GSK 980MDc, User Manual

Page: 55 / 473

GSK980MDc Milling CNC System User Manual
36
I Programming
To program the above paths using the absolute mode and incremental mode respectively:
(1) Absolute mode
G92 X200.0 Y40.0 Z0 ；
G90 G03 X140.0 Y100.0 I-60.0 F300.0
；
G02 X120.0 Y60.0 I-50.0 ；
Or G92 X200.0 Y40.0 Z0
；
G90 G03 X140.0 Y100.0 R60.0 F300.0 ；
G02 X120.0 Y60.0 R50.0
；
(2) Incremental mode
G91 G03 X-60.0 Y60.0 I-60.0 F300.0
；
G02 X-20.0 Y-40.0 I-50.0
；
Or G91 G03 X-60.0 Y60.0 R60.0 F300.0
；
G02 X-20.0 Y-40.0 R50.0
；
The feedrate of circular interpolation is specified by F command; it is the speed of the tool along the arc
tangent direction.
Note 1: I0, J0 and K0 can be omitted; but, it is very necessary to input one of the addresses I, J, K or R, or the system
alarm is generated.
Note 2: The X, Y and Z can be omitted simultaneously when the end and start points share same position. When the
center point is specified by address I, J and K, it is a 360° arc.
G02 I_; (Full circle)
The circle is 0° when using R.
G02 R_; (not move)
It is recommended that programming uses R. In order to guarantee the start and end
points of the arc are consistent with the specified value, the system will move by counting R again
according to the selected plane, when programming using the I, J and K. After calculation, the radius
difference cannot exceed the permissive value set by No.3410.
Plane selection Count the radius R value again
G17
2 2
J I R
+ =
G18
2 2
K I R
+ =
G19
2 2
K J R
+ =
Note 3: The error between the actual tool feedrate and the specified feedrate is ±2% or less. The command speed is
movement speed after tool radius offset along the arc.
Note 4: The R is effective when address I, J and K are commanded with the R, but the I, J and K are disabled at one
time.