Contour Thread G38 - HEIDENHAIN CNC PILOT 640 User Manual

DIN/ISO programming | Thread cycles

Contour thread G38

Cycle G38 machines a thread whose form does not correspond to
the tool form. Use a recessing or button tool for machining.
Describe the contour of the thread turn as Auxiliary contour. The
position of the Auxiliary contour must correspond to the start
position of the thread cuts. You can select the entire Auxiliary
contour or just segments in the cycle.
Parameters:
ID: Auxiliary contour – ID number of the contour to be
machined
NS: Starting block no. of contour – beginning of contour
section
NE: Contour end block no. – end of contour section
Q: Roughing/Finish – process variants
0: Roughing: The contour is roughed out line by line at
maximum infeed I and K. A programmed oversize (G58 or
G57) is taken into account
1: Finishing: The turn of the thread is created in individual
cuts along the contour. Define the distances between the
individual thread cuts on the contour with I and K
X: Final point (diameter value)
Z: Final point
F: Thread pitch
I: Max. approach
If Q = 0: Plunging depth
If Q = 1: Distance between the finishing cuts as arc length
K: Max. approach
If Q = 0: Offset width
If Q = 1: Distance between the finishing cuts on straight line
J: Thread runout length
C: Start angle
O: Type of infeed
0: Rapid traverse
1: Feed rate
Example: G38
%38.nc
N1 T5 G97 S1500 M3
N2 G0 X43 Z4
N3 G38 ID"123" NS3 NE5 X40 Z-30 F1.5 I0.8K0.5 J3 C0
END
HEIDENHAIN | User's Manual smart.Turn and DIN Programming | 12/2017
4
359