Cycle Parameters - HEIDENHAIN TNC 620 User Manual

3
Fixed Cycles: Drilling
3.2 CENTERING (Cycle 240, DIN/ISO: G240, software option 19)

Cycle parameters

Set-up clearance Q200 (incremental): Distance
between tool tip and workpiece surface. Enter a
positive value. Input range 0 to 99999.9999
Select depth/diameter (0/1) Q343: Select whether
centering is based on the entered diameter or
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
Depth Q201 (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
Diameter (algebraic sign) Q344: Centering
diameter. Only effective if Q343=1 is defined. Input
range -99999.9999 to 99999.9999
Feed rate for plunging Q206: Traversing speed of
the tool in mm/min during centering. 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
Coordinate of workpiece surface Q203 (absolute):
Coordinate of the workpiece surface. Input range
-99999.9999 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
68
NC blocks
10 L Z+100 R0 FMAX
11 CYCL DEF 240 CENTERING
Q200=2 ;SET-UP CLEARANCE
Q343=1 ;SELECT DEPTH/DIA.
Q201=+0 ;DEPTH
Q344=-9 ;DIAMETER
Q206=250 ;FEED RATE FOR
PLNGNG
Q211=0.1 ;DWELL TIME AT
BOTTOM
Q203=+20 ;SURFACE COORDINATE
Q204=100 ;2ND SET-UP
CLEARANCE
12 L X+30 Y+20 R0 FMAX M3 M99
13 L X+80 Y+50 R0 FMAX M99
TNC 620 | User's Manual Cycle Programming | 3/2014