HEIDENHAIN TNC 620 (81760x-01) Cycle programming - Manual (Page 107)

Fundamentals of Thread Milling 4.5
4
TNC 620 | User's Manual Cycle Programming | 3/2014
107
4.5 Fundamentals of Thread Milling
Prerequisites
Your machine tool should feature internal spindle cooling
(cooling lubricant at least 30 bars, compressed air supply at
least 6 bars).
Thread milling usually leads to distortions of the thread profile.
To correct this effect, you need tool-specific compensation
values which are given in the tool catalog or are available from
the tool manufacturer. You program the compensation with the
delta value for the tool radius
DR in the TOOL CALL.
The Cycles 262, 263, 264 and 267 can only be used with
rightward rotating tools. For Cycle 265 you can use rightward
and leftward rotating tools.
The working direction is determined by the following input
parameters: Algebraic sign Q239 (+ = right-hand thread / – =
left-hand thread) and milling method Q351 (+1 = climb / –1 =
up-cut). The table below illustrates the interrelation between the
individual input parameters for rightward rotating tools.
Internal
thread Pitch Climb/
Up-cut Work direction
Right-handed + +1(RL) Z+
Left-handed – –1(RR) Z+
Right-handed + –1(RR) Z–
Left-handed – +1(RL) Z–
External
thread Pitch Climb/
Up-cut Work direction
Right-handed + +1(RL) Z–
Left-handed – –1(RR) Z–
Right-handed + –1(RR) Z+
Left-handed – +1(RL) Z+
The TNC references the programmed feed rate
during thread milling to the tool cutting edge. Since
the TNC, however, always displays the feed rate
relative to the path of the tool tip, the displayed value
does not match the programmed value.
The machining direction of the thread changes if you
execute a thread milling cycle in connection with
Cycle 8 MIRROR IMAGE in only one axis.