Cycle Parameters - HEIDENHAIN TNC 620 User Manual

3

Cycle parameters

Q200 Set-up clearance? (incremental): Distance
between tool tip and workpiece surface. Enter a
positive value. Input range 0 to 99999.9999
Q343 Select diameter/depth (1/0): Select
whether centering is based on the entered
diameter or entered depth. If the TNC is to center
based on the entered diameter, the point angle of
the tool must be defined in the T angle column of
the tool table TOOL.T.
0: Centering based on the entered depth
1: Centering based on the entered diameter
Q201 Depth? (incremental): Distance between
workpiece surface and centering bottom (tip
of centering taper). Only effective if Q343=0 is
defined. Input range -99999.9999 to 99999.9999
Q344 Diameter of counterbore (algebraic sign):
Centering diameter. Only effective if Q343=1 is
defined. Input range -99999.9999 to 99999.9999
Q206 Feed rate for plunging?: Traversing speed
of the tool in mm/min while centering. 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
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
72
Fixed Cycles: Drilling | CENTERING (Cycle 240, DIN/ISO: G240, software option 19)
NC blocks
10 L Z+100 R0 FMAX
11 CYCL DEF 240 CENTERING
Q200=2
Q343=1
Q201=+0
Q344=-9
Q206=250
Q211=0.1
Q203=+20
Q204=100
12 L X+30 Y+20 R0 FMAX M3 M99
13 L X+80 Y+50 R0 FMAX M99
HEIDENHAIN | TNC 620 | User's manual for cycle programming | 10/2017
;SET-UP CLEARANCE
;SELECT DIA./DEPTH
;DEPTH
;DIAMETER
;FEED RATE FOR PLNGNG
;DWELL TIME AT DEPTH
;SURFACE COORDINATE
;2ND SET-UP CLEARANCE