HEIDENHAIN CNC Pilot 4290 - Manual (Page 154)

4 DIN PLUS 142
Thread single path G33
G33 cuts threads in any desired direction and position (longitudinal,
tapered or transverse threads; internal or external threads). G33 uses
a single pass to cut a thread starting at the tool position and ending at
”X, Z.” (Spindle and feed drives are synchronized during thread
cutting.)
Parameters
X, Z: Diameter, length to end point of thread (X diameter)
F: Feed per revolution (thread pitch)
B, P: Run-in length, overrun length – default: 0 (see ” 4.8 Thread
Cycles)
C: Starting angle (thread start is defined with respect to rotationally
nonsymmetric contour elements) – default: 0
Q: Number of the spindle
H: Reference direction for spindle pitch - default: 0
■ H=0: Feed rate in Z axis (for longitudinal and tapered threads
up to a maximum angle of +45°/–45° to Z axis
■ H=1: Feed rate in X axis (for transverse and taper threads up
to a maximum angle of +45°/–45° to the X- axis
■ H=2: Feed rate in Y axis
■ H=3: Contouring feed rate
E: Variable pitch – default: 0
■ E=0: Constant pitch
■ E>0: Increase pitch per revolution by E
■ E<0: Decrease pitch per revolution by E
■ ”Feed rate stop” becomes effective
only at the end of a thread cut.
■ Feed rate override is not in effect.
■ Do not use spindle override if the look-
ahead is switched off!
■ Make thread with G95 (feed rate per
revolution).
4.8 T
h
re
a
d
C
y
cles