Cycle Parameters - HEIDENHAIN TNC 620 User Manual

Fixed Cycles: Cylindrical Surface | CYLINDER SURFACE Slot milling (Cycle 28, DIN/ISO: G128, software
option 1)

Cycle parameters

Q1 Milling depth? (incremental): Distance
between cylindrical surface and contour bottom.
Input range -99999.9999 to 99999.9999
Q3 Finishing allowance for side? (incremental):
Finishing allowance on the slot wall. The finishing
allowance reduces the slot width by twice
the entered value. Input range -99999.9999 to
99999.9999
Q6 Set-up clearance? (incremental): Distance
between tool tip and cylindrical surface. Input
range 0 to 99999.9999
Q10 Plunging depth? (incremental): Infeed per
cut. Input range -99999.9999 to 99999.9999
Q11 Feed rate for plunging?: Traversing speed
of the tool in the spindle axis. Input range 0 to
99999.9999, alternatively FAUTO, fu, FZ
Q12 Feed rate for roughing?: Traversing speed
of the tool in the working plane. Input range 0 to
99999.9999, alternatively FAUTO, fu, FZ
Q16 Cylinder radius?: Radius of the cylinder on
which the contour is to be machined. Input range 0
to 99999.9999
Q17 Dimension type? deg=0 MM/INCH=1: The
dimensions for the rotary axis of the subprogram
are given either in degrees or in mm/inches
Q20 Slot width?: Width of the slot to be
machined. Input range -99999.9999 to 99999.9999
Q21 Tolerance?: If you use a tool smaller than
the programmed slot width Q20, process-related
distortion occurs on the slot wall wherever the
slot follows the path of an arc or oblique line.
If you define the tolerance Q21, the TNC adds
a subsequent milling operation to ensure that
the slot dimensions are as close as possible
to those of a slot that has been milled with a
tool exactly as wide as the slot. With Q21 you
define the permitted deviation from this ideal slot.
The number of subsequent milling operations
depends on the cylinder radius, the tool used,
and the slot depth. The smaller the tolerance is
defined, the more exact the slot is and the longer
the remachining takes. Input range for tolerance
0.0001 to 9.9999
Recommendation: Use a tolerance of 0.02 mm.
Function
HEIDENHAIN | TNC 620 | User's manual for cycle programming | 10/2017
inactive: Enter 0 (default setting).
NC blocks
63 CYCL DEF 28 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 F. ROUGHNG
Q16=25 ;RADIUS
Q17=0 ;TYPE OF DIMENSION
Q20=12 ;SLOT WIDTH
Q21=0 ;TOLERANCE
8
259