HEIDENHAIN ITNC 530 - CYCLE PROGRAMMING User Manual page 264

Strategy Q389=1
3 The tool then advances to the stopping point
milling. The end point lies within the surface. The control
calculates the end point from the programmed starting point, the
programmed length and the tool radius.
4 The TNC offsets the tool to the starting point in the next pass at
the pre-positioning feed rate. The offset is calculated from the
programmed width, the tool radius and the maximum path overlap
factor.
5 The tool then moves back in the direction of the starting point 1.
The motion to the next line occurs within the workpiece borders.
6 The process is repeated until the programmed surface has been
completed. At the end of the last pass, the tool plunges to the next
machining depth.
7 In order to avoid non-productive motions, the surface is then
machined in reverse direction.
8 The process is repeated until all infeeds have been machined. In
the last infeed, simply the finishing allowance entered is milled at
the finishing feed rate.
9 At the end of the cycle, the TNC retracts the tool at FMAX to the
2nd setup clearance.
Strategy Q389=2
3 The tool then advances to the stopping point
milling. The end point lies outside the surface. The control
calculates the end point from the programmed starting point, the
programmed length, the programmed safety clearance to the side
and the tool radius.
4 The TNC positions the tool in the spindle axis to the setup
clearance over the current infeed depth, and then moves at the
pre-positioning feed rate directly back to the starting point in the
next line. The TNC calculates the offset from the programmed
width, the tool radius and the maximum path overlap factor.
5 The tool then returns to the current infeed depth and moves in the
direction of the next end point 2.
6 The milling process is repeated until the programmed surface has
been completed. At the end of the last pass, the tool plunges to
the next machining depth.
7 In order to avoid non-productive motions, the surface is then
machined in reverse direction.
8 The process is repeated until all infeeds have been machined. In
the last infeed, simply the finishing allowance entered is milled at
the finishing feed rate.
9 At the end of the cycle, the TNC retracts the tool at FMAX to the
2nd setup clearance.
Please note while programming:
Enter the 2nd setup clearance in Q204 so that no collision
between tool and clamping devices can occur.
264
2 at the feed rate for
2 at the feed rate for
Fixed Cycles: Multipass Milling