HEIDENHAIN TNC 320 User Manual page 201

Cycle parameters
U
Milling depth Q1 (incremental): Distance between
the cylindrical surface and the floor of the contour.
Input range -99999.9999 to 99999.9999
U Finishing allowance for side Q3 (incremental):
Finishing allowance in the plane of the unrolled
cylindrical surface. This allowance is effective in the
direction of the radius compensation. Input range
-99999.9999 to 99999.9999
U
Set-up clearance Q6 (incremental): Distance
between the tool tip and the cylinder surface. Input
range 0 to 99999.9999
U Plunging depth Q10 (incremental): Infeed per cut.
Input range -99999.9999 to 99999.9999
U
Feed rate for plunging Q11: Traversing speed of the
tool in the spindle axis. Input range 0 to 99999.9999;
alternatively FAUTO, FU, FZ
U Feed rate for milling Q12: Traversing speed of the
tool in the working plane. Input range 0 to
99999.9999; alternatively FAUTO, FU, FZ
U
Cylinder radius Q16: Radius of the cylinder on which
the contour is to be machined. Input range 0 to
99999.9999
U Dimension type? deg=0 MM/INCH=1 Q17: The
coordinates for the rotary axis of the subprogram are
given either in degrees (0) or in mm/inches (1).
HEIDENHAIN TNC 320
Example: NC blocks
63 CYCL DEF 27 CYLINDER SURFACE
Q1=-8 ;MILLING DEPTH
Q3=+0 ;ALLOWANCE FOR SIDE
Q6=+0 ;SET-UP CLEARANCE
Q10=+3 ;PLUNGING DEPTH
Q11=100 ;FEED RATE FOR PLNGNG
Q12=350 ;FEED RATE FOR MILLING
Q16=25 ;RADIUS
Q17=0 ;TYPE OF DIMENSION
201