Reducing Display Of A Rotary Axis To A Value Less Than 360°: M94 - HEIDENHAIN TNC 640 User Manual

13
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:
Programmed angular value:
Actual distance of traverse:
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.
Example: Reduce the display of all active rotary axes
N50 M94*
Example: Reduce the display of the C axis
N50 M94 C*
Example: Reduce the display of all active rotary axes and then
move the tool in the C axis to the programmed value
M50 G00 C+180 M94*
Effect
M94 is effective only in the NC block where it is programmed.
M94 becomes effective at the start of the block.
584
Multiple-Axis Machining | Miscellaneous functions for rotary axes
538°
180°
-358°
HEIDENHAIN | TNC 640 | ISO Programming User's Manual | 10/2017