Haas Automation UMC-1000, Operator'S Manual Supplement

Page: 54 / 70

G254 - Dynamic Work Offset (DWO) (Group 23)
36
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.