Siemens SINUMERIK 840D sl Programming Manual page 351

3D radius compensation with CUT3DCC, contour on the machining surface
If CUT3DCC is active with a toroidal miller the programmed path refers to a fictitious
cylindrical mill with the same diameter. The resulting path reference point is shown in the
following figure for a toroidal miller.
The angle between the machining and limitation surface may change from an acute to an
obtuse angle and vice versa even within the same block.
The tool actually used may be either larger or smaller than the standard tool. But the
resulting corner radius must not be negative and the sign in front of the resulting tool radius
must not change.
In CUT3DCC the NC parts program refers to the contour on the machining surface. As with
conventional tool radius compensation, the total radius, which is totaled from
• the tool radius (tool parameter $TC_DP6)
• the wear value (tool parameter $TC_DP15)
and a
• programmed tool offset OFFN.
is used. The position of the limitation surface is determined by the difference between the
two values
• standard tool dimensions and
• tool radius (tool parameter $TC_DP6).
Job planning
Programming Manual, 03/2006 Edition, 6FC5398-2BP10-1BA0
8.5 Activate 3D tool offsets (CUT3DC..., CUT3DF...)
Tool offsets
8-29