CNC processing function: how each control function shapes the part

• 1
  What CNC processing function actually means inside the controller
• 2
  Linear and circular interpolation: building the path
• 3
  Cutter compensation, offsets and coordinate control
• 4
  Feed rate and spindle control: the cutting function
• 5
  Rotary axes: what the 4th and 5th functions add
• 6
  Which function to use for which feature

A CNC processing function is one discrete job the controller performs while a tool is in the cut or moving toward it. Interpolation builds the path between two programmed points. Cutter compensation shifts that path sideways to account for real tool diameter. Feed and spindle control set how fast the tool advances and how fast it spins. Each function runs in its own loop, thousands of times per second, and each one has a boundary where it stops helping.

Engineers often treat the controller as a black box. That habit causes trouble later. When a wall comes out 0.03 mm thin, the cause is usually one function, not the machine as a whole. Maybe the compensation value was entered with the wrong sign. Maybe the feed override was pushed during a finish pass. Knowing which function owns which error is what turns a scrapped part into a corrected program.

This page covers the functions that matter most on 3-axis, 4-axis and 5-axis work. It explains what each one does mechanically, what tolerance and surface finish it can realistically hold, and when a job should be moved to a different machine or a different strategy. No formulas that only a post-processor needs. Just the engineering meaning behind each function.

Linear interpolation (G01) moves the tool along a straight line between two points. The controller splits that line into tiny segments and drives each axis to hit the endpoints at the same time. The result is a straight cut only if every axis reaches its target on schedule. On a 4,000 mm travel machine, a 2 mm segment still has to be planned, and the look-ahead buffer decides how many segments get read before motion starts.

Circular interpolation (G02/G03) fits an arc through a start point, an end point and either a radius or a center. The controller approximates the true circle with short chords. Chord error depends on feed rate and on how many blocks per second the controller can process. Push feed too high on a small radius and the arc flattens. A 5 mm radius at 3,000 mm/min will show visible faceting on an aluminum part unless the controller slows down or the programmer adds more points.

Helical interpolation combines the two. The tool follows a circle while advancing along the Z axis, which lets a single tool cut a threaded or counterbored hole without a second setup. It works well for holes up to about 1.5× the cutter diameter. Beyond that, tool deflection starts to bend the helix and the hole goes out of round.

NURBS and spline interpolation exist for curved surfaces on molds and impellers. They let the controller move along a smooth mathematical curve instead of a chain of G01 lines. The gain is a better surface finish at higher feed, and fewer program blocks. The cost is that not every controller handles splines the same way, so a program that runs clean on one machine may chatter on another.

• 1
  G01 fits straight features, flats, slots and shouldersUse when the drawing calls out a line, not an arc.
• 2
  G02/G03 fits radii, fillets and circular pocketsKeep feed moderate on radii under 10 mm.
• 3
  Helical milling replaces drilling for larger holesGood up to roughly 1.5× cutter diameter.
• 4
  Spline interpolation suits organic surfacesVerify the post-processor output on the target controller.

Cutter compensation lets the programmer write the part geometry and let the controller shift the path by the real tool radius. This is the function that keeps a re-sharpened end mill usable. Measure the new diameter, enter the value in the offset table, and the same program cuts the same size. Without it, every tool change would need a new program.

Work offsets (G54 through G59) define where the part sits in machine space. A fixture change or a second vise is a coordinate change, not a rewrite. This matters on multi-setup parts. A 16-station pallet system can hold several work offsets at once, so the operator loads a new part and calls a new offset instead of re-zeroing.

Tool length offsets are equally important on deep parts. A tool that is 0.02 mm short will cut a floor 0.02 mm high. On a 150 mm deep pocket, thermal growth in the spindle can add another few microns over a long run. Controllers with thermal compensation adjust the offset in real time. Controllers without it need a warm-up cycle and a mid-run check.

These three functions are the backbone of repeatability. Interpolation decides the shape. Compensation and offsets decide where that shape lands. If a part drifts from the first article to the fiftieth, the cause is almost always in this group, not in the cutting parameters.

Feed rate (F) sets how far the tool travels per minute or per revolution. Spindle speed (S) sets how fast it turns. Together they set the chip load, and chip load is what decides tool life. Too light a chip rubs the edge and work-hardens stainless. Too heavy a chip overloads the corner and snaps a small end mill. The usable window depends on material, cutter diameter and rigidity.

On aluminum 6061, a 6 mm carbide end mill at 12,000 rpm and 0.05 mm per tooth holds a clean cut with air blast. On 316L stainless, the same cutter runs closer to 3,000 rpm with a heavier chip and flood coolant. Same function, different numbers. The controller does not decide those numbers. The process engineer does, and the controller enforces them.

Adaptive feed control is a step beyond constant feed. The controller reads spindle load or servo current and raises or lowers feed to keep the tool loaded. It helps in pockets with varying engagement, where a fixed feed either bogs down in a corner or wastes time on a straight wall. It does not fix a bad strategy. If the toolpath buries the cutter, adaptive control just slows the crash.

Rigid tapping and thread milling also belong here. Rigid tapping synchronizes spindle rotation with Z travel, so the tap enters and exits at the same helix. Thread milling uses circular interpolation instead, which lets one tool cut several thread sizes and avoids a broken tap in a deep hole. For holes deeper than 3× diameter in hard material, thread milling is the safer function.

A 4th axis adds rotation around one linear axis, usually the X axis. This lets a part be cut on several faces without a new setup. A shaft with flats, cross-holes and a keyway can be finished in one program. The gain is not just speed. Every setup removed is a stack of tolerance errors removed with it.

A 5th axis adds a second rotation, either as a trunnion table or a swivel head. With both axes moving at the same time, the tool can stay normal to a curved surface. This is what makes impellers, turbine blades and complex medical housings possible in one pass. It also shortens the tool, because the machine tilts the part instead of the cutter reaching around it. A shorter tool deflects less.

Simultaneous 5-axis is not the same as 3+2 positioning. In 3+2, the two rotary axes lock and the cut happens in three linear axes. It is easier to program and more rigid. In simultaneous mode, all five axes move together, which is harder on the controller and the post-processor. If a face can be reached in 3+2, do it that way. Save simultaneous motion for true freeform surfaces.

The limit here is setup and validation. A five-axis program can look correct on screen and still collide, because the stock model and the fixture model are often simplified. Simulation with the real holder and fixture geometry is not optional. On a Ø400 mm rotary table, a swing error of 0.01 mm at the part center becomes a larger error at the edge.