Cycle Parameters - HEIDENHAIN TNC 620 User Manual

8
Fixed Cycles: Cylindrical Surface
8.3 CYLINDER SURFACE Slot milling (Cycle 28, DIN/ISO: G128, software
option 1)

Cycle parameters

Milling depth Q1 (incremental): Distance between
the cylindrical surface and the floor of the contour.
Input range -99999.9999 to 99999.9999
Finishing allowance for side Q3 (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
Set-up clearance Q6 (incremental): Distance
between the tool tip and the cylinder surface. Input
range 0 to 99999.9999
Plunging depth Q10 (incremental): Infeed per cut.
Input range -99999.9999 to 99999.9999
Feed rate for plunging Q11: Traversing speed
of the tool in the spindle axis. Input range 0 to
99999.9999, alternatively FAUTO, FU, FZ
Feed rate for milling Q12: Traversing speed of
the tool in the working plane. Input range 0 to
99999.9999, alternatively FAUTO, FU, FZ
Cylinder radius Q16: Radius of the cylinder on
which the contour is to be machined. Input range 0
to 99999.9999
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).
Slot width Q20: Width of the slot to be machined.
Input range -99999.9999 to 99999.9999
Tolerance Q21: 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
228
inactive: Enter 0 (default setting)
NC blocks
63 CYCL DEF 28 CYLINDER SURFACE
HEIDENHAIN | TNC 620 | User's manual for cycle programming | 9/2015
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 ;DIMENSION TYPE
Q20=12 ;SLOT WIDTH
Q21=0 ;TOLERANCE