HEIDENHAIN TNC 640 User Manual page 493

Miscellaneous Functions | Miscellaneous functions for path behavior
Superimposing handwheel positioning during
program run: M118
Standard behavior
In the Program Run operating modes, the control moves the tool as
defined in the NC program.
Behavior with M118
M118 permits manual corrections by handwheel during the
program run. For this purpose, you program M118 and enter an
axis-specific value (linear or rotary axis).
The M118 handwheel superimpositioning function, in
combination with the Dynamic Collision Monitoring
(DCM) function, can only be used at a standstill.
The M118 handwheel superimpositioning function
cannot be used in combination with the Dynamic
Collision Monitoring (DCM) function and the additional
TCPM or M128 function.
In order to use M118 without restrictions, either
deselect the Dynamic Collision Monitoring (DCM)
function using the soft key from the menu or activate a
kinematics operation without collision objects (CMOs).
Danger of collision!
If you use the M118 function to modify the position of a
rotary axis with the handwheel and then execute the M140
function, the control ignores the superimposed values with the
retraction movement. This results in unwanted and unpredictable
movements, especially when using machines with head rotation
axes. There is a danger of collision during these compensating
movements!
Do not combine M118 with M140 when using machines with
head rotation axes.
Input
If you enter M118 in a positioning block, the control continues the
dialog for this block by prompting you for the axis-specific values.
The coordinates are entered with the orange axis direction buttons
or the ASCII keyboard.
Effect
To cancel handwheel positioning, program M118 once again
without coordinate input.
M118 becomes effective at the start of the block.
HEIDENHAIN | TNC 640 | Conversational Programming User's Manual | 10/2017
NOTICE
11
493