HEIDENHAIN TNC 426B (280 472) ISO programming - Manual (Page 147)

131 HEIDENHAIN TNC 410, TNC 426, TNC 430
7.4 Miscellaneous F
unctions f
or Cont
our
ing Beha
vior
Feed rate factor for plunging movements: M103
Standard behavior
The TNC moves the tool at the last programmed feed rate,
regardless of the direction of traverse.
Behavior with M103
The TNC reduces the feed rate when the tool moves in the negati-
ve direction of the tool axis. The feed rate for plunging FZMAX is
calculated from the last programmed feed rate FPROG and a factor
F%:
FZMAX = FPROG x F%
Programming M103
If you enter M103 in a positioning block, the TNC continues the
dialog by asking you the factor F.
Effect
M103 becomes effective at the start of block.
To cancel M103, program M103 once again without a factor.
Example NC blocks
The feed rate for plunging is to be 20% of the feed rate in the
plane.
...
N170 G01 G41 X+20 Y+20 F500 M103 F20 *
N180 Y+50 *
N190 G91 Z–2.5 *
N200 Y+5 Z–5
N210 X+50
N220 G90 Z+5
M103 is activated with machine parameter 7440; see
section 14.1 “General User Parameters.”
Feed rate in micrometers per spindle revolution: M136
(only TNC 426, TNC 430 with NC software 280 474-xx)
Standard behavior
The TNC moves the tool at the programmed feed rate F in mm/min.
Behavior with M136
With M136, the TNC does not move the tool in mm/min, but rather
at the programmed feed rate F in microns per spindle revolution. If
you change the spindle speed by using the spindle override, the
TNC changes the feed rate accordingly.
Effect
M136 becomes effective at the start of block.
You can cancel M136 by programming M137.
Actual contouring feed rate (mm/min):
500
500
100
141
500
500
Hkap7.pm6 29.06.2006, 08:06 131