HEIDENHAIN iTNC 530 (340 422) ISO programming - Manual (Page 325)

HEIDENHAIN iTNC 530 325
8.5 Cy
cles f
o
r Mac
h
in
ing
Hole
P
a
tt
er
n
s
CIRCULAR PATTERN (Cycle G220)
1 The TNC moves the tool at rapid traverse from its current position
to the starting point for the first machining operation.
Sequence:
n Move to the 2nd set-up clearance (spindle axis).
n
Approach the starting point in the spindle axis.
n
Move to the 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 blocks
N530 G220 POLAR PATTERN
Q216=+50 ;CENTER IN 1ST AXIS
Q217=+50 ;CENTER IN 2ND AXIS
Q244=80 ;PITCH CIRCLE DIA.
Q245=+0 ;STARTING ANGLE
Q246=+360 ;STOPPING ANGLE
Q247=+0 ;STEPPING ANGLE
Q241=8 ;NR OF REPETITIONS
Q200=2 ;SET-UP CLEARANCE
Q203=+30 ;SURFACE COORDINATE
Q204=50 ;2ND SET-UP CLEARANCE
Q203=1 ;MOVE TO CLEARANCE
Q365=0 ;TYPE OF TRAVERSE
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.