First, I am not exactly,- or to be precise, not at all - clear on what Micro is trying to say, but will take up the challenge of understanding it later tonight
after a few glasses of Hofbrau.
In the meantime however...
Your machine is a Haas ST lathe.
That machine is at home when all axes are at their max travel distance ( upper right corner of the envelope ), and this location is called Machine Zero, and it is
also the G53 coordinate system.
Whatever way you send the machine home, let it be G28 or G00 G53 X0 Y0, it will always travel to this exact location.
Now, the tool offsets.
When you install a new tool, you have to tell the machine what it is and where ( how long ) it is. Regardless how you pick up your tool "locations", it is always referenced
in the machine (G53) coordinate system.
Unfortunately, Haas engineers can be dumber than a freshly cut stump sometimes, and their tool pickup is one of those when it comes to the Z offset.
Let's take the X coordinates first as that one is OK.
After installing the tool, you can:
A: Jog to the toolsetter, and touch the probe. The machine now will read the current G53 X coordinate and adds it to the toolsetter offset value. This number is a pre-determined value
stored in parameters and is specific, calibrated to each machine. The resulted sum is then entered into the tool's X offset register.
What this value represents is the actual total distance required from machine home ( G53 ) to put the tool's tip to the center of rotation, or X0.
B: Without a toolsetter, you jog to a part and make a skim cut. Then, without moving in X you measure the diameter, hit "X Dia Mesur", enter the measured value and hit Enter.
The machine will now read the current G53 X coordinate, and then adds the diameter you've entered.
The resulting sum will once again represent the distance ( travel) required from machine home to put the given tool's tip to X0.
Now to the Z coordinates, and this is where Haas gets stupid.
First, assume the toolsetter is installed, so setting: "T Offs. Measure Uses Work" is set to OFF
Easy-peasy, you touch the setter's Z face, machine reads the G53 Z coordinate and enters it into the appropriate offset register.
Without toolsetter, you can still do the exact same thing. Leave the above parameter OFF, take your tool and touch off to a known, permanent fixed
reference. This can be anything of your choosing, gage block on the chuck face is common. When the tip is in contact with this reference block, hit "Z face mesur"
on the control, machine reads the G53 Z coordinate, enters it into the offset register and done.
In both cases the value in the tool's Z offset register represent the distance of travel required to get from machine home to either the tool setter OR the fixed reference block.
Lastly, without the toolsetter you can also set the "T Offs. Measure Uses Work" to ON.
This DOES NOT work with a toolsetter installed!!
Instead, it is used when ( such in my case ) the chuck is often replaced with a 2 jaw chuck or a collet chuck or a faceplate or ...
In any of those cases you would loose the fixed reference point, and all your tools would have to be re-picked again in Z
But, with this setting ON, you can take a KNOWN tool, ANY KNOWN tool ( nut just Nr1 or Master tool or Boss tool ) but ANY of the already picked up tools, clean the
face of your part and hit "Z Offs. Mesur" in the G54 work offset.
After this you can just take a newly installed tool, jog to this freshly cut face, touch it and hit the same "Z Offs. Mesur" but this time for the Tool's Z offset value.
In this case the machine will read the actual G53 Z position, adds it to the Z value in the G54 work offset and the result is entered for the tool Z.
This ensures that all tools will be referenced to the very same length.
May sound a bit confusing the way I wrote it, but that is the best I can do.
So, basically the answer to the OP's question is that in the case of a Haas lathe, the offset value represents the distance from machine zero ( or machine home ) to the
center of spindle rotation for X, and either the toolsetter OR the fixed reference in Z, OR ... in case of the last possibility, to the "imaginary" fixed reference.
