HEIDENHAIN TNC 640 User Manual page 163

Fixed Cycles: Pocket Milling / Stud Milling / Slot Milling | RECTANGULAR POCKET (Cycle 251, DIN/ISO:
G251)
Q206 Feed rate for plunging?: Traversing speed
of the tool in mm/min while moving to depth.
Input range 0 to 99999.999, alternatively FAUTO,
FU, FZ
Q338 Infeed for finishing? (incremental):
Infeed in the spindle axis per finishing cut.
Q338=0: Finishing in one infeed. Input range 0 to
99999.9999
Q200 Set-up clearance? (incremental): Distance
between tool tip and workpiece surface. Input
range 0 to 99999.9999; alternatively PREDEF
Q203 Workpiece surface coordinate? (absolute):
Coordinate of the workpiece surface. Input range
-99999.9999 to 99999.9999
Q204 2nd set-up clearance? (incremental):
Coordinate in the spindle axis at which no collision
between tool and workpiece (fixtures) can occur.
Input range 0 to 99999.9999; alternatively PREDEF
Q370 Path overlap factor?: Q370 x tool radius =
stepover factor k. Input range: 0.0001 to 1.9999
alternatively PREDEF
Q366 Plunging strategy (0/1/2)?: Type of plunging
strategy:
0: Vertical plunging. The TNC plunges
perpendicularly, regardless of the plunging angle
ANGLE defined in the tool table
1: helical plunging. In the tool table, the plunging
angle ANGLE for the active tool must be defined
as not equal to 0. Otherwise, the TNC generates
an error message
2: reciprocal plunging. In the tool table, the
plunging angle ANGLE for the active tool must be
defined as not equal to 0. Otherwise, the TNC
generates an error message. The reciprocation
length depends on the plunging angle. As a
minimum value the TNC uses twice the tool
diameter
PREDEF: The TNC uses the value from the
GLOBAL DEF block
Q385 Finishing feed rate?: Traversing speed of
the tool in mm/min during side and floor finishing.
Input range 0 to 99999.999, alternatively FAUTO,
fu, FZ
Q439 Feed rate reference (0-3)?: Specify what
the programmed feed rate refers to:
0: Feed rate with respect to the tool center point
path
1: Feed rate with respect to the tool edge, but only
during side finishing, otherwise with respect to
the tool center point path
2: Feed rate refers to the tool cutting edge during
side finishing
refers to the tool path center
3: Feed rate always refers to the cutting edge
HEIDENHAIN | User's manual for cycle programming | 10/2017
and floor finishing; otherwise it
NC blocks
8 CYCL DEF 251 RECTANGULAR POCKET
Q215=0 ;MACHINING OPERATION
Q218=80 ;FIRST SIDE LENGTH
Q219=60 ;2ND SIDE LENGTH
Q220=5 ;CORNER RADIUS
Q368=0.2 ;ALLOWANCE FOR SIDE
Q224=+0 ;ANGLE OF ROTATION
Q367=0 ;POCKET POSITION
Q207=500 ;FEED RATE FOR MILLNG
Q351=+1 ;CLIMB OR UP-CUT
Q201=-20 ;DEPTH
Q202=5 ;PLUNGING DEPTH
Q369=0.1 ;ALLOWANCE FOR FLOOR
Q206=150 ;FEED RATE FOR PLNGNG
Q338=5 ;INFEED FOR FINISHING
Q200=2 ;SET-UP CLEARANCE
Q203=+0 ;SURFACE COORDINATE
Q204=50 ;2ND SET-UP CLEARANCE
Q370=1 ;TOOL PATH OVERLAP
Q366=1 ;PLUNGE
Q385=500 ;FINISHING FEED RATE
Q439=0 ;FEED RATE REFERENCE
9 L X+50 Y+50 R0 FMAX M3 M99
5
163