Workpiece Coordinate System (G92); Resetting The Tool Coordinate System (G92.1); Selection Of A Workpiece Coordinate System (G54 To G59) - Siemens SINUMERIK 808D Programming And Operating Manual

Selection of machine coordinate system (G53)
G53 suppresses the programmable and adjustable work offset. Traversing in the machine coordinate system on the basis of
G53 are always programmed if the tool is to traverse to a machine-specific position.
Compensation deselection
If MD10760 $MN_G53_TOOLCORR = 0, then the active tool length and tool radius compensation remains active in a block
with G53
If MD10760 $MN_G53_TOOLCORR = 1, then the active tool length and tool radius compensations in a block are
suppressed with G53.
4.3.1.2

Workpiece coordinate system (G92)

Before machining, you must create a coordinate system for the workpiece, the so-called work piece coordinate system. This
section describes different methods of setting, selecting and changing a workpiece coordinate system.
Setting a tool coordinate system
The following two methods can be used to set a tool coordinate system:
● With G92 in the part program
● manually through the HMI operator panel
Format
(G90) G92 X... Y... Z... ;
The base point traverses to the specified position on outputting an absolute command. The difference between tool tips and
the base point is compensated through the tool length compensation; this way the tool tip can traverse to the target position
in any case.
4.3.1.3

Resetting the tool coordinate system (G92.1)

With G92.1, one can reset a shifted coordinate system before the shift. The tool coordinate system is reset to the coordinate
system that is defined by the active adjustable work offsets (G54-G59). The tool coordinate system is set to the reference
position if no adjustable work offset is active. G92.1 resets shifts carried out through G92 or G52. However, only the axes
that are programmed, are reset.
Example 1:
N10 G0 X100 Y100
N20 G92 X10 Y10
N30 G0 X50 Y50
N40 G92.1 X0 Y0
Example 2:
N10 G10 L2 P1 X10 Y10
N20 G0 X100 Y100
N30 G54 X100 Y100
N40 G92 X50 Y50
N50 G0 X100 Y100
N60 G92.1 X0 Y0
4.3.1.4

Selection of a workpiece coordinate system (G54 to G59)

As mentioned above, you can select one of the already set workpiece coordinate systems.
● G92
Absolute commands function in connection with a workpiece coordinate system only if a workpiece coordinate system
was selected earlier.
● Selection of a workpiece coordinate system from a selection of specified workpiece coordinate systems via the HMI
operator panel
A workpiece coordinate system can be selected by specifying a G function in the area G54 to G59.
Workpiece coordinate systems are setup after the reference point approach after Power On. The closed position of the
coordinate system is set in MD20154[13].
Programming and Operating Manual (ISO Turning/Milling)
01/2017
;Display: WCS: X100 Y100
;Display: WCS: X10 Y10
;Display: WCS: X50 Y50
;Display: WCS: X140 Y140
;Display: WCS: X100 Y100
;Display: WCS: X100 Y100
;Display: WCS: X50 Y50
;Display: WCS: X100 Y100
;Display: WCS: X150 Y150
MCS: X100 Y100
MCS: X100 Y100
MCS: X140 Y140
MCS: X140 Y140
MCS: X100 Y100
MCS: X110 Y110
MCS: X110 Y110
MCS: X160 Y160
MCS: X160 Y160
101