Parallel toolpath using touch surfaces cuts into the part itself

[jw.hendy]

I originally posted this report in Fusion 360 Manufacturing thinking I'd chosen the appropriate subforum, but I now realize that Support is the place for bugs. Since I already described the problem there, I thought I could just link to it and re-summarize:

• I wondered if I could drop a tool change by running a mitered cut using a parallel toolpath and a flat end mill vs. a 90-deg v-bit as I've done in the past. Here's the toolpath:

• It looks fine, and worked great except that the toolpath Fusion generated surprised me: after it ramps up the miter, it extends horizontally below that horizontal surface and into the model itself. It doesn't look like it, but here's my machined part:

• after this happened, I zoomed in on the file to see this from the side (dotted line showing that horizontal "shelf") in both pictures:

• the entirety of dialog in my post in Manufacturing amounted to being told this was predestined to happen because only an idiot with a $200 setup would use a flat mill to machine a 3d surface. A ball end mill is the obvious tool for the job (even though it's not) and that would solve all my problems. Of course Fusion couldn't handle what I did above. /s
  
  Except, a ball end mill does the same, but just doesn't traverse as far into the part. Here's zooming in via the simulation on the same edge as above, but using a 1/4 ball end.

My original intent of posting was to understand why in using this strategy Fusion would ever create a toolpath that hits the model itself. I'm of course familiar with instances where the path and tool chosen won't reach some area, but I've never run into Fusion generating a path that machines the final part.

I would boil this down into the following, which strikes me as a bug. One hypothesis from the other thread was that when using touch surfaces, Fusion basically ignores everything else. I could see that (and learn to adapt to it/remember this moving forward)... but also think of that as a bug as it's technically clipping off the top portion of that selected surface by machining it away.

Thanks for taking a look and for any clarification on why this happens. Part is attached with three parallel toolpaths: one is my original using touch surfaces and a 1/4 flat end mill (non-suppressed), another replicates with a 1/4 ball end mill (ball, suppressed), and my final workaround is using avoid surfaces which stops the end mill right at the top of the miter and does not traverse horizontally (avoid, suppressed).

[HughesTooling]

If you change the tolerance to 0.001mm it looks OK to me. I guess with 0.01 some passes are at top limit some bottom so you can see the total deviation. Also machining in both directions is quite likely to showup any problems with the machine (backlash and rigidity).

[HughesTooling]

Personally if I was machining something like this I'd create some oversize surfaces and only machine the angled face like this. File's attached.

[HughesTooling · Accepted solution]

When I post your original code and inspect in NC Corrector it shows there's only a 0.003mm deviation between the worst pass and the contour you use to finish the face. If you're seeing more than this it's going to be down to the both ways machining and machine accuracy. Could even be the control and constant contouring rounding the corners.

[jw.hendy]

Super interesting findings. Thanks for taking a look! Sorry, I've not heard of "control and constant contouring" before. Is that something in Fusion, or the way that the machine processes the nc instructions?

I'll take a look at the sample file you shared momentarily, and thought the comment about cutting both ways was was really intriguing. I'm using a downcut bit, so perhaps the direction change is sufficient to pull things down there when the direction changes? With the look of the parts I certainly did not expect this was the result of only 0.003mm in the generated code! Overall this was nothing catastrophic by any means, but I have another miter frame that sits against it, and this yielded slight gaps in the corners.

[jw.hendy]

Oh wow. I've never heard of CAM surfaces. This is amazing and exactly what I imagined, though I was thinking of it as a workaround to a "real" problem in the toolpath. I now see it as a workaround to a surprising level of z deflection I just saw due to what I'll chalk up to this combination of tool and path direction.

As an aside, makes me want to cut this with an upcut bit and see if that indeed changes the result significantly. Thanks for the assistance!

[jw.hendy]

Learning even more! Without studying super closely (like the zooming in here), I have only observed the avoid/touch clearance box appearing to affect avoid surfaces, but perhaps in this instance that 0.01 vs. 0.001 setting ends up mattering more? It looks like ultimately you didn't use that strategy (going with the CAM surface + using that as the model). Was the comment about clearnace more of an observation about my initial approach with the touch surfaces? Thanks again.

[HughesTooling]

---

@jw.hendy wrote:

Learning even more! Without studying super closely (like the zooming in here), I have only observed the avoid/touch clearance box appearing to affect avoid surfaces, but perhaps in this instance that 0.01 vs. 0.001 setting ends up mattering more? It looks like ultimately you didn't use that strategy (going with the CAM surface + using that as the model). Was the comment about clearnace more of an observation about my initial approach with the touch surfaces? Thanks again.

---

Yes I made that comment before looking closer, I've seen the total tolerance error cause problems myself but don't think that's the problem here as the max error seems to be only 0.003.

Looking closer now I wonder if the problem is where the tool plunges as it swaps direction, it will load up the machine and as it reaches depth it could over shoot as any flex in the machine is released.

[jw.hendy]

I'll try this on a test piece with only climb milling. If that greatly improves, I think indeed I'll resolve this in my mind as what you've observed. I think the downcut would not help the situation as you're describing what happens (changing direction and now the plunging comment). Thanks!