Haas G-codes38 codesLathe

Haas Lathe G-code List

Turning has its own cycle numbers, and that is what separates this table from the mill's: G70 to G72 roughing and finishing, G74 and G75 pecking and grooving, G76 and G92 threading, and G96 with G50 for constant surface speed. On a Haas lathe G90 is the O.D./I.D. turning cycle and G94 end facing, not the mill meanings.

Haas Lathe G-code: 38 codes

Codes in colour link to a full page with a worked example and controller differences; the rest link to their row on the G-code list, except codes whose Haas meaning differs from that list, which have no link.

Code	Function	Notes
G00	Rapid PositioningMoves the tool at maximum speed to the specified position. Used for non-cutting moves to position the tool quickly. Movement is typically not in a straight line - each axis moves at its maximum rate independently.	WARNING: G00 moves at maximum speed. Ensure clear path to avoid collisions. Movement path may not be linear.
G01	Linear InterpolationMoves the tool in a straight line at a specified feed rate. Used for cutting operations where precise linear movement is required.	Feed rate (F) is modal - once set, it remains active until changed.
G02	Circular Interpolation CWMoves the tool in a clockwise arc. The arc center is defined by I/J/K offsets or R radius. Direction is clockwise when viewed from the positive direction of the perpendicular axis.	I/J/K are usually incremental from current position. R cannot make full circles.
G03	Circular Interpolation CCWMoves the tool in a counter-clockwise arc. The arc center is defined by I/J/K offsets or R radius. Direction is counter-clockwise when viewed from the positive direction of the perpendicular axis.	I/J/K are usually incremental from current position. R cannot make full circles.
G04	DwellPauses program execution for a specified time. Useful for chip clearing, allowing spindle to reach speed, or timing operations.	P format varies by controller: Fanuc uses milliseconds, some use seconds. Check your controller documentation.
G09	Exact Stop CheckNon-modal exact stop. Machine decelerates to a complete stop at the end of the current block only. Unlike G61, it only affects the single block it appears on.	Non-modal, only affects the block it's on. Use instead of G61 when you need exact stop at one point only.
G10	Data Setting / Offset EntryProgrammable data entry for work offsets, tool offsets, and parameters. Allows automatic offset adjustment during program execution.	Powerful but use with caution. L2 sets absolute values, some controls use L20 for incremental. Check controller documentation.
G18	XZ Plane SelectionSelects the XZ plane for circular interpolation. Arc movements will occur in the XZ plane with Y as the perpendicular axis. Common for lathe operations.
G20	Inch ModeSets the unit system to inches. All position values and feed rates will be interpreted as inches and inches per minute.
G21	Metric ModeSets the unit system to millimeters. All position values and feed rates will be interpreted as millimeters and mm per minute.
G28	Return to Reference PointReturns the machine to its reference point (machine home). Can pass through an intermediate point if coordinates are specified. Often used for safe tool changes.	CRITICAL: Always retract Z first before X/Y return to avoid crashes. G91 G28 Z0 is a common safe retract pattern.
G29	Return from Reference PointMoves from reference point through intermediate point to final position. Reverses the G28 path.	Uses the intermediate point stored by previous G28. Rarely used in modern programming.
G32	Single-Pass ThreadingCuts a single threading pass synchronized with spindle rotation. Used for custom thread profiles or when full control is needed. Multiple passes required for full thread.	Requires spindle encoder. F value is pitch, not feed rate. Use G76 for automatic multi-pass.
G50	Scaling Cancel / Max Spindle SpeedOn mills: Cancels scaling (G51). On lathes: Sets maximum spindle speed for constant surface speed mode (G96).	Function varies by machine type. On lathe, critical for CSS operations to prevent over-speed.
G52	Local Coordinate SystemSets a local coordinate system offset that is added to the active work coordinate system. Creates a temporary shift without changing the work offset.	G52 X0 Y0 Z0 cancels the local offset. Useful for pattern work.
G53	Machine Coordinate SystemTemporarily use machine coordinates for the current block only. Coordinates are interpreted relative to machine zero, ignoring work offsets. Non-modal - only affects the block it's on.	Must be used with G00 or G01. Non-modal - only affects current line.
G54	Work Coordinate System 1Selects work coordinate system 1. This is typically the primary/default work offset used for most machining operations. Origin is set during setup.	Work offset values are set in the controller. G54 is the most commonly used work offset.
G54.1	Extended Work Coordinate SystemsSelects additional work coordinate systems beyond G54-G59. Provides up to 48 additional offsets (P1-P48) for complex multi-fixture setups.	Provides 48 additional work offsets beyond the standard G54-G59. Haas uses G154 P1-P99 as an alternative syntax.
G55	Work Coordinate System 2Selects work coordinate system 2. Use for second fixture or part setup.
G56	Work Coordinate System 3Selects work coordinate system 3. Use for third fixture or part setup.
G57	Work Coordinate System 4Selects work coordinate system 4.
G58	Work Coordinate System 5Selects work coordinate system 5.
G59	Work Coordinate System 6Selects work coordinate system 6.
G61	Exact Stop ModeMachine decelerates to complete stop at each programmed point. Ensures precise positioning but slower cycle time. Use for sharp corners.	Use for accurate corners. G64 returns to cutting mode for smoother motion.
G64	Cutting Mode / Continuous PathEnables continuous path mode for smooth motion. Machine does not decelerate fully at corners, allowing faster cycle times with slight corner rounding.	Default mode on most machines. Corners may be slightly rounded based on speed.
G65	Macro CallCalls a custom macro program with optional arguments. Allows parameterized subprograms for repetitive operations.	Arguments A-Z map to local variables #1-#26. Macro must be defined on controller.
G70	Finishing CycleFinishing cycle that follows a previously defined rough profile (G71/G72). Removes the finishing allowance left by the roughing cycle with a single pass.	Must be used after G71 or G72 roughing cycle. Uses same profile blocks.
G71	Rough Turning Cycle (OD/ID)Automatic roughing cycle for turning. Removes material in multiple passes parallel to the Z-axis, leaving a finishing allowance. Used for OD and ID turning.	Two-line format on Fanuc. Profile blocks (P-Q) define the finished shape. Follow with G70 for finishing.
G72	Rough Facing CycleAutomatic roughing cycle for facing. Removes material in multiple passes parallel to the X-axis. Used for face roughing operations.	Similar to G71 but cuts parallel to X-axis. Use for parts with more facing than turning.
G74	Face Grooving / Peck Drilling Cycle (Lathe)On lathe: Peck drilling cycle in Z-axis or face grooving cycle. Plunges with pecks for chip breaking.	Different from mill G74 (left-hand tapping). On lathe, this is peck drilling/grooving.
G75	Grooving Cycle (OD/ID)One block on a Haas lathe, written with X, Z, U, W, I, K, D and F. There is no P or Q in microns as on a Fanuc.
G76	Automatic Threading Cycle (Lathe)One block on a Haas lathe, written with X, Z, U, W, I, K, A, D and F: K is the thread height and D the depth of the first pass.
G90	O.D./I.D. Turning CycleThe Haas lathe meaning, not absolute positioning. The lathe list has no G91.
G92	Threading Cycle (Simple)On lathe: Simple threading cycle for single straight or taper thread pass. Commonly used for threading operations where manual control of each pass is desired.	Simpler than G76 but requires manual programming of each pass depth. Good for learning threading.
G94	End Facing CycleNot feed per minute, which is G98 on a Haas lathe.
G95	End Face Live Tooling Rigid TapNot feed per revolution, which is G99 on a Haas lathe.
G96	Constant Surface SpeedActivates constant surface speed mode (lathe). Spindle RPM varies automatically to maintain constant cutting speed as diameter changes.	ALWAYS set G50 maximum RPM before G96 to prevent spindle overspeed at small diameters.
G97	Constant RPMCancels constant surface speed mode. Spindle runs at the programmed RPM regardless of cutting diameter.	Use for threading operations and when CSS is not appropriate.

Where Haas differs

Setting 56, M30 Restore Default G, applies on the lathe control as it does on the mill: with it on, M30 resets modal G codes to their defaults.
G154 P1 to P99 selects the extended work offsets on the lathe as well.
A G04 P dwell written with a decimal point is read in seconds: G04 P2.5 is two and a half seconds.
G50 sets the maximum spindle speed for G96 constant surface speed. The app's note says to set it before every G96, because a facing cut to centre otherwise asks for infinite RPM.
G74 is peck drilling or face grooving and G76 is the automatic threading cycle, where the same numbers on the mill are left-hand tapping and fine boring. G92 is the simple threading cycle, not the position register.
G74, G75 and G76 are single-block cycles on a Haas lathe, written with X, Z, U, W, I, K, D and F (G76 adds A), not Fanuc's two-block form with P and Q in microns. In G76, K is the thread height and D the depth of the first pass.
G27, G30, G33, G34, G66, G67 and G91 are not on the Haas lathe code list, so the table leaves them out. Feed per minute and feed per revolution are G98 and G99, with G99 the default, while G94 is the end facing cycle and G95 the end face live tooling rigid tap.
G32 single-pass threading takes F as the lead of the thread.
G18 is the working plane for arcs on a lathe; G17 is the mill default.

Frequently asked questions

Why does the lathe list have different codes from the mill list?

Turning cycles use numbers the mill assigns to other things. G74 is a peck or face grooving cycle on the lathe and left-hand tapping on the mill, G76 is the threading cycle rather than fine boring and G92 is the simple threading cycle rather than a position register. The lathe list shows the turning meaning; the Haas mill G-code list shows the other.

What does G50 do on a Haas lathe?

It caps the spindle speed for constant surface speed work. G96 raises RPM as the diameter falls, and without a G50 limit a cut to centre asks for a speed the chuck cannot hold. Program G50 S before G96 every time. See G-code list.

Do I use G76 or G92 for threading?

G76 is the automatic multi-pass cycle: one block sets the depths and passes and the control works through them. G92 is the simple cycle where you program each pass depth yourself. G76 for production, G92 when you want to see every pass.

Which units do G75 pecks use?

Not Fanuc's microns. On a Haas lathe G75 is one block written with X, Z, U, W, I, K, D and F, with no P or Q word, so the Fanuc habit of P2000 for a 2 mm (0.079 in) peck does not carry over. See G-code list.

Other controller lists

Last updated 11 Oct 2026