HEIDENHAIN iTNC 530 (340 49x-04) ISO programming - Manual (Page 441)

HEIDENHAIN iTNC 530 441
8.8 Cy
cles f
o
r Multipass Milling
RUN 3-D DATA (Cycle G60)
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
3-D 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.
 3-D data file name : Enter the name of the file in
which the data is stored. If the file is not stored in the
current directory, enter the complete path.
 Min. point of range: Lowest coordinates (X, Y and Z
coordinates) in the range to be milled.
 Max. point of range: Largest coordinates (X, Y and Z
coordinates) in the range to be milled.
 Set-up clearance 1 (incremental value): Distance
between tool tip and workpiece surface for tool
movements in rapid traverse.
 Plunging depth 2 (incremental value): Infeed per cut.
 Feed rate for plunging 3 : Traversing speed of the
tool in mm/min during penetration.
 Feed rate for milling 4 : Traversing speed of the tool
in mm/min while milling.
 Miscellaneous function M: Optional entry of a
miscellaneous function, for example M13.
Example: NC block
N64 G60 P01 BSP.I P01 X+0 P02 Y+0
P03 Z-20 P04 X+100 P05 Y+100 P06 Z+0
P07 2 P08 +5 P09 100 P10 350 M13 *
4
Y
X MIN
MAX
X
Z
1
2
3
Before programming, note the following
You can use Cycle 30 to run conversational programs
created offline in multiple infeeds.