Extending existing G38.2/G38.3/G38.4/G38.5 codes

I have a 3D touch probe which is always mounted at the same fixed location/orientation, not centered with the spindle. (picture) .

To make full use of the advantages this provides, I created an NGC program that probes a ring of known diameter and produces a file with the offsets to the spindle center for X probing directions (where X is not limited to 4), and a HAL-component that uses this file to generate the correction data for a probe trigger.

The normal sequence of things now becomes, for example:

G38.2 X10 Y10 Z10
#<proberesult_x> = [#5061 - #<_hal[probe-compensation.0.correction-x-make]]
#<proberesult_y> = [#5062 - #<_hal[probe-compensation.0.correction-y-make]]
#<proberesult_z> = [#5063 - #<_hal[probe-compensation.0.correction-z-make]]

Not very handy for files littered with G38.x. Slightly easier is:
G38.x axes
o<compensatie_probe_results> call

But still that requires editing of all files using a probe.

A much nicer way to handle this would be to remap/extend the G38.x codes. But when I read the manual , it says:

14.1. Existing codes which can be remapped
The current set of existing codes open to redefinition is:
Tx (Prepare)
M6 (Change tool)
M61 (Set tool number)
M0 (pause a running program temporarily)
M1 (pause a running program temporarily if the optional stop switch is on)
M60 (exchange pallet shuttles and then pause a running program temporarily)
S (set spindle speed)
F (set feed)

Is there a method to extend existing G-codes not in this list? Or am I forced to either do the correction manually after every G38 or define an e.g. G37.x that mimics G38?

Hi

Is there a method to extend existing G-codes not in this list? Or am I forced to either do the correction manually after every G38 or define an e.g. G37.x that mimics G38?

The problem with trying to remap G38.2 etc is that they are group 1 modal codes ( same as G0, G1, G2, G3 etc)
There is a lot more going on than just the probe move.
I don't think you can remap them easily, or change them without a lot of code rewriting
see
src/emc/motion/control.cc and command.cc for the hard coding of probing

You seem to have quite a good method for dealing with your offset probe, the difficulty adding calls to gcode to fix the offset is minimal.
Much probing requires some sort of offsetting, even if the probe is held in the spindle, probe head diameter / 2 at the minimum, to get the exact edge position

Even if you made G39.2 an alias for G38.2 plus offset calculation, you would have to alter your post or do some other change to amend the number, which is probably no less hassle.

regards

I do not want to rewrite the code, only add an extra prolog/epilog to the existing functionality. It should not be too hard to add that possibility to the existing remap/extend infrastructure, although I am not capable of doing that.

Adding the compensation call before probe results are being processed is not that hard, and a viable workaround. The only minor problem I have with it is that when I decide to use external code (such as probe_screen) I have to modify that code every time a new release appears. In my opinion the control should take care of the internal stuff, not the user programs.
Creating a G39.x is slightly cleaner since then we have an 'uncompensated probe move' called G38 and a 'compensated probe move' called G39.

Another minor issue is that my probe is wireless and outputs a 'system OK' and 'trigger' signal. Communications can fail, the internal measurement electronics can fail, batteries drain, etc, so I need that system OK signal. I also have two probes attached; a tool length sensor and the touchprobe. There is no really clean way to handle this situation. Currently I simply combine the probes like this: motion,probe-input = toolsetter | (motion.digital-out-00 & (touchprobe_trigger | !touchprobe_ok)), which forces me to enable/disable with M64/M65. That already went wrong once; extracting the remaining pieces of sheared off M3 bolts out of an aluminium housing is not funny.
Did some effort to combine these probe signals in a HAL component and look at motion.motion-type, which works for 'make' moves but not so easy for 'break' moves since there is a one servocycle delay and motion complains 'probe was not active at the start of G38.4/G38.5'. That route was not succesful, but I have an idea how to deal with those issues (basically a selector switch, the probe that generates an edge is the one being selected).
Luckily we have HAL and comp, so we can solve all this. But the issue is that there is no generic mechanism to tell LinuxCNC that attached devices are actually working. Example: 'Enable mist coolant', OK, great, but is the misting system OK? Do I actually have air pressure and is the coolant reservoir not empty?

DaBit wrote: But the issue is that there is no generic mechanism to tell LinuxCNC that attached devices are actually working. Example: 'Enable mist coolant', OK, great, but is the misting system OK? Do I actually have air pressure and is the coolant reservoir not empty?

Well all of this is easy to a certain extent: there are cheap humidity sensors or 2 wires in front of the nozle a Darlington transistor and a resistor will do the job easily to report back that you actually have mist, air pressure switches are easy to find and modify like from a compressor (there is one already there if it has a spare contact or just piggy back a small micro-switch), the reservoir again same as mist but in the actual tank. Do a google search for simple humidity sensor or rain detection sensor, mostly used in cars for turning on wind-shield wipers.
Regards,
Tom

He means there is no status feedback in linuxcnc for these requests.
Gmoccapy and gscreen do have message systems (popup dialogs) that you can connect to an
'error' hal pin from your custom component. not very clean but doable.

user configurable error handling in linuxcnc and error handling in HAL components is a weakness.

Chris M

DaBit wrote: To make full use of the advantages this provides, I created an NGC program that probes a ring of known diameter and produces a file with the offsets to the spindle center for X probing directions (where X is not limited to 4), and a HAL-component that uses this file to generate the correction data for a probe trigger.

I think you are making this too hard.

LinuxCNC supports tool offsets in all 9 axes. Just drill a hole with the spindle, probe the centre (with the hole-probing routine in nc_files/examples then touch-off the tool table for the probe tool to 0,0 to store the X and Y offsets of the probe relative to the spindle.

I use T99 for my probe.

M6 T99 G43 then loads the probe XYZ offsets. G43 with any other tool (without XY offsets) then puts the axis system back on the spindle.