DIN/ISO programming | Other G codes
4
442
HEIDENHAIN | User's Manual smart.Turn and DIN Programming | 12/2017
Spindle override 100% G919
G919 is used to deactivate/activate the spindle speed override.
Parameters:
Q: No. of spindle (default: 0)
H: Limiting type (default: 0)
0: Activate spindle speed override
1: Spindle override at 100 %—modal
2: Spindle override at 100 %—for the current NC block
Deactivating datum shifts G920
G920 deactivates the workpiece datum and datum shifts. Traverse
paths and position values are referenced to the distance tool tip –
machine datum.
Deactivating datum shift, tool lengths G921
G921 deactivates the workpiece datum, datum shifts and tool
dimensions. Traverse paths and position values are referenced to the
slide reference point—machine datum.
End position of the tool G922
With G922 you can position the active tool to a defined Angle.
Parameters:
C: Angle – angular position for tool orientation
Fluctuating spindle speed G924
To reduce resonant vibrations you can use G924 to program a
changing spindle speed. In G924 you define the Repetition rate and
the range for the Change of spindle speed. The G924 function is
automatically reset at the end of the program. You can also deactivate
the function through another call with the setting H0 (off).
Parameters:
Q: No. of spindle (default: 0)
K: Repetition rate – time interval in hertz (repetitions per second)
I: Change of spindle speed
H: G924 On=1 Off=0
0: Off
1: On
To Next Page
Loading...
