G70, G71, G72 Lathe Roughing and Finishing Cycles: Complete Guide

Introduction

If a workpiece is not rigidly secured in the clamp or vise jaw, the aggressive directional changes during G71 step-overs can pull the part out of the spindle, leading to severe machine damage. Positioning a CNC lathe tool start point too close or inside the pocket geometry of a workpiece prior to calling stock removal cycles will inevitably plunge the tool into physical machine limits, resulting in a violent hard collision against a vise jaw, clamp, chuck, or turret. This sudden physical interference during heavy roughing will instantly generate a catastrophic servo overload alarm code, shatters the cutting insert, and leaves behind a severely gouged scrap part. To mitigate these catastrophic mechanical risks, programmers must rigorously monitor the cycle start points and verify that the starting position of the tool is located outside the raw workpiece boundaries. If the tool is positioned inside the raw material or too close to convex features, severe crashes will occur when the tool rapids back to its starting clearance plane.

Technical Summary

Technical Attribute	Specification Details
Command Codes	G70 (Finishing Cycle), G71 (Longitudinal Roughing Cycle), G72 (Transverse Roughing Cycle)
Modal Group	Lathe Roughing and Finishing Canned Cycles (Non-modal group 00 / one-shot execution)
Supported Brands	Fanuc, Siemens, Mitsubishi
Critical Parameters	Parameter No. 5146 (Fanuc: unmonotonous shape deviation), MD20360 (Siemens: plane G-code retention priority), Parameter #8051 (Mitsubishi: global depth of cut)
Main Constraint	The first movement block of the contour profile (P block) must be a linear command (G00/G01); circular interpolation (G02/G03) at the contour start is strictly prohibited. Calling cycles in Manual Data Automatic (MDA) mode is barred in Siemens controls (Alarm 14011).

Quick Read

• Spatial Positioning: Position the tool start coordinate safely outside the raw workpiece boundary to define a secure clearance retract plane.
• Monotonic Constraints: Design the Type I contour path to travel in a strictly increasing or decreasing direction to prevent non-monotonic profile alarms.
• Compensation Inhibition: Suspend tool nose radius compensation (G40) during G71/G72 roughing, and reapply (G41/G42) only during the G70 finishing cycle.
• Block Formatting: Choose between conventional two-block and proprietary single-block syntax structures based on the specific brand parameter configurations.
• Instruction Placement: Place the G71/G72 canned cycle command blocks before the physical contour definition blocks to avoid triggering infinite program loops.
• Active Mode Check: Execute fixed turning cycles exclusively in standard Automatic mode, as Siemens controls prohibit execution in Manual Data Automatic (MDA) mode.

Basic Concepts

The practical programming effect of utilizing G71, G72, and G70 cycles is the elimination of massive amounts of manual G-code writing. Instead of programming dozens of individual passes to rough out a stepped shaft or faced disk, the programmer only defines the final geometric profile of the part, and the CNC automatically calculates dozens of necessary roughing passes. The controller mathematically works backward from this finished shape, calculating all intermediate roughing passes automatically based on the specified depth of cut and retract parameters. This automation significantly reduces programming errors and streamlines the creation of optimized turning paths.

When applying these cycles, programmers and operators must actively watch the modal state of their tool nose radius compensation (G40, G41, G42). During the roughing cycles (G71, G72), the CNC automatically suspends tool radius compensation so that the uncompensated rough tool path leaves an exact, uniform layer of finishing allowance over the part. Once the G70 finishing cycle is invoked, the control reapplies the compensation to cut the final precise dimensions. Managing this transition correctly prevents geometry mismatches and ensures critical dimensions remain within tolerance.

Programmers must ensure that the starting position of the tool is located outside the raw workpiece boundaries. If the tool is positioned inside the raw material or too close to convex features, severe crashes will occur when the tool rapids back to its starting clearance plane. A common failure cause when using these cycles is the improper spatial designation of the cycle start point prior to issuing the G71 or G72 block. Safe use dictates that the cycle start point must be placed sufficiently far away from the rough material blank, as the machine uses this exact coordinate as its rapid retract clearance plane after every roughing pass.

Command Structure

The syntax for compound lathe cycles is historically split between standard ISO two-block formats and proprietary single-block configurations. In standard two-block syntax, the first block acts as a setup line that configures the depth of cut per pass and the retraction clearance amount for chip breaking and tool relief. These two settings remain modal throughout the roughing cycle until overwritten or completed.

The second command block specifies the physical contour sequence markers alongside finishing allowances and technological feed data. The start and end points of the contour are flagged by specific sequence numbers, while independent coordinate registers define stock thickness left for the subsequent finishing pass. When executing the cycle, the controller ignores speed and feed variables defined inside the contour block, utilizing only the main cycle parameters during roughing passes.

; ISO Standard Two-Block Syntax:
G71 U[depth] R[retract];
G71 P[start_seq] Q[end_seq] U[allowance_x] W[allowance_z] F[feed] S[speed] T[tool];
G70 P[start_seq] Q[end_seq];

Address Character	Functional Description	Technical Details & Units
U (1st Block)	Depth of cut per pass (depth)	Radial value specified in mm or inches depending on system units.
R (1st Block)	Relief/escape amount (retract)	Radial retraction distance for tool relief and chip breaking.
P (2nd Block)	Start sequence number of finishing profile	Corresponds to the starting N-block number of the contour.
Q (2nd Block)	End sequence number of finishing profile	Corresponds to the ending N-block number of the contour.
U (2nd Block)	Finish allowance in X-axis (allowance_x)	Diameter or radius stock left on the X-axis for finishing.
W (2nd Block)	Finish allowance in Z-axis (allowance_z)	Stock allowance left on the Z-axis for finishing.
F	Machining feedrate	Roughing feedrate specified in mm/rev or mm/min.
S	Spindle speed	Constant surface speed or RPM active during roughing.
T	Tool selection	Specifies the roughing tool geometry and offset index.

Brand Applications

Fanuc

Fanuc controls rely heavily on a rigid two-block format to specify turning and facing cycles. The machine kinematics determine which commands are active; lathes use standard G71 commands, whereas machining centers assign equivalent cycles to G71.7 to execute outer surface rough machining.

The classic G-code structure for a longitudinal roughing pass and subsequent finish profile call is programmed as follows:

G71 U2.0 R1.0;
G71 P100 Q200 U0.5 W0.1 F0.25;
G70 P100 Q200;

To control profile checks and alarm parameters, the control system relies on dedicated parameter registers. For example, Parameter 5146 sets the allowable deviation for unmonotonous shape profiles, while Parameter 5104 bit 2 manages the pre-machining check status.

Category	Item Code	Technical Description / Operation Details
System Parameter	Parameter No. 5146	Defines the allowable value for an unmonotonous shape in G71 and G72. Real path range from 0 to depth of cut.
System Parameter	Parameter No. 5104.2 (FCK)	Determines if the machining profile is checked before cycle begins. 0: Not checked, 1: Checked.
System Parameter	Parameter No. 5102.2 (QSR)	Checks for existence of contour end block Q before starting. 0: Not made, 1: Made.
System Parameter	Parameter No. 5107.0 (ASU)	Specifies if rapid traverse (1) or cutting feed (0) is used to return to the last turning start coordinate.
Alarm Code	PS0064	Monotonic change check failed. Finishing profile does not continuously increase or decrease in Type I cycle.
Alarm Code	PS0322	Finishing shape exceeds starting point. Cycle start coordinate falls short of maximum contour boundary.
Alarm Code	PS0063	Sequence number specified in address Q cannot be found in the active main program when QSR check is enabled.
Kinematics Option	T vs M Series	T-series lathe uses standard G70/G71/G72. M-series machining centers morph these assignments to G70.7/G71.7/G72.7.
Format Version	FS15-TA format	Legacy programming format where roughing allowances I and K in G71/G72 are ignored by the control.

Warning: Misconfiguring Parameter 5107 to pull out at rapid traverse can cause a severe hard collision with the chuck, tail stock barrier, or turret. This configuration error instantly destroys the tool and results in a ruined scrap part.

Siemens

Siemens Sinumerik controls execute G71 commands by capturing the variables through internal system parameters. The controller silently routes these dialect inputs into native Siemens shell cycles such as CYCLE371T for longitudinal roughing.

The standard ISO-dialect syntax programmed in Siemens environment for turning roughing and finishing passes is written as:

G71 U2.0 R1.0
G71 P80 Q120 U0.5 W0.2 F200
G70 P80 Q120

Siemens isolates programmed variables in background channel parameters, ensuring a G71 cycle does not overwrite variables for G72. It also features dynamic dialect shifting to morph cycles depending on the active G-code system.

Category	Item Code	Technical Description / Operation Details
System Parameter	SD55410	$SCS_MILL_SWIVEL_ALARM_MASK controls display of swivel alarms in CYCLE800 (32-bit DWORD).
System Parameter	SD55221	Bit 5 manages technology constraints when geometry axis Y is missing (0 or 1 bit flag).
System Parameter	MD20360	$MC_TOOL_PARAMETER_DEF_MASK Bit 18 controls tool plane G-code retention priority during plane changes.
System Data	GUD registers	Captured variables are stored in Global User Data registers (such as _ZFPR) before shell execution.
Alarm Code	Alarm 14011	Fixed cycles G70 to G73 are programmed or executed inside Manual Data Automatic (MDA) mode.
Alarm Code	Alarm 61805	Absolute and incremental coordinates programmed simultaneously in intermediate Siemens shell contour blocks.
Alarm Code	Alarm 61801	Incorrect value programmed in cycle call or incorrect setting data in active G-code system.
ISO Dialect Mode	System Dialects	Systems A and B map to standard codes. System C maps G70 to G72, G71 to G73, and G72 to G74.

Warning: Attempting to program subroutine call M98 or end subroutine M99 inside the NC blocks defined by sequence markers P and Q is strictly prohibited during cycle execution. This invalid command causes the Siemens underlying shell cycle to fail and halt.

Mitsubishi

Mitsubishi systems offer highly flexible turning cycle architectures, featuring standard two-block command lines alongside a proprietary single-block configuration. This allows the depth of cut and retract amounts to be stored globally in system memory.

Standard two-block format and custom single-block formats (MITSUBISHI CNC Special Format) are command structured as:

; Conventional 2-Block:
G71 U3.0 R1.0 H0 ;
G71 P100 Q200 U0.5 W0.2 F0.25 ;
; Proprietary 1-Block:
G71 P100 Q200 U0.5 W0.2 D2.0 F0.3 ;

Global parameters like parameter #8051 and parameter #8052 act as reversible registers. Programming the U and R addresses dynamically writes directly to these parameter slots in real-time.

Category	Item Code	Technical Description / Operation Details
System Parameter	Parameter #8051	G71 THICK stores the global depth of cut for roughing cycles. Setting range: 0 to 99999.999 mm.
System Parameter	Parameter #8052	G71 PULL UP stores the global retract amount when returning to cycle start. Range: 0 to 99999.999 mm.
System Parameter	Parameter #1270	ext06/bit2 determines if shape search starts from top (0) or matches stored main/seq numbers (1).
System Parameter	Parameter #1265	ext01/bit0 selects between conventional two-block format (0) and special one-block format (1).
Alarm Code	P32	Address R or A commanded inside G71/G72 when special 1-block format is selected via parameter #1265.
Alarm Code	P33	First setup block of compound lathe cycle is omitted when conventional two-block format is selected.
Alarm Code	P204	Sequence numbers P and Q are both omitted when finished shape profile is stored in the same main program.
Kinematics Option	L vs M System	On L-systems G70-G76 function as compound turning cycles. On M-systems G70-G89 map to drilling and tapping.
External Reference	A Address	Allows alphanumeric external subprogram calls by enclosing filenames in angle brackets (e.g., <PROFILE>).

Warning: Omitted starting and ending sequence numbers P and Q while storing the finished shape profile in the main program triggers an immediate P204 alarm. This program error interrupts machining and locks execution until addresses are designated.

Brand Comparison

Feature Comparison	Fanuc Control System	Siemens Sinumerik System	Mitsubishi CNC System
Underlying Engine	Directly interpreted as standard hardware canned cycles by the CNC core.	Routed into internal Siemens native shell cycles (e.g. CYCLE371T) saving variables to GUDs.	Runs as compound canned cycles using local system variables and reversible parameters.
Command Format	Strict two-block command structure.	Two-block or single-block based on cycle and system config.	Supports standard 2-block and a special 1-block format with D address for cut depth.
External Files	Must be called using standard subroutine program numbers (numeric only).	Handled via standard subprogram structures.	Streamlined alphanumeric external file contour referencing via <filename> in the A address.
Pocket Roughing	Supported in Type II cycles with continuous non-monotonic checks and parameter 5146.	Handled via advanced contour shell calculations.	Explicitly selected using pocket machining mode in the H address (0=no, 1=yes).
Machining Center Mapping	M-series systems assign equivalent cycles to G70.7, G71.7, and G72.7.	— (no source)	G70 to G76 map entirely to hole machining cycles (fine boring, tapping) on M systems.

Technical Analysis

Fanuc's architecture exhibits several highly distinct behaviors in its handling of multiple repetitive cycles. First, Fanuc dynamically shifts the base G-code designation of these cycles based on the machine type; it utilizes G71.7 and G72.7 for machining centers, but restricts standard lathes to G71 and G72, keeping the mathematical domains entirely separated. Second, Fanuc integrates a dual-tier geometric evaluation system (Type I versus Type II), actively distinguishing between simple monotonic profiles and complex profiles with pockets, and requiring different parameter configurations (such as Parameter 5105) to govern roughing passes for each type. Finally, Fanuc provides exceptionally granular parameter controls (like Parameter 5146) to mathematically bridge the gap between perfectly calculated CNC logic and imperfect CAM post-processors, allowing the machine to dynamically excuse microscopic code reversals rather than failing a cycle.

Siemens highly distinguishes its turning cycle architecture from other control brands through three advanced background behaviors. First, Siemens processes these ISO-dialect commands by silently routing them into native Siemens "shell cycles" (e.g., CYCLE371T). When an ISO G71 or G72 is read, the controller captures the variables via internal system parameters (like $C_xx) and saves them into channel-specific Global User Data (GUDs, such as _ZFPR) before calling the highly optimized Siemens standard cycles to execute the motion. This guarantees that legacy ISO programs run perfectly while utilizing Siemens' superior underlying kinematics. Second, Siemens features dynamic dialect shifting where the function of the G-code completely morphs based on the active G code system (A, B, or C). If System C is active, the G71 command abandons its roughing role entirely and instead shifts to G73/G74, preventing older programs from executing catastrophic, unintended toolpaths. Finally, Siemens structurally isolates the parameters of each unique cycle in the background memory; the programmed variables for a longitudinal roughing pass (G71) are saved independently from those of a transverse roughing pass (G72), ensuring that complex, interlinked roughing routines do not accidentally overwrite each other's cutting depths or retraction paths when alternating between cycle types.

Mitsubishi distinguishes its turning cycle architecture from other CNC brands through several highly flexible features. First, Mitsubishi heavily employs "Reversible Parameters" (such as #8051 G71 THICK and #8052 G71 PULL UP). This architecture allows the depth of cut and retract amounts to be stored globally; an operator can adjust the roughing depth directly via the parameter screen without altering the G-code, or conversely, programming the U and R addresses in the G71 block will dynamically rewrite the machine parameters on the fly. Second, Mitsubishi features a proprietary 1-block format ("MITSUBISHI CNC Special Format"); while other controls force programmers to use rigid two-block structures to define cut depths and finish profiles, Mitsubishi allows the entire cycle to be condensed into a single block by shifting the cut amount to the D address. Finally, Mitsubishi escapes the restriction of purely numeric subprogram calls; if the finished shape profile is stored in an external file, the programmer can designate the A address using an alphanumeric file name enclosed in angle brackets (e.g., <ROUGH_PROFILE>), significantly streamlining file management on the shop floor.

Program Examples

Fanuc Program Example

G00 X80.0 Z5.0 ; Position tool at cycle start point (clearance plane)
G71 U2.0 R1.0 ; Set depth of cut to 2.0mm and retract amount to 1.0mm
G71 P100 Q200 U0.5 W0.1 F0.25 ; Rough contour N100 to N200 with X/Z allowances
N100 G01 X20.0 Z0.0 F0.15 ; Contour start block (must be linear G01/G00)
G01 X20.0 Z-20.0 ; Linear turning pass
G02 X40.0 Z-30.0 R10.0 ; Circular interpolation pass (arc profile)
G01 X60.0 Z-30.0 ; Facing step
G01 X60.0 Z-50.0 ; Longitudinal turn
N200 G01 X80.0 Z-55.0 ; Contour end block
G70 P100 Q200 ; Execute G70 finishing pass using defined contour N100-N200

Dry Run Walkthrough

To safely perform a dry run of the Fanuc profile, first isolate the machine tool by locking the machine Z-axis and enabling the dry run toggle on the operator panel. Step through the program block-by-block. Observe the turret rapid to Z5.0 and X80.0; check that the cutting tool tip sits exactly 5.0mm clear of the stock face. As G71 executes, watch the tool feed in 2.0mm radial increments, retracting 1.0mm after each pass to verify proper chip breaking. Once the roughing cycles complete, verify the tool returns to X80.0 Z5.0. Next, observe the finishing tool index and trace the exact profile from N100 to N200 with the active feedrate (F0.15), checking for visual tool-path mismatches. Finally, verify that no alarm codes (such as PS0064 or PS0322) are triggered, confirming the path is monotonous and correctly clear of raw workpiece boundaries.

Siemens Program Example

G00 X80.0 Z5.0 ; Rapid to start clearance position
G71 U2.0 R1.0 ; Call Siemens shell-mapped roughing parameters
G71 P80 Q120 U0.5 W0.2 F200 ; Define start/end markers with allowances
N80 G01 X20.0 Z0.0 ; First contour block (linear positioning)
G01 X20.0 Z-25.0 ; Turning shaft section
G03 X50.0 Z-40.0 CR=15.0 ; Circular interpolation with radius CR
G01 X50.0 Z-60.0 ; Turn to shoulder
N120 G01 X80.0 Z-60.0 ; Final contour block
G70 P80 Q120 ; Execute finishing pass over mapped CYCLE371T path

Dry Run Walkthrough

Before running the Siemens G-code, confirm that the control is in standard Automatic mode rather than Manual Data Automatic (MDA) mode to avoid an immediate Alarm 14011. Set the feedrate override knob to 10% and execute the program. Verify the tool rapids to the clearance start point X80.0 Z5.0. Step through the blocks to observe the Siemens native shell cycle (CYCLE371T) computing cutting step-overs based on the U2.0 and R1.0 variables. Check that the cutting tool nose moves in parallel Z-axis paths, retracting outward after each pass. Once the roughing is finished, confirm the tool repositions to the start point before executing G70. Observe the finishing pass trace the contour N80 to N120 at the programmed speed and feedrate, confirming the final geometry matches the target workpiece outline without overloading the tool insert.

Mitsubishi Program Example

G00 X80.0 Z5.0 ; Rapid to safe tool cycle start coordinate
G71 U3.0 R1.0 H0 ; Set 3.0mm cut depth, 1.0mm pull-up retract, no pockets
G71 P100 Q200 U0.5 W0.2 F0.25 ; Define contour sequence range N100-N200
N100 G01 X20.0 Z0.0 ; Start of finished shape contour (linear)
G01 X20.0 Z-30.0 ; Outer diameter turn
G02 X50.0 Z-45.0 R15.0 ; Turning shoulder fillet radius
G01 X70.0 Z-45.0 ; Turn diameter step
N200 G01 X80.0 Z-50.0 ; End of finished shape profile
G70 P100 Q200 ; Execute G70 finishing cycle with radius compensation

Dry Run Walkthrough

Initiate the Mitsubishi dry run by locking the chuck and verifying that the tool nose radius compensation (G40) is active at the start block to ensure correct pre-cycle offsets. Run the program in dry run mode and observe the tool move to the X80.0 Z5.0 clearance plane. During the roughing cycles, check the digital readout to confirm that the CNC has automatically suspended the compensation (leaving a uniform allowance on X and Z axes). Watch the tool step-over at a constant 3.0mm depth of cut, verifying the relief movements do not interfere with the vise jaw or chuck jaws. After the roughing pass, verify the G70 command reapplies tool radius compensation (G68.2 or standard G41/G42) to cut the exact N100 to N200 geometry, and check that no servo alarm or P204 program error is triggered.

Error Analysis

Brand	Alarm Code	Trigger Condition	Operator Symptom	Root Cause / Fix
Fanuc	PS0064	Programmed finishing shape does not continuously increase or decrease along the cutting axis in a Type I cycle.	The CNC machine stops immediately at the cycle call block, throwing an alarm on the CRT display screen.	A microscopic dip or reversal (e.g. 0.001 mm backwards along the Z-axis) was generated by the CAM post-processor. Fix: Program a strictly monotonic profile or configure Parameter No. 5146 to specify an allowable deviation tolerance.
Fanuc	PS0322	The canned cycle start point falls mathematically short of the maximum machining profile boundary.	Cycle execution halts before movement begins, and the tool remains locked at its pre-cycle coordinate.	The physical tool start position was positioned inside the raw material or too close to convex geometry. Fix: Reposition the tool start point safely outside the workpiece profile raw boundary.
Fanuc	PS0063	The sequence number specified in address Q cannot be found in the active NC program when Parameter 5102#2 (QSR) is active.	The machine alarms out instantly upon reading the second G71 or G72 block, halting automatic cycle parsing.	The ending sequence number was omitted, mislabeled, or deleted from the contour profile. Fix: Verify sequence numbers between P and Q match the contour block numbers exactly.
Siemens	Alarm 14011	The programmer attempts to execute the G70, G71, or G72 canned cycle inside Manual Data Automatic (MDA) mode.	The control system blocks the cycle call, raising an alarm status and refusing to execute block motion.	Fixed turning cycles G70 to G73 are strictly prohibited inside MDA mode. Fix: Reprogram and run the cycles from standard Automatic mode instead.
Siemens	Alarm 61805	Simultaneous programming of absolute and incremental values in intermediate Siemens shell contour blocks.	Movement halts mid-contour during roughing, locking the axes and displaying an active contour calculation fault.	Absolute and incremental coordinates (such as X/U or Z/W) are mixed in intermediate contour blocks. Fix: Clean up the intermediate blocks to use only absolute or only incremental registers.
Siemens	Alarm 61801	Incorrect value programmed in cycle call or incorrect setting data in the active G-code system.	The machine cycle call fails immediately, and the controller displays a parameter configuration error.	An impermissible value was programmed in the cycle call parameters. Fix: Verify the active ISO G-code dialect system and correct the cycle parameters.
Mitsubishi	P32	Commanding R or A address in G71/G72 block while Mitsubishi special 1-block format is active via parameter #1265.	The controller triggers a program error immediately at the block, preventing cycle execution.	Address R or A was commanded inside a 1-block format cycle where parameters control retract and depth. Fix: Remove R/A addresses or switch back to conventional 2-block format.
Mitsubishi	P33	The first block of the fixed cycle (containing depth and retract) is omitted when 2-block format is selected by parameter.	The CNC stops with a program error at the cycle call, refusing to parse the second block.	Parameter #1265 ext01/bit0 is set to "0" (2-block format) but the first block of the cycle was omitted. Fix: Program both G71/G72 blocks or change parameter #1265 to enable 1-block.
Mitsubishi	P204	Sequence numbers P and Q are both omitted when finished shape profile is stored in the same main program.	Cycle command execution fails, generating a program error on the operator console.	The finished shape profile is in the same main program but P and Q sequence addresses were omitted. Fix: Explicitly define the start and end N sequence numbers in the P and Q addresses.

Application Note

Catastrophic turret crashes, shattered carbide inserts, and severely gouged scrap parts occur when machine operators overlook the spatial clearance of the cycle start point relative to the workpiece contour. During standard longitudinal roughing (G71) or transverse roughing (G72) cycles, the CNC lathe controller automatically sets the pre-cycle start coordinate as its rapid retract clearance plane. If the programmer positions the tool start point too close or inside pocket geometry, the tool will attempt to rapid back to a trapped coordinate, causing the cutter to bind against the spinning material. This sudden interference will inevitably plunge the tool into physical machine limits, resulting in a violent hard collision against the vise jaw, clamp, chuck, or turret. Such an impact instantly generates a catastrophic servo overload alarm code, shatters the cutting insert, and leaves behind a severely gouged scrap part.

To eliminate these physical collision risks, programmers must rigidly position the starting point safely outside the raw workpiece boundaries. On Fanuc controls, operators should enable Parameter 5104#2 (FCK) to enforce an automatic mathematical pre-check of the entire profile geometry against the starting coordinate before the tool moves. If the finishing shape violates this coordinate, the CNC safely throws a PS0322 alarm rather than driving the cutter through the material in an unpredictable rapid movement. On Siemens systems, programmers must verify that the tool plane G-code retention priority during plane changes is properly governed by configuring Bit 18 of MD20360 ($MC_TOOL_PARAMETER_DEF_MASK) to prevent interpolation mismatches. On Mitsubishi controls, operators can utilize reversible parameters such as #8051 G71 THICK and #8052 G71 PULL UP to globally adjust depth of cut and retract values directly on the parameter screen, safeguarding the machine setup from volatile raw stock variances.

Related Command Network

• G73 (Pattern Repeating Cycle): Mapped for rough cutting formed materials like castings or forgings where a uniform stock layer is removed along a defined contour.
• G74 (Longitudinal Deep-Hole Drilling and Grooving): Utilized for automatic peck drilling or face grooving parallel to the Z-axis to ensure efficient chip clearance.
• G75 (Transverse Deep-Hole Drilling and Grooving): Controls peck grooving or parting-off operations along the radial X-axis with automatic chip relief.
• G76 (Compound Thread Cutting Cycle): Automates single-point thread cutting by computing multiple threading passes with constant volume cutting depths.
• G68 (Coordinate Rotation): Used to rotate the coordinate system for specialized operations, but must be safely deselected prior to executing lathe roughing and finishing cycles to prevent interpolation mismatches.

Conclusion

Successful turning operations depend on a precise balance between safe clearance plane positioning, correct parameter mapping, and rigid workholding. By placing the cycle start coordinate well outside the workpiece blank and configuring brand-specific safety checks—such as pre-cycle profile validations or unmonotonous shape deviation limits—operators can eliminate turret crashes and scrap parts. Rigorous coordinate verification and parameter optimization ensure that high-efficiency roughing canned cycles remain safe, productive, and highly accurate on the shop floor.

FAQ

Why does G71 throw a PS0064 alarm on Fanuc controls?

A PS0064 alarm is triggered during a Type I roughing cycle when the programmed finishing contour is not monotonous, meaning it does not continuously increase or decrease along the cutting axis. This occurs if a CAM post-processor introduces a microscopic profile dip or path reversal, which the cycle flags as a pocketing violation. To resolve this, inspect the code for Z-axis path reversals, or configure Parameter No. 5146 to specify an allowable geometric deviation tolerance that lets the control ignore microscopic flaws.

Can standard lathe cycles be executed inside MDA mode on Siemens controls?

Standard turning fixed cycles like G70, G71, and G72 cannot be executed or simulated within Manual Data Automatic (MDA) mode, which immediately halts the NC control and outputs Alarm 14011. The underlying Siemens shell cycles require complete automatic cycle mapping to calculate contour steps and jumps safely. To prevent this interruption, always program and run these canned cycles from standard Automatic mode on the Sinumerik console.

What is the difference between conventional 2-block and Mitsubishi 1-block G71 format?

The conventional format utilizes two blocks to define roughing parameters and contour sequence numbers, whereas the Mitsubishi special 1-block format condenses the entire cycle into a single command line by moving the cutting depth to the D address and referencing retract amounts globally through user parameters. If the conventional format is active under parameter #1265 but the first block is omitted, the machine will trigger a P33 program error. To apply the 1-block format, verify that parameter #1265 ext01/bit0 is set to 1 and replace U/R addresses with the D address.