Cycle Parameters - HEIDENHAIN TNC 620 User Manual

6
Fixed Cycles: Pattern Definitions
6.2 POLAR PATTERN (Cycle 220, DIN/ISO: G220, software option 19)

Cycle parameters

Center in 1st axis Q216 (absolute): Center of the
pitch circle in the reference axis of the working
plane. Input range -99999.9999 to 99999.9999
Center in 2nd axis Q217 (absolute): Center of the
pitch circle in the minor axis of the working plane.
Input range -99999.9999 to 99999.9999
Pitch circle diameter Q244: Diameter of the pitch
circle. Input range 0 to 99999.9999
Starting angle Q245 (absolute): Angle between the
reference axis of the working plane and the starting
point for the first machining operation on the pitch
circle. Input range -360.000 to 360.000
Stopping angle Q246 (absolute): 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 full 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. Input range -360.000 to 360.000
Stepping angle 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 (negative =
clockwise). Input range -360.000 to 360.000
Number of repetitions Q241: Number of machining
operations on a pitch circle. Input range 1 to 99999
Set-up clearance Q200 (incremental): Distance
between tool tip and workpiece surface. Input range
0 to 99999.9999
Coordinate of workpiece surface Q203 (absolute):
Coordinate of the workpiece surface. Input range
-99999.9999 to 99999.9999
2nd set-up clearance Q204 (incremental):
Coordinate in the spindle axis at which no collision
between tool and workpiece (fixtures) can occur.
Input range 0 to 99999.9999
Traversing to clearance height Q301: Definition of
how the touch probe is to move between machining
operations:
0: Move at set-up clearance between machining
operations
1: Move at 2nd set-up clearance between machining
operations
164
NC blocks
53 CYCL DEF 220 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
Q301=1 ;MOVE TO CLEARANCE
Q365=0 ;TYPE OF TRAVERSE
TNC 620 | User's Manual Cycle Programming | 3/2014