Contour data (cycle g120), G120 contour data (essential) – HEIDENHAIN TNC 410 ISO Programming User Manual
Page 296
270
8 Programming: Cycles
8.7 SL Cy
cles Gr
ou
p II (no
t T
N
C
4
1
0)
CONTOUR DATA (Cycle G120)
Machining data for the subprograms describing the subcontours are
entered in Cycle G120.
U
U
U
U
Milling depth
Q1 (incremental value): Distance
between workpiece surface and bottom of pocket.
U
U
U
U
Path overlap
factor Q2: Q2 x tool radius = stepover
factor k.
U
U
U
U
Finishing allowance for side
Q3 (incremental
value): Finishing allowance in the working plane
U
U
U
U
Finishing allowance for floor
Q4 (incremental
value): Finishing allowance in the tool axis.
U
U
U
U
Workpiece surface coordinate
Q5 (absolute value):
Absolute coordinate of the workpiece surface
U
U
U
U
Set-up clearance
Q6 (incremental value): Distance
between tool tip and workpiece surface.
U
U
U
U
Clearance height
Q7 (absolute value): Absolute
height at which the tool cannot collide with the
workpiece (for intermediate positioning and retraction
at the end of the cycle).
U
U
U
U
Inside corner radius
Q8: Inside “corner” rounding
radius; entered value is referenced to the tool
midpoint path.
U
U
U
U
Direction of rotation ? Clockwise = -1
Q9:
Machining direction for pockets.
n
Clockwise (Q9 = –1 up-cut milling for pocket and
island)
n
Counterclockwise (Q9 = +1 climb milling for pocket
and island)
You can check the machining parameters during a program
interruption and overwrite them if required.
Example: NC block
N57 G120 Q1=-20 Q2=1 Q3=+0.2 Q4=+0.1 Q5=+30
Q6=+2 Q7=+80 Q8=0.5 Q9=+1 *
X
Y
k
Q9=+1
Q8
X
Z
Q6
Q7
Q1
Q10
Q5
Before programming, note the following:
Cycle G120 is DEF active, meaning Cycle G120becomes
effective as soon as it is defined in the part program.
The algebraic sign for the cycle parameter DEPTH
determines the working direction. If you program depth =
0, the TNC does not execute that next cycle.
The machining data entered in Cycle G120 are valid for
Cycles G121 to G124.
If you are using the SL cycles in Q parameter programs,
the cycle parameters Q1 to Q19 cannot be used as
program parameters.