reversed IJK g2 g3 commands from fusion360 ???

has anyone run into this before ? all of my arcs are being inverted, which, is kinda weird, my lathe is backtool. did I mis a setting somewhere ? 

I'm not sure if this is going to help but if you look at the post for linuxcnc you will see that it is written near the beginning:

longDescription = "Turning post for LinuxCNC. Use Turret 0 for Positional Turret, Turret 101 for QCTP on X- Post, Turret 102 for QCTP on X+ Post, Turret 103 for Gang Tooling on X- Post, Turret 104 for Gang Tooling on X+ Tool Post.";

I never cared much about this since my lathe has only a front tool post (x+) and default setting is working for me but maybe this is something you need to set for a machine with a rear post.

 

what on earth does that even mean ? QCTP ? what about a back tool lathe with a tool changer ? and my tool changer works properly, just having this issue with g2 and g3 being wrong, and looking at the gcode output, it's defintely wrong
 

Yeah, I think this is it. You need to set the correct turret

See here: forums.autodesk.com/t5/fusion-360-manufa...l-slant/td-p/6851532
 

smc.collins wrote:

QCTP ?

 

Quick Change Tool Post

guys I am not seeing any of those options anywhere except in the post processor, is there somewhere else to be setting these options ?


edit I found it, when you go into the tool, go into the postproccesor tab, and that is where they have buried the turret number, with no explanation of what the hell it's doing. I swear to god I am buying mastercam as soon as I can afford it. 

thanks for the help guys, good catch !!! 

So, seems that you have to set the turret for each tool  (probably 101?)

 

smc.collins wrote:

edit I found it, when you go into the tool, go into the postproccesor tab, and that is where they have buried the turret number, with no explanation of what the hell it's doing.
 

With inventor cam you can also open the tool library, then open any tool. Turret setting is on the general tab. I don't know if this is the same for fusion360.

^^^^ Found out that this is only for inventor cam. With Fusion 360 you indeed have to go to the postprocessor tab

JPL wrote:

So, seems that you have to set the turret for each tool  (probably 101?)


 

  imagine the dumbest thing possible, and yes. this is a pretty serious design flaw. Apparently if you flips the tool over and do the cam for backtool with counter clockwise, it automatically sets the tool as if the tool is facing at Z sub spindle opposite the primary spindle. This is the kind stuff that makes me mad. if there going to change g2 and g3 based on turret, that dumb, it should be based on which spindle it's facing. IE spindle on the left, normal g2 g3, spindle on the right inverted g2 g3, ugh. 

oh and they just give you a turret number, turret 0 is standard arcs running towards the left side XZ spindle orientation found on 99.9999% of lathes. if you set turret 1, then it reversed the g2g3 arcs AS IF they were facing the spindle heading toward the right.