Programming instructions

3-12
Motion Commands, Dimension Inputs NC Programming 17VRS
DOK-MTC200-NC**PRO*V17-ANW1-EN-P
Programmed Absolute Zero Offset 'G50' Programmed incremental zero
offset 'G51'
The programmed zero offsets G50 and G51 move the machining zero
point with
•
G50 absolute or
•
G51 incremental
to the most recently selected workpiece zero point by the offset values
which were declared together with the address letters.
In addition, the machining coordinate system can be moved using G50
absolute or using G51 incremental to the most recently selected work-
piece coordinate system in order to rotate the active plane using the ad-
dress letter P.
•
The programmed zero offsets G50 and G51 are NC-block active. The
offset remains in effect until the next change of the zero offset or of the
coordinate system.
•
No further functions may be programmed in a NC-block containing
G50 or G51.
Example
Z
X
20
40
60
80
20 40 60 80 100 120
Z
X
20
40
60
80
100
20 40 60 80 100
Z
X
20
40
60
80
100
20 40 60 80 100
P1
X2
P2
P3
P4
P5
G54 :
Z18.0
X15.0
P0
Z0
Fig. 3-12: Programmed zero offset G50
G00 G90 G54 X0 Z0 [P0]
BSR .CONT Branch to the contour subroutine
G50 X2 Zero offset X by 2 mm
BSR .CONT 2nd call of the contour subroutine
RET
.CONT Contour subroutine
G01 X10 Z48 F750 [P1]
X25 Z59 [P2]
Z92 F1500 [P3]
X11 Z100 F600 [P4]
Z113 F1000 [P5]
G00 X40 Return to safety distance
Z0
X0 [P0]
RTS Return to main program