Shapeoko Feeds & Speeds and Machining Tips!

hi guys vince here today we're going to get into using fusion 360 adaptive clearing with desktop machines specifically how to get good feeds and speeds and what to look for while machining we'll do test cuts with both high and low axial depths of cut to show you the differences and benefits of each one we'll go over basic machine setup router and tooling and hopefully i can show you some tips and tricks and things i've learned along the way hope you guys enjoy for those of you that didn't watch the tormach access tech tina video i should probably introduce myself and give you a little bit of background i was recently hired by saunders machine works to work with proven cut on the desktop machine side and that's where we come up with cut recipes that are reliable efficient and repeatable for specific materials in every machine my first cnc was a shape echo just like this although i didn't have a nice fixture plate or mod vises a probe or a tool length offset sensor it didn't take long to really try and push the limits on the shape oco basically if i could fit it on the machine i wanted to cut it right now i'm going to show you one of my favorite parts it's actually one of two assemblies and this is a sheet metal press die and what you do is you put a piece of sheet metal in there under hydraulic press tens of thousands of pounds later and out pops is just perfect part a die like this really couldn't be machined without a tool path like fusion 360 adaptive clearing all right guys enough about me let's get back to the adaptive cutting the first thing i'd like to point out is that all these end mills our name brand we have 2l amana datron helical lakeshore carbide and destiny there are lots of other manufacturers out there as well but these are just some of the tools that i've used over the years with good results on desktop machines cutting aluminum these end mills are arranged by fluke count so let's go over why flute count matters but first let's talk about chip load i like to use a minimum chip load of one thou all these manufacturers do have recommendations for the chip loads that you should run their tools at but you'll find pretty quickly that in a desktop machine it's pretty hard to hit those recommendations and still get a good quality cut without chatter a minimum chip load helps ensure a reliable cut where the tool isn't rubbing and the chip is sufficiently thick enough to manage the heat so chip load is the amount per tooth per revolution that's cut so the more flutes you have the faster you're going to have to feed for that same rpm to maintain that chip look let's say we program the single flute to 40 inches per minute at that same rpm we're gonna have to run this three flute three times as fast 120 inches per minute to maintain that chip load also this three flute is going to take quite a bit more power because it's taking three times the amount of material per revolution also the more flutes you have the less chip space you're going to have for chip evacuation now that's huge when cutting dry basically single flutes i love cutting dry they're almost uncloggable you can full with slot no problem something like a three flute cutting dry you're pretty much going to baby the machine especially if you have a closed geometry where you don't have space to get rid of all those chips i recommend that if you are going to run two or three flutes that you do have at least an air blast or some type of lubrication i've used a wd-40 drip can before but they can be very messy and wd-40 just goes everywhere and i've also used a cheap amazon mister which has worked pretty well but i don't really like to have a air compressor running all the time i found that this minimum chip load is pretty universal with the exception of micro tooling so once you get to about 16 of an inch and under definitely run the manufacturer's recommendations because at that point power and rigidity really isn't a problem so the manufacturer is going to know best how to run that tool but for eighth inch quarter inch three eighths you stick with this and it's kind of hard to go wrong to start out with let's take a look at some of the single flutes we have on the table we have a diamond coated 2l a zrn coated amana and an uncoated datron 4 1 6 millimeter these two end mills right here are what i like to call you know regular duty pretty much a general end mill they are lower cost especially compared to the datron but they don't like to run at the same rpm i generally like to run both of these under 20 000 rpm because they aren't especially balanced and any kind of vibration will end up to some degree in the cut i haven't noticed a difference between the diamond coating and the zrn but it does give peace of mind so you know why not the is specially balanced because it's actually designed for machines that have a much higher rpm range than our desktop machines and it also features a wiper flat on the bottom and that lets you get a pretty good floor finish especially compared to most single flutes which aren't really known for a good floor finish also the datron is pretty much my pick when i want to remove a lot of metal and i don't mind running some rpm so i usually run this one you know anywhere from 25 to 30 000 rpm no problem dry cutting as well so today we are going to pick the datron mainly because i want to spin it faster i want to take a bigger chip and i want to spend as little time machine as possible so let's pick the one we can run the fastest let's talk a little bit about the setup i am running white steel core belts although now shea pocos come with black fiberglass core the steel core is about 20 percent stiffer but it didn't fatigue very well so usually get you know it's a limited lifespan six months to about a year which is not bad for me i think it's worth that 20 percent we're also running a saunders machine works fixture plate with the stiffener rails and on this project because our stock is so big five inch by 16 by 0.5 running two sets of mod vises just so that there's enough clamping on the part that we don't get any kind of unwanted vibrations because of overhang with the new setup the first thing we're going to have to do is tram in the fixed side of these mod vises and what i like to use when having an aluminum fixture plate and vices is the bit zero led to tell me when i'm actually making contact that'll get you within about a thou and that's plenty good for this type of machine [Music] let's talk a little bit about the spindle we'll be using on this machine as you can see it's a makita router this is model xtr01z but stock they come battery powered and that's not going to work very well with cnc operations so it has been converted to dc power supply usage so i could just plug it in the stock speed controller has been converted to a vesk and these are used mainly for electric skateboards or electric bikes or do-it-yourself one wheel type of things it gives me complete control over the makita and lets me pump a little bit more power into it while seeing real time data and letting me log everything for a view after the cut it is over volted right now to 27 volts and my rpm range is 2000 to 38 000 rpm one of the things i really like about these makita routers is you can run up to a 3 8 or 8 millimeter end mill that's a destiny diamondback and this is an eight millimeter daetron foreign one these are some of my favorite ones to run single flutes run super well at high rpm high balance and i don't know they just cut like magic now let's talk about why adaptive clearing is such an efficient roughing strategy and how it differs from traditional pocketing the magic behind adaptive is its constant cutting load by keeping its step over very controlled called the optimal load it eliminates spikes in tool engagement and allows you to run much more aggressively it also gives you the option of running much higher axial depths of cut in comparison here's a traditional pocketing tool path with the same step over as the adaptive as you can tell the tool engagement radically changes in the corners due to part geometry and this definitely means you'll have chatter and you'll have to reduce your feed and speeds accordingly okay let's drop the test part real quick so we can make those test cuts for the uh the high and the low depth and some of the older cuts that i thought were good but ended up not being that great i want to create a sketch we will make a center rectangle and it is a four by six and a half let's dimension it okay finish the sketch we're going to extrude it inch and a half tall now we want to create those slots for the adaptive so we'll create another sketch on the top and we'll do a two point rectangle this time okay i want these to be about an inch and a half wide and i want three of them so i'm going to make a rectangular pattern i'll choose all the lines and then just pull it out looks good finish the sketch okay so i want to extrude these down about a quarter of an inch just because i just want to show you guys the differences between these we have some real cutting to do later on a nice part so there you go looks good now time to put in some cam all right now here's where i'm going to cheat a little bit i've already spent quite a bit of time with proven cut recipes figuring out what to run on this tool on this machine as far as step overs and step downs so what i'm going to do is just copy that tool path go to my new part i'll paste it in my setup hit ok edits pick my new geometry right here there you go nice shallow adaptive tool path let's go to the feeds and speeds real quick 25 000 rpm 75 inches a minute 3000 feet per tooth optimum load of 0.23 so that's almost 100 percent step over and i've found that with these datron end mills you can almost run like a high feed end mill just a shallow depth of cut fast and they leave a beautiful finish make some really nice chips roughing step down 30 thou and because i'm cutting over 50 percent of diameter this feed per tooth is true there is no chip thinning that we have to worry about all right let's go get the deep tool path copy paste okay edit this i'm going to apply it to our new geometry there you go nice deep tool path and so these two tool paths are actually the same material removal rate but as you can tell they're going to be quite a few differences between both of them let's look at the feeds and speeds of this one the same 25 000 rpm cutting feed rate 50 inches per minute feed per tooth of 2000 now we will have an optimum load of 40 thou and a maximum roughing step down of 250 thou and what this means because this is under 50 percent of our diameter this is not actually our feed per tooth that we have to factor in chip thinning so our true feet per tooth is around one and a half thou which is above my minimum chip load so it'll cut fine no problem for our third slot we're going to try some feeds and speeds that i used for a long time and ones that i thought were pretty good but ever since i really started looking at the data and doing the proven cut stuff i realized that i definitely could have cut a lot faster a lot harder and save myself quite a bit of time i'm going to do is we're going to duplicate this deep depth of cut edit a little bit i used around the same parameters at the same spindle rpm the same feed rates the same optimal load but my maximum step down is only a hundred thou so we're going to make it just one pass so minus 0.1 all right and then we're actually going to pick the correct geometry this time okay so there you go what's interesting is i thought i was doing really good with this toolpath you know everyone runs adaptive at first and they they want to cut as deep as possible but the problem with that is the deeper you cut the more axial force you put on your machine and pretty much the more rigid and more powerful machine you're going to need it's all tied together so this is only 100 depth of cut and the mrr the metal or material removal rate was uh 0.2 cubes whereas both of these were 0.5 and that's quite a difference and i really wish i had run some tool paths like these because just the amount of time it would have saved the first cut we're going to make is the shallow adaptive pass and i'll stop halfway and pause the machine just to up the feet override so you can see how it's going to act a little bit more [Music] aggressively [Music] ah [Music] ah cut sounded great really nice even and consistent even with fifty percent override halfway through it performed really well floor finish is nice reflection is nice even though adaptive is not a finishing strategy it doesn't hurt i really like this kind of chip shape it's a nice soft little curl they don't interlock and they're not sharp which can be important if you machine it home or you don't have an enclosure or something like that the next cut will be the high depth adaptive we'll be cutting a little bit deeper than 1d which in my opinion is about the limit for most desktop machines unless they have linear rails or they've been modified to be a little bit more rigid or they have a spindle and they have more power i know everybody wants to cut full depth but when you have to make your radial depth of cut so small there's a certain point where you're just a probability of rubbing and things going bad just goes up way too much for it to be worth it does look cool on instagram though not gonna lie [Music] uh [Music] [Music] ah [Music] totally different sounding right louder and you could definitely hear peakier tones there's also evidence of chatter when it enters and exits the cut floor finish not as great but that's always going to be the issue when you have a high amount of step overs chips look nice and shiny very consistent not sharp at all so that's good but compared to that first cut it just didn't sound like the end mill was having a good time the walls there's some chatter the floor there's some chatter anytime you that end mill is bouncing around it usually means it's gonna not last as long so first cut second cut same material removal rate which one did you pick i'd go for the first one every time the third cut is the old recipe so let's see how it does compared to those first two yes it is a little bit deeper than our first cut a little over three times as deep but we're going to take the same radial step over as our second cut i do predict that it will sound better chips still look good the cuddle look a little bit better than the second one but the numbers will tell you that the actual material removal rate is just not worth it it's less than half of this first one but let's get cutting and i'll let you guys see the difference [Music] ah [Music] [Applause] [Music] [Music] [Music] ah [Music] ah [Music] [Applause] [Music] okay well that didn't sound as bad as that second cut chips look pretty good nice shiny but there was still a little bit of evidence of chatter in the cut you could hear a little bit and even when i bumped the feed override to 200 percent it still didn't match the same material removal rate as that first cut so is using that extra flute length really worth it maybe if you cut a whole lot and you want to you know pinch every penny but i really haven't seen a drop in tool life when using the shallower adaptive type strategies usually i'll you know drop an end mill and break it or i'll crash it and it's my fault before a tool ever wear out i actually don't think i've ever really worn out a tool okay so we've got our low and high depth adaptive cuts we've seen the differences in the sound finish and feel of each one now it's time to get in depth on how we came up with those feeds and speeds i started off using a workbook that estimates machine force tool deflection and spindle power usage these factors are important because those are a desktop machine's biggest limitations recently i've been using a program called millilizer it's a machining simulation software that can predict milling forces and tool deflection as a function of work piece material and machining parameters it can plot the development of the forces acting on the tool during one full revolution let's look at the force plots for those first two adaptive test cuts on the left is the low axial high radial and on the right is the high axial low radial both of these cuts are at the same sfm and very close in mrr here's where it gets really interesting though the peak and average forces are much higher with the high depth adaptive cut it's easy to tell that our shallow cut is a much better option for this tool in this material with my machine force parameters our test cuts back up this data as well now let's apply that shallow adaptive proven cut recipe to a real part this is a custom intake manifold plenum floor with raised velocity stacks there is quite a bit of material to remove so we're going to run it just a little bit more aggressively first thing we're going to do is open up the millolizer and i'm going to keep the same depth of cut and width of cut however i'm going to increase the spindle speed to 30 000 rpm which is the maximum rpm for makita router i'm also going to increase the chip load to 5000 so you can still see really nice looking graph here peaks aren't bad my peak feed is under 18 pounds which is my shape elko force limit uh peak axial is pretty low and wattage is still pretty low under 300 watts tip displacement looks good dual stress looks good the material removal rate is a little bit over one cubic inch per minute and while i know that doesn't sound like much you have to realize this machine weighs under a hundred pounds and we're using a router and belts and plastic v wheels so in my opinion it's pretty respectable especially if it's a nice quality cut without chatter if you're a beginner a nube with aluminum one of the most important things to check before cutting is the mechanical condition of your machine belt should be properly tensioned v wheels should be adjusted until they don't spin by hand the router or spindle should be trammed in and a calibration test like a circle square diamond should be done to ensure accuracy once you feel confident in your machine install a tool that you don't mind possibly destroying and do your cam start out with slower rpm so feeds will be more manageable and if using fusion 360 one of the most important things to do is check the simulation before starting a cut this will save you potential headaches from collisions and crashing listen to your machine if it doesn't sound right it's probably not right inspect your tool before cutting with a loop or microscope to ensure all the cutting surfaces are in good condition a small chip on the leading edge can make or break your project spend time dialing in your work holding if you can't hold your part you can't cut your part a setup like an smw fixture plate and modvice make this easy but if you have an mdf table you might have to get a little bit more creative and last but not least don't be afraid to go easy at first you can start with lower axial depths of cut and work your way up remember it's a cnc machine consistent and reliable is the main goal double check your setup work holding in cam be confident and make sure you're wearing the proper safety equipment and those butterflies you feel right before you hit the start button that's the best [Music] [Laughter] [Music] [Music] [Music] [Music] [Music] now let's open up the vesk tool and look at the data log of the makita router during that cut now this is where it gets really interesting because you see real life data you can actually see what's going on when the machine is cutting so this is the initial helix right here and from what i heard in the video and from what i'm seeing as far as power usage i can afford to push that a little bit higher and i think that additional tool pressure would help with the cut once it gets into its main adaptive cuts it's hitting around 275 to you know 300 watts it's funny because you can actually see the shape of the part in the graph after it finishes the profile it starts to do the bores and that's why there's four different spikes here the initial helix and then it spikes when it starts to rough inside out now let's look at the average power usage and compare it to what the mililizer estimated to be looks to be around 280 watts 275 watts right open up the millilizer estimated 282. that's spot-on and that definitely gives me confidence in all the other factors that it's predicting there's also another interesting thing that i didn't actually see till i was done with the project but if i would have cut in conventional cutting i probably would have had a little bit smoother cut and that's mainly due to just the high step over i was using which is almost 100 percent [Music] after the adapter was done i used scallop in a daetron six millimeter single flute ball end mill for the semi-finish and finished tool paths [Music] once i finished those scallop toolpaths i reinstalled the daetron six millimeter four in one and ran an inside and outside contour to finish the surfaces and free the part this is the final part the finish is right off the machine without any kind of post-processing or polishing now let's check the width i didn't do any kind of fine-tuning infusion or any kind of step count adjustments in the machine controller width is supposed to be three inches see how well we did all thin about a thou that's good enough for me especially for a belt-driven machine be safe guys be smart and happy cutting [Applause] [Music] you

Channel: NYC CNC

Views: 83,814

Rating: 4.9561315 out of 5

Keywords: tormach, fusion 360, how to, cnc, machine shop, nyc cnc, DIY, machining, milling, CAD, cnc machining, cnc milling, learn cnc, john saunders, manufacturing entrepreneurship, provencut, chip rag, CAM toolpaths, workholding techniques, fixturing

Id: b8CndwnfoCM

Length: 29min 12sec (1752 seconds)

Published: Wed Dec 30 2020