Undercut Din 76 With Cylinder Machining G853 - HEIDENHAIN CNC PILOT 640 User Manual

DIN/ISO programming | Undercut cycles

Undercut DIN 76 with cylinder machining G853

G853 machines the adjoining cylinder, the undercut, and finishes
with the plane surface. It also machines a cylinder start chamfer
when you enter at least one of the parameters Cut-in length or
Cut-in radius.
Parameters:
FP: Thread pitch
I: Undercut depth (default: standard table)
K: Undercut length (default: standard table)
W: Undercut angle (default: standard table)
R: Undercut radius (default: standard table)
P: Allowance
P is not defined: The undercut is machined in one pass
P is defined: Division into pre-turning and finish-turning – P =
longitudinal oversize; the transverse oversize is preset to 0.1
mm
B: Cut-in length (no input: no chamfer machined at start of
cylinder)
RB: 1st cut radius (no input: 1st cut radius is not machined)
WB: Cut-in angle (default: 45°)
E: Reduc. Feed for machining the undercut (default: active feed
rate)
H: Type of departure
0: To starting point
1: Plane surface end
Parameters that are not programmed are automatically calculated
by the control from the standard table
FP from the diameter
I, K, W and R from FP (Thread pitch)
Blocks following the cycle call
N.. G853 FP.. I.. K.. W..
N.. G0 X.. Z..
N.. G1 Z..
N.. G1 X..
N.. G80
Undercuts can only be executed in orthogonal,
paraxial contour corners along the longitudinal axis
Cutter radius compensation is active
Oversizes are not offset
HEIDENHAIN | User's Manual smart.Turn and DIN Programming | 12/2017
Cycle call
Corner point of cylinder start chamfer
Undercut corner
End point on plane surface
End of contour definition
4
367