HEIDENHAIN CNC Pilot 4290 - Manual (Page 183)

HEIDENHAIN CNC PILOT 4290 171
Block speed monitoring off G907
The CNC PILOT starts machining operations requiring spindle
revolutions when the programmed speed has been reached. G907 is
used to deactivate speed monitoring block by block - the path of
traverse is started immediately.
Program G907 and the traverse path in the same NC block.
Feed override 100% G908
G908 sets the feed override for traverse paths (G0, G1, G2, G3, G12,
G13) block by block to 100%.
Program G908 and the traverse path in the same NC block.
Interpreter stop G909
The CNC PILOT pre-interprets approx. 15 to 20 NC blocks in advance.
If variables are assigned shortly before the evaluation, ”old values”
would be processed. An interpreter stop ensures that the variables
contain the new value.
G909 stops the pre-interpretation. The NC blocks are processed up to
G909 – after G909 the subsequent NC blocks are processed.
Apart from G909, the NC block should only contain synchronous
functions. (Some G functions generate an interpreter stop.)
Look ahead G918
The look-ahead function can be activated/deactivated with G918.
G918 can be programmed in a separate NC block program before/
after the thread cutting (G31, G33).
Parameters
Q:
Look-ahead function on/off – default: 1
■ Q=0: Off
■ Q=1: On
Spindle override 100% G919
Switched the spindle speed override off/on.
Parameters
Q:
Spindle number – default: 0
H: Type of limit – default: 0
■ H=0: Switch on spindle override
■ H=1: Spindle override to 100% – modal
■ H=2: Spindle override to 100% – for the current NC block
4.13 Other G Functions