HEIDENHAIN TNC 310 (286 140) - Manual (Page 145)

133 HEIDENHAIN TNC 310
Before programming, note the following:
From the current position, the TNC positions the tool at
the starting point 1, first in the working plane and then in
the tool axis.
Pre-position the tool in such a way that no collision
between tool and clamping devices can occur.
ú Starting point in 1st axis Q225 (absolute value):
Min. point coordinate of the surface to be
multipass-milled in the main axis of the working
plane
ú Starting point in 2nd axis Q226 (absolute value):
Min. point coordinate of the surface to be
multipass-milled in the secondary axis of the
working plane
ú Starting point in 3rd axis Q227 (absolute value):
Height in the spindle axis at which multipass-
milling is carried out.
ú First side length Q218 (incremental value): Length
of the surface to be multipass-milled in the main
axis of the working plane, referenced to the
starting point in 1st axis
ú Second side length Q219 (incremental value):
Length of the surface to be multipass-milled in the
secondary axis of the working plane, referenced to
the starting point in 2nd axis
ú Number of cuts Q240: Number of passes to be
made over the width
ú Feed rate for plunging Q206: Traversing speed of
the tool in mm/min when moving from set-up
clearance to the milling depth
ú Feed rate for milling Q207: Traversing speed of the
tool in mm/min while milling.
ú Stepover feed rate Q209: Traversing speed of the
tool in mm/min when moving to the next pass. If
you are moving the tool transversely in the
material, enter Q209 to be smaller than Q207 If you
are moving it transversely in the open, Q209 may
be greater than Q207.
ú Set-up clearance Q200 (incremental value):
Distance between tool tip and milling depth for
positioning at the start and end of the cycle.
8.5 Cycles for Multipass Milling
X
Z
Q200
Q227
Q206
X
Y
Q226
Q225
Q219
Q218
Q207
Q209
N = Q240