Adaptive toolpaths with C110 copper on the Nomad 3

CNC Machines Nomad
1

I had a brief exchange about this with WillAdams through the support email, but figured that I’d like to discuss it further to learn more about my several misconceptions.

I’ve been exploring adaptive toolpaths in Fusion, having so far used Carbide Create 99% of the time. The default settings with the 3D adaptive toolpath seemed all too aggressive, especially the stepdown, so I also had a go with HSMAdvisor to evaluate doc, optimal load and feeds. C110 is arguably not a very good material to go to work with, being gummy and tough, but at this point I just want to try to figure out where I’m going wrong.

What I’m milling is a 30mm coin. The adaptive clearing seems rather straight forward, but I take it that’s where my first misunderstanding is. I tried with a #274Z, single flute cutter at 24k rpm, 41 in/min feed rate, around 10 in/min plunge, 0.0125 in optimal load, 0.035 in maximum stepdown, helix ramping 2 degrees. I’ve got a rather strong shopvac pulling air past the workpiece and end mill, so I figured that would help cool it.

About 1 minute into the operation, the mill broke clean off, during a rather mundane clearing after the second ramp. I figured I’d gone too fast, so I dialed it back to 20k rpm, 34in/min, same stepdown and optimal load, on the same coin. I believe this operation held on for a little bit longer, obviously having milled in thin air for most of the time, but that one snapped as well. No screaming, no particular warning, just milling along one moment, then broken in the exact same spot on the end mill in the next.

So I don’t really get why this is happening. According to HSMAdvisor (which I’ve seen that people here say isn’t suitable for the Nomad 3), there’s no major load on anything with these parameters. Is 20/24k rpm too fast with #274 and gummy C110? Am I not feeding fast enough, and causing work hardening?

2

The F/S app I use recommends 19000 rpm, with a feed rate of 26 ipm, at .035 doc.

1 Like
3

That is interesting. What app is that, and is this for an adaptive tool path, single flute end mill?

4

I use the android version of this, https://app.fswizard.com/ and I used the setting for an 1/8", single flute carbide endmill, coated. There isn’t an option for adaptive cutting paths, so I use the results as a recommended starting point, and adjust from there depending on chip size and sounds. You don’t mention it, so I assume you’re not using a cutting fluid, That would really help alot.

5

And I use the Pro version of FSWizard, as it has a larger list of materials.

6

Re cutting fluid I did use a bit of CRC 5.56.

What’s confusing me here is that the chip load of your operation at 0.00137 isn’t that far off from mine at 0.0017. The DOC is equal to mine, and the optimal load / stepover is the same as in wmoy’s videos cutting copper.

My best guess so far is that I’ve managed to harden the copper with the operation, but I don’t understand that this relatively cautious spproach could do that?

7

20000+ sounds too fast to me. I cut aluminum with a 1/8" O-flute at 15000, 1/4" at 12000
For adaptive I use a step over of 0.010" with the 1/4", 0.006" - 0.007" with an 1/8"
I use mist coolant, but it’s turned down to where I can barely see the mist. I’ve help a piece of paper in front of the nozzle to make sure I’m getting some coolant.

Adaptive is meant for a decent size DOC, with a very small stepover and a higher feedrate.

My guess with that gummy copper is heat. Pause it after a minute or two & check the temp of the tool.
As soon as the smallest bit of copper sticks to the tool… snap!!!

If you can’t use coolant, try air blast. I don’t think vacuum/dust collection is going to draw the heat away quick enough.

Another possibility is the adaptive toolpath is not following the cardinal rule of “Never, Ever exceed the stepover!!”. Some older trochoidal & adaptive toolpaths will create corners that increase the engagement of the tool. The stress multiplies exponentially. An adaptive pattern should look something like this. no sharp corners, smooth transitions into the material, and never exceeding the set stepover.

image
image1054×621 29.3 KB

1 Like
8

What is your feed rate at those rpms?

You’re likely right about my rpms being too high. It was frankly based on the aluminum numbers from Carbide Create, and didn’t seem too off when those were moved into HSMAdvisor. There’s also been no heat when I’ve paused and checked.

I just reran the gcode which broke the second (well third) #274 yesterday, using a two flute, 1/8, non-coted, random China end mill, and that worked OK-ish (more on that in a second).

What I now think, though, is that the ramping down is a little aggressive, and that this causes the machine to lose its Z-point. During the two flute re-run, I noticed that about half way through the operation, the Z was off by about 1 mm, causing it to churn all too hard. I now need to figure out where this issue comes from.

1 Like
9

I can crank a 1/2" tool up to about 120 IPM, 1/4" tool up to 90, and the 1/8" maybe up to 60.
That’s with a DOC of about 0.8 - 1.0 x Cutter Dia.

10

The first question I think needs to be answered is: What is the temper of your copper? If it’s softened/annealed fully it doesn’t matter if you have the ideal alloy, you’re gonna have a miserable time.

Also, as @Vince.Fab has demonstrated in many cases, sometimes you gotta throw out the textbook. Deep DOC might be how Adaptive is “traditionally” used. But in a lot of lighter-weight machines, shallow DOC with wider stepover can be much more effective.

3 Likes
11

If only I knew the answer. This is, sadly, rather random “T2” from China, and the closest I can tell is that it’s C110. Even that is a guess though.

Something I do find strange is that I’ve seen Z drift consistently down doing these adaptive toolpaths, both with a random two flute 1/8 and a 112z. This seems to suggest that the Z motor isn’t able to move the spindle up, skipping steps? Which seems weird, since the retracts should be happening in the open, with no walls adding load. Is this a common problem with potentially gummy material, or am I seeing some other mechanical/electrical issue?

12

Do the cut edges have any ugly quality to them? Example of a “bad” cut here: https://www.youtube.com/watch?v=rm-qSytjFnI
That would indicate the material is inherently difficult to machine, rather than the CNC not being able to handle it.

And have you marked an endmill with a sharpie to ensure there’s not any slippage in the collet? It’s not likely that the Z-axis is drifting unless there’s something wrong with the machine mechanically or electrically. That is of course still a possibility, but best to exhaust all avenues of inquiry that can be answered without more invasive analysis of the machine…

3 Likes
13

Yes and no. With the 274 and 112Z I’d say the edges were pretty much perfect. The random two flute is another story. I think it’s safe to bet that this material is troublesome though.

The endmill isn’t slipping, I know that much. At the same time I can’t say that I find it likely to be an issue with the machine itself, because it has none of these problems doing aggressive adaptive toolpaths in hardwood. I take it I’d see Z drift there too, if there was a mechanical or electronic issue.

14

I’m starting to think that there’s something else at play here, and that the mills didn’t break because of the material being difficult. The copper alloy certainly isn’t optimal, but considering there’s no heat, no unclean cuts and the numbers aren’t completely crazy, I’m reluctant to blame it entirely on the mat.

Exploring the strange downward Z drift further, I just re-ran the gcode that broke the last #274, without any material. The calibration, that is X Y Z, is the exact same as the run that broke the end mills, to replicate any possible coordinate local issues.

Around half-way into the run I started noticing a thumping sound when the Z axis stopped downward movements. I’d heard the same, and stopped, a semi-roughing run with the 102Z a few days back, on the same coin. In that episode, the 274 roughing went fine, but when I stopped the semi-roughing after the thumps, I noticed that Z had drifted down, and that considerable chunks of not-to-be-milled material was gone.

So back to the empty run just now, I heard the thumps, but saw no cause. There was ample room to go further down on Z, and nothing was blocking anything. I stopped the run, extracted the header and surrounding movements from the gcode, and re-ran just that. No thumps. The positions were exactly the same – I checked extensively – but whatever caused the thumps in the first empty run did not manifest in the second, isolated, empty run.

Video and audio of the thump (note that the audio is slightly out of sync here): https://youtu.be/ixR0FfD80x0?si=14wHzu6HJfP0d6Wo

Video and audio of no-thump: https://youtu.be/aA-Exc3TG8Y?si=PazDw9_8y6uwhezY

Any takes on what’s going on here, and how this may relate to the drifting Z?

15

I think I found part of the issue: Carbide Motion 635. The toolpaths were, in general, very jerky, but I thought it was part of the adaptive cycle.

I just upgraded to 636, and the jerky motions are all gone. I’d be unsurprised if this was what actually broke the three #274 mills: Jerky motion that put abrupt strain on them during what was meant to be smooth motion arcs.

1 Like
16

I don’t think there was any change in how CM ingests toolpaths between 635 and 636. Something as minor as your computer installing updates in the background could cause that jerkiness, so I would check to make sure you have Smoothing enabled in Fusion. That makes the Gcode it produces more efficient to process.

2 Likes
17

Also, very difficult to ascertain with such a short video clip. I couldn’t hear anything relating to the Z-axis, maybe I need headphones. But are you using any ramping or other techniques to ease entry of the endmill into the material?

1 Like
18

I didn’t change the toolpath. The gcode file I tested with was the same on every go. The computer had also been rebooted multiple times over the course of the testing, as well as complete power cycles of both computer and Nomad. Automatic updates is disabled, and I monitor PC load extensively. My actual trade for 20+ years has involved system and driver level development, so while I’m improvising my way through CNC, that’s not the case for the computer side of the setup :grinning:

1 Like
19

The sound is likely difficult to pick up without headphones. It’s a soft-ish sort of bump, which happens after rapid moves (into open slots, the ramping operations are slower and without thumps). Since there’s no material being milled in the videos, that sound does not come from the cutter hitting anything. I’ve also confirmed that there’s nothing actually colliding anywhere. All in all it sounds more like stepper coils being powered, but that seems slightly weird after rapid moves which included Z, as I don’t think you’re powering the Z stepper off and then back on at the end of a move?

20

If you grab the spindle with the machine powered on but idle and push/pull it vertically, is there any discernible play? Maybe one of the anti-backlash nuts got loose? If it’s a basic mechanical fix, that would be good, but otherwise you might be best served reaching out to support if you’re not sure.

Edit: Also, what ramping angle are you using?

1 Like