HEIDENHAIN iTNC 530 (340 49x-04) ISO programming - Manual (Page 313)

HEIDENHAIN iTNC 530 313
8.3 Cy
cles f
o
r Dr
illing, T
a
pping and Thr
ead Milling
 Set-up clearance Q200 (incremental value): Distance
between tool tip and workpiece surface. Enter a
positive value.
 Depth Q201 (incremental value): Distance between
workpiece surface and bottom of hole (tip of drill
taper).
 Feed rate for plunging Q206: Traversing speed of
the tool during drilling in mm/min.
 Plunging depth Q202 (incremental value): Infeed per
cut. The depth does not have to be a multiple of the
plunging depth. The TNC will go to depth in one
movement if:
„ the plunging depth is equal to the depth
„ the plunging depth is greater than the depth
 Dwell time at top Q210: Time in seconds that the
tool remains at set-up clearance after having been
retracted from the hole for chip release.
 Workpiece surface coordinate Q203 (absolute
value): Coordinate of the workpiece surface.
 2nd set-up clearance Q204 (incremental value):
Coordinate in the tool axis at which no collision
between tool and workpiece (clamping devices) can
occur.
 Dwell time at depth Q211: Time in seconds that the
tool remains at the hole bottom.
Example: NC blocks
N100 G00 Z+100 G40
N110 G200 DRILLING
Q200=2 ;SET-UP CLEARANCE
Q291=-15 ;DEPTH
Q206=250 ;FEED RATE FOR PLUNGING
Q202=5 ;PLUNGING DEPTH
Q210=0 ;DWELL TIME AT TOP
Q203=+20 ;SURFACE COORDINATE
Q204=100 ;2ND SET-UP CLEARANCE
Q211=0.1 ;DWELL TIME AT DEPTH
N120 X+30 Y+20 M3 M99
N130 X+80 Y+50 M99
N140 Z+100 M2