Polar Pattern (Cycle 220, Din/Iso: G220); Cycle Run; Please Note While Programming - HEIDENHAIN TNC 640 User Manual

Fixed Cycles: Pattern Definitions | POLAR PATTERN (Cycle 220, DIN/ISO: G220)
6.2 POLAR PATTERN (Cycle 220, DIN/ISO:
G220)

Cycle run

1 At rapid traverse, the TNC 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 on a straight line or a circular arc the
starting point for the next machining operation. The tool stops at
the set-up clearance (or the 2nd set-up clearance).
4 This process (1 to 3) is repeated until all machining operations
have been executed.

Please note while programming:

Cycle 220 is DEF active, which means that Cycle 220
automatically calls the last defined fixed cycle.
If you combine Cycle 220 with one of the fixed cycles
200 to 209 and 251 to 267 or with cycle 221, the set-
up clearance, workpiece surface and the 2nd set-up
clearance that were defined in Cycle 220 or 221 will be
effective. This applies in the program until the affected
parameters are overwritten again. Example: If in a
program Cycle 200 is defined with Q203=0 and then
a cycle 220 is programmed with Q203=-5, Q203=-5
is used with the subsequent CYCL CALL and M99
calls. Cycles 220 and 221 overwrite the above-specified
parameters of the CALL-active machining cycles (with
identical input parameters in both cycles).
If you run this cycle in the Single Block mode of
operation, the control stops between the individual
points of a point pattern.
HEIDENHAIN | User's manual for cycle programming | 10/2017
6
207