I was typing this a bit behind Hu but I decided to post it anyway.
Originally Posted by CNCRob Does that mean that G54 would take the place of G53 and you would have to use another G offset to offset the work. Something like G92. Or how does that work. |
Which one; G54, G53 or G92? You have a bit of an open ended question. G54 and G53 are fairly straightforward. G92 is mentioned right at the bottom.
All the following is only applicable when running in absolute mode, G90.
G53 is the machine coordinate system which measures everything from machine zero, also called home. It is not convenient to always specify coordinate locations relative to the machine so work coordinates, or work offsets are used, so that locations can be specified relative to a point on the workpiece. Depending on the machine and controller many work offsets are available numbered G54 thru G59 for the first six.
G54 on most machines is the default work offset so in the absence of any other work offset commands when a motion is commanded the machine moves to the commanded location using as its reference point the values entered into the G54 work offset table. Internally what the machine is doing is adding the G54 values to the machine coordinates and then adding the coordinates for the commanded location to these.
To use another work offset, not G54, simply command the one wanted; G55, G56, etc. The controller will now use the values in the table for this work offset and will continue to do so until another work offset is commanded, or M30 or RESET.
A motion command including G53 in the block will move to the commanded location using only the machine coordinate system. What G53 tells the controller is 'don't use any work offset values for this move".
G53 is only effective in the block in which it appears and if it is not present in the next block in a program the controller reverts to using whatever is the current work offset.
G92 is a different kettle of fish. It is not really a work offset but a means to change other work offsets. Exactly what it does is (not) obvious from this explanation: "A G92 command effectively shifts all work coordinate systems (G54-59) so that the command position becomes the current position in the active work system".
As Hu suggests don't use it. I read an explanation that G92 was created to make many work offsets available back in the dark ages when memory capacity was limited and the machines read code incised into clay tablets.
Regarding your comment about the G401 file that, I think, is more related to tool offsets than work offsets.