Cycle Parameters - HEIDENHAIN TNC 640 User Manual

Cycles: Turning | TURN, LONGITUDINAL PLUNGE EXTENDED
(Cycle 814, DIN/ISO: G814)

Cycle parameters

Q215 Machining operation (0/1/2/3)?: Define
machining operation:
0: Roughing and finishing
1: Only roughing
2: Only finishing to finished dimension
3: Only finishing to oversize
Q460 Set-up clearance? (incremental): Distance
for retraction and pre-positioning.
Q491 Diameter at contour start?: X coordinate of
the contour starting point (diameter value)
Q492 Contour start in Z?: Z coordinate of the
starting point for the plunging path
Q493 Diameter at end of contour?: X coordinate
of the contour end point (diameter value)
Q493 Contour end in Z?: Z coordinate of the
contour end point
Q495 Angle of side?: Angle of the plunging
side. The reference angle is formed by the
perpendicular to the rotary axis.
Q501 Starting element type (0/1/2)?: Define
the type of element at the start of the contour
(circumferential surface):
0: No additional element
1: Element is a chamfer
2: Element is a radius
Q502 Size of starting element?: Size of the
starting element (chamfer section)
Q500 Radius of the contour corner?: Radius of
the contour inside corner. If no radius is specified,
the radius of the cutting insert is generated.
Q496 Angle of face?: Angle between the plane
surface and the rotary axis
HEIDENHAIN | User's manual for cycle programming | 10/2017
Q484
Q463
Q494 Q492
Ø Q493
NC blocks
11 CYCL DEF 814 TURN PLUNGE
LONGITUDINAL EXT.
Q215=+0 ;MACHINING OPERATION
Q460=+2 ;SAFETY CLEARANCE
Q491=+75 ;DIAMETER AT CONTOUR
START
Q492=-10 ;CONTOUR START IN Z
Q493=+50 ;DIAMETER AT CONTOUR
END
Q494=-55 ;CONTOUR END IN Z
12
Q460
Ø Q491
Ø Q483
387