Gmoccapy: make Tool Table exit more verbose

[zz912]

LinuxCNC core behavior:
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.

@hansu was not aware of this in the past. See:
#3706 (comment)
I struggled with this as well.

Therefore, I made exiting the Tool Table in Gmoccapy more verbose and added the option to activate G43 when the active offset changes from zero to non-zero.

I would like to ask @Sigma1912 for their opinion on whether this is OK.

[Sigma1912]

I have no problem with this addition.

[BsAtHome]

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

[rmu75]

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.

[zz912]

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.

[rmu75]

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?

[zz912]

... 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.

[Sigma1912]

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:

linuxcnc/src/emc/rs274ngc/interp_convert.cc

Line 6183 in f82c475

The g49 RS274/NGC command translates into a USE_TOOL_LENGTH_OFFSET(0.0)

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:

linuxcnc/src/emc/rs274ngc/interp_write.cc

Line 110 in f82c475

settings->active_g_codes[9] =

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.

[zz912]

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:

linuxcnc/src/emc/rs274ngc/interp_write.cc

Lines 110 to 113 in f82c475

	settings->active_g_codes[9] =
	(settings->tool_offset.tran.x || settings->tool_offset.tran.y || settings->tool_offset.tran.z ||
	settings->tool_offset.a || settings->tool_offset.b || settings->tool_offset.c ||
	settings->tool_offset.u || settings->tool_offset.v || settings->tool_offset.w) ? G_43 : G_49;

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

[Sigma1912]

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?

[zz912]

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)

[rmu75]

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".

[zz912]

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.

[rmu75]

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.

[Sigma1912]

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

[gmoccapy]

I have a different opinion.
IMHO a tool change with an active G43 should lead to a change and apply after the change directly the new tool offsets!

Tool 1 is in spindle with G43 active and Z-Offset = 22 mm
change to tool 2 with Z-Offset of 75 mm should bring after the tool change
Tool 2 is in spindle with G43 active and Z-Offset = 75 mm

Using only AUTO Mode with generated code by Cam will add a G43 after each tool change, but how often do we change a tool in Manual mode and than we need to take care to enter again G43 to get the correct values.

I do not know, if my wishes are utopia, but I like to dream ;-)
I did implement this behavior in gmoccapy and it did work for years without problems, until one user got problems mixing Halui commands with gmoccapy code. I did never expect that this would lead to random race conditions

Imho G43 can be active, even if the tool offsets are "zero", My touch probe have all offsets to zero and all my tools have there offsets.

Norbert.

[zz912]

Hello Norbert.

I have a different opinion.
IMHO a tool change with an active G43 should lead to a change and apply after the change directly the new tool offsets!

I think you misunderstood the functionality of this PR.

Several Gmoccapy users had problems with race conditions caused by the integrated AUTOMATIC_G43 in gmoccapy.py, not just me.
The integrated AUTOMATIC_G43 in gmoccapy.py was replaced by AUTOMATIC_G43 using the REMAP function. REMAP with AUTOMATIC_G43 was added to all sim configurations and was even added to the PNCconf Wizard. The warning about the end of the integrated AUTOMATIC_G43 in gmoccapy.py was also implemented. I think we did everything to continue your idea of ​​automatic offsets.

I think we have SAME opinion.

• I don't think anyone here is questioning the benefits of AUTOMATIC_G43
• I don't think anyone here wants to disturb AUTOMATIC_G43
• I don't question the benefits of AUTOMATIC_G43
• I don't want to disturb AUTOMATIC_G43

This PR does not apply to AUTOMATIC_G43 when changing a tool. This PR applies to AUTOMATIC_G43(popup message) when changing the offset for the same tool in the tooltable page. We continue with AUTOMATIC_G43 in other situations.

Imho G43 can be active, even if the tool offsets are "zero", My touch probe have all offsets to zero and all my tools have there offsets.

Could you please send me the version of LCNC you are using and the tool.tbl you are using? I can double check, but I think it is impossible. I made video in the past: #2613 (comment)

[rmu75]

Could you please send me the version of LCNC you are using and the tool.tbl you are using? I can double check, but I think it is impossible. I made video in the past: #2613 (comment)

Norbert probably means that there is no reason this behaviour would be harmful, not that it currently is that way.

I don't want to add further to the confusion and am going to implement that G43 can be active with all offsets identical zero.

[Sigma1912]

See #3816

[edit]
update link to new PR

[rmu75]

@Sigma1912 was faster it seems ;)