Programming instructions

ADT-CNC4620 Programming Manual
- 31 -
X: new X axis absolute coordinates of current position;
Z: new Z axis absolute coordinates of current position;
Instruction function: set the absolute coordinates of current position, and thus create
workpiece coordinate system (also floating coordinate system). After executing this
instruction, the system sets current position as the program home. When workpiece
coordinate system is created, absolute coordinate programming enters the coordinates
according to this coordinate system, until G50 is executed again to create new workpiece
coordinate system. G50 is non-modal G instruction.
X or Z isn’t entered in G50 instruction, the coordinate axis isn’t entered sets the coordinates
according to current absolute coordinates; if both X and Z aren’t entered, current
coordinates won’t be changed. Aslong as G50 is executed, current position will be set as the
program home.
Program home
Before setting coordinate system with G50
After setting coordinate system with G50
As shown in the figure above, after instruction “G50 X100 Z150” is executed, the
workpiece coordinate system as shown in the figure is created, and point (X100, Z150) is
set to program home.
Note: If G50 is executed to set coordinate system in tool length compensation state, the
absolute coordinates displayed by the system are the coordinate value after current
tool offset is modified; program home is the position defined by G50 coordinate value
in workpiece coordinate system. Return to program home in tool length compensation
state, the position of home end is the program home position after tool length
compensation is canceled.
For example:
Current tool
compensation state
Coordinates after G50 X20 Z20 is
executed
#01 tool
compensation
T0100 X:20 Z:20 X:12
T0101 X:32 Z:43 Z:23
3.5. Fixed cycle
To simplfy the programming, the system provides a G instruction of single processing cycle
that only uses one block to complete fast moving positioning, linear/thread cutting, and finally
returns to start point:
G90: axial cutting cycle
G94: radial cutting cycle
G92: thread cutting cycle