Reference Point Return Check (G27) - Siemens Sinumerik 802D sl Programming Manual

04.07
2.3.2

Reference point return check (G27)

Format
G27 X... Z... ;
This function checks whether the axes are correctly returned to the reference point
at the completion of the part program which is created so that the program starts
and ends at the reference point in the machine by specifying the commands of
"G27 X(U)... Z(W)... (C(H)... Y(V)...);".
In the G27 mode, the function checks whether or not the axes positioned by the
execution of these commands in the simultaneous 2-axis control mode are located
at the reference point. For the axes not specified in this block, positioning and
check are not executed.
Operation after the check
When the position reached after the execution of the commands in the G27 block
agrees with the reference point, the reference point return complete lamp lights.
The automatic operation is continuously executed when all of the specified axes
are positioned at the reference point. If there is an axis that has not been returned
to the reference point, reference point return check error (alarm 61816, "axes not
reference") occurs and the automatic operation is interrupted.
Supplements to the reference point return check command and other operations
S If G27 is specified in the tool position offset mode, positioning is made at the
position displaced by the offset amount and the positioning point does not agree
with the reference point. It is necessary to cancel the tool offset mode before
specifying G27. Note that the tool position offset function is not canceled by the
G27 command.
S The reference point return check is not executed if G27 is executed in the
machine lock ON state.
© SIEMENS AG 2007 All rights reserved
SINUMERIK 802D sl/840D sl840D/840Di sl/840Di/810D ISO Turning -- 04.07 Edition
Commands Calling Axis Movements
2.3 Reference point return
2-49