HEIDENHAIN TNC 128 (77184x-01) - Manual (Page 379)

HEIDENHAIN TNC 128 379
15.6 CAR
TESIAN P
A
T
T
ERN (Cy
c
le
221)
15.6 CARTESIAN PATTERN
(Cycle 221)
Cycle run
1 The TNC automatically moves the tool from its current position to
the point of the first machining operation
Sequence:
 Move to the 2nd set-up clearance (spindle axis)
 Approach the starting point in the machining plane
 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 of 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 executes the machining operation
6 From this position the tool approaches the starting point of 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 machined in a reciprocating movement
Please note while programming:
X
Y
Z
Cycle 221 is DEF active, which means that Cycle 221
automatically calls the last defined fixed cycle.
If you combine Cycle 221 with one of the fixed cycles, the
set-up clearance, workpiece surface, 2nd set-up clearance
and angle of rotation that you defined in Cycle 221 will be
effective for the selected fixed cycle.
The slot position 0 is not allowed if you use Cycle 254
Circular Slot in combination with Cycle 221.