Screwdriver holder

I just completed the first project on my MPCNC with a router. It is a tool holder for screwdrivers, made from 12mm Baltic birch plywood and attaches to the wall with a couple of pocket screws. I cut it at 8mm/s XY speed, 2mm/s plunge speed and 3mm depth per pass with a 1/8" single flute upcut bit.

The noise from the machine was unbearably loud. It was a high pitch screeching noise and not like anything you would hear from a handheld router. The machine is sitting on a plywood torsion box and I am wondering if that is acting as a resonator amplifying vibrations. Also, the 3mm depth per pass may have been too much. On the last pass when the bit only cut about 1mm into the MDF spoil board, the machine was relatively quiet.

Anyway, I am pretty excited about the result. The cut was very clean and I could not see or feel any ridges between the separate passes.


Looks great.

As for the sound I would try deeper per pass at that speed, and the spindle RPM could have a lot to do with it as well. Cut look great though so you are not too far off of the right settings.

I’m a sucker for shop projects and Baltic Birch. Nice work. Maybe take a video next time and if you’re still worried, we can take a look and listen. How big is your machine?

Thank you. The first try was in foam, worked great and was quiet. First try in plywood ended very quickly with a broken bit. It survived plunging into the wood but snapped immediately when the router moved sideways. The router was set to low speed. Second try in plywood was on max rpm, everything else was the same. The router is a little Bosch trim router that has been abused quite a bit. That, the collet reducer and a very cheap cutter might be responsible for some if not all of the screeching. While cutting the plywood, there was a smell of burned wood, but there were no burn marks on the wood.

The machine is pretty big, about 2’x3’ usable area. The rails are 16ga stainless. It feels pretty solid and I was just beginning to think everything was broken in as it had actually gotten a good bit quieter, but that was just moving a pen around. You cannot hear the steppers or even the router motor over the screeching sound. If I can’t figure out what’s wrong, I will try and figure out how to post a video.

The screeching sound, plus the smell of burned wood probably means you were getting rubbing. (The bit spinning fast enough that some passes of the cutting edge don’t have any wood to cut, so they rub and cause friction, resulting in heat) which means you should back off the RPM or speed up your feed rate. (caveat: feed rates are limited by machine rigidity, and I’m a newbie to the MPCNC, so I don’t yet have a sense of it’s rigidity.)

Chips carry the heat away from the cutter, and heat is the enemy of a sharp bit, so hitting the sweet spot of chip load is important, and a mix of art and science. (More science in engineered materials, more art in natural materials.)

In pine, I generally run 35 IPM at 21,000 RPM with a 1/8" 2-flute up-cut end mill at a 1/8" DOC (not on a MPCNC, so I’m not sure yet if MPCNC will handle those feed rates). Any faster and deflection starts stealing end-mill life.

I just joined this forum, so I’m apprehensive to plug commercial software, but I have found feed and speed calculators to be helpful; I’ll leave it at that. :slight_smile:

He is in the ball park, single flute cutter so roughly cut your feedrate number in half and the feedrate he set is actually a bit faster than you recommend. But the RPM are around 30k (meaning it needs faster) so it is real close.

How we generally get it right is pick a feedrate 8-15mm/s, and RPM (3/4 so you can go up or down a bit). Practice cut shallow until the setting are dialed in and then just keep adding depth until you find your builds rigidity limits, no more than about 5mm DOC per pass max to get the chips out.

Of course these all change when you figure things out more but that makes it pretty quick to hone in on something that works. Adaptive allows for much deeper passes but lets just call that intermediate cuts and ignore it for now.

1 Like

Thank you guys for the information. I am trying to process it all and come up with a plan for finding better settings. I guess the three parameters I need to test are feed rate, depth of cut and spindle speed. If I understand you correctly, my settings were too conservative on feed rate/depth of cut and too aggressive on spindle speed. My first attempt at cutting the tool holder resulted in a broken bit right away. The only thing I changed between that attempt and the successful one was the spindle speed and obviously the bit. I concluded that in attempt #1, the spindle speed was too low, but the bit may well have had a crack and my conclusion may have been completely wrong. The speed was set at 4 out of 6 on the failed attempt and 6/6 on the one that worked.

I think I might try cutting a 3x3 matrix of squares or circles and vary depth of cut along one axis and feed rate along the other and see what happens. The spindle speed is more difficult to vary and I suspect there might be something wrong with the speed control of the router. Just running without load, it sounds like the speed varies sometimes. I might just set the speed to five to leave some room for upward adjustments as Ryan suggests. Maybe I’ll get one of those little tachometers to measure spindle speed as well.

One thing that I am not quite sure about is how I will know that I am at the machine’s “rigidity limit”? What signs should I be looking for that the cut is too deep for the rigidity limit of the machine? It seems to me that the end mill is the weakest link at 1/8" diameter…

You’ll either see the tubes bend, or the torque forces on the bit will overcome the holding power of the steppers, which is both frightening, and funny at the same time. Once that happens, it will ruin whatever you’re cutting, or the bit, and possible both. You’ll flex more over your 3 foot length than your 2 foot length, so watch those rails.

It seems to me that the end mill is the weakest link at 1/8″ diameter…
Yes, sorry, I inadvertently complicated the discussion. The rigidity of the machine has nothing to do with your current problem.
I guess the three parameters I need to test are feed rate, depth of cut and spindle speed.
Exactly right -- generally referred to as "feeds and speeds" in the CNC community, though as @Ryan mentioned, number of flutes, and diameter of cutter are important too. (Really, in the end, the one most important measurement is chip load; your feeds and speeds, and bit geometry all affect chip load.) A "good" feed rate will also minimize bit deflection, which also shortens tool life. And finally, the bit material affects things. High speed steel will have different ideal speeds than carbide, which will be different from a coated bit. (If you're just getting started and only cutting wood, foam, plastic, wax, etc. just stick to carbide and don't worry about it.) All these nuances is why I start with a calculator to get me in the ballpark, then tweak it with multiple cuts to dial it in. For tinkering, just googling settings that others have used for the material and cutter is fine - don't complicate it unless you need to.
If I understand you correctly, my settings were too conservative on feed rate/depth of cut and too aggressive on spindle speed.
That was my take... but in my comment above, and as @Ryan pointed out, I missed that you were using a single-flute cutter. Based on a single flute cutter, your speeds and feeds seem more reasonable to me. Of course that leaves me scratching my head as to why you're getting a horrible screeching noise. I'm not very familiar with single-flute cutters, so if it were me, the first thing I'd try is a different cutter (2 flute), but that's mostly familiarity / laziness on my part.

The bearings in your router are good, right? (Most likely it’s the bit, but worth clarifying just in case, as the solutions are totally different. :slight_smile: If your router was working fine before you dropped it in the MPCNC, I’m sure it’s fine…

Also, FWIW, in my experience 1/4" bits are much less likely to scream than 1/8".

Another thought: how far from the collet was the tip of the bit? In general, the shorter the exposed bit length, the more ridged the bit will be, and the less likely to deflect and/or chatter. If you can, choke up on the bit some more.

I’m new to the MPCNC, but have been using a hobby CNC machine (Shapeoko 3) for about 18 months, so I’ve learned a lot, but have a lot left to learn. (I don’t want to present myself as an expert - I’m certainly not.) However - here’s my take on rigidity: as long as you’re not going crazy fast, the biggest thing you will see with pushing the machine too hard is minor inaccuracies in cuts, especially in natural materials like wood. Cut a small (4-6") circle-diamond-square test, and put your calipers on it to see how close to specification the shapes end up. A well-tuned machine running safely within its rigidity limits will be accurate within a few thousandths. I suspect if you start pushing it too fast, you’ll see odd inconsistencies in the measurements… for example, the measurement of the diamond varying along it’s length as the middle assembly flexes slightly under the loads. If you don’t care about inaccuracies in the thousandths of an inch and/or don’t own a caliper, then don’t push the limits with your feed rate, and don’t worry about it. I don’t want to over-complicate a fun and rewarding hobby - you can make awesome stuff without ever knowing whether your machine is accurate to .003". And like what @Barry said, if you can see your rails flexing while cutting, you’re way behind the limits of the machine. Then you’re going to be measuring your inaccuracies in the .1" increments, not .001".

As @Barry pointed out, a much more likely negative outcome from pushing the machine too hard is the steppers losing steps. This is worth reading up on if you aren’t familiar with the term, but in short, the steppers miss movements because they don’t have enough torque to execute the instruction sent to them, and you get accumulated drift as they lose steps – completely ruining your part.

I cut another little tool holder and it was a lot quieter. I pushed the end mill further into the collet and increased the XY speed to 10mm/s. There was no smokey smell today but still some screeching sound, albeit at a much reduced volume.

When I get a little more time, I will try to investigate the problem a bit more methodically…

Welcome to CNC, the tiniest setting can have a big difference. You will get a quick feel for it, and usually a little tweak of the RPM can fix it, that is why RPM control is so nice. It is the easiest thing to tweak on the fly.

I will try expect the speed control built into the router to be much of a speed control. For one thing, if it’s old, it might not be terribly smooth or making great contact. For another thing, it doesn’t actually control speed, just the percentage if time the motor is getting power, so it will still lower speed when under load.

I wouldn’t worry about it, except for gross adjustments. Anything fine, and you really need closed loop speed control, which requires a speed sensor on all the spindle all the time. There are some cheap diy solutions or expensive commercial stuff. Either way, not really worth optimizing. You can do quite a lot by just moving it 1/5th of the way at a time. It might be nice to know the general speeds you’re getting, but it could slow to 50% when it’s cutting from idle.

I have a SuperPID on my Dewalt 611, and it has been great. The ability to change RPM on the fly (with my hands a safe distance from the router) and have it stay constant RPM through material variations is nice.

Still… I’d try a new, carbide, 1/4" 3-flute cutter before doing anything else. They have been some of the most forgiving end mills in my experience. If you can’t cut cleanly with that, something is wrong.

You gotta try a single flute, they are so much better suited for the Rpm of the spindles commonly in use. I have a video I was cutting 8-10mm DOC adaptive in pine. Super clean. A two flute has a much smaller sweet spot in my opinion and a 3 flute, well I never tried one but I can’t imagine the required feed rates on our machine to keep the chip load in the ballpark.

The 1/4" might just slow it down enough to be similar. The outside is moving half speed of the 1/8, so maybe a 1/4" 3 flute is similar to a 1/8" 1.5 flute (you know, a quantum bit that has two flutes only half the time, unless you look at it).

I naturally like the 1/8". They seem cheaper and like I’m wasting less wood and bit when I’m cutting out a part. I also feel like my table saw is 1/8" kerf (or 3/32" for the thinner version) and that can’t be a mistake. I do occasionally use a dado stack, but I usually would rather just make more 1/8" cuts.

You gotta try a single flute, they are so much better suited for the Rpm of the spindles commonly in use.
I will! I'll buy some from the V1 store and try 'em out, now you have me curious.
[re: 3-flute...] I can’t imagine the required feed rates on our machine to keep the chip load in the ballpark.
That's a good point... my experience is on a slightly heavier machine than a MPCNC, a 3-flute 1/4" might not be well-suited. I'll have to try it and see.
(you know, a quantum bit that has two flutes only half the time, unless you look at it).
Are those in the V1 Sharp Stuff store? I couldn't find them... that sounds like the perfect blend of too few flutes, and too many. I'll ask the staff at Rockler if they have them. :D

Dammit you made me do math…I never thought about it that way but you are right a 1/4 2 flute would be almost equivalent to a 1/8 single flute. In terms of RPM, the chip load I believe would still be higher though, unless your step over was equivalent distances. 50% for the 1/8", 25% for the 1/4"

That took way to much thought to get that straight in my head…

I have the Quantum ballend mills on indiegogo, and the Vbits on kickstarter. Early bird goals are almost sold out get em quick, they might be gone but you can’t be sure unless you check first. Some guy, Schrodinger, already took the top tier goal though (lunch with me, he asked to bring his cat).

Okay I’ll stop…dork through and through.

Oh, his cat is not dead.

Did you verify that it or are you just a pessimist?

Read it again.