Unwanted ripple on baltic birch edges

[samgaddis]

I'm cutting baltic birch with a CAMaster Cobra (very sturdy CNC) with an onion skin method and am ending up with ripples in the edge as shown in this image. I've tried adjusting smoothing and tolerance to .0001 in Fusion 360 to no avail.

My suspicion is that it has something to do with the toolpath setup because I can see the machine sort of jerking its way through the cut. Also the bits are fresh Amanas and the machine is tuned well (I think). 

Feeds and speeds are:

1/4" downcut - 18k climb cut at 450ipm. Leaving .05" for a 1/8in to clean
1/8" compression - 18k conventional cut at 180ipm

[Laurens-3DTechDraw]

Is the 1/8 taking material off?

Or are you not sure?

[samgaddis]

Great question - the 1/8" is taking off a tiny bit of material, but not because of radial stock to leave on the 1/4. Rather, it's because the 1/4" is a climb cut which deflects the bit slightly away from the material. Then the 1/8 conventional comes around and cleans it up. This usually leaves great looking edges, but apparently not on this curved spline.

By the way, this particular onion skinning method was recommended by someone on the CAMaster forums. 

[friesendrywall]

I'd say its a control issue, in that 180ipm is pretty fast for little segments, and its probably choking.  If it was Haas, I'd say you needed HSM for this, I'm not sure what the equivalent is for you.

If you can play with smoothing to get fewer segments that may help.

[samgaddis]

Are you open to elaborating? For instance, why did you say 180ipm is fast when the 1/4" pass is actually at 450? Also, how exactly would you adjust smoothing? 

[DarthBane55]

If I might.  See pictures below.

Also, I would code it and look at the code to see if the points are arcs or lines.  Line to line moves will most likely result in some faceting on the surface machined, as arcs would do a smooth surface finish.  If you have lines, make sure you have a lot of them, with a very tight tolerance, so make sure the tool can sail thru them smoothly and not create say "0.1" long lines on the face, that would be really coarse faceting.  

Hope that makes sense.

  

[friesendrywall]

180 ipm may not be perceived as fast from a cnc router perspective, but depending on your control's corner rounding setup, it has to slow down to make those tiny corners.

It takes a fast control to do things smoothly at speed.  For example, if your control does 1000 blocks a second, at 180 ipm / 60 / 1000 = 0.003, so the machine travels 0.003 before trajectory is recalculated. That is probably irrelevant to this though. It has more to do with how your control software handles these short segments.

Elliptical stuff can be shoe horned into smoothed circles, but there is some point on small radiuses where it doesn't work any more.

[samgaddis · Accepted solution]

Ok I figured it out through the help of a local CNC guru and the problem was actually nothing suggested here.

Turns out Fusion 360, hates splines. The machine was cutting lines instead of acrs which explained the jerkiness.

To remedy, I used a Fusion plugin that converts the splines to polylines and then re-did the CAM on the resulting DXF. It's another step in the workflow, but the machine runs so much smoother and the results are perfect.

Fusion plugin is here: https://apps.autodesk.com/FUSION/en/Detail/Index?id=4611814297957846949&appLang=en&os=Win64&autostar...

[DarthBane55]

Sorry, you don't need a DXF.  See picture below, this is a spline, and I set the tolerance to 0.001, and the smoothing to 0.001, and it did arc fitting and the code is all G2 and G3.  So the solution was in fact as per something someone had suggested, but you didn't bother trying.

 

[samgaddis]

Actually smoothing and tolerance values of .001 were the first thing I tried. Not sure why you are getting different results than I am. 

[DarthBane55]

It will vary depending on the curvature of your spline.  That's why showing the points in simulation helps to see if it's going to be point to point or arcs quickly, before posting.  Still have to confirm in the code, but usually line to line would show a loooot of points close to each other, and arcs would have the points at a reasonable distance (this is just to have a quick look).  So tolerance and smoothing need to be tweaked depending on your spline curvature.  Anyways, it can do this.

[nhfoley]

Hey @DarthBane55 jumping in here as I found this thread due to having a similar problem (CAMaster machine choking on G2/G3 moves from Fusion), and I suspect it's something similar to what you are describing & trying to fix. 


However, ignoring the CAMaster part for a bit, I can't even get Fusion to smoothly convert spline curves into arc segments as you show, even with very large tolerances allowed. Here's a 15mm curvature continuous fillet being turned into a toolpath, and the very tight point spacing Fusion is generating:

This is what is being generated even when I have set my tolerance and smoothing values for this operation to 0.1":

Is there somewhere else that a global tolerance might be over-riding my settings here? Am I doing something entirely else wrong? Thanks.

[DarthBane55]

@nhfoley 

Hi, so this is not a spline if I understand, it's a fillet, radius 15mm?  What operation is it 2d contour?  Is the plane where you pick the profile flat, or is it tilted? (can't really tell from the picture).  If it is tilted, then the fillet where you pick it becomes a spline as it is not a radius anymore due to the angle (if you measure it, at the spot where you picked it, it will not return radius 15.0mm).

That is slightly different than the original problem posted in this thread, but (again, I am making a lot of assumptions on your case here), usually to cure that issue, I have 2 solutions:

1-I create a 2d sketch on a plane that is square to the fillet, and use project edges to project the fillet.  It then becomes radius R15.0 again (you can make sure by measuring it).

2-I create a plane that goes thru the fillet, but is square to it, and use "intersect" to make a slice of the fillet, which again can be measure at R15.0.

I think a spline that is planar, and a 3d edge, are dealt with differently in Fusion.  This makes me wonder if the original case of this thread was in fact not planar.  If it was not planar, @samgaddis  could have sliced it to make it planar and obtain success in smoothing (arc fitting) the spline.

If my assumptions in your case were completely off, could you clarify what operation you are using, and if the fillet is planar where you pick it, or 3d.

[nhfoley]

Hey! Thanks for the input. However, this is indeed a planar curve, and it is not a circular radius, as it is a curvature continuous fillet. That should make it a spline curve. The operation to generate this toolpath is a 2D Contour, as you suspected. 

I think this issue is actually fairly similar, maybe the same, to the issue that started this thread, as it seems like the root problem is that Fusion is taking spline curves and chopping them up into very dense, maybe slightly discontinuous arc movement commands that choke up the motion planning of a CAMaster machine, causing it to move unevenly through corners and cause the rippling effect that the OP documented. I spoke with CAMaster about this yesterday and they confirmed that it seemed to be an issue in Fusion 360 and the toolpath generation, not the acceleration or jerk settings of the machine itself. 

My only working solution presently is similar to what @samgaddis implemented, though I accomplished it by turning off arc moves in the post processor so that my programs generated by Fusion are only very dense line segments. This allows the machine to move as expected, and eliminates the jerking and stalling happening with the arc moves Fusion generates. (In my case as an example, fixing the stalling issue on the file I screenshotted above caused the job time to decrease from 30 minutes to 20 minutes, all feed rates kept the same, which is a big time savings and means the I've eliminated a lot of burning & rippling in the workpiece.) This is a clumsy solution, though, and I suspect will turn into impractically large gcode files once I start doing 3D work on large objects.  

[DarthBane55]

Ok, I understand the issue with the actual machine (probably doesn't have a smoothing or high speed function).  You got a good solution then, that's great.  3d work will always give point to point, so basically you would get large files no matter what in the case of 3d surfacing.

[samgaddis]

Whoa! This sounds like a much better solution than the cumbersome one I have. May I ask how you went about turning off arc moves in the post processor? 

[nhfoley]

I do it by setting the minimum chord length and minimum circular radius to some arbitrarily high number  in the Property window of the post-process menu. 20 seems to be good, seems like the PP measures in mm regardless of your document units. I still get lags when running files with large arc moves (say, cutting a 2" radius as on a corner), but it's less of a problem there. If it ever becomes one, I'll pick a higher number. Probably will bug CAMaster about this more in the future as it really seems like a problem with the motion planning, not the toolpath generation.

[samgaddis]

Dang, I had high hopes for this. I changed the post processor settings per your recommendations but the problem actually got a little worse. Left slice is before change, right slice is after. 

[nhfoley]

Did you examine the gcode to see how things changed?

[samgaddis]

I opened them but honestly I'm not sure what to look for and how to go about comparing them. I'm a bit of a novice when it comes to exploring raw gcode.