Just want to expand further on Aiph5u’s response:
There are a total of 7 “Offsets” with the BuildBotics controller. In GCode, these are referenced as G53-G59. However, G53 is used by the machine as its “Absolute” or “Home” position which is automatically set ever time you power on and “Home” the machine.
Every time you use the electronic probe, or jog the spindle to a position and click the manual buttons to set a particular axis to zero, behind the scenes you are effectively setting work offset number G54.
To utilize additional offsets G55-G59, you will have to do this manually in GCode, including to make sure your CAM software (e.g. VCarve) is properly configured to send the G55-G59 commands as needed. Note, I have never found the need to use these additional offsets.
When recently making a number of jewelry boxes spanning a time frame across a number of days and machine restarts, I used the bench dogs on the bed of my machine to reference a known position for the lower-left corner of the workpiece. Then, after shutdown, startup, and homing the machine, I manually moved to these known coordinates using a GCode command (below) inside the “MDI” tab of the web interface.
Exact steps include:
- Power on and “Home” the machine
- Send this command: G90 G0 G53 X280.564 Y260.267
- Click the buttons in the web interface to set my zero point (i.e. G54 work offset) for X and Y
- Set my Z zero position using the electronic probe
- Load and run any GCode program I uploaded
- Clicking the Home “BUTTON” on the web interface will move to these coordinates and not the machine’s home position
Breaking down the GCode command:
G90: Sets the movement relative to Absolute coordinates of whatever offset you’re referencing and not based incrementally from wherever the spindle is currently located on the bed
G0: Indicates rapid movement or a non-cutting operation.
G53: Instructs the machine to move to a position based on the Absolute offset where the machine was homed.
X280.564 and Y260.267: The specific X and Y coordinates of my bench dogs
After clicking the buttons to set my X-Y zero points, then jogging the machine with the X-Box controller or issuing any GCode command will move the spindle relative to this G54 work offset by default.
If after you configure your work offset (G54) and you want to move the spindle to a position relative to this offset, and not the machine’s Home position, make sure to include G54 instead of G53. Example, if your workpiece is 600x600mm, you set your zero point to the lower-left corner, and you want to move to the center (300x300), issue G90 G0 G54 X300 Y300. Granted, you technically don’t need to use G54 as it should be assumed, but I like to make sure.
Conversely, if your carving finishes and you want to move the spindle all the way up and out of the way to the back-right corner of the machine (Woodworker model with max 800-ish mm square bed), issue this command:
G90 G0 G53 Z5 X800 Y800
Your work offset G54 will still exist and I specified Z5 just to leave a little room at the top.