HEIDENHAIN ITNC 530 User Manual page 385

Enter in MP7441 bit 2 whether the TNC should output an
error message (bit 2=1) or not (bit 2=0) if a positive depth
is entered.
Danger of collision!
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!
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 tool 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.
Pitch circle diameter Q244: Enter the diameter of
the pitch circle.
2nd side length Q219: 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).
Starting angle Q245 (absolute value): Enter the polar
angle of the starting point.
HEIDENHAIN iTNC 530
Z
Q207
Q200
Q203
Q202
Q201
Y
Q248
Q219
Q217
Q216
Q204
X
Q245
X
385