G254 Dynamic Work Offset (DWO) (Group 23)

---

G254 Dynamic Work Offset (DWO) is similar to TCPC, except that it is designed for use with 3+1 or 3+2 positioning, not for simultaneous 4- or 5-axis machining. If the program does not use the B and C Axes, there is no need to use DWO.VMT - G254 - Dynamic Work Offset (DWO) (Group 23)The default mode for programming the VR/GM-2-5AX tracks the position of the spindle face by adding the pivot length vector to the B/C axis pivot point position. Setting 305 stores the magnitude of this vector. If tool length compensation is active, the active tool offset is added to the magnitude of the pivot length vector to track the tool tip.The control knows the centers of rotation for the rotary axes (MRZP), the location of the workpiece (active work offset), and the tool length offset. The control uses this data to calculate the position of tool tip relative to the active work offset as the tool tip moves.Use this mode for 3+1 axis or 3+2 axis positioning. Pivot Length Adjustment and Tool Length Compensation is not for simultaneous 4th or 5th axis machining. The VMT software always uses Pivot Length Adjustment and Tool Length Compensation unless overridden by Tool Center Point Control (TCPC).Pivot Length Adjustment and Tool Length Compensation replaces Dynamic Work Offsets (DWO) G254 on the GM-2-5AX. G254 is not available on the GM-2-5AX.

---

CAUTION: Before rotary motion, use a G53 Non-Modal Machine Coordinate motion command to safely retract the tool from the workpiece and allow clearance for Z-axis motion. Command the Z axis to the home position. Command the rotary motion. Command an X-, Y-, and Z-Axis position before a cutting command, even if it recalls the current position. The program should specify the X- and Y-Axis position in one block and the Z-Axis position in a separate block.

---

G254 Programmer's NotesThese key presses and program codes will cancel G254: [EMERGENCY STOP]
[RESET]
[HANDLE JOG]
[LIST PROGRAM]
G255 -- Cancel DWO
M02 -- Program End
M30 -- Program End and Reset
These codes will NOT cancel G254:M00 -- Program Stop
M01 -- Optional Stop
Some codes ignore G254. These codes will not apply rotational deltas:*G28 -- Return to Machine Zero Through Optional Reference Point
*G29 -- Move to Location Through G29 Reference Point
G53 -- Non-Modal Machine Coordinate Selection
M06-- Tool Change
*It is strongly recommended that you not use G28 or G29 while G254 is active, nor when the B and C Axes are not at zero.

---