how to change 'zero' position

More
11 Aug 2021 20:50 #217570 by dansawyer
This is a general quesiton about changing the 'zero' position during program operation. The machine is a Bridgeport BOSS converted to Linuxcnc. (the result is very impressive, thant you all for your efforts and your support.)
I am manually writing gcode. I am not using any CAD/CAM software. I am simply using a text editor to create and manage program codes.
My first project was circle based. I simply centered the part on the spindle, turned the power on and proceeded. The part and the coordinate system were aligned.
My second project is to machine a rectangular part from blanks. I will afix the part and determine the edges. Once that is complete the program will locate the spindle to the 'center'. At this time I would like to reset the coordinate system.
How can this be done? I believe this can be done using g5x codes. Is this the best way? Is it the only way?
Thank you in advance, Dan

Please Log in or Create an account to join the conversation.

More
11 Aug 2021 21:23 #217573 by MaHa
Replied by MaHa on topic how to change 'zero' position
To set offset for G54 from machine origin to X233.5 Y47
G10 L2 P1 X233.5 Y47

or

To set offset for G55 from actual position to X233.5 Y47
G10 L20 P2 X233.5 Y47

To set actual position ,G54 to zero
G10 L20 P1 X0 Y0

To set G54 X0 Y0 to machine origin, moves are then the same as G53 used,
G10 L2 P1 X0 Y0

I am shure there is a section in the documentation about G10 L2 and G10 L20

Please Log in or Create an account to join the conversation.

More
15 Aug 2021 14:24 #217814 by andypugh
The GUIs all have a "touch off" button that allows you to change where the current part origin is.

This basically generates a G10 instruction in the background, but is probably more convenient than MDI.

Please Log in or Create an account to join the conversation.

More
21 Aug 2021 04:47 - 22 Aug 2021 22:26 #218307 by dansawyer
Thank you. This is a very helpful start. The machine is a Bridgeport BOSS. The project is to create a part program with the blank in an unknown position.
When I start the machine it starts in position x0 y0. When I zero of the part edges the x pos becomes v1 and y becomes v2. Will the following command set the operational offset to x0 y0?
G10 L20 P1 X0 Y0
I sort of understand the G10 command. I don't understand the fuction of L20 and P1 in this example.
(Follow up: I restarted Linuxcnc with the blank in the jig. I then cleared E-Stop and enabled machine power. This allowed positioning the table to zero - zero on the blank in the jig. I then 'homed' the axis. This cleared the x and y offsets. Is this an alternative? )
Last edit: 22 Aug 2021 22:26 by dansawyer. Reason: miss spelled word

Please Log in or Create an account to join the conversation.

More
26 Aug 2021 21:59 #218828 by andypugh
Sorry, I have been rather busy with a broken fire-engine....

In a G10 the L-word defines whether the offset goes into the coordinate system or into the tool table, and whether it is an absolute or a relative offset. ie, if you are saying "put this value in the offset table" or "set the offset table so that the current position is these numbers"

The P-word defines which coordinate system (LinuxCNC supports 9 sets of work offsets) or tool offset (LinuxCNC supports up to 1000 tools)

Please Log in or Create an account to join the conversation.

More
28 Aug 2021 03:26 #218962 by rschires
Sounds like you are trying to do the same thing I have been doing. Changing from the machines x0 y0 to a work piece x0 y0. I use G10 L2 P0 with the xy coordinates for the work piece x0 y0. To establish z0, I touch off each tool and record the number. An example would be G10 L2 P0 X3 Y2 Z-1.5
To change tools,
G53 G00 Z0
M9
G53 G00 X0 Y0
M0
(Press S to continue)
G10 L2 P0 X3 Y2 Z-1.6
G00 X Y start position
M8
G00 Z0

I use M8 M9 because the typical M code s to turn the spindle on/off don't work. Turns the spindle on but not off.
Anyway, this is how I handle my offsets.

Please Log in or Create an account to join the conversation.

Time to create page: 0.112 seconds
Powered by Kunena Forum