Programming and Operating Manual (Turning)
01/2017
193
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.
The contour must contain at least 3 blocks with motions in the two axes of the machining plane.
If the contour program is too short, 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.
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.
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.
See the following illustration for contour definition:
To Next Page
Loading...
