HEIDENHAIN TNC 640 (34059x-02) Cycle programming - Manual (Page 76)

Fixed Cycles: Drilling
3.4 REAMING (Cycle 201, DIN/ISO: G201)
3
76
TNC 640 | User's Manual Cycle Programming | 5/2013
Cycle parameters
Set-up clearance Q200 (incremental): Distance
between tool tip and workpiece surface. Input range
0 to 99999.9999
Depth Q201 (incremental): Distance between
workpiece surface and bottom of hole. Input range
-99999.9999 to 99999.9999
Feed rate for plunging Q206: Traversing speed of
the tool during reaming in mm/min. Input range 0 to
99999.999; alternatively
FAUTO, FU
Dwell time at depth Q211: Time in seconds that
the tool remains at the hole bottom. Input range 0 to
3600.0000
Retraction feed rate Q208: Traversing speed of the
tool in mm/min when retracting from the hole. If
you enter Q208 = 0, the tool retracts at the reaming
feed rate. Input range 0 to 99999.999
Coordinate of workpiece surface Q203 (absolute):
Coordinate of the workpiece surface. Input range 0
to 99999.9999
2nd set-up clearance Q204 (incremental):
Coordinate in the spindle axis at which no collision
between tool and workpiece (fixtures) can occur.
Input range 0 to 99999.9999
NC blocks
11 CYCL DEF 201 REAMING
Q200=2 ;SET-UP CLEARANCE
Q201=-15 ;DEPTH
Q206=100 ;FEED RATE FOR
PLNGNG
Q211=0.5 ;DWELL TIME AT
BOTTOM
Q208=250 ;RETRACTION FEED
RATE
Q203=+20 ;SURFACE COORDINATE
Q204=100 ;2ND SET-UP
CLEARANCE
12 L X+30 Y+20 FMAX M3
13 CYCL CALL
14 L X+80 Y+50 FMAX M9
15 L Z+100 FMAX M2