G50 & G92 G-Code: Spindle Speed Clamp & Coordinate Setting Guide

Introduction

When a CNC lathe operates under Constant Surface Speed (G96) control without a programmed maximum spindle speed clamp, the spindle speed continuously increases as the cutting tool approaches the centerline (X0), generating immense centrifugal forces that can eject the workpiece directly out of the spindle chuck or chuck jaws. This high-speed release leads to a severe impact where the spinning raw stock slams into the tool turret, tool change arm, or machine enclosure, shattering the cutting tools, triggering axis-overload alarms, and leaving a ruined scrap part. Therefore, programmers must always program the spindle clamp prior to or simultaneously with G96 activation to ensure safe operations.

Setup operators must exercise extreme caution when launching programs containing coordinate system settings (G92/G50). Because coordinate presets are modal and shift the absolute position registers without physical axis movement, starting automatic operation from the middle of a program without confirming that the G and F modals, spindle clamps, and coordinate offsets are appropriate is highly dangerous. If the coordinate system is set incorrectly by the operator, subsequent movement commands will deviate. The tool turret will travel along an uncompensated path, driving the spindle or cutting tool into table clamps, tailstock clamps, or the rotating spindle chuck, resulting in a hard collision.

Technical Summary

Technical Specification	Details
Command Code	G50 (Fanuc A, Mitsubishi Lists 2/4/6) / G92 (Fanuc B/C, Mitsubishi Lists 3/5/7, Siemens ISO Dialect) / LIMS (Siemens Native)
Modal Group	Group 00 (Non-modal / one-shot) for turning coordinate settings and spindle speed clamps. Native Siemens LIMS is modal.
Supported Brands	Fanuc, Siemens, Mitsubishi
Critical Parameters	Maximum Spindle Speed (S), Minimum Spindle Speed (Q for Mitsubishi)
Main Constraint	Spindle clamp commands and coordinate presets do not produce physical axes travel. Constant Surface Speed control (G96) must not be active during thread cutting cycles (G33/G76/G78) or synchronous tapping cycles (G84/G88) to prevent lead errors due to servo lag.

Quick Read

• Always program the G50/G92/LIMS spindle clamp prior to or simultaneously with G96 Constant Surface Speed activation to prevent uncontrolled spindle acceleration.
• Position the tool at a safe start point before executing coordinate system settings (G92/G50) as they shift position registers without physical motion.
• Program feedrates as revolutional feedrate (G95) in mm/rev rather than linear feed (G94) when G96 Constant Surface Speed is active.
• Avoid specifying tool change T-codes or tool offsets in the same block as G50/G92 coordinate setting commands to ensure correct position compensation.
• Deactivate Constant Surface Speed (G96) before executing thread cutting (G33/G32) or synchronous tapping (G84/G88) to avoid lead errors caused by servo lag.
• Verify that the machine parameters match the G-code system in use (e.g., Parameter 3401 for Fanuc, cmdtyp #1037 for Mitsubishi, MD 18800 for Siemens).

Basic Concepts

Implementing fener mili speed clamping serves as a critical safety boundary when machining workpieces under Constant Surface Speed (G96) control. As the cutting tool on the tool change carriage or turret moves closer to the centerline of the workpiece (approaching X0), the CNC continuously calculates and increases the spindle revolutions per minute to maintain a uniform surface speed at the cutting edge. Without a predefined maximum spindle speed limit (programmed via G50, G92, or LIMS), the spindle can accelerate excessively, exceeding the mechanical limits of the workholding equipment. This uncontrolled acceleration generates high centrifugal forces that can release the workpiece from the spindle chuck or workpiece clamping fixtures, causing severe damage, triggering axis-overload alarms, and destroying the workpiece.

Setup operators must exercise extreme caution when launching programs containing coordinate system settings (G92/G50). Because coordinate presets are modal and shift the absolute position registers without physical axis movement, starting automatic operation from the middle of a program without confirming that the G and F modals, spindle clamps, and coordinate offsets are appropriate is highly dangerous. If the coordinate system is set incorrectly by the operator, subsequent movement commands will deviate. The tool turret will travel along an uncompensated path, driving the spindle or cutting tool into table clamps, tailstock clamps, or the rotating spindle chuck, resulting in a hard collision.

To prevent such accidents, setup operators can define programmable working area limitations (using G25/G26 commands or axis-specific setting data) to establish protection zones around the spindle chuck and tool turret. These limitations protect surrounding devices—such as the tool turret and measuring stations—against physical damage by stopping axis travel before a crash can occur. Additionally, programmers must make sure that when G96 is active, the feedrate is programmed as a revolutional feedrate (G95) in mm/rev rather than linear feed (G94) to avoid excessive material infeed rates that can overload the cutting tool.

Command Structure

The coordinate system setting and spindle speed clamp command is programmed using non-modal preparatory functions in G-code Group 00. When used for workpiece coordinate system setting, the command registers the absolute distance from program zero to the current position of the tool. This preset operation establishes a hypothetical coordinate system on the lathe without initiating any axis movement. If a tool change or position shift is active, the control registers the coordinate system by factoring in the necessary offset values.

When the same preparatory command is combined with an S address, it defines the spindle speed clamp. This setting restricts the maximum rotational speed of the master spindle during constant surface speed control (G96). On some controls, such as Mitsubishi, a Q address can also be specified to clamp the minimum spindle speed. Programmers can declare the coordinate preset and the spindle clamp separately or combine them into a single command block.

The syntax for configuring coordinate offsets and maximum spindle speed clamps varies across controls:

• Fanuc System A Syntax: G50 X_ Z_ S_ ; (or G92 X_ Z_ S_ ; for System B/C)
• Siemens Native Syntax: LIMS = <value> or LIMS[<spindle_number>] = <value>
• Mitsubishi Syntax: G92 X_ Z_ S_ Q_ ; (or G50 X_ Z_ S_ Q_ ; depending on cmdtyp)

Address / Identifier	Description	System Applicability
X	Coordinate value for the X-axis (diameter value on lathes) to preset tool position.	Fanuc, Siemens (G291), Mitsubishi
Z	Coordinate value for the Z-axis to preset tool position.	Fanuc, Siemens (G291), Mitsubishi
S	Maximum spindle speed clamp value in revolutions per minute (RPM).	Fanuc, Siemens (G291), Mitsubishi
Q	Minimum spindle speed clamp value in RPM.	Mitsubishi
LIMS	Native Siemens spindle speed limit assignment. Array subscript (e.g., LIMS[2]) specifies a specific spindle.	Siemens (Native G290)

Brand Applications

Fanuc

Fanuc controls configure the G50/G92 command mapping using two main parameters: Parameter No. 3401 (selects G-code System A, B, or C) and Parameter No. 3402 (selects clear state of modal G-codes). These parameters determine whether G50 behaves as a position register and spindle clamp, or as a scaling cancel command.

On a Fanuc lathe configured for G-code System A, the programmer sets the workpiece coordinates at machine zero and limits the maximum spindle speed to 1500 r/min by programming the block: G50 X9.0 Z5.0 S1500 ;. Additionally, Parameter No. 5000 Bit 3 (GNI) controls the trajectory of G40 cancel blocks (see g40-compensation-cancel) with no tool movement. We must also ensure that we apply tool radius and offset compensations. For example, tool nose radius compensation is activated with G42 (see g42-tool-nose-radius-compensation) and tool length compensation is set using G43 (see g43-tool-length-compensation).

Category	Reference / Code	Description / Value
Parameter	Parameter No. 3401	Bits GSC and GSB select G-code system A, B, or C.
Parameter	Parameter No. 3402	Bit 6 (CLR) sets modal G-codes clear state at power-up/reset.
Parameter	Parameter No. 5000	Bit 3 (GNI) controls trajectory of G40 cancel blocks with no tool movement (0 or 1).
Alarm	Alarm PS0245	Triggered if G28, G29, G30, G30.1, or G53 is specified with a tool change T-code in the same block.
Alarm	Alarm PS0509	Triggered if a tool offset is specified in a thread cutting (G32, G34, G35, G36) block.
Alarm	Alarm PS5330	Triggered if a T-code and G50.9 format are specified in the same block.
Alarm	Alarm PS0010	Triggered if an improper G-code is specified.
Version Difference	G-Code System A vs B/C	System A uses G50 for coordinate setting and speed clamp. Systems B/C use G92 instead (G50 is scaling cancel).
Version Difference	Series 30i/31i/32i-B Plus vs Legacy	On 30i controls, GNI=0 can cause overcutting on G40 cancel blocks with no tool movement. Set GNI=1 to match legacy 16i/18i/21i behavior.

Warning: Programmers must never program the G50 coordinate setting command in the same block as a tool change T-code, as this prevents the tool position compensation from being applied correctly and can result in severe coordinate drift.

Siemens

Siemens SINUMERIK controls process external ISO Dialect blocks using compiler settings defined in MD 18800 ($MN_MM_EXTERN_LANGUAGE). In native Siemens mode, the active tool length and tool radius compensations can be suppressed using suppression commands depending on MD 10760 ($MN_G53_TOOLCORR).

To clamp the master spindle speed to 1500 RPM in native Siemens mode, program: LIMS=1500 ; or to switch to ISO mode and preset coordinates and clamp speed, program: G291 ; G92 X100.0 Z50.0 S2000 ;.

Category	Reference / Code	Description / Value
Parameter	MD 18800	$MN_MM_EXTERN_LANGUAGE activates external ISO language dialect compiler (0 or 1).
Parameter	MD 10760	$MN_G53_TOOLCORR suppresses (1) or retains (0) tool compensations in G53/SUPA.
Parameter	MD 20734	$MC_EXTERN_FUNCTION_MASK controls external language settings (e.g., Bit 2 dwell unit).
Alarm	Alarm 61800	External CNC system missing. Triggered if G291 or G50/G92 is run while MD 18800 is disabled.
Alarm	Alarm 12080	Syntax error in translating external ISO blocks.
Alarm	Alarm 14800	Channel tangential feed velocity is less than or equal to zero during active movement.
Version Difference	840D sl vs 802D sl	MD 10604 and MD 10706 are read-only and cannot be changed on 802D sl.
Version Difference	840D sl vs 802D sl	Multi-edge turning G51.2 (ON) and G50.2 (OFF) are supported only on 840D sl.

Warning: Do not attempt to change the spindle speed clamp or gear stage while a thread cutting cycle (G33) is active, as spindle speed changes during threading risk losing lead accuracy due to servo lag.

Mitsubishi

Mitsubishi lathe systems map the spindle clamp and coordinate preset functions using G-code list configuration parameter #1037. The safety response for executing a G96 Constant Surface Speed command without a preset speed clamp is determined by parameter #1448.

On a Mitsubishi lathe using G-code List 3, program: G92 S3500 Q150 ; to clamp the maximum spindle speed to 3500 r/min and the minimum spindle speed to 150 r/min.

Category	Reference / Code	Description / Value
Parameter	Parameter #1146	Sclamp allows speed clamp before G96 activation if set to 1 (0 or 1).
Parameter	Parameter #1227	aux11/bit5 determines if spindle speed clamp is active under G97 mode (0 or 1).
Parameter	Parameter #1210	RstGmd/bit19 determines if spindle speed clamp values are retained on reset (0 or 1).
Parameter	Parameter #1448	Sclamp_err_cancel determines action when G96 is issued without speed clamp (0 = Program Error P134, 1 = Operation Error M01 1043).
Parameter	Parameter #1279	ext15/bit5 clears G92 shift when reaching manual reference position (0 or 1).
Parameter	Parameter #3129	cax_spec/bit5 retains coordinate offsets when switching back to C-axis (0 or 1).
Parameter	Parameter #1037	cmdtyp determines G-code list configuration (Lists 2/4/6 use G50; Lists 3/5/7 use G92).
Alarm	Program Error (P134)	CSS (G96) run without speed clamp and parameter #1448 = 0. G96 block is ignored.
Alarm	Operation Error (M01 1043)	CSS (G96) run without speed clamp and parameter #1448 = 1, or clamp invalid for spindle.
Alarm	Operation Error (M01 1113)	G96 issued to spindle running threading/tapping cycles, or vice versa.
Alarm	Program Error (P481)	G96 issued during active G07.1 or G12.1/G13.1 interpolation.
Alarm	Program Error (P485)	Interpolation commanded during active G96 CSS mode.
Alarm	Program Error (P182)	Synchronous tapping executed while G96 is active.
Alarm	Program Error (P186)	G96 active command issued during synchronous tapping.
Alarm	Program Error (P33)	G20/G21 command issued in the same block as G92/G50.
Version Difference	Lists 2,4,6 vs 3,5,7	G50 is Spindle Clamp/Coord Setting on Lists 2, 4, 6. G92 is Spindle Clamp/Coord Setting on Lists 3, 5, 7. Configured via Parameter #1037 cmdtyp.
Version Difference	Lathe vs Milling	Lathe uses G50/G92 as unmodal Group 00. Milling uses G50 as modal Group 11 scaling cancel.
Version Difference	C80 Series	Spindle synchronous acceleration of reference spindle is applied to synchronized spindle via #1300 ext36/bit7.

Warning: Program Error (P33) will occur if an inch/metric changeover command (G20/G21) is programmed in the same block as a G92/G50 coordinate system setting or spindle clamp. These commands must be programmed in separate blocks.

Brand Comparison

Comparison Topic	Fanuc	Siemens	Mitsubishi
Command Code	G50 (System A) / G92 (System B/C)	G291 ISO: G92/G50 · Native: LIMS	G92 (Lists 3/5/7) / G50 (Lists 2/4/6)
Speed Clamp Cancel	Modal reset, G50 S0	Modal reset (LIMS=0 or G92.1)	Non-cancelable via G92 S0 (S0 substitutes Q as max speed)
Spindle Clamping	Single spindle clamp in block	Decoupled native multiple spindle clamps	Multi-part system control rights selection
Programming System	Direct block-level register adjustments	Modular frames and stack dynamics	Direct block-level register adjustments

Technical Analysis

Three distinct programmatic behaviors clearly distinguish Fanuc controls from Siemens and Mitsubishi controls during turning offsets and coordinate settings: First, Fanuc relies on a parameter-driven bimodal function mapping for G50. Depending on the parameter GSC/GSB selections (Parameter No. 3401), G50 shifts from a Group 00 position register and spindle speed clamp in turning (G-code System A) to a Group 11 scaling cancel command in milling (machining center) or turning Systems B/C. Siemens completely omits G50 and G92 coordinate setting commands, utilizing programmable frames (such as TRANS and LIMS) instead. Second, Fanuc implements a strict block format lock that prohibits combining G50/G92 speed clamps and T-codes in the same block. Fanuc rules state that doing so prevents tool position compensation from being applied, and also forbid other Group 00 G-codes in the tool change block under penalty of triggering Alarm PS0245. Siemens and Mitsubishi controls manage tool edge data and offsets (via D registers) independently, allowing greater formatting flexibility without disabling active path compensation. Third, Fanuc applies coordinate system setting by directly subtracting tool offset values in real-time within the active position register block (G50 X_ Z_ T_;). This is completely different from Siemens, which manages tool length and radius offsets dynamically through cutting edge registers (D codes) and independent workpiece coordinates, completely bypassing block-level coordinate subtraction.

Three distinct programmatic and architectural behaviors clearly distinguish Siemens controls from Fanuc and Mitsubishi controls during turning offsets and coordinate settings: First, Siemens utilizes a bilingual toggled interpreter model (G290/G291). While Fanuc and Mitsubishi interpret coordinate presets and spindle speed clamps within a single unified G-code system, Siemens requires the programmer to explicitly switch the compiler to ISO Dialect mode via G291 to parse G92/G50 blocks. The program must then command G290 to switch back to native SINUMERIK mode to process high-level parametric Siemens frames (TRANS / ROT) and technologically advanced cycles. Second, Siemens completely decouples fener mili speed clamping from active motion blocks natively. Instead of relying on a single system spindle clamp, Siemens allows programmers to specify independent maximum speed limits for up to four different spindles (such as a master spindle, a counterspindle, or powered tools on the cross slide) within a single channel block using the expanded LIMS array (e.g., LIMS=300 LIMS[32]=450 LIMS[33]=800). Third, Siemens manages coordinate shifts and offsets as modular components of a dynamic frame stack. Natively, coordinate adjustments are executed via programmable frame commands (TRANS/ATRANS), while G54 to G599 settable offsets are stored in a dedicated, multi-level zero offset memory. These frames and active tool compensations can be suppressed globally or selectively using suppression commands (G53, G153, SUPA) depending on the configuration of parameter MD 10760 $MN_G53_TOOLCORR, providing much greater programming flexibility than Fanuc and Mitsubishi's rigid block-level register adjustments.

Three key programmatic and architectural behaviors clearly distinguish Mitsubishi controls from Fanuc and Siemens controls during turning offsets and coordinate settings: First, Mitsubishi applies a protective, non-cancelable substitution logic to the maximum spindle speed clamp when G92 S0 is commanded. If the operator attempts to cancel a G92 S_ Q_ maximum and minimum spindle speed clamp by commanding G92 S0, Mitsubishi’s motion kernel refuses to cancel the maximum speed clamp. Instead, because S0 < Q, the minimum speed Q is automatically substituted as the maximum speed clamp, and S0 is treated as the minimum. Fanuc and Siemens controls lack this inverted safety substitution under S0 declarations. Second, Mitsubishi integrates its G92/G50 coordinate system and spindle clamp modals directly with its manual arbitrary reverse run function (G127). When manual arbitrary reverse run (G127) is enabled, the operator can manually turn the handwheel backward to retract the tool. During this manual reverse tracing, Mitsubishi's motion kernel successfully recovers and reconstructs G92/G50 coordinate offsets and spindle clamping modals using its specialized modal information storage block, preventing axis drift and maintaining spindle speed constraints. Siemens does not support G92/G50 turning commands, and Fanuc does not support handwheel reverse tracing that can dynamically recover unmodal coordinate registers in this manner. Third, Mitsubishi implements a multi-system spindle control rights arbitration system for turning spindles (G43.1 / G44.1). When multiple spindles (such as a master spindle, a counterspindle, or live rotary tools) are active on a multi-part lathe system, commanding S (surface speed) or spindle M-codes randomly from different part systems to a single spindle can disrupt calculations. Mitsubishi resolves these conflicts by transferring spindle control rights dynamically to the part system that issued the last S command, allowing G43.1 (1st selected spindle) and G44.1 (2nd selected spindle) modes to manage speed clamp registers independently. Fanuc and Siemens manage channel-to-spindle relationships through rigid parameter-driven hardware assignments rather than dynamic program-level control rights transitions.

Program Examples

Fanuc

G20 T0100 ;
G50 X9.0 Z5.0 S1500 ;
M42 ;
G96 S400 M03 ;
G00 G41 X5.5 Z0.1 T0101 ;
G01 X-0.07 F0.012 ;
G00 Z0.2 ;
G40 X9.0 Z5.0 T0100 ;
M30 ;

Dry Run: During first-article setup, the operator must enable the dry run switch and execute a test run with the cutting tool positioned at a safe clearance distance from the workpiece. The operator verifies that the spindle speed clamps at 1500 r/min as the X-axis feedrate moves the tool toward the spindle centerline, confirming that the tool change coordinates and compensations are correctly applied without physical interference.

Siemens

G291 ;
G92 X100.0 Z50.0 S2000 ;
G96 S150 M03 ;
G00 X40.0 Z5.0 ;
G01 Z0 F0.15 ;
X80.0 Z-30.0 ;
G290 LIMS=1500 ;
M30 ;

Dry Run: Before machining, the operator activates the dry run feedrate and runs the program in single-block mode. The controller switches interpreter states between native SINUMERIK mode (G290) and ISO Dialect mode (G291), verifying that the coordinate zero presets register properly. The operator monitors the spindle speed to confirm it clamps at 2000 RPM under G291 and restricts the master spindle to 1500 RPM when switching to native LIMS.

Mitsubishi

G92 S3500 Q150 ;
G96 S220 M03 ;
G00 X150.0 Z80.0 ;
G01 Z-20.0 F0.2 ;
G00 X200.0 Z100.0 ;
M30 ;

Dry Run: During the dry run test, the operator monitors the spindle rotation speed as the tool traverses the workpiece zero coordinates. The operator verifies that the spindle speed increases under CSS mode but strictly clamps at the maximum limit of 3500 r/min and never drops below the minimum limit of 150 r/min. The test ensures that no Program Error (P134) or Operation Error (M01 1043) is triggered.

Error Analysis

Brand	Alarm Code	Trigger Condition	Operator Symptom	Root Cause / Fix
Fanuc	Alarm PS0245	Specifying G28, G29, G30, G30.1, or G53 with a tool change T-code in the same block.	The control displays the alarm code PS0245 and immediately halts execution of the active block, disabling axis movement.	G-codes in the 00 group other than G50 must not be specified in the same block as a T-code. The fix is to program the coordinate reference return or suppression commands and the T-code in separate blocks.
Siemens	Alarm 61800	Commanding ISO G-codes (such as G92/G50) while external compiler data is disabled.	The program aborts immediately on the G291 selection block, displaying "External CNC system missing".	Machine data parameter MD 18800 ($MN_MM_EXTERN_LANGUAGE) is set to 0. Change the parameter to 1 and perform a power-on reset to activate the external dialect interpreter.
Mitsubishi	Program Error (P134)	Activating Constant Surface Speed (G96) without first programming a G92/G50 speed clamp when parameter #1448 is set to 0.	The controller displays error code P134 and ignores the G96 block, maintaining the previous spindle speed or stopping.	The speed clamp command is omitted or invalid. Add a G92 or G50 speed clamp (e.g., G92 S3500 Q150;) before or in the same block as the G96 command.

Application Note

Spindle chuck damage, shattered tools, and ruined scrap parts are the direct consequences of failing to program a maximum spindle speed clamp before activating Constant Surface Speed (G96). When the cutting tool approaches the workpiece centerline, the spindle accelerates to the machine's absolute physical limits, generating high centrifugal forces that throw the raw stock from the chuck jaws. To prevent these catastrophic failures, programmers must establish strict boundaries using G50, G92, or LIMS. On Fanuc controls, coordinate shifts must be registered carefully without combining G50 and T-codes, as miscalculated offsets will drive the tool turret into a hard collision with the tailstock or fixtures. Mitsubishi systems mitigate offset drift during manual interventions by integrating G92/G50 modals with the G127 manual arbitrary reverse run, allowing the motion kernel to reconstruct position coordinates when the operator uses the handwheel to retract. Siemens provides advanced flexibility by decoupling speed limits via the LIMS array, allowing independent maximum limits for up to four spindles while managing coordinate translations through programmable frames (TRANS/ATRANS) in a multi-level zero offset memory.

Related Command Network

• G96: Activates Constant Surface Speed control, which requires a pre-declared spindle speed clamp to prevent excessive rotational speeds at small workpiece diameters.
• G97: Deactivates Constant Surface Speed control and restores the control to constant RPM mode.
• G52: Establishes a local coordinate system setting by defining a temporary offset shift relative to the active workpiece coordinate system.
• G54 to G59: Selects the primary workpiece coordinate systems that define the program zero references on the machine.
• G92.1: Resets coordinate system presets, restoring the workpiece coordinate system to the reference position defined by the active zero offsets.

Conclusion

Safeguarding the lathe, tooling, and operator requires programming a spindle speed clamp prior to any constant surface speed operation. Presetting coordinate systems should only be executed from a verified physical location with dry runs enabled to avoid turret collisions. Proper parameter mapping, such as matching G-code systems and interpreter modes, ensures that coordinate shifts translate correctly across different CNC systems.

FAQ

Why does a G50 or G92 coordinate preset command cause a hard collision if executed from the middle of a program?

A coordinate preset shifts the position registers of the control without physically moving the axes, meaning the machine immediately assumes a new coordinate system based on the command. If the operator starts execution mid-program without ensuring the tool is at the correct starting position, subsequent movements will deviate from the safe toolpath. Setup operators must verify the starting point coordinates and perform a first-article dry run with the tool turret spaced safely away from the rotating chuck.

What is the difference between how Mitsubishi and Fanuc controls handle a spindle clamp cancel command?

Fanuc controls allow the programmer to cancel the maximum spindle speed clamp via a modal reset or G50 S0, returning the spindle to the machine's maximum gear speed. Mitsubishi controls implement a protective substitution logic where commanding G92 S0 will not cancel the clamp; instead, the minimum speed Q is treated as the maximum limit and S0 is treated as the minimum. Programmers must ensure the active Q and S clamp modals are explicitly declared at the start of each tool sequence to avoid unexpected speed clamping during operation.

How does Siemens manage coordinate offsets differently than block-level Fanuc G50 commands?

Siemens does not use G50 for block-level register adjustments; instead, it separates coordinate settings into a modular, multi-level zero offset memory (G54 to G599) and programmable frames (TRANS and ATRANS). Active offsets and tool nose compensations are managed dynamically through a frame stack and can be selectively suppressed using commands like G53 or SUPA. Setup operators must verify that the channel-specific parameter MD 10760 is properly set to suppress or retain tool length compensation during offset suppression blocks.