HEIDENHAIN TNC 410 ISO Programming - Manual (Page 280)

254 8 Programming: Cycles
8.5 Cy
cles f
o
r Mac
h
in
ing
Hole
P
a
tt
er
n
s
CIRCULAR PATTERN (Cycle G220)
1 At rapid traverse, the TNC moves the tool from its current position
to the starting point for the first machining operation.
Sequence:
n Move to second set-up clearance (spindle axis)
n
Approach the starting point in the spindle axis.
n Move to set-up clearance above the workpiece surface (spindle
axis).
2 From this position, the TNC executes the last defined fixed cycle.
3 The tool then approaches the starting point for the next machining
operation on a straight line at set-up clearance (or 2nd set-up
clearance).
4 This process (1 to 3) is repeated until all machining operations have
been executed.
U U U U Center in 1st axis Q216 (absolute value): Center of
the pitch circle in the reference axis of the working
plane.
U U U U Center in 2nd axis Q217 (absolute value): Center of
the pitch circle in the minor axis of the working plane.
U U U U Pitch circle diameter Q244: Diameter of the pitch
circle.
U U U U Starting angle Q245 (absolute value): Angle
between the reference axis of the working plane and
the starting point for the first machining operation on
the pitch circle.
U U U U Stopping angle Q246 (absolute value): Angle
between the reference axis of the working plane and
the starting point for the last machining operation on
the pitch circle (does not apply to complete circles).
Do not enter the same value for the stopping angle
and starting angle. If you enter the stopping angle
greater than the starting angle, machining will be
carried out counterclockwise; otherwise, machining
will be clockwise.
Example: NC block
N53 G220 Q216=+50 Q217=+50 Q244=80
Q245=+0 Q246=+360 Q247=+0 Q241=8
Q200=2 Q203=+0 Q204=50 Q301=1 *
X
Y
Q217
Q216
Q247
Q245
Q244
Q246
N = Q241
X
Z
Q200
Q203
Q204
Before programming, note the following:
Cycle G220 is DEF active, which means that Cycle G220
automatically calls the last defined fixed cycle.
If you combine Cycle G220 with one of the fixed cycles
G200 to G209, G212 to G215 and G262 to G267, the set-
up clearance, workpiece surface and 2nd set-up clearance
that you defined in Cycle G220 will be effective for the
selected fixed cycle.