Coordinate Systems

G55 ; use coordinate system 2
G0 X0 Y0 Z0
G1 F2 Z-0.2000
X1
Y1
X0
Y0
G0 Z0
G54 ; use coordinate system 1
G0 X0 Y0 Z0
M2

(((G54)))(((G55)))(((G56)))(((G57)))(((G58)))(((G59)))(((G59.1)))(((G59.2)))(((G59.3)))G54      uses parameters of coordinate system 1G55       uses parameters of coordinate system 2G56       uses parameters of coordinate system 3G57       uses parameters of coordinate system 4G58       uses parameters of coordinate system 5G59       uses parameters of coordinate system 6G59.1     uses parameters of coordinate system 7G59.2     uses parameters of coordinate system 8G59.3     uses parameters of coordinate system 9----

=== Default Coordinate System

One other variable in the VAR file becomes important when we think about offset systems. This variable is named 5220. In the default files its value is set to 1.00000. This means that when the LinuxCNC starts up it should use the first coordinate system as its default. If you set this to 9.00000 it would use the ninth offset system as its default for start up and reset. Any value other than an integer (decimal really) between 1 and 9, or a missing 5220 variable will cause the LinuxCNC to revert to the default value of 1.00000 on start up.

=== Setting Coordinate System Offsets

The G10 L2x command can be used to set coordinate system offsets:

* 'G10 L2 P(1-9)' - Set offset(s) to a value. Current position irrelevant (see <<gcode:g10-l2,G10 L2>> for details).
* 'G10 L20 P(1-9)' - Set offset(s) so current position becomes a value (see <<gcode:g10-l20,G10 L20>> for details).

[NOTE]
We only give a brief overview here, refer to the G-code sections for a full description.

[[sec:g52-and-g92-offsets]]
== Local and Global Offsets

[[sec:g52]]
=== The G52 command

'G52' is used in a part program as a temporary "local coordinate system offset" within the workpiece coordinate system. An example use case is when machining several identical features at different locations on a part. For each feature, 'G52' programs a local reference point within workpiece coordinates, and a subprogram is called to machine the feature relative to that point.

'G52' axis offsets are programmed relative to workpiece coordinate offsets 'G54' through 'G59.3'. As a local offset, 'G52' is applied after the workpiece offset, including rotation. Thus, a part feature will be machined identically on each part regardless of the part's orientation on the pallet.

[CAUTION]
As a temporary offset, set and unset within the localized scope of a part program, in other G-code interpreters 'G52' does not persist after machine reset, 'M02' or 'M30'. In LinuxCNC, 'G52' shares parameters with 'G92', which, for historical reasons, *does* persist these parameters. See <<sec:g92-persistence-cautions,G92 Persistence Cautions>> below.

[CAUTION]
'G52' and 'G92' share the same offset registers. Therefore, setting 'G52' will override any earlier 'G92' setting, and 'G52' will persist across machine reset when 'G92' persistence is enabled. These interactions may result in unexpected offsets. See <<sec:g92-g52-interaction-cautions,G92 and G52 Interaction Cautions>> below.

Programming 'G52 X1 Y2' offsets the current workpiece coordinate system X axis by 1 and Y axis by 2. Accordingly, on the DRO, the current tool position's X and Y coordinates will be reduced by 1 and 2, respectively. Axes unset in the command, such as Z in the previous example, will be unaffected: any previous 'G52' Z offset will remain in effect, and otherwise the Z offset will be zero.

The temporary local offset may be canceled with 'G52 X0 Y0'. Any axes not explicitly zeroed will retain the previous offset.

'G52' shares the same offset registers as 'G92', and thus 'G52' is visible on the DRO and preview labeled with 'G92'.

[[sec:g92-axes-offsets]]
== G92 Axes Offsets

G92 is the most misunderstood and cleverest command programmable with LinuxCNC. The way it works has changed a bit between the first versions and the current one. These changes have doubt baffled many users. They should be seen as a command producing a temporary offset, which applies to all the other offsets.

[[sec:g92-commands]]
=== The G92 commands

'G92' is typically used in two conceptually different ways: as a "global coordinate system offset" or as a "local coordinate system offset".

The 'G92' set of commands includes:

* 'G92' - This command, when used with axis names, sets values to offset variables.
* 'G92.1' - This command sets zero values to the G92 variables.
* 'G92.2' - This command suspends but does not zero out the G92 variables.
* 'G92.3' - This command applies offset values that have been suspended.

As a global offset, 'G92' is used to shift all workpiece coordinate systems 'G54' through 'G59.3'. An example use case is when machining several identical parts in fixtures with known locations on a pallet, but the pallet location may change between runs or between machines. Each fixture location offset, relative to a reference point on the pallet, is preset in one of the workpiece coordinate systems, 'G54' through 'G59.3', and 'G92' is used to "touch off" on the pallet reference point. Then, for each part, the corresponding workpiece coordinate system is selected and the part program is executed.

[NOTE]
'G10 R-' workpiece coordinate system rotation is specific to the 'rs274ngc' interpreter, and the 'G92' offset is applied 'after' rotation. When using 'G92' as a global offset, workpiece coordinate system rotations may have unexpected results.

As a local coordinate system, 'G92' is used as a temporary offset within the workpiece coordinate system. An example use case is when machining a part with several identical features at different locations. For each feature, 'G92' is used to set a local reference point, and a subprogram is called to machine the feature starting at that point.

[NOTE]
The use of 'G92' is discouraged for programming with local coordinate systems in a part program. Instead, see <<sec:g52,'G52'>>, a local coordinate system offset more intuitive when desired offset relative to the workpiece is known but current tool location may not be known.

Programming 'G92 X0 Y0 Z0' sets the current tool location to the coordinates X0, Y0, and Z0, without motion. G92 *does not* work from absolute machine coordinates. It works from *current location*.

'G92' also works from current location as modified by any other offsets that are in effect when the 'G92' command is invoked. While testing for differences between work offsets and actual offsets it was found that a 'G54' offset could cancel out a 'G92' and thus give the appearance that no offsets were in effect. However, the 'G92' was still in effect for all coordinates and did produce expected work offsets for the other coordinate systems.

By default, 'G92' offsets are restored after the machine is started. Programmers that wish for Fanuc behavior, where 'G92' offsets are cleared at machine start and after a reset or program end, may disable 'G92' persistence by setting 'DISABLE_G92_PERSISTENCE = 1' in the '[RS274NGC]' section of the INI file.

[NOTE]
It is good practice to clear the 'G92' offsets at the end of their use with 'G92.1' or 'G92.2'. When starting up LinuxCNC with 'G92' persistence enabled (the default), any offsets in the 'G92' variables will be applied when an axis is homed. See <<sec:g92-persistence-cautions,G92 Persistence Cautions>> below.

=== Setting G92 Values

There are at least two ways to set G92 values:

* With a right click on the position displays in tklinuxcnc, a window opens where it is possible to enter a value.
* With the G92 command

Both work from the current position of the axis that should be moved.

Programming 'G92 X Y Z A B C U V W' sets the values of the G92 variables so that each axis takes the value associated with its name. Those values are assigned to the current position of the axes. These results satisfy to paragraphs one and two of the NIST document.

G92 commands work from current axis location and add and subtract correctly to give the current axis position the value assigned by the G92 command. The effects work even though previous offsets are in.

So if the X axis is currently showing 2.0000 as its position a 'G92 X0' will set an offset of -2.0000 so that the current location of X becomes zero. A 'G92 X2' will set an offset of 0.0000 and the displayed position will not change. A 'G92 X5.0000' will set an offset of 3.0000 so that the current displayed position becomes 5.0000.

[[sec:g92-persistence-cautions]]
=== G92 Persistence Cautions

By default, the values of a 'G92' offset will be saved in the VAR file and be restored after a machine reset or startup.

The G92 parameters are:

* 5210 - Enable/disable flag (1.0/0.0)
* 5211 - X Axis Offset
* 5212 - Y Axis Offset
* 5213 - Z Axis Offset
* 5214 - A Axis Offset
* 5215 - B Axis Offset
* 5216 - C Axis Offset
* 5217 - U Axis Offset
* 5218 - V Axis Offset
* 5219 - W Axis Offset

where 5210 is the 'G92' enable flag (1 for enabled, 0 for disabled) and 5211 to 5219 are the axis offsets. If you are seeing unexpected positions as the result of a commanded move, as a result of storing an offset in a previous program and not clearing them at the end then issue a G92.1 in the MDI window to clear the stored offsets.

If G92 values exist in the VAR file when LinuxCNC starts up, the G92 values in the var file will be applied to the values of the current location of each axis. If this is home position and home position is set as machine zero everything will be correct. Once home has been established using real machine switches, or by moving each axis to a known home position and issuing an axis home command, any G92 offsets will be applied. If you have a G92 X1 in effect when you home the X axis the DRO will read 'X: 1.000' instead of the expected 'X: 0.000' because the G92 was applied to the machine origin. If you issue a G92.1 and the DRO now reads all zeros then you had a G92 offset in effect when you last ran LinuxCNC.

Unless your intention is to use the same G92 offsets in the next program, the best practice is to issue a G92.1 at the end of any G code files where you use G92 offsets.

When a program is aborted during processing that has 'G92' offsets in effect a startup will cause them to become active again. As a safeguard, always have your preamble to set the environment as you expect it. Additionally, 'G92' persistence may be disabled by setting 'DISABLE_G92_PERSISTENCE = 1' in the '[RS274NGC]' section of the INI file.

[[sec:g92-g52-interaction-cautions]]
=== G92 and G52 Interaction Cautions

'G52' and 'G92' share the same offset registers. Unless 'G92' persistence is disabled in the INI file (see <<sec:g92-commands,G92 Commands>>), 'G52' offsets will also persist after machine reset, 'M02' or 'M30'. Beware that a 'G52' offset in effect during a program abort may result in unintended offsets when the next program is run. See <<sec:g92-persistence-cautions,G92 Persistence Cautions>> above.

== Sample Programs Using Offsets

=== Sample Program Using Workpiece Coordinate Offsets

This sample engraving project mills a set of four .1 radius circles in roughly a star shape around a center circle. We can setup the individual circle pattern like this.

[source, {ngc}]

We can issue a set of commands to create offsets for the four other circles like this.

[source, {ngc}]

We put these together in the following program:

[source, {ngc}]