HEIDENHAIN ITNC 530 - 6-2010 DIN-ISO PROGRAMMING User Manual page 408

Reducing display of a rotary axis to a value less
than 360°: M94
Standard behavior
The TNC moves the tool from the current angular value to the
programmed angular value.
Example:
Current angular value:
Programmed angular value:
Actual distance of traverse:
Behavior with M94
At the start of block, the TNC first reduces the current angular value to
a value less than 360° and then moves the tool to the programmed
value. If several rotary axes are active, M94 will reduce the display of
all rotary axes. As an alternative you can enter a rotary axis after M94.
The TNC then reduces the display only of this axis.
Example NC blocks
To reduce display of all active rotary axes:
N50 M94 *
To reduce display of the C axis only:
N50 M94 C *
To reduce display of all active rotary axes and then move the tool in
the C axis to the programmed value:
N50 G00 C+180 M94 *
Effect
M94 is effective only in the block in which it is programmed.
M94 becomes effective at the start of block.
408
538°
180°
-358°
Programming: Multiple Axis Machining