HEIDENHAIN TNC 310 (286 140) - Manual (Page 139)

127 HEIDENHAIN TNC 310
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 setup clearance (tool axis)
■ Approach starting point in the machining plane
■ Move to setup 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 220 is DEF active, which means that Cycle 220
automatically calls the last defined fixed cycle.
If you combine Cycle 220 with one of the fixed cycles
200 to 204 and 212 to 215, the set-up clearance,
workpiece surface and 2nd set-up clearance that you
defined in Cycle 220 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. 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.
8.4 Cy
cles f
or Mac
hining Hole P
at
ter
ns
X
Z
Q200
Q203
Q204
X
Y
Q217
Q216
Q247
Q245
Q244
Q246
N = Q241