HEIDENHAIN TNC 410 ISO Programming - Manual (Page 314)

288 8 Programming: Cycles
8.8
C
y
cl
es f
o
r Mu
lt
ip
ass Millin
g RUN DIGITIZED DATA (Cycle G60, not TNC 410)
1 From the current position, the TNC positions the tool in rapid
traverse in the tool axis to the set-up clearance above the MAX
point that you have programmed in the cycle.
2 The tool then moves in rapid traverse in the working plane to the
MIN point you have programmed in the cycle.
3 From this point, the tool advances to the first contour point at the
feed rate for plunging.
4 The TNC subsequently processes all points that are stored in the
digitizing data file at the feed rate for milling. If necessary, the TNC
retracts the tool between machining operations to set-up
clearance if specific areas are to be left unmachined.
5 At the end of the cycle, the tool is retracted in rapid traverse to set-
up clearance.
U U U U PGM Name digitizing data : Enter the name of the file
in which the digitizing data is stored. If the file is not
stored in the current directory, enter the complete
path. If you wish to execute a point table, enter also
the file type .PNT.
U U U U Min. point of range : Lowest coordinates (X, Y and Z
coordinates) in the range to be milled.
U U U U Max. point of range : Highest coordinates (X, Y and Z
coordinates) in the range to be milled.
U U U U Set-up clearance 1 (incremental value): Distance
between tool tip and workpiece surface for tool
movements in rapid traverse.
U U U U Plunging depth 2 (incremental value): Infeed per cut.
U U U U Feed rate for plunging 3 : Traversing speed of the
tool in mm/min during penetration.
U U U U Feed rate for milling 4 : Traversing speed of the tool
in mm/min while milling.
U U U U Miscellaneous function M : Optional entry of a
miscellaneous function, for example M13.
Example: NC block
N64 G60 P01 BSP.I P02 X+0 P03 Y+0
P04 Z-20 P05 X+100 P06 Y+100 P07 Z+0
P08 2 P09 +5 P10 100 P11 350
P12 M13 *
14
X
Z
11
13
12
Before programming, note the following:
You can use Cycle G60 to run digitizing data and PNT files.
If you want to run PNT files in which no tool axis
coordinate is programmed, the milling depth is derived
from the programmed MIN point in the tool axis.