Cycle Parameters - HEIDENHAIN TNC 640 User Manual

Cycles: Special Functions | INTERPOLATION TURNING, CONTOUR FINISHING (Cycle 292, DIN/ISO: G292,
software option 96)

Cycle parameters

Q560 Spindle coupling (0=off, 1=on)?: Specify
whether spindle coupling is executed.
0: Spindle coupling off (mill the contour)
1: Spindle coupling on (turn the contour)
Q336 Angle for spindle orientation?: The TNC
orients the tool to this angle before starting the
machining operation. If you work with a milling
tool, enter the angle in such a way that a tooth is
turned towards the center of rotation. If you work
with a turning tool, and have defined the value
"ORI" in the turning tool table (toolturn.trn), then
it is taken into account for the spindle orientation.
Input range 0.000 to 360.000
Q546 Reverse tool rotation direction?: Direction
of spindle rotation of the active tool:
3: Tool turns to the right (M3)
4: Tool turns to the left (M4)
Q529 Machining operation (0/1)?: Specify
whether an inside or outside contour is machined:
+1: Inside machining
0: Outside machining
Q221 Oversize for surface?: Allowance in the
working plane. Input range 0 to 99.9999
Q441 Infeed per revolution [mm/rev]?:
Dimension by which the TNC feeds the tool during
one revolution. Input range 0.001 to 99.999
Q449 Feed rate / cutting speed? (mm/min): Feed
rate relative to the contour starting point Q491.
Input range 0.1 to 99999.9 The feed rate of the
tool's center point path is adjusted according
to the tool radius and the Q529 MACHINING
OPERATION. From these parameters, the TNC
determines the programmed cutting speed at the
diameter of the contour starting point.
Q529=1: Feed rate of the tool's center point path
is reduced for inside machining
Q529=0: Feed rate of the tool's center point path
is increased for outside machining
Q491 Contour starting point (radius)? (absolute
value): Radius of the contour starting point (e.g. X-
coordinate, if tool axis is Z). Input range 0.9999 to
99999.9999
Q357 Safety clearance to the side? (incremental):
Safety clearance to the side of the workpiece
when the tool approaches the first plunging depth
Input range 0 to 99999.9
Q445 Clearance height? (absolute): Absolute
height at which the tool cannot collide with the
workpiece; the tool retracts to this position at
the end of the cycle. Input range -99999.9999 to
99999.9999
HEIDENHAIN | User's manual for cycle programming | 10/2017
NC blocks
63 CYCL DEF 292
CONTOUR.TURNG.INTRP.
Q560=1 ;SPINDLE COUPLING
Q336=0 ;ANGLE OF SPINDLE
Q546=3 ;CHANGE TOOL DIRECTN.
Q529=0 ;MACHINING OPERATION
Q221=0 ;SURFACE OVERSIZE
Q441=0.5 ;INFEED
Q449=2000 ;FEED RATE
Q491=0 ;CONTOUR START RADIUS
Q357=2 ;CLEARANCE TO SIDE
Q445=50 ;CLEARANCE HEIGHT
11
327