Recording coordinates

martig wrote:

Hi I have a 4 axis router setup. What I would like it to is following:
the tool should move according to the G-Codes like a router would otherwise, but upon receiving an input it should record it's current position to a log (file) and just continue moving along the path.

Is the input going to happen during auto-operation? If so, then it is annoyingly difficult to do what you want.

The following will only work if the machine is _not_ in AUTO mode:

Inside G-code you can use (LOG, xxxxxx) to output to a file:
www.linuxcnc.org/docview/html/gcode_main.html#sub:Messages

In theory you could call that code on a pin going high with an MDI_COMMAND
linuxcnc.org/docs/html/gui_halui.html#sub:MDI

Depending on the version of emc2 you are using the current coordinates might be available in #5420 to #5428 (and, in the latest development they are likely to be available as #<_X> etc).
www.linuxcnc.org/docview/devel/html/gcod....html#sec:Parameters

So, you might be able to add the following in the indicated parts of the INI file
[HAL]
{existing stuff}
HALUI=halui

[HALUI]
MDI_COMMAND = (LOG, #5420, #5421, #5422)

and then in the HAL file something like:
net log-now halui.mdi-command-00 <= parport.0.pin-04-in

However, that won't work with older versions, in those you have to use a trick to get the current coordinates:

[HALUI]
MDI_COMMAND = O<lognow>CALL

Then create a file called lognow.ngc, put it in the directory pointed to by PROGRAM_PREFIX (in the INI file) and put the following in it

(Though, I am not sure which version of EMC2 introduced O-sub call from MDI_COMMAND)

It sounds like you might actually be wanting to do probing, though, and you can get G38 probing to automatically log to file.