HEIDENHAIN CNC Pilot 4290 - Manual (Page 125)

HEIDENHAIN CNC PILOT 4290 113
■ If P > parameter value, the parameter
value applies.
■ ”E, F and P” refer to the X or Z axis. The
acceleration/feed rate for the slide is not
higher with axis-parallel traverses.
Actual S > ”absolute maximum speed”
(machine parameter 805, ff), applies to the
parameter value.
4.6.4 Feed Rate and Spindle Speed
Speed limitation Gx26
G26: Spindle; Gx26: Spindle x (x: 1...3)
The speed limit remains in effect until the end of the program or until a
new value is programmed for G26/Gx26.
Parameters
S:
(Maximum) speed
Acceleration (slope) G48
Define the approach acceleration, breaking acceleration, and
maximum feed rate. G48 is a modal function.
If G48 is not programmed,
■ Acceleration and deceleration values will be taken from machine
parameter 1105, ... ”Acceleration/deceleration of linear axis”
■ Maximum feed rate: machine parameter 1101, ... ”maximum axis
velocity”
Parameters
E:
Acceleration starting an axis – default: Parameter value
F: Acceleration for braking an axis – default: parameter value
H: Programmed acceleration On/Off
■ H=0: Switch off programmed acceleration after next traverse
■ H=1: Switch on programmed acceleration
P: Maximum feed rate – default: parameter value
Interrupted feed G64
Briefly interrupts the programmed feed rate. G64 is a modal function.
■ Switch-on: Program G64 with ”E and F”
■ Switch-off: Program G64 without parameter
Parameters
E:
Duration of pause (Interval time: range: 0.01 s < E < 99.99 s)
F: Duration of feed rate (feed period: range: 0.01 s < E < 99.99 s)
4.6 Machining Commands
Feed per minute for rotary axes G192
Feed rate when only a rotary axis (auxiliary axis) is moved.
Parameters
F:
Feed per minute (in °/min)