Sistemas de coordenadas

Independientemente de cualquier offset que pudiera estar activo, un G53 en una línea de código indica al intérprete moverse a las posiciones reales de los ejes (posiciones absolutas) especificadas. Por ejemplo:

moverá de la posición actual a la posición donde las coordenadas de máquina de los tres ejes sean cero. Puedes usar este comando si tienes una posición fija para el cambio de herramienta o si tu máquina tiene un cambiador automático de herramienta. También puedes usar este comando para despejar el área de trabajo y acceder a la pieza de trabajo en la mordaza.

G53 es un comando no modal. Debe usarse en cada bloque en el que se desee un movimiento en el sistema coordenado de la máquina.

Otra variable en el archivo VAR se vuelve importante cuando pensamos en sistemas de offsets. Esta variable es la 5220. En los archivos predeterminados, su valor se establece en 1.00000. Esto significa que cuando LinuxCNC se inicia, debería usar el primer sistema de coordenadas como el predeterminado. Si se configura a 9.00000 usaría el noveno sistema de offsets como predeterminado al iniciar o reiniciar. Cualquier valor que no sea un entero (decimal realmente) entre 1 y 9, o si falta la variable 5220 hará que LinuxCNC vuelva al valor predeterminado de 1.00000 al inicio.

El comando G10 L2x se puede usar para establecer los offsets de sistema de coordenadas:

G52 se usa en un programa de pieza como un "offset del sistema de coordenadas local" temporal dentro del sistema de coordenadas de la pieza de trabajo. Un ejemplo de caso de uso es cuando se mecanizan varias características idénticas en diferentes ubicaciones de una pieza. Para cada una, G52 programa un punto de referencia local dentro de las coordenadas de pieza, y se llama a un subprograma para maquinar la característica relativa a ese punto.

Los offsets de ejes G52 se programan relativos a las coordenadas de offset de la pieza de trabajo G54 a G59.3. Como un offset local, G52 se aplica después del offset de la pieza de trabajo, incluida la rotación. Por lo tanto, una característica parcial será mecanizada de forma idéntica en cada parte, independientemente de la orientación de la parte en el palet.

La programación de G52 X1 Y2 da offsets al sistema de coordenadas actual de la pieza de trabajo, 1 para eje X y 2 para eje Y. Por consiguiente, en el DRO las coordenadas X e Y de la posición actual de la herramienta se reducirán en 1 y 2, respectivamente. Los ejes sin establecer en el comando, como Z en el ejemplo anterior, no se verán afectados: cualquier offset Z G52 previo permanecerá vigente, y en caso de haberlo, el offset Z será cero.

El offset local temporal puede cancelarse con G52 X0 Y0. Cualquier eje no puesto a cero explícitamente retendrá el offset anterior.

G52 comparte los mismos registros que G92, por lo que G52 es visible en el DRO y vista previa, etiquetado como 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.

There are at least two ways to set G92 values:

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.

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.

Podemos emitir un conjunto de comandos para crear offsets para los otros cuatro círculos, como esto.

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)