Tilted Working Plane (G68.2 / G53.1)

Most “5-axis” work is really 3+2: swing the rotary axes to a fixed angle, lock them, and machine a face that isn’t square to the table — a bore on a ramp, a pocket on an angled boss. Doing that by hand-calculating rotated coordinates is miserable and error-prone. G68.2, tilted working plane indexing, is Fanuc’s answer: you tell the control where the tilted feature’s plane is, and it builds a feature coordinate system on that plane so you can program the feature in plain X/Y/Z as if it were flat and facing up. A companion command, G53.1, then swings the rotary axes so the tool points straight into that plane. This page is derived from FANUC’s Series 30i/31i/32i-B Plus Operator’s Manual (B-64724EN), §22.6.

Defining the Feature Coordinate System

G68.2 sets an origin for the feature plane (the X_ Y_ Z_ addresses, in the current work coordinate system) and its orientation. Fanuc offers four ways to state the orientation, selected by a P code — use whichever matches how your drawing or CAD gives the angle:

All four produce the same thing: a coordinate system whose XY plane lies on the tilted feature and whose Z points out of it. From there you program the feature normally — a bolt circle, a pocket, a drill cycle — in that plane’s X/Y/Z. If one or two of X/Y/Z are omitted the control alarms (PS5457, “G68.2/G68.3 FORMAT ERROR”).

Orienting the Tool: G53.1

Defining the plane doesn’t move anything — it only sets up coordinates. G53.1, specified after G68.2, automatically controls the rotary axes to point the tool axis perpendicular to the tilted plane (“tool axis direction control”). This is the “+2” of 3+2: G68.2 handles the coordinates, G53.1 handles the indexing. On a machine whose kinematics the control knows (set by the parameters below), you don’t compute rotary angles by hand — G53.1 solves them.

A minimal 3+2 block sequence looks like: cancel any tool comp → G68.2 X.. Y.. Z.. I.. J.. K.. → G53.1 → approach and machine the feature in its plane → G69 to cancel the tilted plane.

Restrictions Worth Knowing

• Cancel tool length and radius compensation before G68.2. Commanding G68.2 while tool length or cutter compensation is active raises PS5462, “ILLEGAL COMMAND (G68.2/G69)”.
• G69 cancels the tilted working plane and returns to the ordinary work coordinate system.
• The three-point and two-vector forms are multi-block; interrupting the Q sequence raises the same PS5457 format error.
• This is a 3+2 / indexing feature — the rotaries are positioned then held. Keeping the tool tip on a path while the rotaries move during cutting is a different feature: tool centre point control (G43.4/G43.5).

G68.2 vs. G54.4 vs. G43.4 — Which Is Which

Parameters by Axis Configuration

This is where 5-axis setup actually lives, and it is configuration-dependent: the kinematics parameters you populate depend on whether the rotary axes are on the head, the table, or split between them. Parameter No. 19680 declares the type, and that decides which vector parameters matter (FANUC B-64730EN §4.98). Leave the wrong ones at zero and G53.1 either alarms or puts the feature plane in the wrong place. These are machine-tool-builder settings.

The axis pair — AB, AC, BC — is set by direction codes, not by picking offset components. It’s tempting to think “a BC machine uses these components of the intersection offset, an AC machine those.” That’s kinematically intuitive but not how Fanuc encodes it: the pair lives in the axis-direction parameters, while the offset vectors are always the full measured geometry (below). No. 19682 gives the direction of the first rotation axis and No. 19687 the second — each coded 1 = X (an A-axis), 2 = Y (a B-axis), 3 = Z (a C-axis):

(Codes 4–6 are inclined axes for a nutating head.) Rounding out the identities: No. 19681 / 19686 (which controlled axis is 1st / 2nd rotary), No. 19684 / 19689 (each axis’s rotation direction — normally 0 for a tool axis, 1 for a table axis), No. 19657 (master rotation axis), No. 19696 (rotary configuration — invalid here and the control runs as a 3-axis machine), and No. 1006 #0 (mark those axes as rotation axes). Then the position/offset vectors, which depend on the machine type:

Each of these is a full three-component vector obtained by measurement with every rotary axis at 0°, not a per-axis-pair subset: 19700–19702 is machine origin → a point on the 1st table axis; 19703–19705 is that point → a point on the 2nd table axis; on the head side 19709–19711 runs tool-tip point → a point on the tool rotation axis and 19712–19714 the 2nd → 1st tool-axis points. The rule of thumb: the position vectors must be populated for the feature to work at all; the axis-intersection offsets (19703–19705 / 19712–19714) are the accuracy dial-in for a real machine whose two rotaries don’t perfectly cross. The behavioural bit parameters in §4.98 (angle interpretation, singular-posture handling, retract) are MTB-configured — see the parameter manual.

See also: the cross-control overview of 3+2 and 5-axis is in 4th/5th Axis, Tilted Work Planes & TCP. The same idea on other controls: Siemens uses CYCLE800 (swivel plane) and Heidenhain the PLANE function. Neighbouring Fanuc features: tool centre point control (G43.4/G43.5) and workpiece setting error compensation (G54.4).

Sources: FANUC Series 30i/31i/32i-MODEL B Plus Operator’s Manual (Common to Lathe/Machining Center), B-64724EN/01 — §22.6 Tilted Working Plane Indexing; and FANUC Parameter Manual B-64730EN/01 — §4.98 Parameters of Tilted Working Plane Indexing Command.