Remedy:
Please inform the authorized personnel/service department. Check the part program and, if possible, modify the
programming so that inside corners with smaller paths than the correction value are avoided. (Outside corners are not
critical because the equidistants are lengthened or intermediate blocks are inserted, so that there is always a point of
intersection).
Increase the number of reviewed traversing blocks via machine data MD20240
$MC_CUTCOM_MAXNUM_CHECK_BLOCKS (default: 3), this increases the amount of calculation and consequently also
the block cycle time.
Programm
continuation:
Clear alarm with NC START or RESET key and continue the program.
10752
[Channel %1: ] Block %2 overflow of local block buffer with tool radius compensation
Parameters:
%1 = Channel number
%2 = Block number, label
Explanation:
The cutter radius compensation must buffer a variable number of intermediate blocks in order to enable calculation of the
equidistant tool path for each NC block. The size of the buffer cannot be determined by simple means. It depends on the
number of blocks without traversing information in the compensation plane, the number of contour elements to be inserted
and the shape of the curvature in spline and polynomial interpolation.
The size of the buffer is fixed by the system and cannot be changed via the MDs.
Reaction:
Correction block is reorganized.
Local alarm reaction.
Interface signals are set.
Alarm display.
NC Stop on alarm at block end.
Remedy:
Please inform the authorized personnel/service department.
Reduce the size of the buffer that has been assigned by modifying the NC program.
- By avoiding:
- Blocks without traversing information in the compensation plane
- Blocks with contour elements having a variable curvature (e.g. ellipses) and with curvature radii that are smaller than the
compensation radius. (Such blocks are divided up into several subblocks).
- Reduce the number of reviewed blocks for collision monitoring (MD20240
$MC_CUTCOM_MAXNUM_CHECK_BLOCKS).
Programm
continuation:
Clear alarm with NC START or RESET key and continue the program.
10753
[Channel %1: ] Block %2 selection of the tool radius compensation only possible in linear block
Parameters:
%1 = Channel number
%2 = Block number, label
Explanation:
Selection of tool radius compensation with G41/G42 may only be performed in blocks where the G function G00 (rapid
traverse) or G01 (feed) is active.
In the block with G41/G42, 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 selecting 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
continuation:
Clear alarm with NC START or RESET key and continue the program.
10754
[Channel %1: ] Block %2 deselection of the tool radius compensation only possible in linear block
Parameters:
%1 = Channel number
%2 = Block number, label
SINUMERIK 808D ADVANCED alarms
5.2 NCK alarms
Diagnostics Manual
116
Diagnostics Manual, 06/2015, 6FC5398-6DP10-0BA2
