Cycle Parameters - HEIDENHAIN TNC 640 User Manual

6

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
208
Fixed Cycles: Pattern Definitions | POLAR PATTERN (Cycle 220, DIN/ISO: G220)
NC blocks
53 CYCL DEF 220 POLAR PATTERN
Q216=+50 ;CENTER IN 1ST AXIS
Q217=+50 ;CENTER IN 2ND AXIS
Q244=80 ;PITCH CIRCLE DIAMETR
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
HEIDENHAIN | User's manual for cycle programming | 10/2017