Automatically Retracting The Tool From The Contour At An Nc Stop: M148 - HEIDENHAIN TNC 640 User Manual

Miscellaneous Functions | Miscellaneous functions for path behavior
Automatically retracting the tool from the contour at
an NC stop: M148
Standard behavior
In case of an NC stop, the control stops all traverse movements.
The tool stops moving at the point of interruption.
Behavior with M148
Refer to your machine manual.
This function must be configured and enabled by your
machine tool builder.
In the CfgLiftOff (no. 201400) machine parameter, the
machine tool builder defines the path the control is to
traverse for a LIFTOFF command. You can also use
the CfgLiftOff machine parameter to deactivate the
function.
Set the Y parameter in the LIFTOFF column of the tool table for the
active tool. The control then retracts the tool from the contour by 2
mm max. in the direction of the tool axis.
Further information: "Entering tool data into the table", page 238
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
Effect
M148 remains in effect until deactivated with M149.
M148 becomes effective at the start of the block, M149 at the end
of the block.
HEIDENHAIN | TNC 640 | ISO Programming User's Manual | 10/2017
11
477