G94 is the facing canned cycle — the transverse turning canned cycle used to remove roughing stock from the face of the part or to form stepped face surfaces. While the G90 cycle makes its cutting moves parallel to the Z axis (longitudinal), G94 performs its main cutting and pass moves parallel to the X axis (toward the face).
📷 IMAGE AREA — G94 face-cutting cycle: Z plunge (rapid), cut from diameter to centre in X (F), axial retract and rapid return to the start point
Suggested alt text: G94 facing canned cycle four-move diagram
1. The basic purpose and working dynamics of the G94 cycle
When the G94 command line is read, the cutting tool performs the following four automatic moves (the square/rectangular face-cutting cycle) in sequence from the start point:
- Move (rapid – R): approaches the programmed target face-pass depth in Z at rapid feed (G00).
- Move (cut – F): removes stock in X (from the diameter toward the centre) at the cutting feed (F) up to the specified final coordinate.
- Move (cut – F): when the cut ends, it makes a micro axial retract from the part in Z so the tool does not rub and mark the face surface.
- Move (rapid – R): at G00 speed it automatically returns to the first safe start coordinate where the cycle was called.
G94 is a modal code. Once the cycle is called, writing only the axially decreasing new Z depth values on the following lines makes the machine keep facing automatically at the same diameter (X) and the same feed (F).
2. Cycle code name by G-code system (A/B/C)
| Code system | Facing cycle code |
|---|---|
| System A (most common) | G94 |
| System B | G79 |
| System C | G24 |
On the vast majority of FANUC lathes in workshops, System A (G94) is active; however, when a program is taken from another machine, the code system must always be verified.
3. Standard syntax and address details
A) Straight facing:
G94 X_ Z(W)_ F_ ;
B) Tapered (angled toward the front) face cut:
G94 X_ Z(W)_ I_ F_ ;| Address | Function |
|---|---|
| X | The absolute final coordinate (along the diameter) where the facing cut ends. |
| Z | The absolute target length where the face pass is taken axially. |
| W | The incremental axial depth-of-cut distance relative to the start point. |
| I | On face cuts tapering toward the front, the taper/angle difference along the X axis (radius). Omitted on straight facing. |
| F | The feed in mm/rev used during cutting. |
4. System parameters and critical warnings that directly affect the G94 cycle
4.1 Tool-nose radius compensation (G41 / G42) compatibility
When a chamfer or corner radius is machined on the face while G94 runs, tool-nose radius compensation (G41 / G42) is included directly in the calculation behaviour by the system control; the offset is applied automatically according to the tool cutting direction. When the cycle is ended, compensation must be cancelled with G40 at the cycle exit to prevent plunge alarms during the rapid return to the start point.
4.2 Hardware and version limitation (I/K addresses and FS10/11)
According to the source manual details, the I and K addresses cannot be used directly for a canned cycle in the standard CNC tape format. However, if your control is configured in the advanced FS10/11 command format (FANUC Series 10 / 11), the active use of the taper-cut addresses is fully supported by the system.
4.3 Data-clearing and cancel protocol
While G94 is active, if any one-shot G code other than dwell (G04) or a G90 or G92 cycle code from Group 01 is entered, the modal X and Z data belonging to the G94 cycle is cleared from memory entirely for safety. If it is to be reused, all addresses must be defined again.
5. Fully detailed example program (Ø160 flange face roughing)
We rough the face of a Ø160 mm solid flange by stepping to Z-2.0, Z-4.0 and Z-6.0 axial passes in turn; the tool faces down to a Ø40 mm diameter. Thanks to the modal structure, after the first pass only the decreasing Z values are written.
%
O9401 (G94 FACE ROUGH TURNING) ;
G21 G18 G40 G99 ;
G50 S1500 ;
T0101 ;
G96 S160 M03 ;
M08 ;
(SAFE APPROACH BEFORE G94)
G00 X164.0 Z3.0 ; (Part O160, safe X164 and Z3 in front of the face)
(G94 CYCLE FIRST PASS)
G94 X40.0 Z-2.0 F0.25 ;
(MODAL REPEAT: ONLY DECREASING Z PASSES)
Z-4.0 ;
Z-6.0 ;
(EXIT G94 MODE)
G00 X200.0 Z200.0 M09 ;
M05 ;
M30 ;
%G00 X164.0 Z3.0a safe X164 and Z3 in front of the face for the Ø160 part.G94 X40.0 Z-2.0 F0.25the tool approaches Z-2, faces to X40 at F0.25, retracts to Z3 and rapids back to X164.Z-4.0andZ-6.0— thanks to the modal structure, the same X40 and F0.25 are kept and the Z-4 and Z-6 passes are performed automatically in turn.
📷 IMAGE AREA — G94 face roughing: Ø160 flange, X164 safe approach, decreasing Z-2 → Z-4 → Z-6 face passes and the X40 target diameter
Suggested alt text: G94 flange face roughing decreasing passes example
6. Safe test and operator checklist
- Z start position: the rapid positioning Z length before entering G94 must always be in the plus (+) direction, away from the raw face of the material. Otherwise, at the start of the first cycle the tool plunges rapidly into the part in Z and breaks the insert.
- X axis limit: when writing the target X value, account for the part pre-drilled hole diameter (if any) or the insert bottom-clearance limit. On solid material, if facing down to the centre, X0 is written; but to avoid leaving a pip at the exact centre, going into the minus by the radial tool-nose radius (e.g. X-1.6) is more correct from an engineering standpoint.
- First trial: watch the tool path on the graphics screen or perform a dry run.