Characteristics Of The Fixed Cycles - HEIDENHAIN ITNC 530 - CYCLE PROGRAMMING User Manual

Characteristics of the fixed cycles

The TNC automatically positions the tool to the setup clearance
before a cycle.
Each level of infeed depth is milled without interruptions since the
cutter traverses around islands instead of over them.
In order to avoid leaving dwell marks, the TNC inserts a globally
definable rounding radius at non-tangential inside corners. The
rounding radius, which is entered in Cycle 20, affects the tool center
point path, meaning that it would increase a rounding defined by the
tool radius (applies to rough-out and side finishing).
The contour is approached in a tangential arc for side finishing.
For floor finishing, the tool again approaches the workpiece on a
tangential arc (for tool axis Z, for example, the arc may be in the Z/X
plane).
The contour is machined throughout in either climb or up-cut milling.
The miscellaneous functions M109 and M110 (feed rate at circular
arcs) are not effective within SL cycles, even if you programmed
these before a cycle call.
With bit 4 in MP7420 you can determine where the tool is
positioned at the end of Cycles 21 to 24.
Bit 4 = 0:
At the end of the cycle, the TNC at first positions the tool
in the tool axis at the clearance height (Q7) defined in the
cycle, and then to the position in the working plane at
which the tool was located when the cycle was called.
Bit 4 = 1:
At the end of the cycle, the TNC always positions the tool
in the tool axis at the clearance height (Q7) defined in the
cycle. Ensure that no collisions can occur during the
following positioning movements!
The machining data (such as milling depth, finishing allowance and
setup clearance) are entered as CONTOUR DATA in Cycle 20.
HEIDENHAIN iTNC 530 183