G90 is the single OD / ID turning canned cycle — a highly practical single repetitive canned cycle that reduces longitudinal cutting moves to a single line in CNC lathe programming. When multiple repetitive cycles (such as G71) are not needed and the roughing stock is not too large (a few passes will finish it), G90 is preferred instead of writing G01 and G00 codes one after another.
📷 IMAGE AREA — G90 square/rectangular cutting cycle: X plunge (R), Z longitudinal cut (F), X retract (F) and rapid return to the start point (R)
Suggested alt text: G90 single turning canned cycle four-move diagram
1. The basic purpose and logic of the G90 cycle
When G90 is used, the control unit automatically performs the following four basic moves (the square/rectangular cutting cycle) from the tool start point:
- Move (R): plunges in X to the target roughing-pass diameter at rapid feed (G00).
- Move (F): cuts the part longitudinally in Z at the programmed cutting feed (F).
- Move (F): when the cut reaches the final Z coordinate, the tool retracts radially outward in X so it does not rub the part surface.
- Move (R): returns at rapid feed (G00) to the safe start point it began from (travelling back in Z).
2. Standard FANUC G90 syntax and address details
The G90 cycle has a modal structure that can be repeated line by line by writing only the changing X coordinate on the following lines. The cycle can be run in two geometric models:
A) Straight (cylindrical) turning:
G90 X(U)_ Z(W)_ F_ ;
B) Taper turning:
G90 X(U)_ Z(W)_ R_ F_ ;| Address | Function |
|---|---|
| X | The absolute target diameter where the cutting pass ends. |
| U | The incremental radial distance relative to the current start point. |
| Z | The absolute final coordinate where the longitudinal cut ends axially. |
| W | The incremental axial length relative to the current start point. |
| R | In taper turning, the radius difference between the start and end diameters. In straight turning this address is omitted. |
| F | The cutting feed in mm/rev used during turning. |
3. System rules and parameters that directly affect the G90 cycle
3.1 Effect of tool-nose radius compensation (G41 / G42)
Critical rule: when a chamfer or corner radius is added to the part while the G90 canned cycle runs, tool-nose radius compensation (G41 or G42) is included directly in the cycle block behaviour. The compensation direction (right/left) is offset automatically by the control according to the tool cutting direction. However, when the canned cycle is ended, cancelling compensation with G40 while moving away from the part is a technical necessity to prevent unwanted plunges.
3.2 Flexibility to run in MDI mode
Critical distinction: according to FANUC system rules, multiple repetitive cycles such as G70, G71, G72 and G73 absolutely cannot be written or run in MDI mode (they produce P/S alarm No. 67). However, G90 (and the similar single canned cycles G92, G94) has the flexibility to be written directly in MDI mode and run with Cycle Start.
3.3 Sign directions in incremental programming
According to the system coordinate matrix, the signs (+/-) of the incremental programming addresses U, W and R depend entirely on the tool cutting-direction combination. If the tool moves toward the chuck, W must be negative (-); if it plunges toward the centre while cutting, U must be negative (-).
4. Example program: step-by-step straight rough turning
Let us rough-turn a Ø80 mm solid steel bar down to Ø75, Ø70 and finally Ø65 in sequence with the G90 cycle, over a length from the face to Z-50. Thanks to the modal structure, after the first line only the changing X diameter is written; the machine keeps the Z-50 and F0.25 values and repeats the cycle.
%
O9001 (MENTOR CNC - G90 LONGITUDINAL TURNING) ;
G21 G18 G40 G99 ;
G50 S2000 ;
T0101 ;
G96 S180 M03 ;
M08 ;
(SAFE START POINT BEFORE G90)
G00 X84.0 Z2.0 ; (Above O80 raw diameter, in front of the face)
(G90 CYCLE FIRST PASS)
G90 X75.0 Z-50.0 F0.25 ;
(MODAL: ONLY NEW DIAMETER VALUES)
X70.0 ;
X65.0 ;
(CYCLE CANCELLED, MOVE AWAY FROM PART)
G00 X200.0 Z200.0 M09 ;
M05 ;
M30 ;
%G00 X84.0 Z2.0a safe X84 above the Ø80 raw diameter and Z2 in front of the face.G90 X75.0 Z-50.0 F0.25the tool plunges to X75, cuts to Z-50 at F0.25, retracts to X84 and rapids back to Z2.X70.0andX65.0— thanks to the modal structure, the same Z-50 and F0.25 are kept and the Ø70 and Ø65 passes are performed automatically in turn.
📷 IMAGE AREA — G90 rough turning: stepped passes from the Ø80 raw diameter to Ø75 → Ø70 → Ø65 and the modal-repeat logic
Suggested alt text: G90 stepped rough turning passes example
5. Safe test and operator checklist
- Start-point safety: the rapid positioning diameter before entering the G90 cycle must always be radially larger than the largest outside diameter of the raw part. Otherwise, at the end of the first cycle the tool can hit the back of the part while retracting.
- Editing warning: during machining, while active cycle lines are executing, absolutely do not delete, add or change anything in the program; this can distort the coordinate system of the axes and cause serious mechanical damage.
- First trial: when trying the program for the first time, watch the tool path on the graphics screen or perform a dry run.
Want to try what you just learned? Use our G90 Turning Cycle Simulator and G-Code Generator to enter your own parameters, watch the live toolpath simulation and download ready-to-run G-code.