Deactivating CNC Stored Stroke Limit Checks with G23 and WALIMOF

Introduction

Deactivating stored stroke checks or working area limitations removes the virtual software envelopes that protect a machine's spindle and workholding components. When a command like G23, WALIMOF, or WALCS0 is executed, the tool turret can navigate into close-tolerance physical regions, but any subsequent programming error—such as an incorrect offset coordinate or a units mismatch—will drive the tool carrier straight into the rotating chuck, tailstock, table-mounted vise jaws, or pneumatic clamps. This immediate, uninhibited path results in a catastrophic hard collision, a fractured machine spindle, shattered tooling, and a scrapped workpiece. Because the control's preprocessor no longer intercepts the boundary violation, the machine will not trigger a software overtravel stop before the physical impact occurs.

For automated manufacturing cells, deactivating these software barriers is sometimes necessary during tool changeovers or setup procedures to allow the revolver to retract fully into safety zones that lie beyond normal machining limits. However, because CNC controls typically monitor boundaries using only a single hypothetical tool tip checkpoint, indexing a wide-body tool holder with safety limits disabled creates a silent hazard. If the physical tool body envelope exceeds the programmed checkpoint envelope, it will crash into workholding fixtures even if the programmed coordinate path is theoretically calculated as safe by the compiler.

Technical Summary

Technical Specification	Value / Description
Command Codes	G23 (Fanuc, Mitsubishi, Siemens ISO Dialect), WALIMOF (Siemens native BCS), WALCS0 (Siemens native WCS), G23.1 (Mitsubishi M-System)
Modal Groups	Group 04 (Systems A, B) or Group 09 (System C) for Fanuc G23; Group 03 for Siemens WALIMOF; Group 60 for Siemens WALCS0; Group 04 (L-System) or Group 00 (M-System) for Mitsubishi G23; Group 04 for Mitsubishi G23.1
Supported Brands	Fanuc, Siemens, Mitsubishi
Critical Parameters	Fanuc: No. 3402 Bit 7 (G23 default at boot); Siemens: MD10604 (limitation state during geometry axis interchange); Mitsubishi: #12057 (OT_prechkON), #8179 (toolpath trajectory check)
Main Constraint	Boundary checks rely on a single hypothetical tool nose checkpoint. G23 and G23.1 commands must be programmed in separate, independent blocks without motion or other commands. Simple inclined surface control (G176) and tool center point control (G174) must be inactive.

Quick Read

• Deactivating limit checks removes software barriers around the spindle, workpiece chuck, and tailstock, exposing the machine to hard crashes from coordinate mistakes.
• The control evaluates chuck and tailstock barriers using only a single hypothetical tool tip checkpoint, meaning wide-body tool holders can collide even when the path is reported clear.
• G23 (Fanuc, Mitsubishi) and G23.1 (Mitsubishi) must be programmed as standalone commands in their own independent blocks to avoid preprocessor block-split or syntax errors.
• In Siemens native mode, Basic Coordinate System (BCS) limits are deactivated via WALIMOF, while Workpiece Coordinate System (WCS) limits are deselected via WALCS0.
• Mitsubishi controls can evaluate the entire toolpath trajectory during rapid or linear moves if parameter #8179 and #12057 are active, halting control with Program Error P452 before motion begins.
• Before executing automatic operations with deactivated limits, operators must perform a dry run "in the air" to verify physical clearances.

Basic Concepts

The stored stroke limit check is a protective software barrier designed to prevent the machine's axes from traveling into zones occupied by workholding equipment like the chuck and tailstock. When active (via G22 or WALIMON), the CNC preprocessor calculates axis positions and halts movement with an overtravel alarm if the tool's reference point is projected to cross into a prohibited safety envelope. This provides a digital safety net that catches programming errors, incorrect work offsets, or tool wear offsets before they cause mechanical damage.

Deactivating these limits (using G23, WALIMOF, or WALCS0) is a temporary operational requirement on many CNC systems. It is primarily used during automated tool change sequences or coordinate system alignment procedures, where the turret must traverse into the extreme outer boundaries of the machine's physical envelope to clear the spindle area. By modally switching the boundary check off, the axes are allowed to move close to the physical limits without triggering false overtravel alarms that would interrupt the machining cycle.

Once limits are deactivated, the control entirely suspends its safety monitoring for the respective coordinate systems. This means that a coordinate mismatch—such as running a program defined in metric units (G21) on a machine configured in inches (G20)—will not be intercepted by the boundary supervisor. The controller will shift the decimal point rather than mathematically scale the coordinates, causing unexpected rapid movements that can drive the tool carrier directly into clamping fixtures or the spindle nose.

Command Structure

To deactivate the stored stroke limit check on Fanuc and Mitsubishi controls, the G23 command is programmed as a standalone preparatory code. When interpreted by the CNC compiler, G23 modally deactivates the virtual Chuck Barrier and Tailstock Barrier checks. Because G23 is a modal command, it remains active until the control processes a G22 command, which re-establishes the safety zones. In Siemens native mode, the command WALIMOF is utilized to turn off the Basic Coordinate System (BCS) working area limitations, while WALCS0 is used to turn off the Workpiece Coordinate System (WCS) working area limitations. Alternatively, Siemens controls can parse the G23 command if the compiler is switched to ISO Dialect Mode using G291.

A critical constraint when using G23 or G23.1 is the separate block rule. The command must be written in an independent block without axis coordinates or auxiliary functions. If axis movements are combined in the same block as the G23 command, the preprocessor will either halt execution with a syntax error or split the block. For instance, in Mitsubishi's M-System, writing a motion command in the same block as G23.1 causes the control to split the instruction, executing the deactivation prior to motion, which leaves the subsequent move completely unprotected. In Fanuc systems, G23 belongs to Group 04 under G-code Systems A and B, but shifts to Group 09 under G-code System C.

; Fanuc and Mitsubishi (Lathe / L-System)
G23 ;
; Mitsubishi Machining Center (M-System)
G23.1 ;
; Siemens Native Mode (BCS Limitation OFF)
WALIMOF ;
; Siemens Native Mode (WCS Limitation OFF)
WALCS0 ;
; Siemens ISO Dialect Mode
G291 ;
G23 ;
G290 ;

Brand	Parameter No.	Description	Value / Range
Fanuc	Parameter 3402 Bit 7 (G23)	Determines the active stored stroke limit state at boot-up.	0 = G22 ON active, 1 = G23 OFF active
Fanuc	Parameter 3401 Bit 7 (GSC) & Bit 6 (GSB)	Configures the active G-code system.	G-code System A, B, or C
Fanuc	Parameter 3402 Bit 6 (CLR)	Determines if G-code modals are cleared or retained on reset or power-up.	0 or 1
Fanuc	Parameter 5040 Bit 3 (TCT)	Tool length compensation shift type.	0 or 1
Siemens	MD10604 ($MN_WALIM_GEOAX_CHANGE_MODE)	Defines working area limitation behavior during geometry axis interchange.	0 = deactivated, 1 = remains active
Siemens	MD10710 ($MN_PROG_SD_RESET_SAVE_TAB)	Determines if programmed working area limit values (via G25/G26) are retained in setting data after reset.	Channel configured
Siemens	Option Bit 19800 ($MN_EXTERN_LANGUAGE)	Enables compiler interpretation of external languages.	Active / Inactive
Mitsubishi	Parameter #12057 (OT_prechkON)	Toggles the stroke check before travel in stored stroke limit area function.	0 = OFF, 1 = ON
Mitsubishi	Parameter #8179	Determines if the complete tool path trajectory is evaluated for stroke check before travel instead of just the block endpoint.	0 = OFF, 1 = ON
Mitsubishi	Parameter #12058 (OT_prechkTYPE)	Controls whether stroke check before travel is active during skip (G31) and auto tool measurement (G37).	0 = OFF, 1 = ON
Mitsubishi	Parameter #8202 (OT-CHECK OFF)	Axis-independent overtravel check toggle.	0 = active, 1 = inactive
Mitsubishi	Parameter #8204 (OT-CHECK-N)	Stored stroke negative limit coordinate.	±199999998 (0.5µm increments)
Mitsubishi	Parameter #8205 (OT-CHECK-P)	Stored stroke positive limit coordinate.	±199999998 (0.5µm increments)

Brand Applications

Fanuc

On Fanuc controls, the G23 command modally deactivates the virtual Chuck and Tailstock barriers (modal Group 04 or Group 09 depending on the G-code System configured by Parameter 3401). If Parameter 3402 Bit 7 is configured to 1, the control will default to G23 (barriers inactive) upon system boot. While G23 is active, the preprocessor disables all safety zone boundary checking, allowing the machine turret to move close to the spindle for face-machining operations.

To deactivate and reactivate safety boundaries on a Fanuc lathe, G23 and G22 are programmed modally in separate blocks:

G23 ;
G90 G00 X100.0 Z50.0 ;
G22 ;

• Parameters: Parameter 3402 Bit 7 (determines boot-up state of G23), Parameter 3401 Bit 7 & 6 (configures G-code system), Parameter 3402 Bit 6 (determines if modals clear on reset), and Parameter 5040 Bit 3 (tool length compensation shift type).
• Alarms: Alarm PS0368 (triggered if modifying Parameter 5040 Bit 3 while coordinate offsets are active), Alarm PS0325 (triggered if G22/G23 is specified inside canned cycle G71/G72 shape definitions), and Alarm PS0011 (feed zero limit).
• Version Differences: On Series 15, FCV Parameter 0001 Bit 1 enables legacy programming formats. On Series 16i/18i/21i, tool path pocket deactivation and retract movements must be closely monitored to prevent tool gouging. Under Systems A/B, G23 is in Group 04; under System C, it is in Group 09.

Warning: Fanuc controls evaluate boundaries using only a single hypothetical tool tip checkpoint. If a wide-body tool is indexed while G23 is active, the physical body of the tool can collide with the spindle or workholding even if the path calculations indicate a safe clearance.

Siemens

Siemens SINUMERIK controls manage working area limitations through native modal commands WALIMOF (deactivates Basic Coordinate System limits) and WALCS0 (deactivates Workpiece Coordinate System limits). In native Siemens mode, axes limits are set using G25 and G26 commands. To maintain compatibility with external G-code programs, Siemens parses G23 in ISO Dialect mode (G291), translating the command into its internal safety structure.

To native Siemens controls, working area limitations are turned off and on using separate commands:

WALIMOF ;
WALCS0 ;
; Perform operations
WALIMON ;

• Parameters: Machine data MD10604 ($MN_WALIM_GEOAX_CHANGE_MODE) defines deactivation behavior during geometry axis interchange, MD10710 ($MN_PROG_SD_RESET_SAVE_TAB) determines if limits are saved on reset, and Option Bit 19800 ($MN_EXTERN_LANGUAGE) enables external ISO compilation.
• Alarms: Alarm 12080 (unknown G-code during G291 parsing), Alarm 14800 (programmed path velocity less than or equal to zero), and Alarm 22280 (programmed run-in path too short due to acceleration overload).
• Version Differences: On SINUMERIK 802D sl, machine data MD10604 and DB21 switchover parameters are locked as read-only, whereas they are editable on the 840D sl. Multi-edge turning (G51.2/G50.2) and widescreen touchscreen HMIs are restricted strictly to 840D sl.

Warning: Deactivating limitations via WALIMOF or WALCS0 completely suspends software envelope monitoring. If tool length compensation is inactive, the reference point for boundary checks defaults to the toolholder reference point instead of the tool tip, which can cause unexpected mechanical interference.

Mitsubishi

Mitsubishi controls use G23 to cancel chuck and tailstock barriers in the lathe L-system (Group 04) or to deactivate standard Stored Stroke Limit II checks (Group 00). In the machining center M-system, G23 is repurposed as a subprogram return command, and G23.1 is used to cancel active travel stroke checks. Parameter #12057 (OT_prechkON) toggles the stroke check before travel function, allowing the preprocessor to inspect the path before movement.

To cancel active workpiece barriers in a Mitsubishi L-system program, G23 must be commanded in its own block:

G23 ;
G90 G00 X120.0 Z80.0 ;
G22 ;

• Parameters: Parameter #12057 (toggles stroke check before travel), Parameter #8179 (enables trajectory path evaluation), Parameter #12058 (OT_prechkTYPE), Parameter #8202 (OT-CHECK OFF), Parameter #8204 (negative limit), and Parameter #8205 (positive limit).
• Alarms: Program Error P452 (path passes through or terminates inside prohibited zone), Program Error P451 (stroke check enabled without option support), Operation Error M01 0007 (non-target axis passes through prohibited zone), and Program Errors P951/P952 (G23 executed while inclined surface control G176 is active).
• Version Differences: The Lathe L-system uses G22/G23 for barriers, whereas the Machining Center M-system uses G22.1/G23.1. Version C3 firmware on M800V/M80V series adds G188/G189 format switches to dynamically toggle between L and M G-code systems. Compact M80V TypeB controls trigger Program Error P39 for G54.4 or P34 for G144.

Warning: Mitsubishi's preprocessor splits blocks if travel moves are written alongside safety cancellation commands. Executing a command like G23.1 X100.0 ; will cause the control to deactivate the limit check in the first block, leaving the axis unprotected during the subsequent move.

Brand Comparison

Feature / Behavior	Fanuc	Siemens	Mitsubishi
Deactivation Command	G23 (Modal Group 04 or 09)	WALIMOF (BCS Group 03), WALCS0 (WCS Group 60), or G23 in ISO Dialect mode	G23 (Modal Group 04 or unmodal Group 00), G23.1 (M-system Group 04)
Boot-up Default State Configuration	Parameter No. 3402 Bit 7 dictates boot state (0 = G22 ON, 1 = G23 OFF)	— (no source)	Configurable via overtravel check parameter #8202
Trajectory Path Check Method	Typically checks only block endpoint	Checks endpoint and axis limits; swiveled plane checks vary	Full path trajectory check available via Parameter #8179 and #12057
Block Concurrency Violation	Halts program execution with a syntax error	Natively processes coordinates; deactivates limitations in ISO Dialect	Preprocessor splits concurrent block automatically (e.g. G23.1 X100.0 ;)
Workpiece coordinate limits	Chuck and tailstock barriers prioritized over soft limits	Up to 10 channel-specific limitation groups (WALCS1 to WALCS10) defined in WCS/SZS	Chuck and tailstock barriers defined in MCS; dynamic axis switch (G111) maps safety zones

Technical Analysis

The core differences between Fanuc, Siemens, and Mitsubishi controls lie in their safety supervisor architectures and parameter integration. Fanuc relies on a static parameter-configurable boot setup (Parameter 3402 Bit 7) and enforces a strict Overlap Precedence Rule. When both the chuck/tailstock barriers and stored stroke checks 2 or 3 are programmed concurrently, Fanuc isolates and prioritizes the chuck/tailstock barrier option, completely ignoring stored stroke check 2 or 3. This rigid priority logic is unique to Fanuc's safety supervisor and requires programmers to understand the hierarchical ranking of safety options within the control parameters.

Siemens SINUMERIK controls deviate entirely from the G22/G23 syntax by managing limitations dynamically in the native NC language. Instead of relying on static coordinate boundaries, Siemens features workpiece-specific Working Area Limitation Groups (WALCS1 to WALCS10). This allows operators to define up to 10 channel-specific limitation groups directly in the Workpiece Coordinate System (WCS) or Settable Zero System (SZS), so boundaries dynamically shift relative to the active work origin rather than remaining locked to machine coordinates. Furthermore, Siemens features parameter-driven deactivation choices on axis interchange (MD10604). Unlike standard controls that handle axis swaps using background algorithms, Siemens allows the machine builder to define whether active working area limitations are deactivated or retained when a geometry axis interchange occurs, preventing unexpected deactivation during complex multi-channel operations.

Mitsubishi offers a highly dynamic approach by allowing programmers to swap G-code interpreters mid-program via G188/G189. Swapping formats dynamically shifts G23 from a Group 04 lathe command to a Group 00 machining center command. Additionally, Mitsubishi features a trajectory-passing stroke check (Parameters #8179 and #12057). While Fanuc and Siemens typically only inspect whether the final programmed endpoint of a block lies within a prohibited zone, Mitsubishi evaluates the complete tool path trajectory during rapid or cutting interpolation. If the tool path intersects the prohibited boundary at any point, the control triggers Program Error P452 and halts axis travel before the movement starts. However, under the Machining Center format, Mitsubishi enforces a strict separate compiler block-split rule. Programming coordinate movement in the same block as a cancellation command like G23.1 splits it into two distinct blocks, executing the cancellation prior to movement and leaving the axis temporarily unprotected.

Program Examples

Fanuc G-Code Example

O1001 ;
T0101 ;
G23 ;                      (Modal stroke check OFF - independent block)
G90 G00 X80.0 Z130.0 ;     (Traverse turret close to chuck spindle)
G01 X50.0 Z120.0 F0.15 ;   (Perform close-proximity machining)
G00 X100.0 Z150.0 ;        (Retract turret to safe clearance)
G22 ;                      (Modal stroke check ON - independent block)
M30 ;

Dry Run Explanation: During a dry run setup, the operator must execute this program block-by-block with the feedrate override active. In the third block, G23 deactivates the virtual Chuck and Tailstock barriers, meaning the control will not trigger an alarm if the tool moves within the standard safety zone. The operator must visually confirm that the turret and tool holder clear the chuck jaw by at least 10 mm when moving to X80.0 Z130.0. After the G01 cut, the turret retracts to X100.0 Z150.0 before G22 is commanded in the eighth block. The operator must verify that G22 is successfully reactivated before automatic high-speed operation is permitted, ensuring safety barriers are restored for subsequent operations.

Siemens SINUMERIK Example

N10 T="ROUGH_TURNING" D1
N20 WALIMOF ;              (Deactivate BCS working area limitations modally)
N30 WALCS0 ;               (Deactivate WCS working area limitations modally)
N40 G0 X80 Z130 ;          (Rapid traverse tool carrier to position)
N50 G1 X50 Z120 F0.15 ;    (Execute cutting feed)
N60 G0 X120 Z200 ;         (Retract tool carrier to safety zone)
N70 WALIMON ;              (Re-activate Basic Coordinate System limitations)
N80 M30 ;

Dry Run Explanation: The dry run sequence begins with the operator setting the dry run feedrate active on the SINUMERIK HMI panel. At block N20 and N30, WALIMOF and WALCS0 are executed, disabling all coordinate-based working area limitations. During the rapid traverse to X80 Z130, the operator must watch the digital readout (DRO) and the physical machine position to ensure the revolver does not interfere with the chuck face or workholding clamps. Once the cut is complete and the axis retracts to the tool change coordinate at X120 Z200, WALIMON modally restores the working area limits. The operator must confirm that the limits are active before initiating automatic cycles, ensuring that any subsequent out-of-boundary commands are caught by the NCK.

Mitsubishi Example

%
O2001 ;
T0202 ;
G23 ;                      (Cancel active chuck/tailstock barriers modally)
G00 X80.0 Z130.0 ;         (Traverse to absolute position close to spindle)
G01 X50.0 Z120.0 F0.15 ;   (Perform contouring cut)
G00 X100.0 Z150.0 ;        (Retract turret to safe clearance area)
G22 ;                      (Re-establish chuck/tailstock safety barriers)
M30 ;
%

Dry Run Explanation: During dry run verification on the Mitsubishi control, the operator utilizes the handwheel or manual feedrate override. G23 is executed in its own block, disabling the Chuck and Tailstock barriers. The preprocessor will not monitor the tool's path against the boundaries. The operator must slowly jog the turret toward X80.0 Z130.0, visually confirming that the physical clearance is safe. After completing the G01 cut, the turret is retracted to X100.0 Z150.0. The operator must execute G22 to re-enable the safety barriers. If the operator forgets to retract before G22, or if G22 is commanded while the turret is still inside the barrier zone, the control will immediately lock the axes and trigger Program Error P452, requiring the operator to switch to manual jog mode to retract the tool.

Error Analysis

Brand	Alarm Code	Trigger Condition	Operator Symptom	Root Cause / Fix
Fanuc	Alarm PS0325	G22 or G23 command specified within finishing shape definition blocks (P to Q) of canned cycles G71/G72.	The machine halts immediately mid-cycle and displays "UNAVAILABLE COMMAND IS IN SHAPE PROGRAM" on the CRT screen.	Remove G22 or G23 commands from the canned cycle contour definition blocks. Only command barrier toggles outside the P and Q block range.
Fanuc	Alarm PS0368	Attempting to modify Parameter No. 5040 Bit 3 (TCT) tool length compensation shift type while coordinate offsets or compensations are active.	The control triggers a system fault, halting axis movement and showing the parameter offset warning.	Cancel all active tool offsets and coordinate system offsets (such as tool nose compensation and G54-G59) before modifying parameter settings.
Siemens	Alarm 12080	An unrecognized G-code is processed during ISO Dialect Mode (G291) when scanner error processing is active.	NCK halts program parsing, displays "unknown G-code", and prevents program execution.	Verify that G-code commands in external programs are valid for the active ISO mode dialect, or adjust system mask configurations.
Siemens	Alarm 22280	Axis acceleration required for lead-in or lead-out path during thread cutting/interpolation exceeds configured tolerances.	Program interrupts with "Programmed run-in path too short", preventing axis movement.	Increase the programmed lead-in/lead-out path length or reduce the programmed feedrate to allow proper axis acceleration.
Mitsubishi	Program Error P452	Linear or circular travel path intersects or terminates inside the prohibited stored stroke zone when stroke check is active.	Axis travel halts immediately, and "P452 Stroke Limit Over" appears on the screen.	Switch to manual mode, jog the turret to a safe coordinate, and check the program trajectory. Temporarily deactivate the barrier using G23 if retraction space is restricted.
Mitsubishi	Program Error P951 / P952	G23 or G69.1 barrier check cancel command is executed while simple inclined surface control (G176) is active.	The control halts automatic operation and flags a surface control conflict error.	Programmatically deactivate G176 simple inclined surface control before attempting to cancel workpiece barriers with G23.

Application Note

A catastrophic hard collision, shattered carbide inserts, and a buckled machine spindle are the direct consequences of executing rapid G00 movements after deactivating stored stroke checks without verifying tool geometry offsets. In automated production environments, programming G23 (or WALIMOF) to bypass chuck and tailstock barriers allows the turret to index wide-body toolholders close to the spindle, but it simultaneously disables the digital envelope supervisor. If the operator fails to clear tool wear registers or executing a program with a metric-imperial mismatch, the preprocessor will not intercept the path deviation. To prevent mechanical destruction, operators must execute first-article setups using manual feed overrides and verify that the physical envelope of the entire tool assembly clears all chuck jaws and table clamps prior to running the cycle at full velocity.

Related Command Network

• G22 (Stored Stroke Limit Check ON): This command modally reactivates the Chuck Barrier and Tailstock Barrier safety checks, restoring the virtual protection zones.
• G25 / G26 (Program working area limits): Natively programmed on Siemens controls to set the lower (G25) and upper (G26) boundary coordinates of the working area.
• G290 / G291 (Bilingual mode switch): Used on Siemens controls to switch between native Siemens commands (G290) and external ISO Dialect parsing (G291) where G23 is active.
• G22.1 / G23.1 (Stroke check before travel ON/OFF): Programmed in Mitsubishi Machining Center (M-System) G-code formats to control the pre-travel trajectory checks.

Conclusion

Operating a CNC machine with G23 or WALIMOF active requires a strict process of physical verification. Because deactivating the stored stroke limits removes the virtual safety barriers, operators must rely on physical dry runs and manual override verification rather than the controller's safety preprocessor. Ensuring that safety boundaries are modally reactivated via G22 or WALIMON immediately after completing close-clearance maneuvers is a mandatory practice for protecting the turret, workholding, and spindle from high-speed programming collisions.

FAQ

Can G23 be programmed in the same block as coordinate motion commands?

No. Both Fanuc and Mitsubishi controls enforce a separate block rule for G23. Programming coordinate movements or auxiliary commands in the same block will cause a syntax error on Fanuc controls. On Mitsubishi controls, it triggers a block-split behavior where the limit check is deactivated prior to motion, leaving the tool unprotected during the transition. Always write G23 in an independent block prior to executing close-tolerance moves.

What happens to Siemens working area limits during a geometry axis interchange?

The behavior is determined by machine data MD10604. If set to 0, the active working area limitations are automatically deactivated during an axis interchange. This can catch operators off-guard, leading to hard collisions. Check your machine data settings and set MD10604 to 1 if you require working area limitations to remain active during geometry axis switchovers.

How does tool length compensation affect Siemens working area limits?

When tool length compensation is active, the reference point for boundary checking is the physical tool tip. However, if tool length compensation is canceled or inactive, the control defaults to checking from the toolholder reference point. This shift can cause premature overtravel alarms or physical crashes. Always verify that tool offsets are active before deactivating and reactivating limits using WALIMOF and WALIMON.