Cycle Parameters - HEIDENHAIN TNC 620 User Manual

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

Cycle parameters

Q216 Center in 1st axis? (absolute): Pitch circle
center in the reference axis of the working plane.
Input range -99999.9999 to 99999.9999
Q217 Center in 2nd axis? (absolute): Pitch circle
center in the minor axis of the working plane.
Input range -99999.9999 to 99999.9999
Q244 Pitch circle diameter?: Diameter of the
pitch circle. Input range 0 to 99999.9999
Q245 Starting angle? (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
Q246 Stopping angle? (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 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. Input
range -360.000 to 360.000
Q247 Intermediate stepping angle?
(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
Q241 Number of repetitions?: Number of
machining operations on a pitch circle. Input range
1 to 99999
Q200 Set-up clearance? (incremental): Distance
between tool tip and workpiece surface. Input
range 0 to 99999.9999
Q203 Workpiece surface coordinate? (absolute):
Coordinate of the workpiece surface. Input range
-99999.9999 to 99999.9999
Q204 2nd set-up clearance? (incremental):
Coordinate in the spindle axis at which no collision
between tool and workpiece (fixtures) can occur.
Input range 0 to 99999.9999
Q301 Move to clearance height (0/1)?: Definition
of how the tool moves between machining
operations:
0: Move at safety clearance between machining
operations
200
NC blocks
53 CYCL DEF 220 POLAR PATTERN
Q216=+50
Q217=+50
Q244=80
Q245=+0
Q246=+360
Q247=+0
Q241=8
Q200=2
Q203=+30
Q204=50
Q301=1
Q365=0
HEIDENHAIN | TNC 620 | User's manual for cycle programming | 10/2017
;CENTER IN 1ST AXIS
;CENTER IN 2ND AXIS
;PITCH CIRCLE DIAMETR
;STARTING ANGLE
;STOPPING ANGLE
;STEPPING ANGLE
;NR OF REPETITIONS
;SET-UP CLEARANCE
;SURFACE COORDINATE
;2ND SET-UP CLEARANCE
;MOVE TO CLEARANCE
;TYPE OF TRAVERSE