Siemens SINUMERIK 840D sl Programming Manual page 764

Work preparation
3.13 Tool offsets
Approach behavior
The approach behavior is always NORM for the 3D variant of the tool radius compensation.
Behavior at outside corners
Outside corners are treated as circles with radius 0 for face milling, whereby the circle plane
extends from the end tangent of the first block to the start tangent of the second block. In this
way, the orientation can be changed during block transition. A circle is therefore always
inserted as contour element at an outside corner. The intersection procedure is not available
with face milling.
Behavior for changes in orientation at outside corners
The ORIC and ORID G commands are used to determine whether changes in orientation
programmed between two blocks forming the corner are executed before the inserted circle
block (ORID) is processed or at the same time (ORIC).
Tool radius compensation referred to a differential tool
3D tool radius compensation referring to a differential tool is selected using the CUT3DFD
command. It should be applied if the programmed contour refers to the center-point path of a
standard tool, and a tool other than a differential tool is used for machining. When calculating
the 3D tool radius compensation, only the wear value of the radius of the active tool
($TC_DP15) and any programmed tool offsets OFFN and TOFFR/TOFFLR are taken into
account. The basic radius ($TC_DP6) of the active tool is not taken into account.
3D face milling with CUT3DFD is only possible in combination with "Smoothing of surface
normals in 3D face milling". This is activated by calling the "Top Surface" function (requires a
license) via CYCLE832(...). Activation must take place before the tool offset is activated with
G41/G42; not directly before tool intervention, but rather one path length before that, which
corresponds to approx. 1000 times the contour tolerance (e.g. 1000 x 0.01 mm = 10 mm).
Deactivation must be executed in reverse order: First switch off the tool offset with G40, then
deactivate with e.g. CUT2D (or similar) after a path length which corresponds with
approximately 1000 time the contour tolerance.
In order to be able to use the "Smoothing of surface normals in 3D face milling", the
"Interpolation of surface normals via polynomials" function must also be enabled:
MD28291 $MC_MM_SMOOTH_SURFACE_NORMALS = TRUE
Note
For 3D face milling with CUT3DFD in combination with "Top Surface", the setting
recommendations regarding "Top Surface" must be observed.
A special test program is provided in the SIOS portal for checking the set data.
→ Test program for Top Surface
109738423)
See also
CYCLE832 - High-Speed Settings (Page 1107)
764
(https://support.industry.siemens.com/cs/ww/en/view/
Programming Manual, 12/2019, 6FC5398-2EP40-0BA0
NC programming