HEIDENHAIN TNC 620 Programming Station User Manual

Multiple-Axis Machining | Miscellaneous functions for rotary axes
13
HEIDENHAIN | TNC 620 | Conversational Programming User's Manual | 10/2017
567
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.
Example: Reduce the display of all active rotary axes
L M94
Example: Reduce the display of the C axis
L M94 C
Example: Reduce the display of all active rotary axes and then
move the tool in the C axis to the programmed value
L C+180 FMAX M94
Effect
M94 is effective only in the NC block where it is programmed.
M94 becomes effective at the start of the block.

HEIDENHAIN TNC 620 Programming Station Specifications

General

Brand	HEIDENHAIN
Model	TNC 620 Programming Station
Category	Control Systems
Language	English