forum.cncdrive.com

I know there is not much support for turning yet but I want to use UCCNC for a small Emco lathe I have converted to UCCNC with the UC400ETH and I´m experimenting with Fusion 360.
However I have a problem with the G-code and UCCNC and got ARC ERROR but I cant figure out what the problem is?
Could it be that UCCNC does not support radius movement in the X Z plane?

I have attached a screenshot and the NC file.
Also, the toolpath seem to be somewhat of, the radius shoud not be that long.
If I select a postprocessor without arcs it work fine (like the UCCNC Generic post) but as soon as I use one with arcs like the posts for Mach3 or Fanuc I get the error.

Arcs are supported on all planes.
The UCCNC gives you an arc error if the programmed radius*2 is smaller than the distance between the start and the endpoint of the arc, because then the arc is not valid, it mathematically can't be defined.

I think you should check the CAM settings and try to set the arc tolerances tighter, because probably that will be the problem,
because I remember the same problem with Fusion which Autodesk later resolved with setting the tolerances lower in their post.

Problem solved!
The problem was that fusion was set to define the radius with the radius R, but UCCNC seem to want I J K mode.
Sollution: Set useRadius to NO.

Here are the postprocessors for mill and turn.
I have lowered the tolerance to 0.01mm
Changed use radius to false
Added turn capability to be able to use the postprocessor in a turn operation.
Otherwise its nothing special for turning in the turn post bit that will hopefully be added soon.

I corrected an error in the Millpost.