HEIDENHAIN TNC 620 Programming Station

Multiple-axis machining | Miscellaneous functions for rotary axes
11
Reducing display of a rotary axis to a value less than
360°: M94
Standard behavior
The control moves the tool from the current angular value to the
programmed angular value.
Example:
Current angular value: 538°
Programmed angular value: 180°
Actual distance of traverse: -358°
Behavior with M94
At the start of block, the control first reduces the current angular
value to a value less than 360° and then moves the tool to the
programmed value. If multiple rotary axes are active, M94 will reduce
the display of all rotary axes. As an alternative, you can specify a
rotary axis after M94. The control then reduces the display of this
axis only.
If you entered a traverse limit or a software limit switch is active,
M94 is ineffective for the corresponding axis.
21 L M94
; Reduce the display values of all
rotary axes
21 L M94 C
; Reduce the display value of the C
axis
21 L C+180 FMAX M94
; Reduce the display values of all
active rotary axes and then move
in the Caxis to the programmed
value
Effect
M94 is effective only in the NC block where it is programmed.
M94 becomes effective at the start of the block.
464
HEIDENHAIN | TNC620 | Klartext Programming User's Manual | 01/2022