HEIDENHAIN TNC 320 (340 551-01) - Manual (Page 250)

250 8 Programming: Cycles
8.4 Cy
cles f
o
r Mac
h
ining P
o
int P
at
ter
ns
LINEAR PATTERN (Cycle 221)
1 The TNC automatically moves the tool from its current position to
the starting point for the first machining operation.
Sequence:
„ Move to 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 221 is DEF active, which means that Cycle 221 calls
the last defined fixed cycle automatically.
If you combine Cycle 221 with one of the fixed cycles 200
to 209, 212 to 215, 265 to 267, the set-up clearance,
workpiece surface and 2nd set-up clearance that you
defined in Cycle 221 will be effective for the selected fixed
cycle.