Cycle Parameters - HEIDENHAIN TNC 640 User Manual

12

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?: Reserved, currently
without function
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
Q478 Roughing feed rate?: Feed rate for
roughing. If M136 has been programmed, the
value is interpreted by the TNC in millimeters
per revolution, without M136 in millimeters per
minute.
Q483 Oversize for diameter? (incremental):
Diameter oversize for the defined contour
Q484 Oversize in Z? (incremental): Oversize for
the defined contour in axial direction
Q505 Finishing feed rate?: Feed rate for
finishing. If M136 has been programmed, the
value is interpreted by the TNC in millimeters
per revolution, without M136 in millimeters per
minute.
Q463 Maximum cutting depth?: Maximum infeed
(radius value) in radial direction. The infeed is
divided evenly to avoid abrasive cuts. Input range
0.001 to 999.999
Q507 Direction (0=bidir./1=unidir.)?: Cutting
direction:
0: Bidirectional (in both directions)
1: Unidirectional (in contour direction)
Q508 Offset width?: Reduction of cutting length.
After clearance roughing, the remaining material
is removed with a single cut. If required, the TNC
limits the programmed offset width.
Q509 Depth compensat. for finishing?:
Depending on factors such as workpiece material
or feed rate, the tool tip is displaced during a
turning operation. You can correct the resulting
infeed error with the turning depth compensation
factor.
Q488 Feed rate for plunging (0=auto)?: Feed rate
for machining plunging elements. This input value
is optional. If it is not programmed, then the feed
rate defined for turning operations applies.
428
Cycles: Turning | SIMPLE AXIAL RECESSING
(Cycle 851, DIN/ISO: G851)
Q494
Q484
NC blocks
11 CYCL DEF 851 SIMPLE REC TURNG,
AX
Q215=+0 ;MACHINING OPERATION
Q460=+2 ;SAFETY CLEARANCE
Q493=+50 ;DIAMETER AT CONTOUR
END
Q494=-10 ;CONTOUR END IN Z
Q478=+0.3 ;ROUGHING FEED RATE
Q483=+0.4 ;OVERSIZE FOR DIAMETER
Q484=+0.2 ;OVERSIZE IN Z
Q505=+0.2 ;FINISHING FEED RATE
Q463=+2 ;MAX. CUTTING DEPTH
Q507=+0 ;MACHINING DIRECTION
Q508=+0 ;OFFSET WIDTH
Q509=+0 ;DEPTH COMPENSATION
Q488=+0 ;PLUNGING FEED RATE
12 L X+65 Y+0 Z+2 FMAX M303
13 CYCL CALL
HEIDENHAIN | User's manual for cycle programming | 10/2017
Q460
Ø Q493
Ø Q483