G68 Mirror Image and Balance Cut Programming for CNC Lathes

Introduction

A catastrophic hard collision occurs when a turning tool or indexable turret gantry crashes directly into the revolving jaws of a spindle chuck or workpiece clamp at rapid traverse. Under uncompensated coordinate shifts, macro loop errors, or uncoordinated multi-path overrides, the tool post travels along an unaligned path, shatters the cutting insert, bends the axis ball screw, and triggers high-current axis-overload servo alarms. In multi-turret and multi-path turning centers, managing symmetrical machining on facing tool posts and coordinating dual-tool synchronization (balance cutting) requires precise execution of coordinate mirroring and feed synchronization. When machining long, thin raw stock held in chuck jaws or vise clamps, simultaneous dual-sided cutting prevents workpiece deflection, suppresses structural slack, and eliminates vibration, but a single synchronization mismatch will cause the thin stock to vibrate violently, producing chatter marks and converting raw materials into ruined scrap.

Technical Summary

Parameter / Attribute	Technical Specification
Primary Commands	G68 (Mirror / Balance Cut ON), G69 (Cancel); G15 (Mitsubishi Balance Cut ON), G14 (Cancel); MIRROR/AMIRROR (Siemens Native)
Modal Group / Class	Group 04 (Fanuc, Siemens ISO), Group 15 / Group 18 (Mitsubishi)
Supported Brands	Fanuc, Siemens, Mitsubishi
Critical Parameters	Fanuc: No. 1022 (basic axes), No. 8103 (P-code format); Siemens: MD 10610 ($MN_MIRROR_REF_AX), SD 42900 ($SC_MIRROR_TOOL_LENGTH); Mitsubishi: #1202 (mirofs cutter distance), #1118 (wear comp direction), #1244 (sync feed blocks)
Main Constraints	Balance cut only synchronizes cutting feed start (no dynamic path/velocity tracking); mirroring and balance cutting are mutually exclusive under identical modal groups; high-speed high-accuracy modes are incompatible.

Quick Read

• Activate mirror image coordinates with G68 (or MIRROR/AMIRROR in Siemens) when cutting symmetrical geometries with a facing tool post to automatically reverse the X-axis coordinate sign.
• Use G68 Pp (Fanuc) or G15 [L__] (Mitsubishi) to synchronize the start of the cutting feed on two opposing turrets when performing balance cutting on long, thin workpieces.
• Always verify that tool length mirroring settings (like Siemens SD 42900) and facing turret wear compensation direction (like Mitsubishi Parameter #1118) are active to prevent uncompensated paths.
• Ensure feedrates, travel distances, feed holds, overrides, and interlocks are identical in both programs for balance cutting, as the control does not dynamically coordinate speed after synchronization.
• Avoid executing program format switches (like Mitsubishi G188) or macro calculations while mirroring or balance cutting is active to prevent program errors like P29 or look-ahead buffer overruns.
• Deactivate mirroring or balance cutting using G69 (or G14 / bare MIRROR) and confirm that coordinate offsets are restored before resuming standard single-axis automatic operations.

Basic Concepts

The practical programming of double turret mirror imaging allows application engineers to write symmetrical toolpaths for a facing tool post on the opposite side of the coordinate system as if it were on the same side, simplifying multi-axis program development and reducing engineering hours. When turning complex profiles on opposing spindles, the profile is defined once in a subprogram and executed across both spindles by applying coordinate system offsets and mirroring the Z-axis. By dynamically reversing coordinate signs, the controller translates the base turret path into a symmetrical path for the opposed turret without manual recalculation.

For balance cutting, feed synchronization permits the simultaneous coordinate start of two independent tool posts. When machining long, thin workpieces on turning centers, applying cutting tools from opposite sides of the raw stock prevents workpiece deflection, suppresses structural slack, avoids severe vibrations, and reduces overall cycle times by half. By balanced distribution of mechanical forces, the risk of part distortion during heavy stock removal is minimized, ensuring tight dimensional tolerances.

Setup operators and programmers must remain highly vigilant during setup and program execution. Prior to starting an automatic cycle, the raw stock must be positioned and clamped securely within the spindle chuck, table clamps, or custom workholding. Because balance cutting only coordinates the start of the cutting feed but does not dynamically track synchronization thereafter, the programmer must ensure that the feedrates, travel distances, feed holds, overrides, and interlock keys of both part systems are configured identically. If a programming mismatch is executed, the uneven forces on the opposing turrets will cause the thin workpiece to vibrate violently, resulting in chatter marks, tool breakage, and a completely ruined scrap part.

Command Structure

The command structure of G68 depends on whether it is used for mirror imaging on facing tool posts or for balance cutting. For mirror imaging, G68 acts as a modal switch that intercepts coordinate instructions for the target axis (typically X) and negates the value. The coordinate shift amount is defined by physical turret distance parameters in the controller, allowing the tool to move symmetrically. When the mirror function is canceled via G69, the controller restores the original coordinate system.

For balance cutting, the syntax includes a path selector or a synchronization number. The G68 or G15 block acts as a wait-gate or interlock. When both paths execute this code block, they synchronize their start timing. Depending on the system parameters, the controller evaluates the path combinations as binary sums or direct digits.

Syntax layouts for the primary systems are configured as follows:

; Fanuc & Mitsubishi Mirror Image
G68 ; (Mirror image ON)
G69 ; (Cancel mirror image)
; Fanuc Balance Cut
G68 Pp ; (Balance cut ON, path combination p)
G69 ; (Cancel balance cut)
; Siemens Native Mirroring
MIRROR X0 Y0 Z0 ; (Absolute mirroring)
AMIRROR X0 Y0 Z0 ; (Additive mirroring)
MIRROR ; (Cancel mirroring)
; Mitsubishi Lathe Balance Cut
G15 [L__] ; (Balance cut ON, synchronization number L)
G14 ; (Cancel balance cut)

Address / Address Argument	Target System	Function / Description
P	Fanuc	Specifies path combination for balance cut. When Parameter No. 8103 Bit 1 is 0, it is a sum of binary weights (e.g., P3 represents Path 1 + Path 2). When 1, it represents a direct list of path digits (e.g., P123 for Paths 1, 2, and 3).
L	Mitsubishi	Timing synchronization operation number (value range: 0 to 9999). Specifies the identifier for matching G15 blocks across turrets.
X, Y, Z	Siemens (Native)	Defines the coordinate value of the mirroring plane. Mirroring is applied relative to the defined reference coordinate (typically X0, Y0, or Z0).

Brand Applications

Fanuc

In Fanuc lathe controllers, double turret mirror imaging and balance cutting are managed via Group 04 commands. Symmetrical cutting coordinate shifts apply to the axis defined by Parameter No. 1022. The P-address formatting for path combinations is set by Parameter No. 8103.

To activate coordinate mirroring on the opposing turret, program a standalone G68 block. For balance cutting, program G68 P_ to synchronize the start of pulse distribution. Tool compensations must be cancelled before toggling modes to prevent buffer issues.

• Parameter No. 1022: Defines the basic 3 axes. Symmetrical cutting applies coordinates inversion strictly to the X-axis of these axes.
• Parameter No. 8103 Bit 1 (MWP): Determines input format for balance cut path combination. 0 uses binary sum (e.g., P3 represents path 1 and path 2); 1 uses path numbers (e.g., P123).
• Parameter No. 19625: Sets the number of blocks (N) that the controller reads ahead in offset mode. Active tool compensation allows a maximum of N-2 non-movement blocks.
• Alarm PS0191: Triggered by a taper height violation in G78/G77 cycles where the logic |u/2| >= |r| is violated. Fix: Correct cycle parameters.
• Alarm PS0082: Triggered when a tool offset change (T code) is specified in the same block as an automatic tool length measurement cycle (G37). Fix: Separate commands into individual blocks.
• Alarm PS0370: Value from P1 to P8 specified without activating the multi-step skip function.
• Version Differences: Series 15 Program Format (Parameter No. 0001 Bit 1 FCV = 1) implements a legacy format where rough-cutting parameters are disabled, and G71/G72 Type I/II shapes are restricted.

Pressing the NC reset key will immediately cancel G69 mirroring and restore the base coordinate system, which can cause severe axis movements if manual jog is performed afterwards.

Siemens

Siemens SINUMERIK controls handle dual turret coordinate operations using external language mode (G291) or native Siemens frames (G290). The axis around which mirroring occurs is defined in MD 10610 $MN_MIRROR_REF_AX. Axis evaluation behavior is set by MD 10612 $MN_MIRROR_TOGGLE.

In native mode, program MIRROR X0 Y0 Z0 to apply absolute mirroring, or AMIRROR for additive mirroring. In ISO Dialect mode, program a standalone G68 to activate the dual turret mode. Tool length sign mirroring requires SD 42900 configuration.

• MD 10610 $MN_MIRROR_REF_AX: Specifies the axis around which mirroring is performed (0: programmed axis negation; 1, 2, or 3: reference axis X, Y, or Z).
• MD 10612 $MN_MIRROR_TOGGLE: Determines evaluation behavior (0: programmed values evaluated; MIRROR X0 deactivates X-axis mirroring).
• SD 42900 $SC_MIRROR_TOOL_LENGTH: Non-zero values invert signs of tool length ($TC_DP3 to $TC_DP5) and base components ($TC_DP21 to $TC_DP23) of mirrored axes.
• MD 10604 $MC_WALIM_GEOAX_CHANGE_MODE: Working area limitation mode during geometry axis switchover (hard-locked on SINUMERIK 802D sl).
• MD 18800 $MN_MM_EXTERN_LANGUAGE: External language option flag (must be 1 to compile G68/G69 commands).
• Alarm 61800: Triggered when G291 or G68/G69 is commanded but MD 18800 is not set. Fix: Set MD 18800 to 1 and perform an NCK reset.
• Alarm 61815: Technological turning cycle (e.g. CYCLE374T/CYCLE376T) executed under active tool nose radius compensation mode. Fix: Ensure G40 is active before cycle call.
• Version Differences: Machine parameter MD 10604 is locked and unchangeable on 802D sl but changeable on 840D sl. Multi-edge turning (G51.2/G50.2) is supported on 840D sl but omitted on 802D sl.

Calling MIRROR without axis parameters will cancel all previously programmed frames, including active rotation or scale frames.

Mitsubishi

Mitsubishi turning centers support both G-code based and T-code based coordinate mirroring. Whether the tool selection code can activate mirror imaging is controlled by Parameter #1119 Tmiron. The cutter distance offset is set in Parameter #1202 mirofs.

Activate mirroring on the facing tool post using a standalone G68 block, or initiate balance cutting by programming G15 L_. Tool nose wear direction inversion is governed by parameter #1118.

• Parameter #1119 Tmiron: T-command Mirror Image selection (1: valid, 0: invalid).
• Parameter #1203 TmirS1 / #1204 TmirS2: Turret selection masks for T-command mirror image (tools 1-32 and 33-64). Value range: 0 to FFFFFFFF.
• Parameter #1202 mirofs: Distance between cutters (radius value physically separating base and facing turrets).
• Parameter #1273 ext09/bit4: Mirror-valid axis (0: first axis in part system; 1: plane selection linked).
• Parameter #1118 mirr_A: Reverses X-axis tool nose wear compensation sign for facing turret (1: automatic).
• Parameter #1244 set16/bit2: Configures whether G15 synchronization executes on cutting feed blocks only or all blocks.
• Program Error (P371): G68 commanded while external mirror image or parameter mirror is already active. Fix: Cancel prior mirroring mode.
• Program Error (P29): G188 program format switch commanded in active T-code mirror mode, or mirror/balance cut issued during active high-speed control. Fix: Deactivate active mirroring first.
• Operation Error (M01 1035): Mirror image turned ON for an axis in a part system whose axes are currently exchanged with complex control. Fix: Deactivate axis exchange.
• Version Differences: Under standard lathe lists, balance cut is G15/G14 (Group 18). Under G-code list 6 & 7, balance cut is mapped to G68/G69 (Group 15). If both functions are active under list 6/7, G68/G69 defaults to mirror image and disables balance cut.

Do not attempt to trigger G188 format switches or manual jog resets when T-code mirroring is active, as this will trigger high-current axis-overload alarms or program errors.

Brand Comparison

Topic / Feature	Fanuc	Siemens	Mitsubishi
Primary Command	G68 / G69 (Group 04) for double turret mirror or balance cut path combination	MIRROR / AMIRROR (native frame statements); G68 / G69 (Group 04) in ISO dialect mode	G68 / G69 (Group 15) for double turret mirror; G15 / G14 (Group 18) for balance cut
T-Code Integration	— (no source)	— (no source)	Supported; parameter-defined tool select codes can dynamically trigger mirroring ON/OFF
Compensation Adjustments	Requires manual programming of arc directions (G02/G03) and compensation vectors (G41/G42)	Automatically inverts path compensation vectors (G41 <-> G42) and arc interpolation directions (G02 <-> G03)	Compensations tracked via specialized modal info storage block during arbitrary reverse run
Tool Length Mirroring	Defines coordinate inversion strictly for X-axis in Parameter No. 1022	Sign inversion of tool length and wear components using setting data SD 42900 and SD 42910	Wear compensation sign reversed automatically for facing turret using Parameter #1118 mirr_A
Multi-Path Standby Interlock	Rigid hard-coded interlock halts active path until other path reads corresponding G68/G69 block	Decoupled native frame handling	Timing synchronization option #1244 set16/bit2 runs on all blocks or cutting feed blocks only
Compiler Register Safeguards	— (no source)	MIRROR frame reset cancels all previously set programmable frames	Blocks G188 switch under active T-code mirroring, throwing Program Error P29

Technical Analysis

The underlying architectural difference between the controllers lies in how coordinate inversion is treated. Fanuc implements coordinate mirroring strictly on the axis level mapped in Parameter No. 1022, forcing the programmer to manually swap G02/G03 arc directions and G41/G42 tool nose radius compensation vectors in their subprograms. Conversely, Siemens SINUMERIK natively integrates mirroring into its geometric frame engine. When MIRROR or AMIRROR is active, the control automatically reverses the sign of the programmed coordinate values, adjusts the path compensation vectors (G41 swaps to G42 and vice versa), and inverts circular interpolation directions (G02 swaps to G03 and vice versa). This reduces subprogram programming errors but requires setup operators to verify that tool length mirroring is active through the setting data SD 42900 to prevent tool crashes.

Mitsubishi provides a hybrid solution, allowing both G-code based mirror commands (Group 15 G68) and automated T-code mirror activation. By configuring Parameter #1119 Tmiron and defining the turret mask in parameters #1203 and #1204, a tool selection command can automatically invoke mirroring when a tool on the facing turret is selected. Additionally, the wear compensation sign for the facing turret is dynamically reversed via Parameter #1118 mirr_A, which is calculated using the distance between cutters defined in Parameter #1202 mirofs.

During balance cutting, Fanuc's synchronization relies on the G68 Pp command, which uses binary weighting (sum of paths, e.g., P341 when Parameter No. 8103 is 0) or path combinations (e.g., P123). This triggers a hard standby state where the paths wait for one another. In contrast, Mitsubishi uses G15 [L__], where the L parameter coordinates the exact timing synchronization number. Mitsubishi's parameter #1244 set16/bit2 allows operators to configure whether synchronization is evaluated on all blocks or restricted to cutting feed blocks only, providing flexibility in high-feed air cuts.

Program Examples

Fanuc Double Turret Mirroring

O1001 ;
G21 G40 G90 G95 ;
T0101 ; (Select tool 1, wear offset 1 on base tool post A)
G00 X100.0 Z10.0 ; (Position base turret)
G68 ; (Shift coordinate system to facing turret B, mirror image ON)
T0202 ; (Shift tool offset to facing turret tool)
G01 X80.0 Z-20.0 F0.2 ; (Symmetrical cutting with inverted X-axis sign)
G00 X120.0 Z10.0 ; (Retract turret)
G69 ; (Cancel mirror image, restoring base coordinate system)
M30 ;

dry run

First, G21 sets metric units, G40 cancels cutter compensation, G90 establishes absolute positioning, and G95 selects feed per revolution. Next, T0101 indexes Tool 1 on the base tool post A and positions it rapidly to X100.0, Z10.0. The G68 command is executed in a standalone block, shifting the coordinate system and inverting the X-axis sign. Tool offset T0202 is then applied for the facing turret tool. The subsequent G01 feeds the tool to X80.0 (physically mirrored on the opposite side of the spindle) and Z-20.0 at 0.2 mm/rev. After retracting to safety coordinates, G69 cancels the mirroring mode to restore standard coordinate registers, and the program terminates with M30.

Siemens Native Frame Mirroring

; Siemens SINUMERIK Native mode
G290 ; Switch to native Siemens mode
G90 G95 ;
TRANS X0 Z100.0 ; Set zero point offset at Spindle 1
T1 D1 ; Select Tool 1 with tool offset D1
G0 X80.0 Z10.0 ; Rapid positioning
G1 Z-30.0 F0.25 ; Machining on Spindle 1
G0 X100.0 Z10.0 ; Retract tool
TRANS X0 Z0 ; Clear zero offset
TRANS Z200.0 ; Shift coordinate to Spindle 2
AMIRROR Z0 ; Apply additive mirroring on the Z-axis for Spindle 2
G0 X80.0 Z10.0 ; Position tool relative to mirrored coordinate system
G1 Z-30.0 F0.25 ; Machining mirrored profile on Spindle 2
G0 X100.0 Z10.0 ; Retract tool
MIRROR ; Cancel mirroring and reset active mirroring frames
M30 ;

dry run

The program initiates by executing G290 to switch to native Siemens programming language, configuring absolute coordinates and feed per revolution. The TRANS command shifts the active zero offset to Z100.0 for Spindle 1 machining. Tool 1 is selected, positioned at Z10.0, and feeds to Z-30.0 at 0.25 mm/rev. The tool is then retracted, the offset is cleared, and a new TRANS offset is applied at Z200.0 for Spindle 2. The AMIRROR Z0 command applies an additive mirror frame on the Z-axis. Due to the mirrored frame, the toolpath feed to Z-30.0 is physically reversed along the Z-axis, executing an identical contour relative to the Spindle 2 face. Finally, MIRROR resets all active mirroring frames, restoring standard linear coordinate systems prior to M30 execution.

Mitsubishi G15 Balance Cutting

; Mitsubishi Part System 1 (Turret 1)
O2001 ;
G21 G40 G90 G95 ;
T0101 ; (Index Tool 1 on Turret 1)
G00 X60.0 Z5.0 ; (Position to standby start coordinate)
G15 L10 ; (Activate balance cut timing sync number L10)
G01 Z-40.0 F0.2 ; (Standby and execute synchronized cutting feed with Turret 2)
G00 X80.0 Z5.0 ; (Retract tool)
G14 ; (Cancel balance cut mode)
M30 ;

dry run

First, the controller selects metric unit mode, cancels tool nose radius compensation, and applies absolute positioning. Next, Tool 1 is indexed and positioned at X60.0, Z5.0. When the controller reads G15 L10, Part System 1 enters an interlock standby state, halting movement. Once Part System 2 reads its corresponding G15 L10 command block, the sync condition is met, and both systems simultaneously feed to Z-40.0 at 0.2 mm/rev, canceling workpiece deflection. The tool then rapids to clearance, G14 cancels the balance cut synchronization, and the program terminates with M30.

Error Analysis

Brand	Alarm Code	Trigger Condition	Operator Symptom	Root Cause / Resolution
Fanuc	Alarm PS0082	Tool offset change (T code) is specified in the same block as an automatic tool length measurement cycle (G37).	The machine halts execution mid-program, the cycle start light turns off, and "PS0082 G37 SPECIFIED WITH T CODE" is displayed on the CRT screen.	Modify the NC program to separate the T-code tool select block and the G37 cycle block. Ensure the tool offset is active prior to calling G37.
Siemens	Alarm 61800	G291 ISO dialect mode switch or G68/G69 external command is executed when the external language parameter MD 18800 is not set to 1.	The control displays "Alarm 61800: External CNC system missing" and enters a feed hold state, refusing to run the ISO blocks.	Set machine data MD 18800 $MN_MM_EXTERN_LANGUAGE to 1 and perform an NCK reset to activate the external ISO compiler option.
Siemens	Alarm 61815	Executing technological turning cycles (e.g. CYCLE374T or CYCLE376T) under active tool nose radius compensation mode (G41/G42).	CNC program stops at the cycle call block, the alarm buzzer sounds, and "Alarm 61815: G40 not active" is displayed.	Insert a G40 command to deactivate tool nose radius compensation prior to invoking the turning cycle, then re-enable G41/G42 inside the subprogram if required.
Mitsubishi	Program Error (P29)	G188 program format switch commanded in active T-code mirror image mode, or mirror/balance cut issued during active high-speed control.	Program halts immediately, showing "P29 Program Error", and block execution is blocked.	Cancel the active T-code mirror or high-accuracy mode (e.g. G05 P0) before commanding the G188 format switch.

Application Note

Workpiece deflection and severe structural slack are prevented during the machining of long, thin raw stock by applying cutting forces symmetrically from both sides of the part using simultaneous dual-turret balance cutting. The setup operator must physically secure the raw stock in the rotating jaws of a spindle chuck or a custom table vise jaw. Since the controller only coordinates the initial feed start point during a G68 (Fanuc) or G15 (Mitsubishi) synchronization block, any subsequent velocity or override mismatch will cause uneven forces, producing intense chatter marks and tool breakage. The programmer must ensure that feedrates, travel distances, and override locks are programmed identically in both part programs. Under offset mismatch conditions, the indexing turret will travel along a shifted trajectory, resulting in a catastrophic hard collision where the turning tool crashes directly into the revolving jaws of the spindle chuck or workpiece clamps, shattering the tool assembly and triggering overload alarms.

Related Command Network

• G00 / G01: Provides the basic rapid positioning and linear cutting movements that are modified by G68 coordinate mirroring. See the G00 Rapid Traverse and G01 Linear Interpolation reference guides.
• G40 / G41 / G42: Controls tool nose radius compensation vectors, which must be deactivated before changing mirror frames or cycles to prevent offset errors. See the Tool Nose Radius Compensation reference guide.
• G290 / G291: Switches between Siemens native mode and external ISO dialect mode, enabling G68/G69 compile compatibility.
• G51.1: Controls programmable axis mirroring for machining centers, which serves as a mill-specific counterpart to lathe G68 dual-turret mirror commands. See the G51.1 Programmable Mirror Image guide.
• G52: Sets the local coordinate system shift. See the G52 Local Coordinate System guide.
• G65: Calls custom macros non-modally, which can pass arguments to sync routines. See the G65 Custom Macro Call guide.

Conclusion

Successful implementation of dual turret mirroring and balance cutting hinges on verifying that coordinate offsets, axis parameters, and override states are completely synchronized. Setup operators must perform dry runs in single-block mode and closely monitor tool offsets to eliminate collision risks. Before resuming standard turning cycles, the cancel commands G69 or G14 must be explicitly executed to restore the default coordinate registers.

Frequently Asked Questions

How does G68 mirror imaging differ from G15 balance cutting?

G68 mirroring shifts workpiece coordinate registers and inverts axis signs (typically the X-axis) to allow a program written for a base turret to cut symmetrical profiles on a facing turret. G15 balance cutting is a timing synchronization command that coordinates the start feed pulse of two independent turrets to cut a single part from both sides. To prevent tool crashes, verify that you do not call G68 mirroring and G15 balance cutting concurrently on the same part system axis unless parameter list priorities are established.

Why does a balance cut program fail when feedrate overrides are adjusted?

The balance cut command only acts as a start-sync gate and does not dynamically coordinate feedrates or axis overrides once the tools begin feeding. If an operator adjusts the override switch on one part system but not the other, the turrets will travel at different feedrates, leading to uneven force distribution, severe vibration, and scrap parts. Always lock the override keys during automatic operation to guarantee that both tool posts move at identical velocities.

What causes Alarm 61815 on Siemens SINUMERIK controllers during mirroring?

Siemens Alarm 61815 is triggered when a technological turning cycle (such as CYCLE374T) is called while tool nose radius compensation (G41/G42) is active. Because native mirroring automatically swaps compensation vectors, executing a canned cycle with active compensation confuses the path engine. To resolve this, program a G40 command to cancel compensation before the cycle call, and rely on the cycle's internal radius compensation parameters to govern toolpath offsets.