Linear Pattern (Cycle 221, Din/Iso: G221, Software Option 19); Cycle Run; Please Note While Programming - HEIDENHAIN TNC 620 User Manual

6
Fixed Cycles: Pattern Definitions
6.3

LINEAR PATTERN (Cycle 221, DIN/ISO: G221, software option 19)

6.3 LINEAR PATTERN (Cycle 221, DIN/ISO:
G221, software option 19)

Cycle run

1 The TNC automatically moves the tool from its current position
to the starting point for the first machining operation.
Sequence:
2. Move to the 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 for the next
machining operation in the positive reference axis direction at
set-up clearance (or 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.

Please note while programming:

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 200 to 209 and 251 to 267 , the set-up
clearance, workpiece surface, 2nd set-up clearance
and the rotational position 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.
166
TNC 620 | User's Manual Cycle Programming | 3/2014