HEIDENHAIN ITNC 530 User Manual page 444

Starting point in 1st axis Q225 (absolute value):
Minimum point coordinate of the surface to be
multipass-milled in the reference axis of the working
plane.
Starting point in 2nd axis Q226 (absolute value):
Minimum-point coordinate of the surface to be
multipass-milled in the minor axis of the working
plane.
Starting point in 3rd axis Q227 (absolute value):
Height in the spindle axis at which multipass-milling is
carried out.
1st side length Q218 (incremental value): Length of
the surface to be multipass-milled in the reference
axis of the working plane, referenced to the starting
point in 1st axis.
2nd side length Q219 (incremental value): Length of
the surface to be multipass-milled in the minor axis of
the working plane, referenced to the starting point in
1st axis.
Number of cuts Q240: Number of passes to be made
over the width.
Feed rate for plunging Q206: Traversing speed of
the tool in mm/min when moving from set-up
clearance to the milling depth.
Feed rate for milling Q207: Traversing speed of the
tool in mm/min while milling.
Stepover feed rate Q209: Traversing speed of the
tool in mm/min when moving to the next pass. If you
are moving the tool transversely in the material, enter
Q209 to be smaller than Q207. If you are moving it
transversely in the open, Q209 may be greater than
Q207.
Set-up clearance Q200 (incremental value): Distance
between tool tip and milling depth for positioning at
the start and end of the cycle.
444
Y
N = Q240
Q226
Q218
Q225
Z
Q227
Example: NC blocks
71 CYCL DEF 230 MULTIPASS MILLING
Q225=+10 ;STARTING PNT 1ST AXIS
Q226=+12 ;STARTING PNT 2ND AXIS
Q227=+2.5 ;STARTING PNT 3RD AXIS
Q218=150 ;1ST SIDE LENGTH
Q219=75 ;2ND SIDE LENGTH
Q240=25 ;NUMBER OF CUTS
Q206=150 ;FEED RATE FOR PLUNGING
Q207=500 ;FEED RATE FOR MILLING
Q209=200 ;STEPOVER FEED RATE
Q200=2 ;SET-UP CLEARANCE
Q207
Q209
X
Q206
Q200
X
8 Programming: Cycles