Siemens SINUMERIK 808D ADVANCED Programming And Operating Manual page 165

DT and DAM (dwell time and path length)
These parameters can be used to achieve an interruption of the individual roughing steps after certain distances traversed in
order to carry out chip breaking. These parameters are only relevant for roughing. The parameter DAM is used to define the
maximum distance after which chip breaking is to be carried out. In DT, an appropriate dwell time (in seconds) can be
programmed which is carried out at each of the cut interruption points. If no distance is specified for the cut interruption
(DAM=0), uninterrupted roughing steps without dwell times are created.
_VRT (lift-off distance)
Parameter _VRT can be used to program the amount by which the tool is retracted in both axes when roughing.
For _VRT=0 (parameter not programmed), the tool will retract by 1 mm.
Contour definition
The contour must contain at least 3 blocks with motions in the two axes of the machining plane.
If the contour program is shorter, the cycle is aborted after the alarms 10933 "Number of contour blocks contained in the
contour program not sufficient" and 61606 "Error in contour preparation" have been output.
Relief cut elements can be connected directly one after the other. Blocks without motions in the plane can be written without
restrictions.
In the cycle, all traversing blocks are prepared for the first two axes of the current plane since only these are involved in the
cutting process. The contour program may contain any motions programmed for other axes; their distances to be traversed,
however, will not come into effect during the whole cycle.
Only straight line and circle programming with G0, G1, G2 and G3 are permitted as the geometry in the contour.
Furthermore, it is also possible to program the commands for rounding and chamfer. If any other motion commands are
programmed in the contour, the cycle is aborted with the alarm 10930 "Illegal type of interpolation in the stock removal
contour".
The first block with a traversing motion in the current machining plane must contain a motion command G0, G1, G2 or G3;
otherwise, the cycle is canceled, and alarm 15800 "Incorrect prerequisites for CONTPRON" is issued. This alarm is also
issued if G41/42 is active. The starting point of the contour is the first programmed position in the machining plane.
To machine the programmed contour, a cycle-internal memory is prepared which can accommodate a certain maximum
number of contour elements; how many, depends on the contour. If a contour contains too many contour elements, the cycle
is canceled, and alarm 10934 "Contour table overflow" is issued. In this case, the contour must be split over several contour
sections, and the cycle for each section must be called separately.
If the maximum diameter is not at the programmed end or starting point of the contour, the cycle will automatically add an
axis-parallel straight line to complete the contour maximum, and this part is removed as the undercut.
Programming and Operating Manual (Turning)
165
6FC5398-5DP10-0BA2, 06/2015