HEIDENHAIN TNC 426, User Manual

Page: 247 / 502

HEIDENHAIN TNC 426, TNC 430 221
8.3 Cy
cles f
o
r Dr
illing, T
a
pping and Thr
ead Milling
U Set-up clearance Q200 (incremental value): Distance
between tool tip and workpiece surface.
U Depth of counterbore Q249 (incremental value):
Distance between underside of workpiece and the
top of the hole. A positive sign means the hole will be
bored in the positive spindle axis direction.
U Material thickness Q250 (incremental value):
Thickness of the workpiece
U Off-center distance Q251 (incremental value): Off-
center distance for the boring bar; value from tool
data sheet
U Tool edge height Q252 (incremental value): Distance
between the underside of the boring bar and the main
cutting tooth; value from tool data sheet
U Feed rate for pre-positioning Q253: Traversing
speed of the tool when moving in and out of the
workpiece, in mm/min
U Feed rate for counterboring Q254: Traversing
speed of the tool during counterboring in mm/min
U Dwell time Q255: Dwell time in seconds at the top of
the bore hole
U Workpiece surface coordinate Q203 (absolute
value): Coordinate of the workpiece surface
U 2nd set-up clearance Q204 (incremental value):
Coordinate in the tool axis at which no collision
between tool and workpiece (clamping devices) can
occur.
U Disengaging direction (0/1/2/3/4) Q214:
Determine the direction in which the TNC displaces
the tool by the off-center distance (after spindle
orientation).
Example: NC blocks
11 CYCL DEF 204 BACK BORING
Q200=2 ;SET-UP CLEARANCE
Q249=+5 ;DEPTH OF COUNTERBORE
Q250=20 ;MATERIAL THICKNESS
Q251=3.5 ;OFF-CENTER DISTANCE
Q252=15 ;TOOL EDGE HEIGHT
Q253=750 ;F PRE-POSITIONING
Q254=200 ;F COUNTERBORING
Q255=0 ;DWELL TIME
Q203=+20 ;SURFACE COORDINATE
Q204=50 ;2ND SET-UP CLEARANCE
Q214=1 ;DISENGAGING DIRECTN
Q336=0 ;ANGLE OF SPINDLE
1 Retract tool in the negative reference axis
direction
2 Retract tool in the negative secondary axis
direction
3 Retract tool in the positive reference axis
direction
4 Retract tool in the positive secondary axis
direction
Danger of collision
Check the position of the tool tip when you program a
spindle orientation to the angle that you enter in Q336 (for
example, in the Positioning with Manual Data Input mode
of operation). Set the angle so that the tool tip is parallel to
a coordinate axis. Select a disengaging direction in which
the tool moves away from the edge of the hole.