Fusion 360 G3 errors SOLVED

I have tried everything. This is my latest program an it is still saying arc radius to small to reach end point. Or arc radius different at end point. I found tool.tbl in my computer and set the x z both to +0. The only entries in it were for x z. Unless the table is set up wrong I am at a loss. No idea. If I put a program in by hand it will cut a radius, but it won't from 360. I have attached the latest program I tried. Can someone please check to see if this runs in there machine?

What else am I missing? Could someone send me a program to see if I can put it in my machine?

Looking through the code one thing that looks odd is that there are lots of G40 and G42 commands, but at no point does it load a tool or set a tool diameter.

Which postprocessor are you using in Fusion?

I am not currently anywhere near Fusion or LinuxCNC, but is there a way to set Fusion to do the tool compensation in the postprocessor rather than in the control, as a first step?

My suspicion is that Fusion is using the wrong control point for the offset. Do the tool orientations and diameter match exactly between the Fusion360 tool table and the LinuxCNC tool table?
(And do LinuxCNC and Fusion even agree on how tool orientation and control point are defined?)

Doing radius comp In the control is techically better as you can tweak the offset to compensate for wear or if you change to a different insert. But generally on a lathe you can nearly always ignore tool radius as long as you don't care about fillet radiuses being spot-on. Diameters and lengths come out correct regardless (unless using tool orientation 0) and in fact I hardly ever bother with it for the parts I make.

One thing I can see in the G code is that "J" is used for the center offset of the arc in the X direction. That is wrong, it should be "I". In the G3 lines.

I propose you try the post processor I attached earlier in this thread. Do tool compensation "in computer".
The code that comes out from that one has worked for me the last 500 times or so. No modifcations should be
needed, just run.

Place the cps file somewhere like on the Desktop. When posting, browse and select it.

I figured it out. So the J was an issue and I got it to post with I. K. So for some reason I need 5 decimal place in order for it to read the radius. I went into the post processor and edited so it would post 5 places. Low an behold it worked. I am now successfully running fusion 360 Thank you all for the help. Now on to figuring out why the Z axis is drifting a few thousands over multiple passes.

in the postprozessor area there are modified postprocessors
to solve many issues on linuxcnc from fusion g-code

you may find a better one there

Hello, I am using the Fusion 360 post-processor for plasma and when I use figures with radii I have the same problem of different arcs, someone can help me with a recommendation or something that I have to modify, thank you very much.