Setting up Z Tool Offsets and Z Work Offsets

I've been using my Haas GR408 router(2006) setting tools off the workpiece with the tool offset register and plugging in Zero for the Z value on work offsets. While that works-- one has to touch off each tool when changing material thickness rather than choosing the appropriate work offset for Z.

I thought I'd be setting the tools off the table and then plugging in the distance from the table to the top of the workpiece and typing that value into the appropriate Z work offset G54, G55 etc. I thought the Z Tool Offset Register Value was the distance from G28 to location where the tip of the tool touches off from G28-- and therefore not dependent on any work offset numbers.

My confusion is that I get a different value for the tool offset Z zero depending on which work offset register I last used and what value was in that z offset register. This totally negates the way I thought it was supposed to work.

Example:
In MDI: G49 G55

G55 Z OFFSET SET TO 0
T2 TOOL OFFSET MEASURE = .5

GO BACK TO G55 AND CHANGE WORK OFFSET TO 1.0
THEN GO BACK TO Z TOOL OFFSET MEASURE AND THE SAME TOOL NOW READS -.5

IN MDI: G49 G54 (note g54 z vale was -1.0)

Go back to work offset G55 and change z value back to 0

now go back to T2 tool offset measure and it changes to 1.5 (when pressed)

Therefore-- If I'm setting up 4 tools to the table when my G55 work offset was set at 0-- then get the workpiece on the table and now see that its 2" above the tool offsets and I put that in my G55 Z work offset. Then-- if I come back to add tools 5 and 6: if I don't go back and change the work offset value to the same it was when setting up tools 1-4, and then back again to run the program-- the tools won't go to the same part z zero.

note, my G52 and G92 are at zero

Am I not doing or thinking something correctly here?

There is a setting you can toggle. It will either apply the length based on the current offset, or absolute. You want it absolute. Here you go:

64 - T. Ofs Meas Uses Work

The (Tool Offset Measure Uses Work) setting changes the way the TOOL OFFSET MEASURE key works. When this is ON, the entered tool offset is the measured tool offset plus the work coordinate offset (Z-Axis). When it is OFF, the tool offset equals the Z machine position.
(at least I think this is the one you want)

Mike, that fixed it-- now it functions as anticipated.
Thanks,
Dan