HEIDENHAIN TNC 426, TNC 430 215
8.3 Cycles for Drilling, Tapping and Thread Milling
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 hole
U Feed rate for plunging Q206: Traversing speed of
the tool during reaming in mm/min
U Dwell time at depth Q211: Time in seconds that the
tool remains at the hole bottom
U Retraction feed rate Q208: Traversing speed of the
tool in mm/min when retracting from the hole. If you
enter Q208 = 0, the tool retracts at the reaming feed
rate.
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.
Example: NC blocks
10 L Z+100 R0 FMAX
11 CYCL DEF 201 REAMING
Q200 = 2 ;SET-UP CLEARANCE
Q201 = -15 ;DEPTH
Q206 = 100 ;FEED RATE FOR PLUNGING
Q211 = 0.5 ;DWELL TIME AT BOTTOM
Q208 = 250 ;RETRACTION FEED TIME
Q203 = +20 ;SURFACE COORDINATE
Q204 = 100 ;2ND SET-UP CLEARANCE
12 L X+30 Y+20 FMAX M3
13 CYCL CALL
14 L X+80 Y+50 FMAX M9
15 L Z+100 FMAX M2
To Next Page
Loading...
Need help?
General
