Pre-Calculating Radius-Compensated Contours (Look Ahead): M120 (Option 21) - HEIDENHAIN TNC 620 User Manual

7
Pre-calculating radius-compensated contours
(LOOK AHEAD): M120 (option 21)
Standard behavior
If the tool radius is larger than the contour step that needs to be
machined with radius compensation, then the control interrupts
program run and issues an error message. M97 inhibits the error
message, but this results in dwell marks and will also move the
corner.
Further information: "Machining small contour steps: M97",
Page 229
The control might damage the contour in case of undercuts.
Behavior with M120
The control checks radius-compensated contours for undercuts and
tool path intersections, and calculates the tool path in advance from
the current NC block. Areas of the contour that would be damaged
by the tool will not be machined (shown darker in the figure). You
can also use M120 to calculate the tool radius compensation for
digitized data or data from an external programming system. This
means that you can compensate for deviations from the theoretical
tool radius.
The number of NC blocks (99 max.) to be calculated in advance
can be defined with LA (Look Ahead) following M120. Note that the
larger the number of NC blocks you choose, the higher the block
processing time will be.
Input
If you define M120 in a positioning block, the control continues
the dialog and prompts you for the number of LA NC blocks to be
calculated in advance.
Effect
Program the function M120 in an NC block that also contains an RL
or RR radius compensation. This way, you can achieve consistent
programming, resulting in clearly structured programs. You can
deactivate the function M120 with the following NC syntax:
R0
M120 LA0
M120 without LA
PGM CALL
Cycle 19 or PLANE functions
M120 becomes effective at the start of the block and remains
effective beyond the milling cycles (option 19).
234
Miscellaneous functions | Miscellaneous functions for path behavior
HEIDENHAIN | TNC 620 | Klartext Programming User's Manual | 01/2022