Siemens SINUMERIK 840D sl Function Manual page 580

TE4: Transformation package handling
13.6 Tool orientation
GCODE_RESET_VALUES [24] = 1 → ORIWKS is initial setting
GCODE_RESET_VALUES [24] = 2 → ORIMKS is initial setting
GCODE_RESET_VALUES [24] = 3 → ORIPATH
When ORIPATH is active, the orientation is calculated from the lead and side angles relative
to the path tangent and surface normal vector.
Improper tool orientation
If the tool orientation is programmed in conjunction with the following functions
• G04 Dwell time
• G33 Thread cutting with constant lead
• G74 Approach reference point
• G75 Approach fixed point
• REPOSL Repositioning
• REPOSQ Repositioning
• REPOSH Repositioning
Alarm 12130 "Illegal tool orientation" is output when Euler angles and direction vectors are
selected. The NC program stops (this alarm can also occur in connection with G331, G332
and G63). Alarm 17630 or 17620 is output for G74 and G75 if a transformation is active and
the axes to be traversed are involved in the transformation. This applies irrespective of
orientation programming.
If the start and end vectors are inverse parallel when ORIWKS is active, then no unique plane
is defined for the orientation programming, resulting in the output of alarm 14120.
Alarm 14400 is output if the transformation is switched on or off when a tool offset is active.
In the reverse situation, i.e. a tool offset is selected or deselected when a transformation is
active, no alarm message is output.
Multiple input of tool orientation
According to DIN 66025, only one tool orientation may be programmed in a block, e.g. with
direction vectors:
N50 A3=1 B3=0 C3=0
If the tool orientation is input several times, e.g. with direction vectors and Euler angles:
N60 A3=1 B3=1 C3=1 A2=0 B2=1 C2=3
error message 12240 "Channel X block Y tool orientation xx defined more than once" is
displayed and the NC part program stops.
580
Function Manual, 09/2011, 6FC5397-2BP40-2BA0
Special Functions