Cycle Parameters - HEIDENHAIN TNC 640 User Manual

3

Cycle parameters

Q200 Set-up clearance? (incremental): Distance
between tool tip and workpiece surface. Input
range 0 to 99999.9999
Q201 Depth? (incremental): Distance between
workpiece surface and bottom of hole. Input range
-99999.9999 to 99999.9999
Q206 Feed rate for plunging?: Traversing speed
of the tool in mm/min while reaming. Input range
0 to 99999.999, alternatively FAUTO, fu
Q211 Dwell time at the depth?: Time in seconds
that the tool remains at the hole bottom. Input
range 0 to 3600.0000
Q208 Feed rate for retraction?: Traverse speed
of tool when moving out of the hole in mm/min.
If you enter Q208 = 0, the feed rate for reaming
applies. Input range 0 to 99999.999
Q203 Workpiece surface coordinate? (absolute):
Coordinate of the workpiece surface. Input range 0
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
84
Fixed Cycles: Drilling | REAMING (Cycle 201, DIN/ISO: G201)
NC blocks
11 CYCL DEF 201 REAMING
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
HEIDENHAIN | User's manual for cycle programming | 10/2017
Q200=2 ;SET-UP CLEARANCE
Q201=-15 ;DEPTH
Q206=100 ;FEED RATE FOR PLNGNG
Q211=0.5 ;DWELL TIME AT DEPTH
Q208=250 ;RETRACTION FEED RATE
Q203=+20 ;SURFACE COORDINATE
Q204=100 ;2ND SET-UP CLEARANCE