HEIDENHAIN TNC 360 ISO Programming - Manual (Page 156)

8-3
8 Cycles
TNC 360
8.1 General Overview of Cycles
Cycle call
The following cycles become effective immediately upon being defined in
the part program:
• Coordinate transformation cycles
• Dwell time
• The SL cycle G37 CONTOUR GEOMETRY
All other cycles must be called separately. Further information on cycle
calls is provided in the descriptions of the individual cycles.
If the cycle is to be executed after the block in which it was called up,
program the cycle call
• with G79
• with the miscellaneous function M99.
If the cycle is to be run after every positioning block, it must be called with
the miscellaneous function M89 (depending on the machine parameters).
M89 is cancelled with M99.
Prerequisites:
The following data must be programmed before a cycle call:
• Blank form for graphic display
• Tool call
• Positioning block for starting position X, Y
• Positioning block for starting position Z (setup clearance)
• Direction of rotation of the spindle (miscellaneous functions M3/M4)
• Cycle definition.
Dimensions in the tool axis
The dimensions for tool axis movement are always referenced to the
position of the tool at the time of the cycle call and interpreted by the
control as incremental dimensions. It is not necessary to program G91.
The algebraic signs for SETUP CLEARANCE, TOTAL HOLE DEPTH and
JOG INCREMENT define the working direction. They must be entered
identically (usually negative).
The TNC assumes that at the beginning of the cycle the tool is positioned over the workpiece at the clearance
height.