G54 - general use and G54 operation question

I think am beginning to understand how G54 works.
This is a setup question. I have a part that had to be moved during machining. The program is setup to start the operation on a 'close to origen' point and then execute the program to machine the part. I am trying to reset the part at the origen. Let's say for arguement I can manually set that to within 15 thou on X and Y. (Z does not matter.)
Now for sake of example there is an X edge 1 inch from the true, original origen. If I use an edge finder to manually find the edge and lets say the edge finder locates the edge at 1.005, after correction for the tool diameter. If I use touch off to set G54 to 1.000 will this automatically apply the 5 thou correction?
The same process can then be applied for Y.

If I use my 6mm diameter edge finder on my manual mill to locate X & Y, I set the DRO's to be X -3 and Y -3. That means 0,0 is right on the corner of the piece.
If I was ever to CNC my mill, I would do a G54 X -3 Y -3. Or I could do a 3mm relative move on both X &Y and touch off at G54 X0 Y0

Might not really answer your question but it is easilly relatable to using G54

In theory your 0,0,0 point could be well outside the machine work envelope. When you set a G54 you are setting what that point indicated (edge finder, wiggler, hammer, probe) should be in comparison to the 0 point. Follow a simple checklist when confirming the point:
1) are you setting the correct axis
2) are you setting G54 (if another work offset was used last you are most likely setting that)
3) is the value correct, label the point before you probe, write on the part or a sticky note, what the value should be + edge finder compensation and then the value you want to actually enter

Be systematic and have a way of checking, either of these work for me (confirm the dro is in G54):
1) With the z clear of the part, use the mdi to G0 X0 Y0 this will rapid to your origin and you can verify it visually. If you don't want to rapid the same would work as G1 F20 X0 Y0 and you can control the speed by increasing or decreasing the F value

2) a bit more accurate way to check would be to indicate the x1 position and set G54 x1. Then move to x2 plus the cutter radius (for a 1/4" diameter cutter you would go to x2.125) and try and slide a 1" gauge block or 123 block between the cutter and part. Make sure the spindle is off.

I'm not sure I 100% follow what you are asking.

G53 is machine co-ordinate system / space - set by home switches usually.

G54 is the first work coordinate system (there iare G55-G59 also).

When you touch off G54, LinuxCNC forgets the previous G54 values. It does not compare the new values to the old values.
You are setting where the work co-ordinate system is in relation to the machine co-ordinate system.