Haas Automation UMC-1000, Дополнение к руководству оператора

Страница: 49 / 70

G234 - Tool Center Point Control (TCPC)
31
%
G234 Programmer’s Notes
These key presses and program codes cancel G234:
•
[ EMERGENCY STOP]
• [ RESET]
• [ HANDLE JOG]
• [ LIST PROGRAM]
•
M02
– Program End
•
M30
– Program End and Reset
•
G43
– Tool Length Compen
•
G44
– Tool Length Compensation -
•
G49
– G43 / G44 / G143 Cancel
These codes will NOT cancel G234:
•
M00
– Program Stop
•
M01
– Optional Stop
These key presses and program codes impact G234:
•
G234 invokes TCPC and cancels G43.
• When using tool length compensation, either G43 or G234 must be active. G43 and
G234 cannot be active at the same time.
• G234 cancels the previous H-code. An H-code must therefore be placed on the same
block as G234.
• G234 cannot be used at the same time as G254 (DWO).
These codes ignore 234:
•
G28
– Return to Machine Zero Through Optional Reference Point
•
G29
– Move to Location Thru G29 Reference Point
•
G53
– Non-Modal Machine Coordinate Selection
•
M06
– Tool Change
Invoking G234 (TCPC) rotates the work envelope. If the position is close to the travel limits,
the rotation can put the current work position outside of travel limits and cause an over
travel alarm. To solve this, command the machine to the center of the work offset (or near
the center of the table on a UMC), and then invoke G234 (TCPC).
G234 (TCPC) is intended for simultaneous 4- and 5-axis contouring programs. An active
work offset (G54, G55, etc.) is required to use G234.