Hello, I have a model with horizontal and vertical planes, both with slight inclines (not perp to each other) that I have added a 12mm R fillet to join the two surfaces. My problem comes not from the drawing of the surface fillet, but from when I run RhinoCAM. In theory since I am running a horizontal finish step around the object, the bit should be running at the same z height for the full trip around. RhinoCAM is looking at my model and sees when it is cutting around the fillet, the z height changes enough that it cuts in segments, not in arcs, making my machine not run smooth so I need to cut feedrate in half. My guess is when I built the fillet, it is segmented, not truly round giving me the change in z height. I have tried rebuilding the surface fillet, using the surface fillet tool, and making my own fillet with a sweep2 rail. You can see in the picture the light blue lines are segmented line cuts, and the dark blue are arc cuts. (The blue lines show the path of the tip of the router bit, I did not put those in)
Any suggestions so I can change how I build this so I can achieve arcs instead of line segments?
Here is Tech support from RhinoCAM explaining why I am getting line segments instead of arcs.
" The Z values on the linear motions do not appear to remain constant as it follows the radius. The toolpath is generated based on tool & part geometry based on the contact point. So you are unable to see arcs being fit at a few Z levels at the start of the path."
This is not your fault (or Rhino’s)… to be brutally honest, this has been a problem spot for RhinoCAM for as long as I have been using it - I complained about this and similar behavior years ago. The problem is (IMO) inadequate filtering of the Z values gotten from the toolpath calculation mesh (toolpaths are generated on meshes made from the NURBS surfaces, not the surfaces themselves). The minor variations in Z - usually well below that of the file or operation tolerance - prevent the arc fitter from working. if you look at the gotos in your toolpath, you can see variations in Z of a couple of tenths of thousandths - way below the operation tolerance of 0.01 and the file tolerance of 0.001.
This also affects a number of other 3D operations and yes, depending on your machine, can induce stutter. This problem is eminently solvable - the proof is that 20 years ago I was using another CAM program that could do this all in arcs with no problem. RhinoCAM is a great program, but sometimes it is frustrating to have to avoid or use workarounds for the weak spots or simply accept them…
Update on that, as you have turned “Optimized XY Machining” on under cut parameters in horizontal finishing, this is introducing linear motions for the part in question. Turning off Optimized XY machining & regenerating the toolpath should generate arcs around the fillet.
I confirm unchecking “Optimized XY Machining” produces smooth arc paths without the linear motions for this file in RhinoCAM 2019. Would a user adjustable z tolerance make sense?
No, having a separate Z tolerance will not help because this behavior is not tolerance related. What the optimized machining algorithm does is identify areas between successive Z levels where the tool can create projected toolpaths. In order to minimize these areas making the step down values between successive Z levels smaller will be the only way to do it. In this particular case, the optimized machining is not necessary at all and can be safely eliminated.