Smoothing With Acorn or Fusion or Both

[CNCMaryland]

I use Fusion 360 for all my gcode, and utilize the smoothing option on all toolpaths, smoothing to .01mm.

Acorn has its own Smoothing parameters, and I am using those as well, but not sure what I should be doing, so.

So, should smoothing be done only using the option in fusion, or only using the option in Acorn, or both?

Thanks in advance.

[Crosshatch]

Hi,

I'm definitely not going to be able to answer you in full because I have a thread about this a couple posts down.

Here is what I know from my experience. My Acorn was originally set at "Exact Stop". This gave me poly contoured arcs and the machine would jitter doing these arcs. I tried all sorts of smoothing in the CAM, but smoothing helps with splines and not so much with a radius contour. I still have it checked though in the CAM.

So what happened? I changed Acorn to Precision Machine F2 smoothing and all those arcs now are smooth and clean. Machine "moves" alot better and rightfully so without "exact stops" (bang bang bang). Having said that, as my thread mentiones...ramping and feedrate has been increased which is NOT what I want in ramping or contour moves (despit not being poly).

I'll hopefully get that sorted out this weekend.

As always, the Centroid moderators will want a report of your controller settings, so post it up.

Regards,

Jason

[CNCMaryland]

Hi Jason,

I appreciate the reply. Currently I have it set in fusion for smoothing at .01mm. I have the smoothing in acorn set to F2 - Precision Machine as well, have on arcs I am experiencing the polygon effect. Machine movement is very smooth, no jitter, nothing. This is only noticed on sweeping arcs. Circles are perfect.

I'm wondering if a better smoothing preset would be the answer for me, but I just don't know.

Greg

[Crosshatch]

Interesting, F2 Precision Machine smoothing eliminated all the poly arcs I had problem with, less the increased feedrate at those arcs.

Again, create a report and post it (need to do the same in my thread).

Regards,

Jason

[CNCMaryland]

Hey Jason - What CAM are you using out of curiosity?

What materials are you cutting?

[Crosshatch]

Inventor HSM express and Fusion 360.

Aluminum, plastics...mainly aluminum.

Regards,

Jason

[cnckeith]

depends on what the Fusion 360 smoothing is actually doing.
post g code with it and without it of the exact same tool path and take a look.
cnc12 smoothing works best with short vector 2d or 3d g code files and a good CPU with single thread bench mark of 1200 or higher.

[CNCMaryland]

Thanks Keith, that is my first plan of action tonight.

I'll be sure to report back.

[agsweeney1972]

I use Fusion 360 for all my gcode, and utilize the smoothing option on all toolpaths, smoothing to .01mm.

Acorn has its own Smoothing parameters, and I am using those as well, but not sure what I should be doing, so.

So, should smoothing be done only using the option in fusion, or only using the option in Acorn, or both?

Thanks in advance.

A smoothing tolerance in Fusion of 0.01mm (0.0003937 inches) is not going to smooth out anything unless you are making watches. You need to open up that tolerance if you expect Fusion360 to do anything at all with the path to blend arcs and lines.

In my experience with smoothing on the Acorn it will not likely do what you want it to do. I have spoken with Keith about this and it is undesirable in my use case which is a CNC plasma. The increased feed rates during a "smoothing move" by the controller are unpredictable in my opinion and should not be used in general cases.

Motor tuning is far more important to get a handle on before you try to "fix" an issue caused by poor mechanics or poor tuning with smoothing (trust me I tried that!). There are some magic settings under the hood that Keith might privately and on a case by case basis suggest you work with that are clearly labeled DO NOT MODIFY. In my case I not only modified them but did so grossly until I was satisfied with the performance at 500IPM+ cutting feed rates.

[Commotion]

Smoothing in fusion I find is mainly to reduce file size and data points for old machines. I have a ‘96 mazak vtc at work and I have to run real loose smoothing tolerances therwise it sounds and looks like it’s having an epileptic fit. I found cnc12 can process the data plenty quick enough and doesn’t need smoothing in fusion360.

In my bit of playing around with my acorn I usually leave smoothing off in fusion and run smoothing in cnc12. I was having troubles with the servos accelerating and decelerating during non engagement feedrates at small arcs. I sped up the acceleration on the drives to the point it was banging and jittering at each point. Selecting smoothing in cnc12 got rid of the banging. Oddly enough the line of code it was getting hung up on was a G03, all lines before it were G01 so having smoothing on in fusion would have done nothing.