G-Code from Fusion 360

[Aiph5u (Aiph5u (not affiliated with Onefinity))]

Hey Chris,

@ChrisM

Even people that use multiple tools in the same Gcode file have to stop and touch off the next tool to Z0. Then that new tool’s offset gets put in the one and only register.

What you mean here are the parameters #5211, #5212, and #5213 for X, Y and Z offsets that you can also see in the “offsets” column on the control page. They are filled by the probing routine which calls G92, or you can call G92 directly to set the workpiece zero directly in the command entry field of MDI tab.

@ChrisM

Is this true that OneFinity does not keep track of a tool table and thus ignores these H offsets?

Yes it is true. When you set your tool to Z0 with the probe or by paper method or whatever, that value is stored in the one and only Z offset register.
[…]
So the controller knows when G43 is called to get the offset from that register - no matter what number is called by H. You may even be able to leave the H off all together - though I have never tried it.

then what do you think of this? The tool offsets are correctly stored in the parameters #5401 ff, which is part of the tool table, and applied when the new tool is selected with Tx M6, or by G43 Hx, as I showed by trying it out. They are stored separately and not ignored, but applied.

When I do G43 H1, the tool offset is 12 mm because I loaded the tool table with 12 mm for tool 1.
When I then do G43 H2, the tool offset is 14 mm because I loaded the tool table with 14 mm for tool 2.

Does not seem to me that the tool specified with H is ignored. In fact the Onefinity Controller does keep track of the tool table and honors the H value on G43.

Here you can see two interesting things:

1. After having defined a tool Nr. 3 with 16 mm Z tool offset and having selected it with G43 H3, and having homed the machine, the offset in the offset column is 16 mm.
2. If you then request the content of the Z offset register, it is NOT 16, but 0 (!).
3. If you then request the content of the tool table, Z offset for tool 3, it shows 16.

So it’s clear that what the Buildbotics/Onefinity Controller shows here in the “offsets” column is not the offset you set by probing Z (as this offset register is 0), as most users would expect, but an offset that is clearly from the tool table, from the entry of tool Nr. 3. Voilà.

Note that the tool in the status table is still 2, because this tool was selected previously and I did not yet do T3 M6. If I do, the selected tool will change to 3. So G43 Hx sets the tool offset from the tool table, but only Tx M6 selects the tool then.