Resolving Fanuc PS0062 Alarm: Illegal Depth in Rough Cut Cycles

Introduction

When a CNC lathe turret rapidly indexes and approaches a raw steel billet for a high-volume roughing run, a single mistyped character in the depth of cut parameter can instantly trigger a PS0062 alarm, locking the machine controller and halting production. If the operator attempts to bypass these canned cycle alarms without resolving the underlying coordinate boundaries, the tool nose can plunge directly into the chuck jaws or tailstock, causing a severe mechanical collision that scatters carbide fragments and damages the spindle bearings. During multiple repetitive cycles like G71 or G72, the lathe is subjected to intense, continuous cutting forces that demand absolute rigid workholding and precise toolpath definition. A failure to clamp the workpiece correctly or an error in setting up software barriers can result in the part shifting inside the chuck, leading to immediate dimensional scrap or total tool destruction.

While some controller faults, such as a paper-tape reader error, can be resolved using a standard TH error resolution procedure, canned cycle errors demand deep parameter inspection. Similarly, physical collisions or axis-overloads can result in a hardware-level excess velocity alarm if the turret slams into a tailstock barrier. For PLC-related clamp issues, operators must also monitor diagnostic tools to identify specific PMC alarms that might indicate incomplete clamping sequence signals.

Technical Summary

Technical Attribute	Details / Values
Command Code	G71, G72, G71.7, G72.7
Modal Group / Modality	Multiple repetitive canned cycles (Lathe Group 00 / Non-modal)
Supported Brands	Fanuc (T Series and M Series)
Critical Parameters	Parameter 0001 bit 1 (FCV), Parameter 5107 bit 0 (ASU), Parameter 5108 bit 1 (DTP), Parameter 5108 bit 3 (NSP)
Main Constraint	The depth of cut parameter must strictly be a positive, non-zero value; the first block of the shape program must command G00 or G01.

Quick Read

• Always verify that the depth of cut parameter in multiple repetitive cycles is defined as a positive, non-zero value to prevent the PS0062 controller alarm.
• Insert either a G00 or G01 linear motion command in the first block of the target shape profile (the block matching sequence number P).
• Activate Type II roughing for non-monotonic profiles by specifying movement commands along both the Z (or W) and X (or U) axes in the first contour block.
• Utilize G71 and G72 cycle commands for T Series lathe operations, and apply G71.7 and G72.7 specifically for M Series machining centers.
• Configure the FCV bit in parameter 0001 to toggle backward compatibility, shifting the cycle syntax to interpret address D as the escape amount.
• Verify tailstock and chuck boundaries in the controller configuration to guarantee the turret path does not violate physical zone limits.

Basic Concepts

When programming the G71 or G72 roughing cycles, programmers and operators must strictly verify that the defined depth of cut is a positive, non-zero value. A common failure cause during setup is an incorrectly typed depth value, such as zero or a negative value, which directly triggers the PS0062 alarm code and prevents the machine from starting the cycle. Beyond basic syntax, safe operation requires a comprehensive review of the physical setup, including verifying the chuck and tail stock barrier parameters to prevent the tool from crossing safe zones during automated roughing.

The geometry of the target profile requires equally close attention, as the control stringently monitors the toolpath for safety. If the specified path does not continuously increase or decrease in the required axes, the machine will halt and generate a PS0064 or PS0329 alarm code to prevent unpredictable cutting behavior. A practical programming effect is available if a CAD/CAM system generates a microscopic non-monotonic step; operators can configure an unsigned allowable value in the control parameters to clamp this allowance to the specified depth of cut, permitting the cycle to execute safely without triggering an alarm. Operators must also watch for improper tool nose radius compensation; applying G41 or G42 incorrectly on the blank side during a G71/G72 cycle will trigger the PS0328 alarm code, preventing severe overcutting.

Fanuc controls exhibit several distinctive behaviors in multiple repetitive cycles compared to other brands. First, the control relies on a highly specialized axis-command trigger to dynamically switch between Type I (strictly monotonic) and Type II (non-monotonic) roughing logic; commanding both the Z (or W) and X (or U) axes simultaneously in the very first block of the shape profile seamlessly activates Type II without requiring a unique G-code. Second, the system heavily distinguishes its cycle commands by machine type, utilizing G71.7 and G72.7 for M Series machines while keeping G71 and G72 exclusive to T Series lathes. Finally, the control offers profound backward compatibility through structural parameter changes; flipping a single bit (FCV in parameter 0001) fundamentally alters the address structure of the cycle to the older Series 15 format, changing the machine to interpret Address D for tool escape amounts instead of the modern P and Q addresses.

Command Structure

The syntax of Fanuc's multiple repetitive cycles revolves around defining a specific sequence of block numbers that map out the target profile. The start and end of this profile are designated by sequence numbers P and Q, which are non-modal addresses read by the canned cycle controller to compute the depth, direction, and number of passes required. The depth of cut, typically specified under address U (for G71 radial depth of cut on older single-line systems) or in a preceding block's address D, tells the control exactly how much metal to remove in each pass.

Depending on the active format configured in parameter 0001 (FCV), the address mapping changes significantly. Under the standard format, the cycle executes roughing passes and leaves finishing allowances specified by U (for the X-axis) and W (for the Z-axis) before returning the tool to the starting position. In Series 15 compatibility mode, address D controls the escape amount at the bottom of each cut. Programmers must ensure the initial block of the shape program contains a G00 or G01 command to set the starting interpolation mode, otherwise the controller halts execution immediately.

; Standard Two-Line Format (G71/G72)
G71 U[depth of cut] R[escape amount] ;
G71 P[start block] Q[end block] U[X finishing allowance] W[Z finishing allowance] F[feedrate] ;

; Series 15 Format (FCV parameter set to 1)
G71 P[start block] Q[end block] U[X allowance] W[Z allowance] D[escape amount] F[feedrate] ;

Parameter Address	Technical Description	Value / Range Specification
P	Start block sequence number defining the finishing profile contour.	Positive integer (e.g., 100)
Q	End block sequence number defining the finishing profile contour.	Positive integer (e.g., 200)
U (1st block)	Depth of cut per roughing pass (radial value in G71).	Positive decimal (must be non-zero)
R (1st block)	Escape amount (relief amount) after each roughing pass.	Positive decimal
U (2nd block)	Finishing allowance in the X-axis direction (diameter/radial depending on system).	Decimal value (positive or negative)
W (2nd block)	Finishing allowance in the Z-axis direction.	Decimal value (positive or negative)
D	Tool escape amount at the cutting bottom (used in Series 15 format).	Positive decimal
F	Feedrate specified for the roughing passes.	Decimal value (mm/rev or mm/min)

Brand Applications

Fanuc

Fanuc control systems implement multiple repetitive cycles by checking the modal G-code system and machine configuration. For T Series lathes, G71 and G72 roughing cycles are modal within Group 00, processing outer diameter and end-face profiles respectively. In contrast, M Series machining centers running lathe-like configurations require G71.7 and G72.7.

The transition between Type I and Type II roughing is entirely implicit: commanding both X (or U) and Z (or W) axes in the sequence block P triggers Type II, enabling the control to rough out non-monotonic profiles with pockets. When G41 or G42 nose compensation is active, parameter 5106 bit 2 (NT1) regulates if an alarm triggers or if the command is quietly bypassed inside the canned cycle profile definition.

Brand Comparison

Feature / Parameter	Fanuc Series 16i / 18i / 21i	Fanuc Series 0i	Fanuc Series 15i
Default Cycle Format	Standard 2-line format (G71/G72 with P, Q, U, W, R)	Standard 2-line format (G71/G72 with P, Q, U, W, R)	Series 15 1-line program format (utilizes Address D for escape amount at cutting bottom)
Format Switching Capability	Supported via Parameter 0001 bit 1 (FCV) to emulate Series 15 structure	Supported via Parameter 0001 bit 1 (FCV) to emulate Series 15 structure	Native Series 15 format (D address used for escape, does not require 2-line syntax)
M-Series Support	G71.7 and G72.7 commands for multi-tasking and M-series controls	G71.7 and G72.7 commands for modern multi-tasking controls	Requires standard G71/G72 or specific M-series emulated cycle calls
Type II Path Control (NSP)	Parameter 5108 bit 3 (NSP) toggles path execution method	Parameter 5108 bit 3 (NSP) toggles path execution method	Older native path control logic managed via system parameters

Technical Analysis

The analytical differences between Fanuc model series depend heavily on the evolution of their control formats and parametric settings. On contemporary controls like the Series 16i, 18i, 21i, and Series 0i, the standard two-line G71 command structure is default. The first block dictates depth of cut (U) and escape amount (R), while the second block provides coordinates and allowance parameters. However, in the Series 15i control, a singular G71 block is processed natively where address D is explicitly parsed for the escape amount at the cutting bottom. Programmers operating a mixed shop floor with both modern Series 0i and older Series 15 machines can force modern controllers to emulate the older single-block format by switching the FCV bit (Parameter 0001 bit 1) to 1. This parameter change shifts the interpreter, preventing syntax alarms when running legacy programs.

Parameter 5108 bit 1 (DTP) and Parameter 5108 bit 3 (NSP) further differentiate path control and return behavior. When running a Type I monotonic cycle, the DTP parameter determines if the turret returns to the cycle start position or directly from the finishing contour's final programmed point. For Type II non-monotonic profiles, the NSP parameter controls if a conventional path is repeated or bypassed to optimize execution time. Additionally, modern Series 16i/18i/21i controllers support the NT1 bit in parameter 5106, which manages tool-nose compensation commands inside the figure program. Setting NT1 to 0 triggers an immediate alarm if G41/G42 is encountered, whereas setting it to 1 suppresses the alarm and ignores the command, shifting responsibility to the CAD/CAM post-processor.

Program Examples

; Example 1: Standard Two-Line G71 Outer Roughing Cycle (T-Series Lathe)
G54 G90 G21 G40 ;
G00 X100.0 Z5.0 ;          ; Rapid to cycle start point
G71 U2.0 R1.0 ;            ; 2.0mm depth of cut per side, 1.0mm tool relief escape
G71 P100 Q200 U0.5 W0.1 F0.25 ; ; Define profile block range, X allowance 0.5mm, Z allowance 0.1mm
N100 G01 X40.0 Z0.0 F0.15 ; ; First block of contour (Type I monotonic)
G01 Z-30.0 ;
G01 X60.0 Z-50.0 ;
G01 Z-80.0 ;
N200 G01 X90.0 ;           ; End of contour profile
G00 X150.0 Z150.0 ;        ; Retract to safe position
; Example 2: Series 15 Format G71 Cycle (Parameter 0001 FCV set to 1)
G54 G90 G21 G40 ;
G00 X100.0 Z5.0 ;
G71 P300 Q400 U0.5 W0.1 D2.0 F0.25 ; ; D2.0 defines the tool escape amount at the bottom
N300 G01 X45.0 Z0.0 ;
G01 Z-35.0 ;
G01 X70.0 Z-55.0 ;
N400 G01 X90.0 ;
G00 X150.0 Z150.0 ;

Dry Run Verification Procedure:

Before executing the cycle on a raw workpiece, operators must perform a dry run to verify command interpretation and prevent physical collisions:

1. Clamp a dummy plastic workpiece or remove the raw stock entirely, ensuring the chuck and tailstock barriers are clear.
2. Enable the Dry Run switch and Single Block mode on the machine controller panel.
3. Set the feedrate override to 0% and slowly increase it to trace the initial rapid approach to X100.0 Z5.0.
4. Step through the G71 canned cycle initialization; verify that the control reads the depth of cut without triggering a PS0062 alarm.
5. Observe the simulated turret path as it performs repetitive passes. Ensure that the tool retracts by 1.0mm (Standard format) or uses the 2.0mm escape amount defined by D2.0 (Series 15 format) at the end of each pass.
6. Confirm the final toolpath retracts cleanly back to the cycle starting point without violating the tailstock safe zones.

Error Analysis

Brand	Alarm Code	Trigger Condition	Operator Symptom	Root Cause & Resolution
Fanuc	PS0062 / Alarm 062	Depth of cut parameter (U or D) in G71/G72 cycle is set to zero or a negative value.	The controller locks up immediately upon parsing the cycle start block, preventing turret movement.	Verify that the depth of cut value (U in standard, D in Series 15) is positive and non-zero. Correct the G-code block.
Fanuc	PS0064	The target contour in a Type I roughing cycle has a non-monotonic change in the primary axis.	The machine executes the approach but halts with an alarm right before entering the profile cycle.	Enable Type II roughing by programming both primary axes (e.g., X and Z) in the block matching sequence number P, or adjust parameter 5108.
Fanuc	PS0065	The sequence block P does not contain a G00 or G01 interpolation command.	Cycle execution fails immediately at block P, flashing an alarm light on the operator panel.	Insert an explicit G00 or G01 command in the very first block (P-number block) of the shape program.
Fanuc	PS0322	The finishing shape profile coordinate boundary extends beyond the cycle starting coordinate point.	Turret motions halt mid-cycle or before the initial plunge, showing coordinates limit exceeded.	Adjust the initial G00 rapid start position (X/Z) so that it lies completely outside the target contour envelope.
Fanuc	PS0328	The blank side selection for tool-nose compensation (G41 or G42) is incorrect inside the cycle.	The control generates a tool nose R compensation alarm, refusing to execute the shape path to prevent overcutting.	Correct the blank side selection parameters or ensure that G41/G42 directions align with the raw material boundary, or configure NT1 in parameter 5106.

Application Note

Heavy cutting forces generated during multiple repetitive canned cycles will rip a raw steel billet out of the chuck if the operator fails to confirm the workpiece clamp signal before initiating the G71 profile. A major setup mistake—such as typing a zero or negative value for the radial depth of cut—will instantly trigger the PS0062 alarm code, blocking the turret from starting the machining run. To avoid physical tool crashing or scraping expensive workpieces, programmers must strictly align the start coordinates with the physical boundaries of the chuck and tail stock barrier parameters. In high-precision shops where CAD/CAM post-processors introduce microscopic non-monotonic steps into monotonic profiles, setting an unsigned allowable value in the parameter register clamps this allowance to the active depth of cut, letting the controller execute the toolpath safely without halting. Furthermore, adjusting parameter 5106 bit 2 (NT1) to suppress nose compensation errors represents a critical control optimization, preventing unexpected alarms when G41 or G42 commands are read in the profile program.

Related Command Network

• G70: Executes the finishing pass following the exact sequence blocks P and Q defined in the G71 roughing cycle.
• G72: Performs end-side (facing) rough-cutting cycles using the same parametric logic as G71 but roughing along the X-axis.
• G73: Executes pattern repeating cycles designed for pre-formed parts like castings or forgings, where metal removal follows a constant offset profile.

Conclusion

Achieving error-free multiple repetitive roughing requires checking the depth of cut parameters, contour monotonicity, and controller-specific settings before cycling the machine. Operators should systematically run dry tests with single block mode enabled to verify the turret's escape behavior and spatial limits relative to physical workholding. Taking these proactive steps keeps the production floor running continuously without unexpected alarms or mechanical tool collisions.

FAQ

How can I resolve a PS0062 alarm on a Fanuc lathe?

A PS0062 alarm triggers when the controller detects a zero or negative depth of cut in the G71 or G72 canned cycle blocks. To resolve this, examine your program and ensure the U address (first line of modern double-line syntax) or the D address (in Series 15 format) is set to a positive decimal value larger than zero. Always review your active program format using parameter 0001 (FCV) to confirm the controller is parsing the correct address for the depth value.

Why does my canned cycle halt with a PS0064 alarm when cutting curves?

The PS0064 alarm occurs when the canned cycle profile contains a non-monotonic path (a profile that dips or changes direction) in a Type I monotonic cycle. To fix this, enable Type II roughing by explicitly commanding movements along both the X and Z axes in your contour's starting N-block (e.g., N100 G01 X40.0 Z0.0). Alternatively, configure an unsigned allowable non-monotonic step value in the parameters to let the machine clamp microscopic deviations up to the depth of cut value without raising an alarm.

What is the difference between standard G71 and G71.7 commands?

The standard G71 command is dedicated to T Series lathe controllers for outer surface roughing, whereas G71.7 is a specialized variant engineered for M Series machining centers with turning capabilities. If you receive a syntax alarm when migrating programs between machine types, check your controller series configuration and adjust the canned cycle command suffix accordingly. Always run a dry run with single block mode active to confirm the machine's interpreter supports the selected cycle command.