, slower tool.
• 2
  Wall thicknessBelow about 0.8 mm in aluminium, deflection and chatter become the main risk.
• 3
  Surface finishRa 0.8–1.6 μm is a normal machined finish; Ra 0.2–0.8 μm needs finishing passes and may need polishing.

Accuracy is not one number. It is the sum of machine geometry, tool wear, thermal drift and fixture rigidity. A machine that cuts a good first article can still drift over a long run. That is why in-process measurement matters more than a single final inspection.

We hold ±0.005 mm on critical features and inspect 100% of parts before shipment. That includes a raw material check, in-process monitoring and a final inspection, with reports available on request. For a first article, the report shows the actual measured values, not just a pass or fail.

Thermal drift is the usual cause of a slow shift in the afternoon. The spindle warms up, the ball screws expand and the zero point moves a few microns. A warm-up cycle at the start of the shift, plus a re-check of the first part after two hours, catches most of it.

Tool wear is the other long-run risk. A carbide end mill running aluminium can hold size for hundreds of parts, but the same tool in 17-4PH stainless may need changing after a few dozen. Tracking tool life by material and feature is how a shop keeps a run inside tolerance without inspecting every part.

• 1
  First article inspectionFull dimensional report before the batch is released.
• 2
  In-process checksCritical dimensions checked at set intervals during the run.
• 3
  Final inspection100% of parts checked before shipment, reports on request.