Interpolation operations of the CNC system

• 1
  What interpolation operations of the CNC system actually do
• 2
  Linear, circular and spline interpolation
• 3
  How servo loop type changes interpolation accuracy
• 4
  Settings that decide the real path
• 5
  Which interpolation type fits which geometry

A part program only lists key points: the start of a cut, a corner, the end of a contour. The tool has to travel the whole path between them. Interpolation is the function that computes thousands of intermediate positions and feeds them to the axes as coordinated motion commands. Every axis moves at its own feed rate so the tool tip follows the intended curve.

The control recalculates these intermediate points on a fixed cycle, often 1 ms to 4 ms. At a feed of 3,000 mm/min that is roughly 0.05 mm to 0.20 mm of travel per cycle. Shorter cycles give a smoother path and a tighter following error; longer cycles show up as facets on a curved wall.

Interpolation is not a suggestion box. It is a hard constraint on accuracy. If the control cannot resolve the curve fast enough, the servo lags, and the cutter leaves the nominal path. This is why a machine with good mechanicals but a slow control still cuts a wavy surface.

Two numbers matter when you read a control spec. The interpolation period tells you how often the path is recomputed. The block processing time tells you how fast the control digests new G-code lines. A control that stalls on dense CAM output will stutter even with a short interpolation period.

• 1
  Interpolation period1–4 ms is typical on modern machining centers.
• 2
  Block processingDense CAM output can starve a slow control.
• 3
  Following errorLag between commanded and actual axis position.

Linear interpolation moves the tool along a straight line between two points. G01 is the code. It is the workhorse of every program: face milling, pocket clearing, straight walls. The math is simple, so the control handles it at full feed with almost no path error. If a feature can be cut with straight moves, cut it that way.

Circular interpolation fits an arc through a start point, an end point and a center or radius. G02 and G03 drive it. The control resolves the arc into short chords, so the surface is not a true circle but a polygon with very fine sides. On a 50 mm radius, a 0.01 mm chord height error shows up as a scallop you can measure with a profilometer.

Spline interpolation fits a smooth curve through a series of points. G06.2 and similar codes on Fanuc-style controls, plus NURBS options on other brands, let the control blend multiple points into one continuous motion. This removes the corner hesitation you get when a CAM system posts thousands of tiny G01 moves along a free-form surface.

The choice is not about which algorithm is better. It is about what the geometry needs. Straight walls and flat faces want G01. Bolt circles, fillets and O-ring grooves want G02 or G03. Turbine blades, impeller vanes and organic housings want spline or NURBS, because the point density from CAM would otherwise choke the control.

Open-loop control sends pulses to the motor and assumes the axis arrived. There is no position feedback, so nothing corrects a missed step. It is cheap and fast on light loads, but it cannot hold tolerance on a heavy cut. On a part that needs ±0.005 mm, open loop is not the right tool.

Semi-closed loop reads a encoder on the motor or the ball screw. It corrects for motor slip and screw rotation error, but it does not see the table itself. Thermal growth in the screw, backlash in the nut and flex in the frame stay invisible. Most general-purpose vertical mills run this way and do fine work within their thermal envelope.

Closed loop reads a linear scale mounted on the moving axis. It sees the table position directly, so screw pitch error and thermal growth get corrected in real time. This is what lets a machine hold ±0.005 mm through a long cut or a warm spindle. The trade-off is cost and more setup care on the scale.

The loop type sets the ceiling on what interpolation can deliver. A perfect interpolation algorithm on an open-loop machine still produces an imperfect part. When a drawing calls for tight true position on a curved contour, ask what feedback the machine has before you blame the CAM output.

Acceleration and deceleration constants shape how the tool enters and leaves a cut. Set them too aggressive and the servo overshoots the corner. Set them too soft and the machine rounds every internal corner the CAM system tried to keep sharp. A typical machining center runs 300 mm/s² to 800 mm/s² on the linear axes, lower on the rotary.

Look-ahead is the control's ability to read ahead in the program and slow down before a tight corner. Without it, the machine enters a corner at full feed and overshoots. With 50 to 200 blocks of look-ahead, the control plans the deceleration curve and holds the corner within a few microns.

Servo gain is the other knob. Higher gain tracks the commanded path more closely but can chatter or buzz. Lower gain is stable but lags on fast direction changes. On a five-axis cut with a Ø400 mm rotary table, gain that is fine on a three-axis job can be too hot once the rotary axes are also moving.

Thermal drift is the slow error. A spindle that has run for two hours grows, and the tool tip moves with it. Closed-loop feedback on the linear axes does not correct spindle growth, so warm-up cycles and in-process probing still matter on tight work. On our own cells we hold ±0.005 mm and inspect 100% before shipment, but we still warm up before the first critical cut.

• 1
  Accel / decel300–800 mm/s² on linear axes is a common working range.
• 2
  Look-ahead50–200 blocks gives the control room to plan corners.
• 3
  Warm-upRun the spindle before the first tight-tolerance feature.