HEIDENHAIN iTNC 530 (340 49x-03) ISO programming - Manual (Page 395)

HEIDENHAIN iTNC 530 395
8.6 SL Cy
cles
SIDE FINISHING (Cycle G124)
The subcontours are approached and departed on a tangential arc.
Each subcontour is finish-milled separately.
8 Direction of rotation ? Clockwise = -1 Q9:
Machining direction:
+1: Counterclockwise
-1: Clockwise
8 Plunging depth Q10 (incremental value): Dimension
by which the tool plunges in each infeed.
8 Feed rate for plunging Q11: Traversing speed of the
tool during penetration.
8 Feed rate for milling Q12: Traversing speed for
milling.
8 Finishing allowance for side Q14 (incremental
value): Enter the allowed material for several finish-
milling operations. If you enter Q14 = 0, the remaining
finishing allowance will be cleared.
Example: NC block
N61 G124 SIDE FINISHING
Q9=+1 ;DIRECTION
Q10=+5 ;PLUNGING DEPTH
Q11=100 ;FEED RATE FOR PLUNGING
Q12=350 ;FEED RATE FOR ROUGHING
Q14=+0 ;ALLOWANCE FOR SIDE
X
Z
Q11
Q12
Q10
Before programming, note the following:
The sum of allowance for side (Q14) and the radius of the
finish mill must be smaller than the sum of allowance for
side (Q3, Cycle G120) and the radius of the rough mill.
This calculation also holds if you run Cycle G124 without
having roughed out with Cycle G122; in this case, enter "0"
for the radius of the rough mill.
You can use Cycle G124 also for contour milling. Then you
must:
„
define the contour to be milled as a single island
(without pocket limit), and
„ enter the finishing allowance (Q3) in Cycle G120 to be
greater than the sum of the finishing allowance Q14 +
radius of the tool being used.
The TNC automatically calculates the starting point for
finishing. The starting point depends on the available
space in the pocket and the allowance programmed in
Cycle G120.