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 make use of the tilt and rotary Axes, there is no need to use DWO.
With DWO, you no longer need to set the workpiece in the exact position as programmed in the CAM system. DWO applies the appropriate offsets to account for the differences between the programmed workpiece location and the actual workpiece location. This eliminates the need to repost a program from the CAM system when the programmed and actual workpiece locations are different.
The control knows the centers of rotation for the rotary table (MRZP) and the location of the workpiece (active work offset). This data is used to produce the desired machine motion from the original CAM-generated program. Therefore, it is recommended that G254 be invoked after the desired work offset is commanded, and after any rotational command to position the 4th and 5th axes.
After G254 is invoked, you must specify 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 in a separate block.
The block in the figure below was programmed in the CAM system with the top center hole located at the center of the pallet and defined as X0, Y0, Z0.
Original Programmed Position
In the figure below, the actual workpiece is not located in this programmed position. The center of the workpiece is actually located at X1, Y-1, Z0, and is defined as G54.
Center at G54, DWO Off
DWO is invoked in the figure below. The control knows the centers of rotation for the rotary table (MRZP), and the location of the workpiece (active work offset G54). The control uses this data to apply the appropriate offset adjustments to make sure that the proper toolpath is applied to the workpiece, as intended by the CAM-generated program. This eliminates the need to repost a program from the CAM system when the programmed and actual workpiece locations are different.
Center with DWO On
G254 Program Example
G254 Programmer’s Notes
These key presses and program codes will cancel G254:
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.
G254 (DWO) is intended for 3+1 and 3+2 machining, where the B and C Axes are used to position only.
An active work offset (G54, G55, etc.) must be applied before G254 is commanded.
All rotary motion must be complete before G254 is commanded.
After G254 is invoked, you must specify an X-, Y-, and Z-Axis position prior to any cutting command, even if it recalls the current position. It is recommended to specify the X and Y Axes in one block, and the Z Axis in a separate block.
Cancel G254 with G255 immediately after use and before ANY rotary motion.
Cancel G254 with G255 any time simultaneous 4- or 5-axis machining is performed.
Cancel G254 with G255 and retract the cutting tool to a safe location before the workpiece is repositioned.