Siemens SINUMERIK 840D sl Programming Manual page 292

Fundamentals
2.10 Tool radius compensation
Further information
The original functionality has been modified as follows:
● A change from G40 to G41/G42 and vice-versa is no longer treated as a tool change.
Therefore, a preprocessing stop no longer occurs with TRANSMIT.
● The straight line between the tool edge center points at the block start and block end is used
to calculate intersection points with the approach and retraction block. The difference
between the tool edge reference point and the tool edge center point is superimposed on
this movement.
On approach and retraction with KONT (tool circumnavigates the contour point, see above
subsection "Contour approach and retraction"), superimposition takes place in the linear
part block of the approach or retraction motion. The geometric conditions are therefore
identical for tools with and without a relevant tool point direction. Deviations from the
previous behavior occur only in relatively rare cases where the approach or retraction block
does not intersect with an adjacent traversing block, see the following figure:
● In circle blocks and in motion blocks containing rational polynomials with a denominator
degree > 4, it is not permitted to change a tool with active tool radius compensation in cases
where the distance between the tool edge center point and the tool edge reference point
changes. With other types of interpolation, it is now possible to change when a
transformation is active (e.g., TRANSMIT).
● For tool radius compensation with variable tool orientation, the transformation from the tool
edge reference point to the tool edge center point can no longer be performed by means of
a simple zero offset. Tools with a relevant tool point direction are therefore not permitted for
3D peripheral milling (an alarm is output).
Note
The subject is irrelevant with respect to face milling as only defined tool types without
relevant tool point direction are permitted for this operation anyway. (A tool with a type,
which has not been explicitly approved, is treated as a ball end mill with the specified radius.
A tool point direction parameter is ignored).
292
Programming Manual, 12/2019, 6FC5398-2EP40-0BA0
NC programming