G254 - Dynamic Work Offset (DWO) (Group 23)

Next Generation Control Mill Operator's Manual

The Online Interactive Operator's Manual is currently available in English only.

A PDF version of the Operator's Manual is available for download in multiple languages. Click the link below to view the Operator's Manual in your language. Click "Continue" to view the online version in English.

Get a translated PDF Download Continue

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.

caution: The B-Axis value of the work offset you use with G254 MUST be zero.

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.

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 the rotary motion. After the rotary motion finishes, 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 position in a separate block.
caution: Be sure to cancel G254 with G255 when your program does simultaneous 4- or 5-axis machining.
note: For clarity, the illustrations in this section do not depict workholding.

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

% O00004 (DWO SAMPLE) ; G20 ; G00 G17 G40 G80 G90 G94 G98 ; G53 Z0. ; T1 M06 ; G00 G90 G54 X0. Y0. B0. C0. (G54 is the active work offset for) ; (the actual workpiece location) ; S1000 M03 ; G43 H01 Z1. (Start position 1.0 above face of part Z0.) ; G01 Z-1.0 F20. (Feed into part 1.0) ; G00 G53 Z0. (Retract Z with G53) ; B90. C0. (ROTARY POSITIONING) ; G254 (INVOKE DWO) ; X1. Y0. (X and Y position command) ; Z2. (Start position 1.0 above face of part Z1.0) ; G01 Z0. F20. (Feed into part 1.0 ) ; G00 G53 Z0. (Retract Z with G53) ; B90. C-90. (ROTARY POSITIONING) ; X1. Y0. (X and Y position command) ; Z2. (Start position 1.0 above face of part Z1.0) ; G01 Z0. F20. (Feed into part 1.0 ) ; G255 (CANCEL DWO) ; B0. C0. ; M30 ; %

G254 Programmer’s Notes

These 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.

  1. G254 (DWO) is intended for 3+1 and 3+2 machining, where the B and C Axes are used to position only.

  2. An active work offset (G54, G55, etc.) must be applied before G254 is commanded.

  3. All rotary motion must be complete before G254 is commanded.

  4. 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.

  5. Cancel G254 with G255 immediately after use and before ANY rotary motion.

  6. Cancel G254 with G255 any time simultaneous 4- or 5-axis machining is performed.

  7. Cancel G254 with G255 and retract the cutting tool to a safe location before the workpiece is repositioned.

Be aware: Many service and repair procedures should be done only by authorized personnel. The service technicians at your Haas Factory Outlet (HFO) have the training, experience, and are certified to do these tasks safely and correctly. You should not do machine repair or service procedures unless you are qualified and knowledgeable about the processes.

Danger: Some service procedures can be dangerous or life-threatening. DO NOT attempt a procedure that you do not completely understand. Contact your Haas Factory Outlet (HFO) and schedule a service technician visit if you have any doubts about doing a procedure.

Feedback