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

04.07
2.2.2

Reference point return check (G27)

Format
G27 X... Y... 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⋅⋅⋅Y⋅⋅⋅Z⋅⋅⋅;".
In the G27 mode, the function checks whether or not the axes positioned by the
execution of these commands in the simultaneous 3-axis (* 5-axis) control mode
are located at the reference point. For the axes not specified in this block, and not
moved although the axis command specified, positioning and check are not execu-
ted.
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 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 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 and tool length offset functions are not
canceled by the G27 command.
S Check is not made if G27 is executed while the machine lock state is valid even
for one axis. For example, if an X-axis movement command is specified in the
G27 block while in the Z-axis neglect state, X-axis position is not checked.
S The mirror image function is valid to the direction of axis movement in the refer-
ence point return operation called by G27. To avoid a position unmatch error,
the mirror image function should be canceled before executing G27.
© Siemens AG 2007 All rights reserved
SINUMERIK 802D sl/840D/840D sl/840Di/840Di sl/810D ISO Milling (PGM) -- 04.07 Edition
Commands Calling Axis Movements
2.2 Reference point return
2-37