Mitsubishi G68.2 Inclined Surface Machining: Programming & Parameters Guide

Introduction

Activating coordinate system rotations while a tool length offset is active, without subsequently commanding spindle alignment, results in a severe tool collision. In multi-axis milling setups, failing to align the tool axis to the inclined working plane causes the physical spindle trajectory to mismatch the programmed tool offsets. As the CNC machine commands movements, the spindle head drives the cutting tool directly into a vise jaw, fixture clamp, or the machine chuck, shattering the tool and scrapping the workpiece. To eliminate this hazard, programmers must understand how to establish feature coordinates and physically align the machine tool axis.

Mitsubishi CNC systems utilize the G68.2 command to resolve this problem by defining an inclined coordinate system on any arbitrary spatial plane. This feature coordinate system rotation decouples the NC program from the machine tool's specific rotary axis kinematics. By automatically converting 3-axis orthogonal movements to match the tilted surface angle, the system allows the operator to execute operations on tilted faces without manual coordinate math or rotation calculations.

Technical Summary

Property	Details
Command Code	G68.2
Modal Group	Group 16 modal
Brands	Mitsubishi
Critical Parameters	#7915 (SLCT_SLOPE_CRD_MOD), #1247 (set19/bit2), #8901 to #8906
Main Constraint	Feedrate capped at 100 m/min during fine-segment execution (G68.2/G68.3) on M800V/M80V. Cannot be applied on combined machines if tool-side axis is C axis or both side axes share the same rotation axis.

Quick Read

• Select Cancel Code by Machine: Cancel active inclined surface machining with G69.1 on lathe systems, and G69 on machining centers.
• Command Standalone G68.2 Blocks: Program G68.2 entirely alone in its NC block to prevent triggering a P954 program error.
• Execute Tool Axis Alignment: Always command G53.1 immediately after G68.2 to physically align the spindle axis with the tilted coordinate system Z-axis.
• Avoid Interventions During Active G68.2: Do not switch to reference position return, MDI, or PLC interruption modes during active G68.2, or the control will halt with alarm M01 0185.
• Keep Radius Compensation Standard: If tool nose radius compensation (G41/G42) is active, ensure the tool nose point P is set to 0 to guarantee correct positioning.
• Observe 100 m/min Feed Limit: Respect the feedrate limit of 100 m/min during fine-segment execution on Mitsubishi M800V/M80V controls.
• Nest Coordinate Planes: Program G68.4 to build nested incremental coordinate planes relative to the active G68.2 plane.

Basic Concepts

The practical programming effect of Mitsubishi's G68.2 Inclined Surface Machining is the ability to easily define a new feature coordinate system on an arbitrary spatial plane, effectively decoupling the machining program from the machine tool's specific rotary axis kinematics. This function allows programmers to issue standard 3-axis orthogonal commands for complex multi-surface machining tasks without manually calculating axis rotations. By commanding orthogonal X, Y, and Z movements within the newly defined feature coordinate system, the controller dynamically translates these into physical rotation and linear motions.

A behavior that clearly distinguishes this brand's implementation is its R-Navi integration, which uniquely allows programmers to invoke a pre-registered machining surface directly via the G68.2 P10 syntax. Another distinguishing feature is Mitsubishi's strict separation of cancellation commands by machine type, utilizing G69.1 for Lathes and G69 for Machining Centers. Furthermore, Mitsubishi explicitly supports deep plane nesting without restriction by providing G68.4 to generate incremental multi-commands relative to the previously defined feature coordinate system.

Command Structure

The command structure for G68.2 inclined surface machining employs a variable syntax depending on the chosen coordinate plane definition method. Programmers select this method using the P parameter, which dictates how the control interprets the subsequent rotation angles and vectors. Writing G68.2 alone on its block is mandatory; combining this command with axis travel movements or other G-codes triggers a program error immediately.

When defining a plane using the standard Roll-Pitch-Yaw method (P1), the Q parameter defines the order of rotations (such as 123), while I, J, and K parameters determine the rotation angles about the respective axes. For other methods, such as three points in a plane (P2) or two vectors (P3), separate data blocks containing specific coordinates and vectors must immediately follow the G68.2 call to fully define the tilted plane.

G68.2 P1 Q__ X(U)__ Y(V)__ Z(W)__ I__ J__ K__ ;
G68.2 P2 Q0 X__ Y__ Z__ R__ ; (followed by Q1, Q2, Q3 blocks)
G68.2 P3 Q1 X__ Y__ Z__ I__ J__ K__ ; (followed by Q2 block)
G68.2 P4 X__ Y__ Z__ I__ J__ K__ ;
G68.2 P10 Q__ D__ ;

Parameter	Description	Details
P	Definition method selection code	1: Roll-Pitch-Yaw, 2: Three points, 3: Two vectors, 4: Projection angles, 10: R-Navi surface
Q	Rotation order or index specifier	Specifies rotation order (e.g., 123 in P1), points sequence in P2/P3, or workpiece number in P10
X, Y, Z	Coordinate system origin coordinates	Defines the zero point location of the feature coordinate system
U, V, W	Incremental coordinate origin values	Specifies the incremental shift of the coordinate system zero point
I, J, K	Rotation angles or vector components	Indicates angles around axes (in P1/P4 modes) or vector components (in P3 mode)
R	Rotation angle or auxiliary value	Value varies based on definition method
D	R-Navi registered surface number	Identifies the pre-registered machining surface index (used with P10)

Brand Applications

Mitsubishi

Mitsubishi controls implement G68.2 using parameters #7915 (SLCT_SLOPE_CRD_MOD) to specify the basic position basis for the rotary axes and parameters #8901 to #8906 to enable active feature coordinate display on the control counter. The system maintains modal plane information using parameter #1247 during emergency stops, and parameters #1151 and #1210 during resets.

An example of a Roll-Pitch-Yaw definition is: G68.2 P1 Q123 X33.3333 Y33.3333 Z66.6666 I45. J-35.2644 K-30.;. This defines the coordinate origin and applies sequential rotations.

Type	Identifier	Function & Behavior
Parameter	#7915 (SLCT_SLOPE_CRD_MOD)	Selects rotary axis basic position (0: Zero degree position basis, 1: Start position basis).
Parameter	#8901 to #8906	Dictates feature coordinate system display (Value 23 displays coordinates on position counter).
Parameter	#1247 (set19/bit2)	Emergency stop or power OFF behavior (0: Cancels mode, 1: Retains mode).
Parameter	#1151 (rstint) / #1210 (RstGmd/bitF)	Modal G-code retention during reset (0: Retains modal, 1: Cancels modal).
Alarm	P10	Program Error: Linear axis and two rotary axes commanded in the same block.
Alarm	P954	Program Error: Address P omitted, incorrect P value, or G68.2 not alone in block.
Alarm	M01 0185	Operation Error: MDI/PLC interruption or reference position return mode attempted during G68.2.

Warning: Attempting manual operations, switching modes to reference position return, or initiating MDI/PLC interrupts while G68.2 is active will trigger a critical M01 0185 operational error. The G68.2 mode must be completely cancelled via G69 or G69.1 before any manual interventions or setup actions are performed.

Version and Series Comparison

Mitsubishi Configuration	Cancellation Command	Feedrate Constraint	Axis Control Method
M800V/M80V Machining Center	G69	Capped at 100 m/min during fine-segment execution (G68.2/G68.3)	Align spindle axis with new coordinate Z-axis via G53.1
M800V/M80V Lathe	G69.1	Capped at 100 m/min during fine-segment execution (G68.2/G68.3)	— (no source)
Older Series (e.g. M70 / M80 / Standard)	— (no source)	— (no source)	— (no source)

Technical Analysis

The division of cancellation commands between lathes (G69.1) and machining centers (G69) in the Mitsubishi M800V/M80V series represents a critical distinction in coordinate system management. On lathe systems, the coordinate rotation cancellation must specifically address turning-oriented geometries, whereas milling machines use the standard G69 code. If a programmer mistakenly commands G69 on a lathe system to end G68.2, the system will not cancel the coordinate rotation, leaving the feature coordinates active and causing subsequent moves to offset in unexpected directions.

Another key constraint in the M800V/M80V series is the feedrate limit during fine-segment execution in inclined surface machining. When executing G68.2 or G68.3, the system caps the feedrate at 100 m/min. This performance constraint ensures block processing stability and contour accuracy when performing rapid multi-axis movements over short, fine toolpath segments. Simultaneously, setting parameter #7915 (SLCT_SLOPE_CRD_MOD) dictates the basic position basis for plane calculation. By switching between a zero degree position basis (0) and a start position basis (1), the operator controls the reference angle utilized by the controller's internal kinematics solver, preventing unexpected physical rotary axis motions during coordinate alignment.

Program Examples

; Mitsubishi Milling Machining Center Example
G94 G17 G90 ; Active feedrate per minute, XY plane, absolute coordinates
G00 X0 Y0 Z100. T01 M06 ; Spindle retraction and tool change
G68.2 P1 Q123 X33.3333 Y33.3333 Z66.6666 I45. J-35.2644 K-30. ; Define inclined plane
G53.1 ; Physically align tool spindle axis perpendicular to the tilted plane
G00 X0 Y0 Z10. ; Move to starting coordinates within tilted coordinate system
G01 Z-5. F200 ; Feed tool into work
G01 X50. Y0 F500 ; Cut slot on the inclined face
G01 X50. Y30. ; Continue path
G00 Z100. ; Retract tool
G69 ; Cancel inclined surface machining coordinate rotation
G00 X0 Y0 ; Return to base coordinates

Dry Run Verification:

dry run: Set the feedrate override to 10% and enable single block mode before starting execution. In block G68.2, verify on the coordinate status counter that the active coordinates shift to represent the new tilted plane. In the G53.1 block, closely monitor the rotation of the machine table or spindle head to ensure the tool aligns perpendicular to the workpiece plane without hitting the vise jaws or clamps. Step through the linear interpolation blocks to confirm the tool path tracks parallel to the inclined face. Finally, execute G69 and confirm the position display returns to the machine base coordinates.

; R-Navi Surface Selection Example
G94 G17 G90 ; Absolute milling parameters
G00 X0 Y0 Z50. ; Move to safe clearance
G68.2 P10 Q1 D2 ; Invoke pre-registered machining surface 2 for workpiece 1
G53.1 ; Align tool axis to the registered surface Z-axis
G00 X0 Y0 Z10. ; Safe approach on the tilted plane
G69 ; Cancel inclined plane mode and restore base coordinate system

Dry Run Verification:

dry run: Execute in single block mode with the cutting spindle disabled. Ensure that the R-Navi database has workpiece 1 and surface 2 correctly registered on the control before starting. Step through the G68.2 P10 block and verify that the coordinates shift. Watch the spindle rotation during G53.1 to ensure it moves safely. Confirm G69 successfully resets the coordinates to base settings.

Error Analysis

Alarm Code	Classification	Trigger Condition	Operator Symptom	Root Cause / Fix
P10	Program Error	Linear axis and two rotary axes commanded in the same block	Cycle start halts, alarm P10 displays	Simultaneous contouring axes is 4 or less; modify the NC program to prevent commanding linear and two rotary moves in a single G68.2 block.
P954	Program Error	Address P omitted, incorrect P value, or G68.2 not alone in block	Execution stops, alarm P954 displays	The command is written with invalid P values or travel motion in the same block; rewrite G68.2 on an isolated block by itself.
M01 0185	Operation Error	Attempting MDI interruption, PLC interruption, or reference position return mode during G68.2	Machine halts operation, alarm M01 0185 displays	Manual mode change or PLC interruption attempted before canceling G68.2; command G69/G69.1 to cancel the coordinate rotation before manual operations.
P35	Program Error	Address I, J, or K exceeds the setting range (-360.0 to 360.0)	NC interpreter halts, alarm P35 displays	The programmed rotation angles exceed the maximum allowed limits; edit the angles to lie within the valid -360.0 to 360.0 degree range.
P952	Program Error	Cancel command issued during active circular interpolation or canned cycle	Alarm P952 displays, path halts	Attempting to cancel inclined coordinate system while a modal canned cycle or arc move is active; program G80 to cancel canned cycles or change feed to linear G01 before commanding G69/G69.1.
P955	Program Error	Points designated are identical, collinear, distance is less than 0.1mm, vectors not perpendicular, or ra/rb parallel	Alarm P955 displays, program stops	Invalid geometry definition in P2 (three points) or P3 (vectors) modes; correct the coordinates or vectors to establish valid perpendicular planes.

Application Note

Activation of G68.2 during active tool length offset compensation without immediate tool axis direction control via G53.1 leads to a mismatch between the physical tool spindle orientation and the new feature plane. The resulting misalignment will drive the milling spindle or turning tool directly into a physical obstruction such as a vise jaw, chuck barrier, or fixture clamp, damaging the machine head and scrapping the workpiece. To eliminate this crash risk, operators must ensure that all manual turret turning and clamp adjustments are performed only after executing a full coordinate cancellation via G69 (on machining centers) or G69.1 (on lathes), and that tool path coordinates are displayed using counter parameters #8901 to #8906 for visual verification before cycle start. Additionally, any manual PLC or MDI interruption must be avoided until G69 or G69.1 has successfully returned the CNC system to base coordinates, ensuring the spindle operates within a safe workspace envelope.

Related Command Network

• G68 (Coordinate Rotation): The standard 2D coordinate rotation command that G68.2 extends for full 3D spatial tilted plane calculations.
• G68.2 (Tilted Working Plane): Establishes the feature coordinate system on the inclined surface, which serves as the core mechanism for multi-axis face machining.
• G65 (Macro Call): Used to execute custom macro subprograms that can dynamically calculate G68.2 parameters for variable inclined angles.
• G53.1 (Tool Axis Direction Control): Aligns the machine tool's spindle axis perpendicular to the newly defined G68.2 feature coordinate system.
• G68.3 (Inclined Surface Tool Axis): Defines the inclined surface coordinate system based directly on the current orientation of the tool axis.
• G68.4 (Incremental Inclined Surface): Allows deep plane nesting by defining a new coordinate system incrementally relative to the active G68.2 plane.

Conclusion

Achieving reliable multi-axis results with Mitsubishi G68.2 requires strict separation of coordinate definition, axis alignment, and mode cancellation. By isolating the G68.2 command on its own block, immediately following it with G53.1 tool axis control, and using the correct machine-specific cancel code (G69 for machining centers or G69.1 for lathes), operators protect the machine spindle and fixture setup from costly alignment collisions.

Frequently Asked Questions

How does parameter #7915 affect Mitsubishi G68.2 plane alignment?

Parameter #7915 (SLCT_SLOPE_CRD_MOD) dictates the basic position calculation of the machine's rotary axes. Setting it to 0 sets a zero degree position basis, while setting it to 1 sets a start position basis; choose the value that matches your post-processor output to prevent rotary axis positioning errors.

What causes the M01 0185 alarm code during active inclined surface machining?

The M01 0185 operation alarm occurs when an operator attempts to switch modes to reference position return, or initiates an MDI or PLC interruption while G68.2 is active. Always command a G69 or G69.1 cancellation block before performing manual setup interventions or coordinate adjustments.

Why is G68.2 commanded on a block entirely by itself?

Including axis travel coordinates or other G-codes in the same block as G68.2 will trigger a P954 program error because the control requires the plane definition math to resolve before any physical motion occurs. Write G68.2 as a standalone block, and place all subsequent movements in subsequent blocks.