Programming instructions

4-16
Motion Blocks NC Programming 17VRS
DOK-MTC200-NC**PRO*V17-ANW1-EN-P
G00 G90 G54 G06 G08 Motion commands, interpolation conditions
X0 Y0 Z10 S3000 M03 Starting position, spindle ON
G01 X26.26 Y18 Z5 F2000 [P1] start machining position
Z-5 Infeed Z axis
Y80 F1200 [P2] linear interpolation, 1 axis
X41 Y93.5 [P3] linear interpolation, 2 axes
X111 [P4] linear interpolation, 1 axis
G00 Z10 M05 Z axis to safety distance
RET
Example Linear interpolation in 3 axes
20
40
60
80
100
20 40 60 80 100
X
Y
[P3]
[P2]
[P1]
20
40
60
80
100
X
Z
-10010
[P1]
[P3]
[P2]
Fig. 4-21: Linear interpolation, feedrate G01 with 3 axes
G00 G90 G54 G06 G08 Motion commands, interpolation conditions
X0 Y0 Z10 S3000 M03 Starting position, spindle ON
G01 X40 Y25.5 Z5 F2000 [P1] start machining position
Z-5 Infeed Z axis
X95.74 Y80 Z-10 F1200 [P2] linear interpolation, 3 axes
X100 Y100 Z10 F2000 [P3] Z axis to safety distance
M05 Spindle OFF
G00 X0 Y0 Return to starting point
RET Return to program begin
Circular Interpolation 'G02' / 'G03'
The tool programmed with G02 or G03 is moved along a circular path to
the programmed end point using the effective or programmed feedrate
(F-value). The programmed axes are started simultaneously, and they all
reach their programmed end point at the same time.
The circular motion in the direction of the programmed end point is pro-
duced:
•
in the clockwise direction with G02 and
•
in the counter-clockwise direction with G03 (see Fig. 4-22).
The tool is moved about the programmed center point of the circle.
A circular motion can be performed in each plane when the corresponding
G-codes are selected (G17, G18, G19). The programmed center of the
circle and the end points must lie on the same machining plane as the
starting point.