How do I set the tool table?

Cayenne wrote: Sounds like my problem!
If my machine has no limit or home switches and no tool changer why do we need to home the axis?

It is very useful to allow restarting of jobs, and also means that the system can know that it can machine the part without hitting the end stops. It also means that the software can avoid ever hitting the end stops.

I have no idea why folk are so resistant to fitting a few extra switches and wires.

But, if you really object to home switches then there is an INI file option ( [TRAJ]NO_FORCE_HOMING ) that means that homing is not enforced. There is also the option to record the shut-down position too. ([TRAJ]POSITION_FILE)

I am using a manual quick change tool post.
what would a tool length offset be relative to???

If this is a lathe, then typically the tool length offset of any tool is relative to the length of a probe or another tool. All my tool lengths are relative to my Tool 1 (turning and facing) tool. I jog to the material end, touch-off G54 to zero, and take a facing cut at Z=0 with tool 1. Then take a test cut to a diameter with the same tool and set that as the G54 X offset. Then I can change tools to (for example) a threading tool and the diameter and length are correct.
Actually, I don't do that second part very often, as I have my lathe set up with single-turn absolute resolvers and a bit of cleverness with the POSITION_FILE means that my lathe always knows exactly (to the micron) where it is at power-up)

now it's just mathematical insanity where nothing is reproducible. even the inputs for touchoff, and tool touchoff seem to randomly prefer radius or diameter. Can someone please point me to a current startup work flow for turning?

Whether radius or diameter is set depends on whether the machine is in G7 or G8 mode. I think it starts up in radius mode. A STARTUP_G_CODE can change this.

There shouldn't be any mathematical insanity. Perhaps you are touching-off tools when you should be touching-off coordinate systems? (and possibly your system, too, is set to "touch off to fixture"?

Thank you very much for this concise info!
Yes, "Lathe" that is why i posted in this sub forum.
"touch off to fixture" is not in effect !
LCNC is set to radius mode.
When I first start LinuxCNC the "touch off" obeys the radius mode input.
The "tool touch off" wants diameter inputs and later, it wants radius inputs (bug?) maybe I'm not understanding things. and yes, operator error is a strong possibility!
So if I use tool for tool I should only need "touch off" correct?
How do we zero out all offsets?? because ounce I enter the wrong tool g54 offset, no matter what I do i can never zero out the g54 in order to start over.
I have been using F360 for toolpaths, which compensates for tool tip radi (i believe) so should i enter a tool tip radius in LCNC tool table? Again, Thank You!

Cayenne wrote: When I first start LinuxCNC the "touch off" obeys the radius mode input.
The "tool touch off" wants diameter inputs and later, it wants radius inputs (bug?) maybe I'm not understanding things.

If the machine is in G7 / Diameter mode then the number you type in will become the current diameter.
If the machine is in G8 / Radius mode then the number you type in will become the current radius.
You can experiment with this, switch between G7 and G8 using MDI and try touching-off your G54 coordinates.
(This is rather more obvious in Touchy as that permanently displays both radius and diameter.) And I quite often find it not doing what I expect, but that is because the lathe has been left in an unexpected mode (I work nearly always in diameter)

How do we zero out all offsets?? because ounce I enter the wrong tool g54 offset, no matter what I do i can never zero out the g54 in order to start over.

"tool G54 offset" is a phrase that makes no sense, and if that is what you really meant then this might explain part of the problem.
In any case MDI will zero-out all tool-table data for tool 10. will zero out the work offsets for the current coordinate system. Use P1 for G54, and so on.
linuxcnc.org/docs/2.7/html/gcode/g-code.html#gcode:g10-l1

I have been using F360 for toolpaths, which compensates for tool tip radi (i believe) so should i enter a tool tip radius in LCNC tool table?

The radius in the tool table doesn't matter unless G41 / G42 are active. and Fusion CAM does not use those.