HEIDENHAIN TNC 426B (280 472) ISO programming - Manual (Page 203)

187 HEIDENHAIN TNC 410, TNC 426, TNC 430
CIRCULAR PATTERN (Cycle 220)
1 At rapid traverse, the TNC moves the tool from its current
position to the starting point for the first machining operation.
The tool is positioned in the following sequence:
■ Move to 2nd set-up clearance (tool axis)
■ Approach starting point in the working plane
■ Move to set-up clearance above the workpiece surface
(tool 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.
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 G208 and G212 to G215, 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.
ú Center in 1st axis Q216 (absolute value): Center of the
pitch circle in the main axis of the working plane
ú Center in 2nd axis Q217 (absolute value): Center of the
pitch circle in the secondary axis of the working plane
ú Pitch circle diameter Q244: Diameter of the pitch circle
ú Starting angle Q245 (absolute value): Angle between
the main axis of the working plane and the starting
point for the first machining operation on the pitch
circle
ú Stopping angle Q246 (absolute value): Angle between
the main 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.
ú ANGLE STEP Q247 (incremental): Angle between two
machining operations on a pitch circle. If you enter an
ANGLE STEP of 0, the TNC will calculate the ANGLE
STEP from the STARTING and STOPPING
ANGLES and the number of pattern repetitions. If you
enter a value other than 0, the TNC will not take the
STOPPING ANGLE into account. The sign for the
ANGLE STEP determines the working direction (- =
clockwise).
8.5 Cy
cles f
or Mac
hining P
oint P
a
tt
er
ns
X
Z
Q200
Q203
Q204
X
Y
Q217
Q216
Q247
Q245
Q244
Q246
N = Q241
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*
Kkap8.pm6 29.06.2006, 08:06 187