Speeds & Feeds Tutorial for CNC Machines! WW164

hi folks welcome to a video on speeds and feeds let's cover four things in this video number one some starting recipes number two let's talk about how to calculate the basics of feeds and speeds if you want to move beyond those starting recipes number three let's talk about some tips and tricks on how to use different materials and how to use different size tools and the number four really important chip thinning and how to calculate horsepower even if you're new to machining I want you to understand the basics of this I love making stuff but having good feeds and speeds makes it so much more fun to make your parts welcome to other Wednesday widget [Music] [Music] starting recipes these contemplate using a tormach milling machine and either aluminum or steel we've included a link to the end mill that I would like you to buy you're welcome to use whatever you want but this beets and feeds here contemplate this 3 flute lakeshore I recommend using the TTS set screw style holder as you see right here some tips you don't need the Weldon flat that's a flat spots ground that's designed to mate up with the set screw that's important for higher horsepower and machines it's not important for a quarter-inch tool in the tormach we've never had one turn on us we find that the set screw holders are actually better to use generally they're easier to use they're a little bit more rigid than er columns that's not to say you're collets aren't great and they have their purpose but my go-to is the set group choke up on your tool you're purchasing this tool it's got a shank section in a flute section when you insert that tool and tighten it I want it choked all the way up so that the only portion extending beyond is the flute now obviously if you've got to reach in deeper you can extend it but be careful you sacrifice a lot of rigidity when you do that one of the things I recommend doing is take that tormach set screw holder and replace the set screw that's the only thing I don't like on them with a quarter 28 or for the larger set screw holders a 3/8 24 McMaster part numbers are included here much easier and much more reliable to use and not have that thread strip out and then FYI this tool from lakeshore has a three thousandths or so radius ground on the very corner of the tip of the flute and what that does is it reduces the weakest portion of the tool it's the most likely to break first and when it breaks it causes this kind of downward spiral where the next flute then sees additional material an additional load and it will then fracture and chip and it can work result in harmonics and and finishes and shatter and so forth you're starting to up the cut quarter inch that's one hundred percent of the tool diameter you're starting width of cut twenty percent or 0.05 inches if you're using using 360 the adaptive strategies called this optimal load if you're new to machining you may think in rpms and inches per minute and that's okay in this case 50 100 rpms 15.3 inches per minute but I want you to start understanding service feet per minute which is 330 for an inch per tooth or IPT of 1,000 here also discourage you from going less than one thousandth of an inch per tooth and the absolute minimum is 5/10 again we'll come back to that with chip thinning for steel basically the same thing a different tool happens to be five flute ironically about the same inches per minute but it's a different recipe we're having a lower rpms but because it has five flutes instead of three we actually go about the same speed or in inches per minute to maintain that chip load same starting depth of cut in width of cut what I like about this is you're not going to break tools you're not gonna wear those tools out because you're rubbing rubbing happens when you don't take enough cut with the tool think of it like a backhoe or an excavator that bucket wants to reach out and wants to scoop in that soil and take a cut too many folks burn out tools because they think they're just gonna take very light skin cuts and you burnish you don't let that leading edge of the flute actually dig in and cut material away if you want to move beyond this you've got a different size tool with different size material I recommend using the feeds and speeds tab here these two boxes the exact same information it's just the way you input it so in the way we run Excel files is blue or yellow and blue cells are input cells so in the BI surface feet-per-minute you would input the sfm that's very useful because many tooling companies will not give you RPM they'll only give us FM so we put in the diameter let's say it's a 375 tool we want to run two thousands per tooth and it's three flutes so if I were in steel I would start out lower like this one hundred service a minute 1,000 rpms but if I'm in aluminum I'd go a little bit higher say 250 or even 300 what's important is the ratio between the RPM and the inches per minute because that's what maintains this ever important inch per tooth thing against this you're not rubbing if you'd rather use rpm same information here depth of cut you can go up to 200% of the tool diameter so that's gonna show the quanta cut with more depth of cut in a thinner width of cut and that has a ton of benefits that we'll get into in future videos some exceptions anything smaller than 1/8 of an inch starts to get into micro machining really micro machining would be smaller than say 50 thousandths of an inch but the different rules apply you've got to maintain good chip evacuation and sometimes and this is crazy you will violate that inch per tooth rule that I talked so much about my recommendation is Harvey tool they've got some great information they've got some great tools and they've got some really good technical information and speeds and feeds on micro machining shear hog is one of our favorite tools that tool our recipe is point two inch width of cut point to each depth of cut as a general rule the more flutes you have in a tool the stronger that tool is because as a thicker core and what's great is because we're doing a thinner width of cut the chip that forms when we cut more naturally flows and fits inside of what's called the gullet that's the area between the outside of the flute and the core of the tool one of the reasons that Russia Cal works is there's long thin chips fit so well and evacuate so well if you're new to machining or new to a machine with steel I would go lower rpms and with aluminum I would go higher rpms or surface footage keep that chip load I say one thousandth of an inch per tooth here I'm probably going to even revise that to be one point five thigh or even tooth out to speeds and fees are easy for the most part what is difficult is optimizing them but I highly encourage you start with a recipe that works and by that I mean you don't want to chatter it's ever okay to have chatter and one of the problems with chatter is it can quickly compromise the tool which means further testing will be compromised itself because you may have a tool that has a cracked edge or micro cracking or other problems with it start with something that works work your way up that could be frustrating because let's say I have to run a half inch tool with four flutes and I'm gonna take it easy so something super low 75 surface feet per minute that's only 573 rpms 4.6 inches per minute most of us wanted to go faster than that start somewhere that works build your way up as you're building up a recipe it can be really useful to know something called the material removal rate that's the cubic inches of material that you are removing because that can be helpful to know as you change your recipe is it actually a more efficient recipe is removing more material we've created a formula here it's quite simple its inches per minute times a width of cut times depth of cut and that gives you that cubic inches that's also the key input for understanding how to calculate horsepower now horsepower is a really tricky thing and the two big caveats are what's the material you're cutting and the specifics of that material and we're talking about horsepower here at the cutter and that's going to be different than the motor rating of the horsepower on your machine because there are losses that happen through gears and belts and pulleys and so forth what we've done though is we've started to build out the basics of how to look at horsepower it's this thing called K factor if you look down here in the excel file tab k factor detail we've imported this list of all of these materials along with their corresponding K factor and Burnell hardness and it's fun to see them this is what drives most of the speeds and fees calculators out there and it's actually pretty simple what's frustrating is it can vary greatly so we'll take a very common material 6061 aluminum what's important is making sure that Brinell hardness matches now if you're not sure you want to check McMaster tends to be a pretty good way to do that if I go to aluminum click on sheets and bars and then expand this about aluminum you'll be able to see if we look at multi-purpose 6061 actually they give me the exact Braille hardness I'm looking for sometimes you may need to compare that between a Rockwell B or C scale which is a different Hart dis rating to get an idea of what you're looking for if you don't find the exact material or you're not sure I would emphasize matching the Brinell hardness worried more about that and less about the specific nomenclature or perhaps some of the even branded names behind some of these types of Steel's and alloys so well we've got that K factor the horsepower formula is really simple it's simply the material removal rate divided by that K factor so I've got them linked in here if you're familiar with Excel and if not you can just go click on the detail and say let's say 86 21.6 9 K factor so we could manually type something in here and just say 86 20 and 1.69 and we could see that gives us the horsepower rating of 0.3 not very much let's say we bumped it up point 5 inch depth of cut point 1 inch width of cut now all of a sudden we're removing 2 cubic inches and that's going to take 1.2 horsepower that's really useful to understanding when you're gonna start pushing the limit of your machine but also understanding the limitation of things like the workholding and how secure is the setup for our friends in the rest of the world we've also got the same information in metric last thing i want to talk about something called chip thinny and please do not close the video now this is awesome stuff it's really important what the heck is chip thinning I think Dartmouth C&C did a great job posting this information here on his Instagram channel when we program that feed rate of one thousandth of an inch per tooth again the idea there is that as we rotate that tool and as we move it forward through the cut each flute will be cutting with a starting thickness of one thousandth of an inch so you can see that in this picture here the green area well what happens is that that only works that's only correct if we were cutting with a 50% step over we don't do that I just told you with most of our modern cutting recipes we're gonna do something like 0.05 which is about 20% of the tools diameter this is basically old news this whole 50% step over stuff so when you do that take a look at the right-hand one your chip thickness is reduced the Sandvik technical guide will put a link in the video description I think also does a great job showing that if we were at 50% step over which we will never do it would be this FZ this width right here but because we're cutting with less radial engagement it's this reduced value they called a chi X or hex and I know it's so easy to get complicated here but again I want you to look at this picture because remember when I was mentioning the backhoe example that's what's so important when we cut this is creating a thick to thin chip and I want you all to watch this video here we'll put a card in it as well as a link in the video description it's only 2 minutes but if you're pressed for time just start at 40 seconds santak explains why it's so important to create a thick chip when you start and go it out too thin the two things that really resonated with me number one again is that insert or flute starts the cut it needs to be able to dig in if it started on a thin side it would rub before it actually dug in the second thing is that is you exit that cut because it's now findout you're less likely to tear the material or crack the workpiece even on a micro level so what does heck does all this mean for you why should you even care so there's this formula that looks complicated it's not too bad and we put it into Excel so take mark typical example here quarter inch tool 20% step over one thousandth of an inch programmed what's our actual our actual is eight tenths so believe it or not when we're at 20 percent width of cut which again is what I'm giving you in our starting recipe even though I told you to run one thousand of an inch per tooth and that's what you're going to do at the fifteen point three inches per minute if actually one thousandth of an inch per tooth it ends up being a little bit less than that how much less not much about two tenths so here I'm not too worried here's where this really matters how many of you out there myself included when you're programming your parts in your cam will do a small radial stock to leave say one thousandth of an inch or how many of you in a 2d contour will do multiple finishing passes or repeat finishing passes or a spring pass and when you do that you end up cutting with only a radial step-over of about one thousandth of an inch and what happens there is your actual cut is only about one point three tenths in many situations that width of cut or this teal blue area here is less than the sharp edge of your cutting tool the sharpest knife the sharpest razor still has some bluntness to that edge and in fact a lot of tools are made a slightly honed edge to increase strength and tool life and when you cut with a actual chip load that's less than that sharp edge you will rub so let's take a look this is our go-to recipe our quarter-inch tool to 20% step over one thousandth of an inch per tooth you can see here we're making a real chip yeah it happens to be calculated as eight tenths instead of one thousandth of an inch but no big deal that ship clearly is something that's being sheared away from the material I like it take a look at this though this is now a one thousandth of an inch spring pass or finishing pass on that same part look at how those chips now I'm okay with this I was really excited to do this test this is still a chip it's really small and it's really thin but there's still a continuous chip it's just thinner we're right on the edge I'm actually excited to do some more testing because I think pretty quickly with a thinner engagement this is going to turn into Pixy dust and it's going to result in true burnishing here we're still cutting but it's close this is so important because aluminum is pretty forgiving it's pretty easy on tools and your aluminum end mills tend to be sharper which means they're more resistant to shift fitting but two of the videos we have coming up are on 304 stainless and on cutting hardened a2 tool steel and when we do those harder materials that are less forgiving and we've got to be more aware of this so we put this graph together what does this show well remember here how I've got this ability to input and let's say when we're at our standard cut of 50 thousandths and a one thousandth of an inch per flute programmed feed rate our actual feed rate is about eight tenths but if we say drop down to a 1000 a 1000 this graph plots out what that actual output value is as we decrease our radial engagement so the first value all the way here on the left assumes that we were at 50% step over so 0.125 inches for a quarter-inch tool and at that point our programmed feed rate of 0.001 matches the actual feed rate of 0.001 just like we saw in the Sandvik graph but as we decrease that radial engagement the actual feed rate diverges from the programmed feed rate and what we've been told by tool manufacturers is again that magic number you want to avoid is going under half a thousand or five tenths per flute but our job as machinist is to make sure the actual chip per tooth stays above that sort of no-go zone so what I like about this is we've just added this red bar which I can move around anywhere but what I care about is where does my actual IP t this blue curve intersect with the zero point zero zero five that I don't want to go below so it's about right there so I drag this bar over this is kind of look looks like if my programmed feed rate was one thousandth of an inch per tooth I cannot go below a seventeenth a lick and see if that matches up with this formula up here if I see we're at one thousandth of an inch programmed radio step over of zero point zero one seven sure enough that's right at five ten so you wouldn't want to go say 0.01 because now or underneath that value so let's say you're doing a five foul radial finishing pass that's only two or three tenths that's too little per the rules I'm telling you follow what do you do pretty simple all you've got to do is increase your program to feed rate so we'll change it from one thousandth of an inch to two thousand seven inch and that alone was enough to increase the actual two above that magic number again go watch that Sandvik video folks we've got a ton of information coming in fact we're just about to launch a new website focus on everything of regarding learning c and c learning fusion 360 learning speeds and feeds more information on specific materials and specific tools folks I love doing this stuff thanks for watching take care see you soon [Music] [Music]

Channel: NYC CNC

Views: 135,926

Keywords: tormach, fusion 360, how to, cnc, machine shop, nyc cnc, DIY, machining, milling, CAD, cnc machining, cnc milling, speeds and feeds, chipload, tutorial

Id: uw8uL2jjEBs

Length: 19min 48sec (1188 seconds)

Published: Wed Sep 20 2017