Coordinate Systems

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.

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

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.

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.

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:

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.

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.

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.

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.

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:

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.

G52 and G92 share the same offset registers. Unless G92 persistence is disabled in the .ini file (see 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 G92 Persistence Cautions above.

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.

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

We put these together in the following program:

Now comes the time when we might apply a set of G92 offsets to this program. You’ll see that it is running in each case at Z0. If the mill were at the zero position, a G92 Z1.0000 issued at the head of the program would shift everything an inch. You might also shift the whole pattern around in the XY plane by adding some X and Y offsets with G92. If you do this you should add a G92.1 command just before the M2 that ends the program. If you do not, other programs that you might run after this one will also use that G92 offset. Furthermore it would save the G92 values when you shut down the LinuxCNC and they will be recalled when you start up again.

(To be written)