Hey Dave,
noting and restoring the offsets makes only sense if you let the workpiece clamped on the machine bed until the next pass. If you reposition it, you would re-probe instead.
Let’s say you have a workpiece clamped on the machine bed and prior to first pass, you probe XYZ. The result is that you have the offset numbers which in fact designate the workpiece zero in relation to the absolute machine zero.
-
If you let the machine on until next pass, you avoid homing and you can directly run the next pass, as these values did not change.
-
But if you switch the machine off or have a power outage, you got to re-enter these offsets before you can run the same program (or a pass that is based on the same program and workpiece) again.
There are two possibilities:
-
One is if you didn’t change the carriages, i.e. the program was pausing when the power outage or the shutdown occured, so in this case you don’t re-home, and not only enter the offsets but also tell the machine where its carriages are (=the positions in absolute machine coordinates. I described this case here yesterday.
-
Or the more simpler case, you home the machine after bootup and need only to enter the offsets, which in fact means to set the workpiece zero to its previous values (that were lost on power loss).
-
To enter these values, you use the G92 command and you enter it into the command entry field of the MDI Tab, but with their sign changed (i.e. the Additive Inverse):
Let’s say according to your image, your offsets for the workpiece were X=117.702, Y=129.392 and Z=-57.41. You re-home the machine, then you enter this into the command entry field of the MDI Tab:
G92 X-117.702 Y-129.392 Z57.41
Take care of the signs in front of the numbers, which were changed!
This command activates a new coordinate system, which is the workpiece coordinate system, which has its zero exactly where the workpiece zero is in your 3D model.
You can check whether a G92 offset is active by entering:
(debug, Offset=#5210)
If the output is 1, then there is a G92 offset active, if it is 0, not. (Don’t forget the parantheses when you use ‘debug’.)
Now to go to the workpiece zero, you enter:
G0 X0 Y0 Z0
Magic, eh? 
To delete any offset, use
G92.1
PS: If you forgot to note the offsets and they were lost due to a power outage, they can be extracted at any time later from the file /var/log/bbctrl.log.