Automatically Retract Tool From The Contour At An Nc Stop: M148 - HEIDENHAIN TNC 320 User Manual

Automatically retract tool from the contour at an NC
stop: M148
Standard behavior
At an NC stop the TNC stops all traverse movements. The tool
stops moving at the point of interruption.
Behavior with M148
The M148 function must be enabled by the machine
tool builder. The machine tool builder defines in
a machine parameter the path that the TNC is to
traverse for a LIFTOFF command.
The TNC retracts the tool by up to 2 mm in the direction of the
tool axis if, in the LIFTOFF column of the tool table, you set the
parameter Y for the active tool See "Enter tool data into the table",
page 144.
LIFTOFF takes effect in the following situations:
An NC stop triggered by you
An NC stop triggered by the software, e.g. if an error occurred
in the drive system
When a power interruption occurs
Danger of collision!
Remember that, especially on curved surfaces, the
surface can be damaged during return to the contour.
Retract the tool before returning to the contour!
In the CfgLiftOff machine parameter, define the
value by which the tool is to be retracted. In the
CfgLiftOff machine parameter you can also switch
the function off.
Effect
M148 remains in effect until deactivated with M149.
M148 becomes effective at the start of block, M149 at the end of
block.
TNC 320 | User's Manual HEIDENHAIN Conversational Programming | 5/2013
Miscellaneous functions for path behavior
9
9.4
323