Thread Single Path G33 - HEIDENHAIN CNC PILOT 640 User Manual

4

Thread single path G33

G33 conducts a single thread cut. The direction of the single thread
path is as desired (longitudinal, tapered or transverse threads;
internal or external threads). You can make successive threads by
programming G33 several times in succession.
Position the tool in front of the thread by the Slop.length B if
the slide must accelerate to the feed rate. And remember the
Overflow length P before the Final point of thread if the slide has
to be decelerated.
Parameters:
X: Final point (diameter value)
Z: Final point
F: Feed per rot. (thread pitch)
B: Run-in lgth
P: Overflow length
C: Start angle
H: Ref. direction for thread pitch (default: 0)
0: Feed rate on the Z axis (for longitudinal and taper threads
up to a max. angle of +45°/–45° to the Z axis)
1: Feed rate on the X axis (for transverse and taper threads
up to a max. angle of +45°/–45° to the X axis)
3: Contouring feed rate
E: Variable gr. (default: 0)
Increases/decreases the pitch per revolution by E. (no effect at
present)
I: Retraction distance X – retraction path for cycle stop in the
thread (incremental value)
K: Retraction distance Z – retraction path for cycle stop in the
thread (incremental value)
Slop.length B: The slide requires a run-in distance at the start of
thread in order to accelerate to the programmed contouring feed
rate before starting the actual thread. Default:
SafetyDist
Overflow length P: The slide needs an overtravel at the end of
the thread to decelerate again. Remember that the paraxial line P
needs overtravel even with an oblique thread run-out.
P = 0: Start of a successive thread
P > 0: End of a successive thread
Start angle C: At the end of the Slop.length B the spindle is at the
Start angle C position.
NC stop – the control retracts the tool from the
thread groove and then stops all tool movements
Lift-off distance in the threadLiftOff machine
parameter (no. 601804)
Feed rate override is not effective
Create thread with G95 (feed rate per revolution)
354
cfgAxisProperties/
HEIDENHAIN | User's Manual smart.Turn and DIN Programming | 12/2017
DIN/ISO programming | Thread cycles