Keeping zero position

[Aiph5u (Aiph5u (not affiliated with Onefinity))]

Hey Festdewalkita,

@Festdewalkita

1F non-Masso controllers use Buildbotics, which is based on LinuxCNC.

Buildbotics is not based on LinuxCNC, as Buildbotics is the own work of its creator, but its g-code syntax is patterned after the LinuxCNC g-code syntax

@Festdewalkita

I cannot find G02 documentation anywhere on that website, and don’t know if the interpreter would equate that with G2 (which has completely different functionality).

G2 (Clockwise Arc Move) is identical to G02, just as M3 is identical to M03.

@Festdewalkita

I’m wondering if I can manipulate my J-man’s workable area via G28.1. To be more specific, I’m contemplating a doghole-with-metal-dog-combination centered at (96, 96) to tell my machine where its workable area is via the G28.1 MDI command.

The numbered parameters #5161 – #5169 store the machine coordinates of the home position for the axes X, Y, Z, A, B, C, U, V & W, therefore after homing, G28 moves to machine origin (aka ‘home’)

G28.1 sets these parameters to the values of the current position, but the position is in absolute machine coordinates.

You can check the values at any time with the g-code command:

M0 (debug, G28 settings: X=#5161, Y=#5162, Z=#5163)

I don’t know if you rather are interested in the G52 and G92 commands. After probing your workpiece in XYZ, the G92 command sets the new workpiece zero as the X,Y,Z zero position of the workpiece coordinate system. Any subsequent G0, G1, G2 and G3 motion commands will then take the workpiece zero as coordinate system zero. E.g. G0 X0 Y0 Z0 will then move to the workpiece zero. You can still move to machine zero (‘home’) with G53 G0 X0 Y0 Z0 when a workpiece coordinate system is in effect.

The G52 command is useful if you have multiple identical pieces to be milled at different positions.