Where should linux cnc tool offsets be stored?

Coming from a background in mostly mazak programming and alittle haas the way linux cnc handles tool offsets has been confusing me and maybe it's because I'm not setup with somthing like the carousel macros.

I am currently using axis since it's the only thing that supports the weird display size I accidentally went with. So anyways when I set tool height it moves g54s z value to the tooltip like I was touching off the part not the tool. Currently I have been storing all tool heights too p59 as a work around.

This seems like a weird way of being setup rather then storing it too it's own unique tool height reference for a tool setter. 

I'd be curious too see how the tool setter macros work exactly where do they store the height of the tool setter 

Maybe this is somthing super basic I have never had to setup a tool setter at work before and as far as I fan tell and when manually setting tool lengths mazak seems to base them on a unique height offset.

Thanks for any and all responses!

I am not an expert, but I was confused about offsets when I started out, and took the time to "get it".  I hope I'll share that here
There are two ways to measure a tool:
1. Measure it relative to some predictable surface, on the bench.  I.e. use a jig and height gauge to measure the actual "length" of the tool.
2. Move the tool tip to a known point in-machine, and do the math.
The first case is common in bigger shops (they can justify the extra equipment but is typically limited to a Z measurement, typically referenced to the center of the bottom of the spindle itself.  It also assumes the tool sticks out the bottom of the spindle (Z-) and not in any other direction.
The second case is used with toolsetters.  On my machine, I probe the toolsetter to get the machine Z at the probe point, subtract some arbitrary number I store the XY and mostly Z location of the toolsetter in the INI file), and that's the "offset".  It's no longer a *length*, it's an *offset* from a reference point.  My "reference point" is near the end of a 1/4 endmill (about 2" below the spindle), by design, so if you forget to set it at least your crash will be less spectacular.
In LCNC you can also do a "tool touch off", where you've probed or touched off your workpiece, change tools, move the tool tip to a known location, and tell LCNC "the tool tip is at XYZ, please set the tool offsets so you agree."  This is useful if you have multiple "spindles" on your machine (my Z carriage has both a spindle and laser, so the laser "tool" has a non-zero XY offset too).  If I touch off 0,0,0 to a point with the spindle's tool, then move the machine so the laser is at that point, the display will show the laser's "offset" from *the current tool* (i.e. it displays machine+G54+T1+T2) but LCNC can do the math for you.

Fundamentally, they're all just offsets in the nine-axis space LCNC uses.  If you want to move the tool tip to a work-local XYZA coordinate (my machine has 4 axes), you take that XYZA, add the G54 XYZA offset, add the G92 XYZA offset, and add the Tool XYZA offset, and move the machine to that absolute XYZA location.
So a "workpiece touch off" assumes the tool offset is correct and sets the G54 offset, and a "tool touch off" assumes the G54 offset is correct and sets the tool offset.

So to return to your question: "it seems like it's moving the G54 Z".  No, it's not.  The displayed Z is the machine's absolute location, plus the G54 (or other WCS) offset, plus the Tool offset.  If you hit the "View->Show Offsets" menu these additional offsets will be displayed.
So it's important to remember that a "touch off" moves the G54 relative to ALL the tools, and a "tool touch off" moves one tool relative to the others.  Thus, you can't change tools and then touch off with that unmeasured tool, because you've changed both sets of offsets at once, and LCNC will be confused.  Put the tool in, measure it, then touch off; or touch off with an existing measured tool, then change tools and measure it.

Also, I think all CNC machines handle offsets basically the same way, but present it to the user different ways (different words, macros, buttons, etc.).
 

Seeme like Linuxcnc is set up assuming premeasured tools in a magazine. HOweer you can do this with repeatable tooling or adopt TTD in your MT3 or R8 spindle. When I set up QtDragon, I bought a tool setter and the tiny marble plate with a hole in it from Tormach. I measured all my tools in the toolsetter Including the 3D probe as tool 99.So after touching off with tool 99 with the probing routines, QTdragon asked me to change the tool manually and continue. This worked very well as you could run out a singlee gcode file instead of running  out seperate files for each tool the eold fashioned way!

I suspect ALL cnc's apply offsets the same way. And as long as the offsets add up to the right tool location, it doesn't matter if you change G54 or T1 when you manually change tools. If you're using a trim router with a collet and change tools all the time but never issue a T command, you just have to know how to change the G54 so that it does the right thing.

So external measurement, toolsetters, manual tool touch off, part touch off, they're all just ways of making those offsets add up to the right thing.

I will add, though, that when I started using my ATC I mixed the old and new ways, and it was a disaster