How a CNC Machine Works: From G-Code to Finished Cut

• 1
  Key takeaways
• 2
  What the controller actually does
• 3
  Servo drives, ball screws, and what limits accuracy
• 4
  Tool offsets, wear, and why the first part is not the part
• 5
  Where CAM stops and the operator starts
• 6
  In-process checks that catch drift early
• 7
  How a CNC machine works, step by step
• 8
  When a CNC machine works well, and when it does not

A CNC machine works by turning a coordinate list into controlled motion. The CAM post-processor writes G-code such as G01 X10.0 Y20.0 F400, and the controller reads it block by block. Each block tells the axis where to go, how fast, and which spindle or coolant command to run at the same time.

The controller does not just replay the numbers. It compares the commanded position with the actual position from the encoder or linear scale, then adjusts the drive current. That loop runs at the servo update rate, often 1–4 kHz. On a good machine the following error stays in the single-digit micrometre range during a normal contour cut.

This is why a cheap control on a rigid frame can still hold tolerance, and a good control on a loose machine cannot. The control only corrects what the mechanics let it correct.

• 1
  Block look-aheadThe controller reads 20–200 blocks ahead to plan deceleration before corners.
• 2
  Feed overrideOperators trim feed from 50% to 150% without editing the program.
• 3
  Optional stopM01 pauses the cycle for a quick gauge check without losing position.

Each linear axis is a closed system: servo motor, coupling, ball screw, linear guide, and feedback device. The ball screw converts rotation into travel. A typical rolled screw has 0.05 mm per 300 mm lead error; a ground screw is much tighter. That error shows up directly in the part unless the control compensates for it.

Thermal growth is the quiet problem. A spindle running at 12,000 rpm for two hours can move 20–40 μm in Z. Shops that hold ±0.005 mm on long runs warm up the machine for 30–60 minutes first, and some run a warm-up program overnight.

Backlash and lost motion appear when the axis reverses direction. Climb milling with a light finishing pass hides some of it, but a worn thrust bearing will still leave a step on a wall. If a bore measures 0.02 mm different when approached from the other side, the backlash is the first thing to check.

• 1
  Linear scale vs encoderScales measure the table, not the motor, so they catch screw error.
• 2
  PreloadBall nut preload removes axial play but adds drag and heat.
• 3
  Rapid positioningRapids do not cut, but a bad approach vector can still scrap the part.

Every cutter has a length and a diameter that the control must know. The operator touches off each tool on a setter or a probe, then stores the offset in the register. If a 10 mm end mill is entered as 9.98 mm, every wall on that feature shifts by 0.01 mm.

Tools wear during the run. A carbide insert in 4140 steel may lose 0.02–0.05 mm of diameter over a few hundred parts. Shops that hold tight limits either probe the tool between parts or run a wear-compensation table that steps the offset as the count rises.

This is why the first article matters. We cut it, measure it, and adjust offsets before the run continues. On a ±0.005 mm feature the setup can eat the whole tolerance band if it is rushed.

• 1
  Touch-off errorA chip under the tool tip can shift the offset by 0.01 mm.
• 2
  RunoutA holder with 0.02 mm TIR cuts oversize on one flute.
• 3
  Pull-outA loose collet lets the tool creep deeper during heavy cuts.

CAM software turns the solid model into toolpaths, but it does not know the shop floor. The programmer picks the stock, the workholding, and the order of operations. A good setup cuts most of the part in one or two fixturings, because every refixture adds stack-up error.

Simulation catches collisions and gouges before the spindle turns. It does not catch chatter, thin-wall deflection, or a tool that cannot reach a corner. Those are judgment calls. On a deep pocket with a 6 mm cutter, a 4:1 length-to-diameter ratio is already pushing it; past 6:1 the finish will show it.

For 5-axis work the extra rotary axes let the tool approach a face at an angle. That shortens the effective stick-out and improves surface finish on contoured surfaces. It also means the post-processor and the machine kinematics must match exactly, or the part comes out in the wrong place.

• 1
  Rest machiningSmall cutters clean corners the roughing tool could not reach.
• 2
  Trochoidal pathsSpreads radial load so a 10 mm cutter can slot at full depth.
• 3
  Stock modelAn accurate stock keeps the first pass from cutting air or overloading.

A machine that only cuts and never measures is guessing. Probing the workpiece between operations confirms the datum is still where the program expects it. On a long run a 30-second probe cycle can save a scrapped batch of 200 parts.

CMM checks after machining give the final verdict, but they come too late to save the parts already cut. In-process gauging, tool breakage detection, and spindle load monitoring are the early warning systems. Spindle load climbing by 15% on the same program usually means a dull tool or a chip pack.

For a ±0.005 mm tolerance we inspect 100% before shipment and keep the reports on request. The point is not the paperwork. It is catching a shift before it becomes a trend.

• 1
  Datum checkProbe the fixture before the first cut on a new setup.
• 2
  Load monitoringRising spindle load points to wear or chip recutting.
• 3
  Temperature logA warm shop shifts dimensions more than most operators expect.