Screwdriver holder

New Home Forum Things You Have Made Screwdriver holder

This topic contains 43 replies, has 7 voices, and was last updated by  Tchad Rogers 6 months ago.

Viewing 30 posts - 1 through 30 (of 44 total)
  • Author
    Posts
  • #52317

    Hubert
    Participant

    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.

     

    #52320

    Ryan
    Keymaster

    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.

    #52326

    Jeffeb3
    Participant

    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?

    #52346

    Hubert
    Participant

    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.

    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.

    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?

    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.

    #52347

    Tchad Rogers
    Participant

    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. 🙂

    #52349

    Ryan
    Keymaster

    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 user thanked author for this post.
    #52351

    Hubert
    Participant

    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 3×3 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…

    #52358

    Barry
    Participant

    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 3×3 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.

    #52361

    Tchad Rogers
    Participant

    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. 🙂 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.

    #52381

    Hubert
    Participant

    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…

    #52391

    Ryan
    Keymaster

    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.

    #52394

    Jeffeb3
    Participant

    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.

    #52408

    Tchad Rogers
    Participant

    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.

    #52417

    Ryan
    Keymaster

    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.

    #52420

    Jeffeb3
    Participant

    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.

    #52436

    Tchad Rogers
    Participant

    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. 😀

    #52437

    Ryan
    Keymaster

    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.

    #52439

    Jeffeb3
    Participant

    Oh, his cat is not dead.

    #52441

    Ryan
    Keymaster

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

    #52442

    Jeffeb3
    Participant

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

    Read it again.

    #52443

    Ryan
    Keymaster

    hahahhahhahahaha, Yup, dorks

    #52446

    Tchad Rogers
    Participant

    you are right a 1/4 2 flute would be almost equivalent to a 1/8 single flute.

    I’m confused, can you explain? I’d think the velocity of the cutting edge of a 1/4″ bit would be double that of the 1/8″ at the same RPM, because the cutting edge is farther from the center so it has farther to travel each revolution. I’d think the extra flute would further compound that and you’d get (very roughly speaking) 4x the cutting ability at the same RPM.

    …already took the top tier goal though (lunch with me, he asked to bring his cat).

    If you observe the cat as alive, do the quantum end mills have 3 flutes? Maybe they’re entangled!

     

    #52448

    Ryan
    Keymaster

    Think of it this way, twice as fast (at the cutting edge), but also take twice the power (or twice the rigidity) to cut at that distance. A ten pound weight in your arm extended straight out, or a ten pound weight at the end of a broomstick at the end of your arm extended straight out.

    It is the same with the Z axis half the extension is twice as rigid.

    So yes, the more flutes the more cutting ability but also the more rigidity and/or more torque needed in the spindle (or system) to do it. To keep all those flutes fed you need to move faster, to move faster you need more rigidity (or spindle torque depending on the systems weak link). For most all cnc’s torque is far cheaper than rigidity so you will typically get chatter before a stall of any kind (spindle or stepper).

    Check it out in a calc, keep all things equal and only vary the flutes and diameter.

    I could be totally wrong, but I spent enough time in that rabbit hole for today. Tomorrow though…new day.

    #52449

    Jeffeb3
    Participant

    I’m confused, can you explain? I’d think the velocity of the cutting edge of a 1/4″ bit would be double that of the 1/8″ at the same RPM,

    Yeah. That’s true. Why did I think it was slower? If I got it right through some feeds/speeds/rigidity jujitsu, that was not intentional.

    Now I’m also not sure the speed of the “tooth” makes much difference. If it’s one flute, moving at 10mm/s and 100 rotations per second, the depth of cut will be about 0.1mm deep, no matter the radius or the outside speed of the flute.

    #52453

    Hubert
    Participant

    I have a SuperPID on my Dewalt 611, and it has been great.

    I googled SuperPID, looks pretty nice but a bit pricey… Does it work with Marlin firmware?

    #52454

    Hubert
    Participant

    I am wondering if you can tell anything from the “chips” produced during cutting, sort of like you know if your chainsaw chain is dull just from looking at the chips. Both times I have used the machine, it produced a fine powder like a coarsely milled flour. Somewhere between grits and AP flour, but closer to the flour. I have never produced such small “chips” using a handheld router or on the router table.

    #52457

    Tchad Rogers
    Participant

    I googled SuperPID, looks pretty nice but a bit pricey… Does it work with Marlin firmware?

    The SuperPID is firmware-agnostic. It can run in two different modes, depending on your preference:

    1. With a dial pot, and no connection at all to your PC or microcontroller – just turn the dial to move the RPM up and down. I’d say 90% of people on the Shapeoko forums run it like this.
    2. Listening to a PWM or analog voltage signal from either your PC or your microcontroller.

    I have a switch wired that changes it between those, so most of the time my microcontroller controls the speed, but if I want to test something, (or if I forgot to set an appropriate RPM in my CAM/gcode) I can flip the switch and manually trim the RPM with the pot.

    I know that Marlin can output a PWM signal based on S commands, so yes, you could control it via Marlin if that’s what you wanted. I haven’t done this before, but in theory it should be very similar to configuring in GRBL. You do need both a PWM wire, and a RUN wire coming from your microcontroller (and a GND wire, but that’s easy). Depending on the board you have, this can be trivial, or it might require some soldering. I had to solder a couple of pins to available (but not populated) output holes on my motion board.

    The only thing I dislike about the SuperPid, is that it’s still just running a trim router or other AC motor, so at higher RPMs it’s always going to be louder than a real spindle. If you don’t mind the volume of a trim router though, the SuperPid is a very nice device. I can cut all the way down to 5,000 RPM now and maintain torque.

    I recently purchased an inexpensive Chinese 1.5kW spindle, which has the same functionality as a trim router with a SuperPid, but should be quieter (especially at higher RPMs). I wouldn’t put 1.5kW on the MPCNC (it’s really heavy) but a smaller Chinese spindle might have the benefits of the SuperPid, plus be quieter, at about the same price as the SuperPid by itself. Of course, you have to play build-quality roulette, compared to a DeWalt and SuperPid that are always very well made and have good customer support.

    #52458

    Tchad Rogers
    Participant

    I am wondering if you can tell anything from the “chips” produced during cutting, sort of like you know if your chainsaw chain is dull just from looking at the chips.

    I believe that is true, but I’m not yet experienced enough to tell you what it *should* look like. I can say that I tend to get dust from my 1/8″ bits, and actual chips from my 1/4″ bits, using feeds and speeds for each that produce good results from each. I’m not sure if this is optimal or not, but dust (similar in composition as the dust from a circular saw) from an 1/8″ bit is normal in my experience.

    #52459

    Tchad Rogers
    Participant

    From @Jeffebe3:

    I’m also not sure the speed of the “tooth” makes much difference.

    From @Ryan:

    Check it out in a calc, keep all things equal and only vary the flutes and diameter.

    I understand and agree with everything both of you said… we’re on the same page again. 🙂

    What I’m wondering now, is how to quantify the extra lateral force a 1/4″ 3-flute bit needs, compared to a 1/8″ 1-flute bit. Anecdotally from hand-routing, moving from 1/8″ to 1/4″ doesn’t seem that different to me.

    I tend to run 35 IPM at 21,000 RPM and 1/8″ DOC with 1/8″ 2-flute bits, and I tend to run 55 IPM at 17,000 RPM with a 1/4″ 2-flute bits and 1/4″ DOC. If 55 IPM at 1/4″ DOC is too fast for the MPCNC, I’d just reduce the DOC, feedrate, and RPM to get back to a healthy chip load at a reduced torque requirement. I wonder if there exists a way to quantify the difference in required lateral force (stepper torque and rigidity) between a 1/8″ and 1/4″ bit at the same feed rate and DOC, with RPMs tuned for each.

    Someday I may do a semi-scientific comparison, cutting circle-diamond-square tests and measure precision and speed… but probably that’s a pipe dream… I don’t really have time. 🙂

    #52464

    Ryan
    Keymaster

    Someday I may do a semi-scientific comparison, cutting circle-diamond-square tests and measure precision and speed… but probably that’s a pipe dream… I don’t really have time. 🙂

    Yup. So many things I want to try but it cuts within my needs so this never comes about. After a few cuts your ear should know if you are close. For me test cuts get ran in every material anyway so I haven’t had the need to dial in my settings with the utmost precision.  Once it works I hit run.

    In wood it is pretty easy to understand what is wrong. Burning means too high of RPM (or moving too slow), broken or wandering bit means you are moving too fast (or your RPM is too slow). Once you understand wood  then you can cut some other stuff which is not so easy to diagnose, plastic and metal.

Viewing 30 posts - 1 through 30 (of 44 total)

You must be logged in to reply to this topic.