Cutting Maple with .25" cutter is VERY Loud

How To
1

Anyone have any experience cutting hard woods with a 1/4" cutter? If so, do you find it extremely loud? Like nearly as loud as a table saw? I’ve set my feeds and speeds, etc, based on the manufacturers specifications, and I’ve double checked with G-Wizard, but no matter what stepover, plunge rate, etc, I choose, it’s seems to have very little effect on the noise.

Are maple - and other hard woods - just noisy materials? Is a 1/4 inch cutter a great deal louder than one that’s 1/8"? Does RPM have a lot to do with noise? It suddenly occurs to me I haven’t tried changing the RPM - perhaps that’s the key?

2

Yep, it’s loud cutting maple with a .250" cutter.

However, one of the things you can try is, per your idea, upping the RPM.

With my .125" cutter, I’ve been using 8000rpm with a .035" depth per pass and 50ipm feed. It still makes noise, but it doesn’t scream like it does at a lower rpm.

3

Ok, so after I posted this I continued to do some research, and found this link, thanks to another thread on the forum. On that page they say:

Any rotating system has speeds where transverse vibration is at a minimum (nodal points) and speeds where the vibration is more pronounced, sometimes violently so (referred to as resonance points, like unbalanced automobile tires at high speeds). … To improve surface finish, minimize bearing wear, reduce the cutting noise level and preserve the life of your cutting tools, it is a VERY good idea to ALWAYS operate at a quiet nodal point.

They go on to describe a method for finding the “quiet” nodal points on your spindle, essentially by running it at different speeds with your hand on the top of it and listening/feeling where the quiet spots are, then recording these in a log. The full process is described on the page I linked.

Obviously we don’t have a knob for turning down the speed on the Nomad incrementally, so that’s not going to work. But would it be possible to write some g-code to achieve this task? I was thinking it might be worthwhile to try it, though I’ve got almost no idea how to go about it. Perhaps g-wizard editor? Before I bother monkeying around with things, I’d love to know if my idea seems reasonable/useful.

Would it work to start the spindle at max rpm (10k), run it for 10 seconds or so, then decrease spindle speed by 250, run for 10 more seconds, decrease again, etc? Can that even be done with G-code? For clarity it seems like it might be smart to set up the g-code to bob the cutter up and down along the Z axis a bit before it changes speeds. And it might be good to make several of these programs to test the spindles in 1,000 or 2,000 RPM increments - to help prevent losing track.

Is this possible? More important: is it worth doing? I’m a total beginner so please feel free to tell me if I’m barking up the wrong tree!

4

This is all reasonable stuff to do, but as we can agree, at the moment there isn’t an easy or automatic way to do it.

Writing custom G-code to do it would be reasonable to do, or to output a series of passes from a CAM package like the HSMworks integration in Fusion360 would work also. You’d just set a bunch of different 2D contour operations back-to-back with the same tool, but different spindle speeds & feed-rates, and you’d run it for ~2 inches per speed/feed combo, to see what’s ideal.

I don’t have time to program that up this week unfortunately, but maybe @Randy would be interested… :wink:

-Jonathan

5

Jonathan, thanks for the shout out :slight_smile: As it happens, I was already starting to type the below earlier but had only saved a draft…

Well, the precisebits.com link is talking about air-cutting to isolate the spindle itself. That is dead easy. After Carbide Motion measures the tool, it keeps the carriage up in the air. So the gcode just needs to start the spindle and control the RPM.

M3 S5000 (turn the spindle on at 5000 rpm (just for example)
G4 P4 (wait for 4 seconds while you listen/feel)
S5500
G4 P4
S6000
G4 P4
. . .
M5 (turn spindle off)

But actual cuts will be under different conditions (i.e. side loading of the tool), and full-width “slotting” cut (i.e. the first cut at a given level) will be different than subsequent stepover cuts (assuming you keep to the conventional 50% or lower stepover for roughing). And that will be different than contouring/finishing cuts, which are taking off only a few thousanths and will be more like the air-cutting but still in contact with the workpiece.

Another factor is that the Nomad is belt-driven. The belts themselves are like springs and will have their own resonant frequency when driven by the cut. While I was doing my step-glitch experimenting, I discovered it is not hard to flex the carriage back and forth by a couple thousandths of an inch while it was being held static by the motor. I haven’t used the Nomad enough yet to really have a feel, but I think that the optimum machining strategy might be to make very shallow passes at a high feed rate rather than deeper passes at a slower feed. People are experimenting with how slow they need to move to not stall the spindle or carriage at a given depth of cut but the cut will become inaccurate far before that point.

Rather than .035" depth of cut, maybe .015" depth of cut at a faster feed rate. On my Millennium Falcon I was going 20 ipm at a .020" depth of cut with the .125" cutter, maybe I’d be better off with .010" depth of cut and 40 ipm? CNC machines are very patient and methodical. That is a very early lesson I learned with my Sherline.

6

@Darren - I tried your settings, or close to them, and it’s still pretty darn loud. I think partially it’s the maple. All day today I’ve been thinking - so THIS is why they make instruments out of the stuff. It’s resonant as hell. What fun. :cry:

@UnionNine Thanks for the suggestions! I did something similar, but in a much less sophisticated way. As follows:
I had a piece of maple that I wanted to shave down from 24mm to 15mm, so I setup the same cutting job, the same way, with different speeds, and just ran them one after the other. I kept the depth and stepover the same, and only varied the speeds, feeds, and plunge rate, so that the machine used the same horsepower - according to g-wizard - for each iteration. I also ran a couple at MUCH higher depth and stepovers, matching the manufacturer’s suggestions, just to see what that was like. It was not nice.

Here’s my completely unscientific observations, for my 1/4" endmill from Harvey Tool, 72199-C3
Overall length: 2.5"
Shaft: .25"
Flute Diameter: .25"
Flute Length: .75"

I do think it’s interesting that the machine seems noisiest on the even numbered thousands - 4k, 6k, 8k. There was a definite difference in both the volume and the tone of the noise for the odd numbers. No idea why this would be.

Overall by FAR the greatest factor for noise seems to be depth and stepover. Everything else had marginal effects. I still plan to test for the resonance of my spindle, but really if I want my jobs to run quietly I’ll need to set the depth and stepover at no more than around 25% - at least for my 1/4" cutter in a resonant hardwood like Maple. And much less than that if I want to run it overnight without disturbing my kids.

To give you a sense of the sounds, here’s some video. The settings for these are listed in the table above. Pretty bad!

EDIT: these video clips don’t want to play here. I’ve made them into links. Hopefully this will work better.

Here it is cutting in small passes.

And here you can listen to it reach its full voice - takes a minute but eventually that wood starts to sing along and it’s pretty nasty.

7

@Randy Thanks so much for the code! I will try it out tonight and report back if I discover the perfect spindle speed…

Can you possibly please also tell me how I could make the cutter “bounce” down and back up by 1cm or .25" or something? I’d like to set it to do that every so often to help me keep track of how many RPMs have gone past…

Thanks again for the help!

8

@MrHume, the first thing to do is choke up on that endmill. The flexibility of the cutter itself goes up as you extend more out of the collet, and also provides more of a lever arm for leading forces back into the mechanism. It is always best to only extend enough of the cutter to just clear the stock/clamps when making the deepest cut. That itself will reduce the chattering. Of course, don’t clamp with the top of the flutes up in the collet…

Now to have the spindle “curtsy” each time the speed changes is a little more involved. Just running the spindle was unit-agnostic, but now it will make a difference using mm or inches when making actual movements. And it will be best to use relative motions since we don’t know where the homing/length initialization left the cutter.

So for mm we’ll use

G21 (set mm units)
G91 (set relative coordinates)
M3 S5000 (turn the spindle on at 5000 rpm (just for example)
G0 Z-10.0 (move down 10 mm from where it is)
G0 Z10.0 (move up 10mm from where it is now, so back to where it started)
G4 P4 (wait for 4 seconds while you listen/feel)
S5500
G0 Z-10.0
G0 Z10.0
G4 P4
S6000
G0 Z-10.0
G0 Z10.0
G4 P4
. . .
M5 (turn spindle off)
G90 (set back to absolute coordinates for safety)

and for inches we’ll use

G20 (set inch units)
G91 (set relative coordinates)
M3 S5000 (turn the spindle on at 5000 rpm (just for example)
G0 Z-0.25 (move down .25" from where it is)
G0 Z0.25 (move up .25" from where it is now, so back to where it started)
G4 P4 (wait for 4 seconds while you listen/feel)
S5500
G0 Z-0.25
G0 Z0.25
G4 P4
S6000
G0 Z-0.25
G0 Z0.25
G4 P4
. . .
M5 (turn spindle off)
G90 (set back to absolute coordinates for safety)

1 Like
9

Thanks @Randy, I really appreciate it!

Unfortunately that cutter is already bottomed out in my collet - the only thing I can do is to try taking my dremel and a stack of cutoff wheels to it and see if I can’t shorten it - but this seems a bit drastic. I’ll order a new one - maybe Carbide 3D will have some .25" back in stock soon… :grin:

10

I see that you have been diligently testing and working on finding a solution and know how frustrating it can be but,
1 thing you need to keep in mind when finding that sweet spot is that each parameter is relative to one another.
For example, if you are running the machine at 40 ipm for every test run you do only changing the Spindle speed youre not going to get much of a different result.

40 ipm is probably too fast for this material seeing as you are going to have a Max spindle speed of 10,000 rpm.

Start at a high spindle speed with a low Feed rate and then start slowly boosting the Feed rate after that.

The nomad is a small machine lacking in rock solid rigidity which is limited by small cutters and spindle speed, there will be no way to eliminate vibrations past a certain level cutting something so hard.
The faster you run, the more vibrations in all components in the machine, also this can bend and break carbide bits like dry noodles.

Maple is one of the hardest most dense solid woods there is so this is something that you are going to have to take your time cutting with your set up.

But I would think that you could get the noise levels down to acceptable by more experimenting.

11

Well MrHume,

I have had the pleasure of experiencing first hand your dilemma

Over the past few days I have been trying to machine some simple parts using some pieces of Walnut I have.
I just got in some new .25 cutters this past week and was ready to rock using these for my roughing passes should speed up my machine time----- IN THEORY

So I set up my file in MeshCam with what I thought would have been completely appropriate Feed, Speeds and Depth of Cut for what I was machining.

First Try, Attempting to cut 3/16" depth of cut, 8000 RPM, 50 IPM…
Result - Completely Stopped the Spindle, clang, clang - I was shocked.

Second try, 10000 RPM, 40 IPM
Result - Spindle stopped dead - Oh My God

3rd Try, Reducing Depth of Cut to 1/8", 10000RPM, 40IPM
Result - Jammed

Long story short by the time I actually got a tool path that would run I had to drop the depth of cut to a 32nd of an inch at 10 IPM Feed with a Plunge of 5 IPM and even then it was really growling.

This is just Walnut, I mean I am intending to machine exotic hardwoods and laminations that are far harder and Im seriously doubting that this spindle can handle it.

With these parameters it took about an hour and a half just to rough out the material in 1 small pistol grip, then when I did the tool change to the ball cutter for the finishing passes the machine went the opposite end of the material, plunged full depth and completely stalled the spindle out.

Wasting my material and all of that time.

I didnt really consider it at the time when I looked over the specs before I received the Nomad 883
but a max spindle speed of 10,000 RPM is really slow compared to even a trim router.

My DeWalt trim routers Minimum is 16,000 RPM with a Max of 27,000.

I didnt think much of it based on all of the Design Hype that went into this machine but I feel like this was something that was totally overlooked.

Another thing that I am noticing is the Extreme amount of heat that builds up in this spindle.
It is almost hot enough to burn after running it just for a short time.

I have been running an Industrial Sized, Thermwood router for 5 Years, Its my career, so its not like I dont know what Im talking about,

Is anyone else experiencing these issues ??

12

Try again with a 1/8" cutter. I’ve been able to use a 50ipm feed and a .040" depth per cut with no issues.

And I mentioned this in the other thread, but you should try cutting 1/2" off the end of your .250 cutters so they stick out less from the collet. I’m actually gonna give that a shot and see what the results are.

One other thing to consider - how are you securing the stock to the table? I would often run into issues when I was using the carpet tape supplied with the machine bc it wasn’t strong enough. I picked up some duck tape brand carpet tape and it has been much better.

However, if the wood is warped even a slight bit, the tape won’t do much to avoid messing up a job. I’ve had this happen a few times with hardwood that was totally straight, but must have picked up some moisture in my shop bc a week later it wasn’t perfectly level.

For me, the solution has been to order up hardwood blanks in 8" x 8" x 0.5" and drill holes so I can secure it to the wasteboard. The bolts are m6, and I believe the length I’m using is 20mm. When I bolt the wood down, I never have a problem with the cutter skipping or binding.

Eventually I think a table upgrade would be a great product improvement - one that has built in tracks so we can use hold down brackets for our stock.

13

I had the tool buried all the way into the spindle shaft as far as it will go.

I seriously dont think that has anything to do with it

There is no way this little machine has the force to cause a .25" bit to bend, if anything Id say some other component in the assembly would flex first.

I run a Full Size Thermwood Router for a living and I run 1/4" Cabride bits at 3-400 IPM No Problem

I just dont think that spindle can handle it, plus we generally use 2 Flute tools, these .25 bits from Carbide 3D are 3 Flute bits so Im not sure if that has something to do with it.

All of my stock is professionally prepared, it is Joined, Planed, and Ran through a wide belt down to the thousandth.

I work in a Cabinet shop and am the Router operator

I have been using carpet tape but I dont see that being the problem when the spindle is dying in the first plunge at the highest spindle speed it is capable of.
Its not like it is pulling up off of the table and getting bound some how.

The method you are using is probably the best way you can secure anything to this table, Ive used that technique many times before.

I have a large vacuum table on my router at work, wish it was possible with this.

In my case Im doing something very simple and it should not be putting enough pressure on the stock to be able to move it with the tape alone.

Carbide 3D does offer that Vise that would hold it very tightly but its $120
I havent been able to choke that up yet.

14

@Darren

I just ran the same part using my 1/8" cutters and you are absolutely right,
I was able to run them Deeper and Faster than the 1/4" tools and that shouldnt be possible especially if bit flex was in fact a factor.

50 IPM Feed and .040 Depth Per Pass with the 1/8" cutters
vs.
10 IPM Feed and .030

I still hold my opinion that the spindle doesnt have enough power to remove the amount of material that one of the .25 bits would remove so it just gets stuck in the wood and stalls the motor.

Too bad

Ill be interested in a return in the cutters, collet and nut I just bought

15

Yeah i can confirm, i just tried your settings that you described as ‘Pretty Good - […]’ and they worked to cut through Sapele, but there were times where i thought the spindle stalls any second because of the noise it was making.

Maybe @ApolloCrowe knows the correct settings? :smile:

16

The 1/4" cutters in the Nomad work well in wax and renshape. The larger diameter requires more torque, and is pushing the limits of the power balance of the machine.

17

Thanks for the input! So we shouldn’t really use them with wood?

18

I would reserve the 1/4" cutter for softer materials.
Heres a 3D Hardwod toolpath setting file.
Works great for VERY Hardwoods;
I rough with the .125" ball end and finish with the .0625" ball end.
hardwood 3d 125 063.tps (2.1 KB)

1 Like
19

Thanks for clarification and the toolpath settings Apollo!

That also makes those .25 cutters useless for me unfortunately. I just got them Friday including the extra collet. Is there a way to return them or at least exchange them for other endmills?