Siemens SINUMERIK 808D ADVANCED Diagnostic Manual page 117

Explanation: Deselection of tool radius compensation with G40 can only be performed in blocks where the G function G00 (rapid
traverse) or G01 (feed) is active.
In the block with G40, at least one axis in the plane G17 to G19 must be written. It is always advisable to write both axes
because, as a rule, both axes are traversed when deselecting the compensation.
Reaction: Correction block is reorganized.
Local alarm reaction.
Interface signals are set.
Alarm display.
NC Stop on alarm at block end.
Remedy: Correct the NC program and put the compensation selection in a block with linear interpolation.
Programm Clear alarm with NC START or RESET key and continue the program.
continuation:
10755 [Channel %1: ] Block %2 selection of the tool radius compensation via KONT not possible at the
current starting point
Parameters: %1 = Channel number
%2 = Block number, label
Explanation: When activating the cutter radius compensation with KONT the starting point of the approach block is within the
compensation circle and therefore already violates the contour.
If the cutter radius compensation is selected with G41/G42, the approach behavior (NORM or KONT) determines the
compensation movement if the present actual position is behind the contour. With KONT, a circle is drawn with the cutter
radius around the programmed initial point (= end point of the approach block). The tangent that passes through the current
actual position and does not violate the contour is the approach movement.
If the start point is within the compensation circle around the target point, no tangent passes through this point.
Reaction: Correction block is reorganized.
Local alarm reaction.
Interface signals are set.
Alarm display.
NC Stop on alarm at block end.
Remedy: Place selection of the CRC such that the starting point of the approach movements comes to rest outside of the correction
circle around the target point (programmed traversing movements > compensation radius). The following possibilities are
available:
Selection in the previous block
Insert intermediate block
Select approach behavior NORM
Programm Clear alarm with NC START or RESET key and continue the program.
continuation:
10756 [Channel %1: ] Block %2 deselection of the tool radius compensation via KONT not possible at
the programmed end point
Parameters: %1 = Channel number
%2 = Block number, label
Explanation: On deselection of the cutter radius compensation, the programmed end point is within the compensation circle. If this point
were in fact to be approached without compensation, there would be a contour violation.
If the cutter radius compensation is deselected via G40, the approach behavior (NORM or KONT) determines the
compensation movement if the programmed end point is behind the contour. With KONT, a circle is drawn with the cutter
radius about the last point at which the compensation is still active. The tangent passing through the programmed end
position and not violating the contour is the retraction movement.
If the start point is within the compensation circle around the target point, no tangent passes through this point.
Diagnostics Manual
Diagnostics Manual, 06/2015, 6FC5398-6DP10-0BA2
SINUMERIK 808D ADVANCED alarms
5.2 NCK alarms
117