You need to have two dimensions on your box tool. The distance between the touch off point in both X and Z on what can reach the tool eye. Then you need the distance from this to the desired set point on your cutting tool.
After touching off the edges you can get to, go in and incrementally adjust the set values of the taught X and Z offset. In X, all offsets are diameter values, so the number has to be doubled. Z is always the actual true distance. These adjustments are the dimensions for set point to desired set point on the cutting tool.
Write numbers down and think through whether plus or minus numbers should be taught.
A neutral turning tool. 60 degree insert. 60 degree leading and trailing angle. The set point in Z cannot be touched off, but the side of the tool can. For a 1" square shank tool, touch off the side of the shank in Z. That sets the edge of the tool as the driving point in Z. This value is off by .50000". arrow to the Z offset register, turn on the incremental switch, and input -.50000". This incremental adjustment has now brought the Z offset value to match the Z cutting point, which is the center of the tool.
An example in X.
A .50000" dia gage pin in a drill collet holder, oriented in drilling at main spindle. Touch off X at the 12:00 position on the tool eye. This sets the lower circumphrence as the set point, but you want to set the centerline as the set point, for a drill. Arrow to the X register, incremental s/k switch on, key in -.50000" -input. Now the X offset is driving the centerline of the holder/gage pin.
If you touched off the 6:00 tool eye position, then you would incrementally adjust by .50000", a positive number in this case.
12:00 tool eye is also known as X minus. 6:00 tool eye is X plus. 3:00 is Z minus, and 9:00 is Z plus. So named because thats the direction the axis must take to make a reading.
Write the numbers down and do an eyeball MDI position check to make sure you got the +/- and value correct. Remember - all X is diameter numbers, not radial (aka true distance)