HEIDENHAIN TNC 426, User Manual

Page: 301 / 502

HEIDENHAIN TNC 426, TNC 430 275
8.4 Cy
cles f
o
r milling poc
k
e
ts, st
uds and slots
U Set-up clearance Q200 (incremental value): Distance
between tool tip and workpiece surface.
U Depth Q201 (incremental value): Distance between
workpiece surface and bottom of slot
U Feed rate for milling Q207: Traversing speed of the
tool in mm/min while milling.
U Plunging depth Q202 (incremental value): Total
extent by which the tool is fed in the tool axis during
a reciprocating movement
U Machining operation (0/1/2) Q215: Define the
machining operation:
0 : Roughing and finishing
1 : Only roughing
2 : Only finishing
U Workpiece surface coordinate Q203 (absolute
value): Coordinate of the workpiece surface
U 2nd setup clearance Q204 (incremental value):
Z coordinate at which no collision between tool and
workpiece (clamping devices) can occur
U Center in 1st axis Q216 (absolute value): Center of
the slot in the reference axis of the working plane
U Center in 2nd axis Q217 (absolute value): Center of
the slot in the minor axis of the working plane
U Pitch circle diameter Q244: Enter the diameter of
the pitch circle
U Second side length Q219: Enter the slot width. If you
enter a slot width that equals the tool diameter, the
TNC will carry out the roughing process only (slot
milling).
U Starting angle Q245 (absolute value): Enter the polar
angle of the starting point
U Angular length Q248 (incremental value): Enter the
angular length of the slot
U Infeed for finishing Q338 (incremental value):
Infeed per cut. Q338=0: Finishing in one infeed.
Example: NC blocks
52 CYCL DEF 211 CIRCULAR SLOT
Q200=2 ;SET-UP CLEARANCE
Q201=-20 ;DEPTH
Q207=500 ;FEED RATE FOR MILLING
Q202=5 ;PLUNGING DEPTH
Q215=0 ;MACHINING OPERATION
Q203=+30 ;SURFACE COORDINATE
Q204=50 ;2ND SET-UP CLEARANCE
Q216=+50 ;CENTER IN 1ST AXIS
Q217=+50 ;CENTER IN 2ND AXIS
Q244=80 ;PITCH CIRCLE DIAMETR
Q219=12 ;SECOND SIDE LENGTH
Q245=+45 ;STARTING ANGLE
Q248=90 ;ANGULAR LENGTH
Q338=5 ;INFEED FOR FINISHING