Asynchron motion of 4 axis with 2 Interpreter

I have an Index GS30 lathe with 2 turrets (4 axis).

I assume this is a "Swiss" lathe, and that the workpiece emerges from the hole in the back-right corner between the toolholders?

My question now: Is it possible to load two RS274 Interpreter which have both access to all axis?

I am not sure about running two interpreters and trajectory planners simutaneously. I don't think it is possible, but might be wrong. I think they would both want to create "pins" with the same names in the HAL shared memory and that would lead to conflict.
I think the possibility has been discussed before on the mailing list, it might be worth asking there too. lists.sourceforge.net/lists/listinfo/emc-users

In any case, you can not allow both interpreters to have access to all axes, as it then becomes impossible to decide who "wins" if they both try to move the same axes.
The simplest solution, considering how cheap PC hardware is compared to the the rest of the system, might be to have two PCs running EMC2, each controlling one head. They can communicate with M66 which will pause a G-code program until a pin changes state: wiki.linuxcnc.org/emcinfo.pl?Mword

And is it also possible to change the axis identifier from U to X1 and V to Z1?

No, because G-code ignores spaces, and so it is impossible to differentiate between G0 X 10 and G0 X1 0.

You have presumably already noted that you can write G-code in XZ and UW (though I don't think you can make arcs in the UW plane, which is a limitation). That would allow you to use both heads simultaneously, except that all the moves have to start and stop at the same time too.

One more problem I have is, that the tool change is done with a move of the Z (turret 1) and the X axis (turret 2). I will write a subprogram for that, but I would appreciate to do that with a M6.

You can define a toolchange position in the INI file (in machine absolute coordinates, I believe) that might do what you want.

For something as unusual as this to get the best exposure to EMC2 enthusiasts you might also post your questions on the mailing list.

John

The toolchange is done with setting a hydraulic valve and moving the Z axis (turret 1) or the X axis (turret 2). The linear movement of the axis leads to a rotation of the turret. (ca. 1 tool per mm)

If you look at the way that hal_manualtoolchange is integrated into the sample configs, it would seem reasonably simple to write a new hal component using "comp" to do what you need.
linuxcnc.org/docs/html/hal_comp.html
I envisage a hal component that takes an axis position, tool cange request and a tool number, and passes through the position unchanged to the PID or stepgen controlling the axis under normal circumstances, but passes out a ramped delta to the position and a valve control signal when a toolchange is requested.

I was thinking that you could use MDI_COMMAND ( linuxcnc.org/docs/2.3/html/gui_halui.html#sub:MDI ) but those are not active with the program in Auto. (It is possible, though, that the system drops out of auto during a toolchange...)

That's simple, but an unattractive solution, because I have to control two PCs, load 2 programs and start emc2 on both PCs.

It would be reasonably simple to slave the two "run" and "stop" buttons together in HAL (via physical interwiring of the two machines) and you would need two programs anyway. I don't know of any system that runs a single G-code program asynchronously.

XX and ZZ could be used instead of X1 and Z1. When the interpreter would check if already one instance is loaded, it could change the identifier to XX, so there won't be a problem in the HAL.

Possible, perhaps. It breaks the G-code standard of all commands being single letters ("X" is a command, not a variable.)

Where is the interpreter loaded? I browsed already through a few files, but I haven't found the corresponding line yet...
Does anybody know where I can find it?

Possibly
git.linuxcnc.org/gitweb?p=emc2.git;a=blo...4d1a97ae496f;hb=HEAD