Cylinder Surface (Cycle 39, Din/Iso: G139, Software Option 1); Cycle Run - HEIDENHAIN TNC 620 User Manual

Fixed Cycles: Cylindrical Surface | CYLINDER SURFACE (Cycle 39, DIN/ISO: G139, software option 1)
8.5 CYLINDER SURFACE (Cycle 39, DIN/ISO:
G139, software option 1)

Cycle run

This cycle enables you to machine a contour on a cylindrical
surface. The contour to be machined is programmed on the
unrolled surface of the cylinder. With this cycle the TNC adjusts the
tool so that, with radius compensation active, the wall of the open
contour is always parallel to the cylinder axis.
The contour is described in a subprogram identified in Cycle 14
CONTOUR.
In the subprogram you always describe the contour with the
coordinates X and Y, regardless of which rotary axes exist on your
machine. This means that the contour description is independent
of your machine configuration. The path functions L, CHF, CR, RND
and CT are available.
Unlike Cycles 28 and 29, in the contour subprogram you define the
actual contour to be machined.
1 The TNC positions the tool over the starting point of machining.
The TNC locates the starting point next to the first point defined
in the contour subprogram, offset by the tool diameter.
2 The TNC then moves the tool to the first plunging depth.
The tool approaches the workpiece on a tangential path or
on a straight line at the milling feed rate Q12. A finishing
allowance programmed for the side is taken into account. (The
approaching behavior depends on the parameter ConfigDatum,
CfgGeoCycle, apprDepCylWall.)
3 At the first plunging depth, the tool mills along the programmed
contour at the milling feed rate Q12 until the contour train is
completed.
4 The tool then departs the ridge wall on a tangential path and
returns to the starting point of machining.
5 Steps 2 to 4 are repeated until the programmed milling depth
Q1 is reached.
6 Finally, the tool retracts in the tool axis to the clearance height.
HEIDENHAIN | TNC 620 | User's manual for cycle programming | 10/2017
8
263