Siemens Sinumerik 840D sl Diagnostic Manual page 106

Overview of Alarms
NCK alarms
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 out-
side of the correction circle around the target point (programmed traversing movements > compensa-
tion radius). The following possibilities are available:
Selection in the previous block
Insert intermediate block
Select approach behavior NORM
Program Con- Clear alarm with NC START or RESET key and continue the program.
tinuation:
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
Definitions: On deselection of the cutter radius compensation, the programmed end point is within the compensa-
tion 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.
Reaction: Correction block is reorganized.
Local alarm reaction.
Interface signals are set.
Alarm display.
NC Stop on alarm at block end.
Remedy: Place deselection of the CRC such that the programmed end point comes to rest outside the compen-
sation circle around the last active compensation point. The following possibilities are available:
Deselection in the next block
Insert intermediate block
Select retract behavior NORM
Program Con- Clear alarm with NC START or RESET key and continue the program.
tinuation:
10757 [Channel %1: ] Block %2 changing the compensation plane while tool
radius compensation is active not possible
Parameters: %1 = Channel number
%2 = Block number, label
Definitions: In order to change the compensation plane (G17, G18 or G19) it is first necessary to deselect the cut-
ter radius compensation with G40.
Reaction: Correction block is reorganized.
Local alarm reaction.
Interface signals are set.
Alarm display.
NC Stop on alarm at block end.
Remedy: Insert an intermediate block in the part program using the correction deselection. After the plane
change, the cutter radius compensation is to be selected in an approach block with linear interpolation.
Program Con- Clear alarm with NC START or RESET key and continue the program.
tinuation:
2-106
SINUMERIK 840D sl, 840Di sl, SINAMICS, Diagnostics Manual (DAsl), 03/2009
© Siemens AG, 2009. All Rights Reserved
03/2009