I have no problem with this addition.

Please resolve the review if the changes are OK. Then we can merge it.

IMO this PR needs a proper commit message, I have no idea what a "Tool Table exit" is and why / how it affects (only?) gmoccapy.

Current LinuxCNC behavior:

1. Change the parameter of the selected tool
2. Save the tool table
3. Leave (exit) tooltable page
4. You will get popup message
5. If you give Yes, G43 will be executed and the corrections will be updated

This PR adds another popup message (4.) for situations when the operator selects offset == 0, or previously was offset == 0 and the operator changed the offset != 0.

Activating G43 with zero offsets deactivates tool compensation.

I wonder what the rationale is justifying this behaviour or if it is simply a bug in the interpreter. It certainly isn't documented here https://linuxcnc.org/docs/devel/html/gcode/g-code.html#gcode:g43

Playing around with this a bit in qtvcp and axis, it seems there are bugs like this in other GUIs too.

Maybe the proper place to fix this is somewhere else?

... or if it is simply a bug in the interpreter.

That's an interesting question. I just took it for properties. It didn't occur to me that it could be a bug.
Does anyone know how it is with other systems (Fanuc, Heidenhain, Mach, Siemens ...)?

Maybe the proper place to fix this is somewhere else?

If this is a bug, it should be fixed elsewhere. But that's beyond my capabilities.

Activating G43 with zero offsets deactivates tool compensation.

Looking at this a bit more closely makes me think that this is actually a phantom problem as I'm not sure there IS an internal state like 'activated' / 'deactivated' tool offset as such. All we seem to do with G43/G49 is change the values of the internal tool length compensation. For G49 they are all set to zero.
See:

The displayed 'G43' / 'G49' in the 'active gcodes' only reflects whether the current internal tool length values are all zero ('G49') or not ('G43')
See:

So 'activating G43 with zero offsets' does not actually 'deactivate' tool compensation it only makes 'G49' appear in the active gcodes list because all internal tool offset values are zero.

Thank you for looking into this.

I agree that for LCNC developers this sentence "Activating G43 with zero offsets deactivates tool compensation." is inaccurate. However, for a CNC machine operator it is correct.

For LCNC developers, the sentence should be "Activating G43 with zero offsets makes 'G49' appear in the active gcodes list." However, a CNC machine operator will not even know what a "gcode list" is.

We are currently in a situation where LCNC developers should decide whether:
"Activating G43 with zero offsets makes 'G49' appear in the active gcodes list."
is correct behavior or whether it is a bug.

If this is correct behavior, it should be added to the documentation and this PR should be merged.
If this is a bug, it should be fixed and this PR shouldnt be merged

I consider myself an LCNC tester, not a developer. Both options are acceptable to me.

BTW:
I searched for these lines for many hours with ChatGPT and couldn't find it:

These lines prove that LCNC really works with zero values ​​and not with 10E-9.

What made you think that it used 10E-9 for tool offsets?

These lines prove that LCNC really works with zero values ​​and not with 10E-9.

What made you think that it used 10E-9 for tool offsets?

#3792 (comment)

Activating G43 with zero offsets deactivates tool compensation.
In this situation, G43 behaves like G49.
If the CNC operator is not aware of this, it can have dangerous consequences.

I wonder what dangerous consequences that could have? If tool offsets are 0, then there are no offsets, and it doesn't matter if machine displays "G43" or "G49".

I wonder what dangerous consequences that could have? If tool offsets are 0, then there are no offsets, and it doesn't matter if machine displays "G43" or "G49".

This situation can occur when you use a CNC machine as a conventional machine. It is the case when you use manual mode for machining as well.

You have for example:
Tool number 1 offset = 0
Tool number 2 offset = 5.256
Tool number 3 offset = 0.5
Tool number 4 offset = -3
Tool number 5 offset = -50

1. You have g43 activated and work with tool 3. You are watching DRO, everything is OK.
2. In MDI you change the tool M6T4. Gmoccapy has automatic G43. So the offsets are updated, you don't worry about anything and the offsets are updated. Everything is OK.
3. In tooltable page you change the offset for tool 4 to -3.5. You leave the tooltable page and get a message asking if you want to update the offset. You click Yes, the offsets are updated. Everything is OK.
4. In MDI you change the tool M6T1. Gmoccapy has automatic G43. However, it turns out that G49 appears in gcode.list.
5. In tooltable you change the offset of tool 1 to -45. You leave the tooltable page and you don't get any message, because G49 appears in gcode.list (state before this PR)
6. You don't notice that G49 is active. You look at the DRO and then you crash into the vice.

Another situation:
You are LinuxCNC beginner or student. You are learning work with tooloffset.

1. You work only with tool number 5
2. In tooltable page you change the offset for tool 5 to -3.545. You leave the tooltable page and get a message asking if you want to update the offset. You click Yes, the offsets are updated. Everything is OK.
3. You have found that you have measured the offsets incorrectly. You will return to the tooloffset page.
4. In tooltable page you change the offset for tool 5 to 0. You want to try what happens. You leave the tooltable page and get a message asking if you want to update the offset. You click Yes, it turns out that G49 appears in gcode.list.
5. You will return to the tooloffset page.
6. In tooltable you change the offset of tool 5 to -45. You leave the tooltable page and you don't get any message. (state before this PR)
7. You don't notice that G49 is active. You look at the DRO and then you crash into the vice.

I think this is a problem mainly for Gmoccapy users who are spoiled by automatic G43.
This PR makes it so that if you keep pressing Yes, you will always have correct tool compensation.
"Activating G43 with zero offsets deactivates tool compensation." is not dangerous if you know about it and if the GUI warns you about it.

Thanks for the explanation, I understand how that can be surprising and annoying. Still not sure if there is something in the interpreter that should be changed, allowing an active G43 in case tool offsets are zero would be an easy change.

allowing an active G43 in case tool offsets are zero would be an easy change.

I would be in favor of changing it.

IMO it IS a bit problematic to present G43, G43.1, G49 as being modal and then silently change it to G49 when the tool offset values happen to be all zero. This is indeed rather unexpected behavior.
https://www.linuxcnc.org/docs/html/gcode/overview.html#gcode:modal-groups