HEIDENHAIN TNC 320 (340 55x-03) - Manual (Page 276)

276 8 Programming: Cycles
8.3 Cy
cles f
o
r Milling P
o
c
k
ets, St
uds and Slots
 Set-up clearance Q200 (incremental value): Distance
between tool tip and workpiece surface.
 Depth Q201 (incremental value): Distance between
workpiece surface and bottom of slot.
 Feed rate for milling Q207: Traversing speed of the
tool in mm/min while milling.
 Plunging depth Q202 (incremental value): Total
extent by which the tool is fed in the spindle axis
during a reciprocating movement.
 Machining operation (0/1/2) Q215: Define the
machining operation:
0: Roughing and finishing
1: Only roughing
2: Only finishing
 Workpiece surface coordinate Q203 (absolute
value): Coordinate of the workpiece surface.
 2nd set-up clearance Q204 (incremental value):
Z coordinate at which no collision between tool and
workpiece (clamping devices) can occur.
 Center in 1st axis Q216 (absolute value): Center of
the slot in the reference axis of the working plane.
 Center in 2nd axis Q217 (absolute value): Center of
the slot in the minor axis of the working plane.
 First side length Q218 (value parallel to the
reference axis of the working plane): Enter the length
of the slot.
 Second side length Q219 (value parallel to the minor
axis of the working plane): Enter the slot width. If you
enter a slot width that equals the tool diameter, the
TNC will carry out the roughing process only (slot
milling).
Danger of collision!
Use the machine parameter displayDepthErr to define
whether, if a positive depth is entered, the TNC should
output an error message (on) or not (off).
Keep in mind that the TNC reverses the calculation for pre-
positioning when a positive depth is entered. This
means that the tool moves at rapid traverse in the tool axis
at safety clearance below the workpiece surface!
X
Z
Q200
Q201
Q207
Q202
Q203
Q204
X
Y
Q21
9
Q218
Q217
Q216
Q224