HEIDENHAIN iTNC 530 (340 422) ISO programming - Manual (Page 288)

288 8 Programming: Cycles
8.4 Cy
cles f
o
r Mil
ling P
o
c
k
e
ts, St
ud
s an
d Slo
ts
CIRCULAR POCKET (Cycle G252)
Use Cycle G252 CIRCULAR POCKET to completely machine circular
pockets. Depending on the cycle parameters, the following machining
alternatives are available:
n Complete machining: Roughing, floor finishing, side finishing
n
Only roughing
n Only floor finishing and side finishing
n Only floor finishing
n
Only side finishing
Roughing process
1 The tool penetrates the workpiece at the pocket center and
advances to the first plunging depth. Specify the plunging strategy
with Parameter Q366.
2 The TNC roughs out the pocket from the inside out, taking the
overlap factor (Parameter Q370) and the finishing allowance
(Parameter Q368) into account.
3 This process is repeated until the programmed pocket depth is
reached.
Finishing process
4 If finishing allowances have been defined, the TNC first finishes
the floor of the pocket from the inside out. The pocket floor is
approached tangentially.
5 The TNC then finishes the pocket walls, in multiple infeeds if so
specified. The pocket wall is approached tangentially.
Before programming, note the following:
Pre-position the tool in the machining plane to the starting
position (circle center) with radius compensation R0.
The TNC runs the cycle in the axes (machining plane) with
which you approached the starting position. For example,
in X and Y if you programmed G79:G01 X... Y... or in U
and V if you programmed G79:G01 U... V...
The TNC automatically pre-positions the tool in the tool
axis. Note Parameter Q204 (2nd set-up clearance).
The algebraic sign for the cycle parameter DEPTH
determines the working direction. If you program
DEPTH = 0, the cycle will not be executed.
At the end of the cycle, the TNC returns the tool to the
starting position.