HEIDENHAIN CNC Pilot 4290 Pilot - Manual (Page 76)

76
Thr
ead cy
cle gr
oup
Individual thread cut G33
G33 cuts threads in any desired direction and position (longitudinal,
tapered or transverse threads; internal or external threads). The thread
starts at the current tool position and ends at ”X, Z”.
Parameters
X, Z: Diameter, length to end point of thread (X diameter)
F:
Feed rate per revolution (thread pitch)
B, P: Chamfer length, overrun length – default: 0 (see G33)
C:
Starting angle – default: 0
Q: Number of the spindle
H: Reference direction for spindle pitch - default: 0
■ H=0: Feed rate on 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 (increases/reduces the pitch per revolution by E) –
default: 0
• ”Feed rate stop” becomes effective only at the end of a
thread cut.
• Feed rate override is not effective.
• Do not use the spindle override if the feedforward is
switched off!
• Create thread with G95 (feed rate per revolution).
Calculation of ”thread run-in/runout distances”
The slide requires a run-in distance to accelerate to the programmed
feed rate before starting the actual thread, and a runout distance at the
end of the thread to decelerate again.
Calculation of chamfer (run-in) length:
BA > 0.75 * (F*S)² / a + 0.15
Calculation of runout length:
BE > 0.75 * (F*S)² / e + 0.15
BA: Minimum run-in length
BE: Minimum runout length
F: Spindle pitch in mm/revolution
S: Speed in revolutions/second
a, e: Acceleration in mm/s² (a = ”acceleration at
start of block”; e = ”acceleration at end of
block” from Machine Parameter 1105, ff)