Checking The Reference Position (G27); Reference Point Approach With Reference Point Selection (G30) - Siemens SINUMERIK 808D Programming And Operating Manual

Return to reference point - rotary axes:
Additions to the commands for automatic reference point approach:
Tool radius compensation and defined cycles
G28 should not be used in operation with tool radius compensation (G41, G42) or in a defined cycle!
Note
G28 is used to interrupt the tool radius compensation (G40) with eventual axis traverse movement to the reference point.
Hence, tool radius compensation is to be deactivated before G28 is issued.
Tool offset in G28
In G28, the interpolation point is approached with the current tool offset. The tool offset is deselected when the reference
point is finally approached.
4.2.2.2

Checking the reference position (G27)

Format
G27 X... Y... Z... ;
This function is used to check whether the axes are on their reference point.
Test procedure
If the check with G27 is successful, the processing is continued with the next part program block. If one of the axes
programmed with G27 is not on the reference point, Alarm 61816 "Axes not on reference point" is triggered and "AUTO"
mode is interrupted.
Note
Function G27 is implemented with the cycle 328.spf as with G28.
To avoid a positioning error, the function "mirroring" should be deselected before executing G27.
4.2.2.3

Reference point approach with reference point selection (G30)

Format
G30 Pn X... Y... Z... ;
For the commands "G30 Pn X... Y... Z;", the axes are positioned on the specified intermediate point in the continuous-path
mode, and finally traversed to the reference point selected with P2 - P4. With "G30 P3 X30. Y50.;", The X- and Y-axes return
to the third reference point. The second reference point is selected on omitting "P". Axes that are not programmed in a G30
block are also not traversed.
Reference point positions
The positions of all the reference points are always determined in relation to the first reference point. The distance of the first
reference point from all subsequent reference points is set in the following machine data:
Element
2. Reference point
3. Reference point
Programming and Operating Manual (ISO Turning/Milling)
01/2017
MD
$_MA_REFP_SET_POS[1]
$_MA_REFP_SET_POS[2]
99