Calling A Cycle - HEIDENHAIN TNC 620 User Manual

2

Calling a cycle

Requirements
The following data must always be programmed before
a cycle call:
BLK FORM for graphic display (needed only for test
graphics)
Tool call
Direction of spindle rotation (M functions M3/M4)
Cycle definition (CYCL DEF)
For some cycles, additional prerequisites must be
observed. They are detailed in the descriptions for each
cycle.
The following cycles become effective automatically as soon as
they are defined in the part program. These cycles cannot and
must not be called:
Cycle 220 for point patterns on circles and Cycle 221 for point
patterns on lines
SL Cycle 14 CONTOUR
SL Cycle 20 CONTOUR DATA
Cycle 32 TOLERANCE
Coordinate transformation cycles
Cycle 9 DWELL TIME
All touch probe cycles
You can call all other cycles with the functions described as follows.
Calling a cycle with CYCL CALL
The CYCL CALL function calls the most recently defined fixed
cycle once. The starting point of the cycle is the position that was
programmed last before the CYCL CALL block.
To program the cycle call, press the CYCL CALL
key
Press the CYCL CALL M soft key to enter a cycle
call
If necessary, enter the miscellaneous function M
(for example M3 to switch the spindle on), or end
the dialog by pressing the END key
Calling a cycle with CYCL CALL PAT
The CYCL CALL PAT function calls the most recently defined
machining cycle at all positions that you defined in a PATTERN DEF
pattern definition or in a points table.
Further information:
Page 58
Further information:
52
"PATTERN DEF pattern definition",
"Point tables", Page 65
Using Fixed Cycles | Working with fixed cycles
HEIDENHAIN | TNC 620 | User's manual for cycle programming | 10/2017