HEIDENHAIN TNC 407 (280 580) User Manual - Manual (Page 167)

TNC 425/TNC 415 B/TNC 407 5-68
5 Programming Tool Movements
Ignore points for calculating the rounding arc with M112: M124 T...
Standard behavior – without M124 T...
All existing points are taken into account for calculating the rounding arc
between two straight lines with M112.
Ignore points – with M124 T...
Particularly when machining digitized 3D surfaces, the distance between
contour points at sections with sharp changes in direction may be too
small to insert a rounding arc with M112. With the miscellaneous function
M124 T..., the TNC filters out such points before calculating the rounding
arc. M124 T... is programmed by entering a minimum distance between
points for T.
If the distance between two points is less than the programmed value,
the TNC automatically ignores the second point and uses the next contour
point for calculating the rounding arc with M112.
NC block: L X+123.723 Y+25.491 R0 FMAX M124 T0.01
Parameter programming
You can also define T through Q parameters.
Duration of effect
M124 T... is effective at the start of block and only if M112 T... A... is
active. M124 T... is cancelled by M113.
5.7 M Functions for Contouring Behavior
Shorter-path traverse of rotary axes : M126
Standard behavior — without M126
The TNC moves a rotary axis whose display has been reduced to a value
less than 360° as follows:
Actual position Nominal position Actual path of traverse
350° 10° –340°
10° 340° +330°
Shorter-path traverse of rotary axes — with M126
The TNC moves a rotary axis whose display has been reduced to a value
less than 360° as follows:
Actual position Nominal position Actual path of traverse
350° 10° +20°
10° 340° –30°
NC block: L C+10 A+340 R0 F500 M126
Duration of effect
M126 is effective at the start of block. M126 is cancelled by M127 or
automatically at the end of the program.