HEIDENHAIN iTNC 530 (340 49x-04) ISO programming - Manual (Page 392)

392 8 Programming: Cycles
8.5 Cy
cles f
o
r Mac
h
ining P
o
int P
a
tt
er
ns
LINEAR PATTERN (Cycle G221)
1 The TNC automatically moves the tool from its current position to
the starting point for the first machining operation.
Sequence:
„ Move to the 2nd set-up clearance (spindle axis)
„ Approach the starting point in the spindle axis.
„ Move to the set-up clearance above the workpiece surface
(spindle axis).
2 From this position the TNC executes the last defined fixed cycle.
3 The tool then approaches the starting point for the next machining
operation in the positive reference axis direction at the set-up
clearance (or the 2nd set-up clearance).
4 This process (1 to 3) is repeated until all machining operations on
the first line have been executed. The tool is located above the last
point on the first line.
5 The tool subsequently moves to the last point on the second line
where it carries out the machining operation.
6 From this position the tool approaches the starting point for the
next machining operation in the negative reference axis direction.
7 This process (6) is repeated until all machining operations in the
second line have been executed.
8 The tool then moves to the starting point of the next line.
9 All subsequent lines are processed in a reciprocating movement.
X
Y
Z
X
Y
Q226
Q225
Q224
Q238
Q237
N = Q242
N = Q243
X
Z
Q200
Q203
Q204
Before programming, note the following
Cycle G221 is DEF active, which means that Cycle G221
automatically calls the last defined fixed cycle.
If you combine Cycle G221 with one of the fixed cycles
G200 to G209 and G251 to G267, the set-up clearance,
workpiece surface, 2nd set-up clearance and the rotational
position that you defined in Cycle G221 will be effective
for the selected fixed cycle.
The slot position 0 is not allowed if you use Cycle G254
Circular Slot in together with Cycle G221.