If that Z-Zero never (or rarely) changes because you’re zeroing off of a fixture plate or your wasteboard, I’d just use a macro (quick action?) that re-establishes that Z-zero with a G10L2Znnn command.
When you set zero the “standard” way, you (or your machine controlling UI of choice…Carbide Motion in this case) are sending a G10L20 command. Let’s say you are setting your XYZ zero by eye, you would jog to the location of your desired work origin and then send G10L20X0Y0Z0. When you use the BitZero, the numbers for XY&Z are adjusted for the probe thickness. Behind the scenes, that is calculating your work offsets or how far away your work zero (origin) is from your home location (your limit switches, MACHINE zero, the absolute reference).
Another way to set zero is to tell the controller your work offset, rather than have it calculate it. To do this you’d use a G10L2 command (notice the two in place of the twenty). If I know my wasteboard is exactly 122.37mm below my Z limit switch (Z-122.37 MACHINE position), I can send the command G10L2Z-122.37 to set my Z-zero at the surface of my wasteboard. You can do this regardless of your actual position on the machine. You can home the machine, send that command, and that’s where your zero will be. If you want your zero to be 19mm above that because that’s where you set it in CAM, then just add 19mm to -122.37 and send G10L2Z-103.37.
I hope that makes sense. Now, your relying on the repeatability of the homing switches for this to be perfect. Personally, despite my enjoyment of automating probing, I find that a V-bit and my eye is currently more reliable than inductive or conductive switches / probes.
To directly address the thread…I would guess that C3D doesn’t have an probe XY only option because the Z location is needed to ensure proper probing depths on the other axes.
These would be “Quick Actions” in Carbide Motion. I don’t use Motion, so take my advice as a guide. Testing will be required. The gcode works with GRBL, but Motion might require something else. For example, Motion might not like the command without a P-word. By default the P value is zero when not included, like this: G10L2P0Z-88
That P0 means that the offset is changed for the currently active WCS (Work coordinate system) which is, by default, P1, or G54. Motion might want a P1 there instead…I don’t know.
It’s just a one-liner of gcode, like I posted above.
No. You can add a G20 to the beginning of the line to ensure you are in inch mode. G20G10L2Z-103.37 . If you’re switching units, always double check things. I recommend using metric for everything (design can be done in any unit of measurement) because GRBL’s internals use metric anyway.