How to Program & Machine INCONEL 625 | XL TITAN-1M Tutorial

Hey what's up everybody this is Titan from Titans of CNC and today I'm excited because we're gonna take the level of teaching up a notch. Alright so today we're gonna actually focus on aerospace and machining a very hard material. So the material that I'm talking about is Inconel 625. So you may be asking why do I have to Titan 1M right here? Guess what? It's a little different. It's bigger now. So now instead of being 3 quarters of an inch it's actually one and a quarter by three by six. So it's a big part and we're not machining it out of aluminum we're machining it out of Inconel 625 which is a standard material that we use in the aerospace industry. This is one of the reasons why Titans of CNC Academy has now come out with BB Aero, Building Blocks Aero, which consists of actual aerospace components because we want you guys to actually learn on real parts that matter. But running Inconel is not as easy right? It doesn't cut like butter it is hard material so you have to upgrade your tools. Now when you step up to titanium and Inconel and monel and 15-5 and harder materials you need a different tool. You need a different approach but then when we step up and cut a material with a high nickel content the cooling the lubricity all of it comes into play and the coolant can literally make you or break you. All right so the first thing that we're gonna do is actually cut the top surface of our part and to do that we're gonna use a 3-inch Dodeca mini shell mill. So the insert that we're using is not the insert that I used 10 years ago this is a new insert this is the KCSM 40. It's a special blend of carbide so you can machine a perfect part consistently. So we're using this shell mill to create the first datum the first perfect surface and then when we drop down and create pockets and holes all the dimensions will come off that surface. So you see the part right here I got my excess Inconel the material I'm holding on to on the outside and then I got material all the way around and I got material on the top. Okay so if we actually go into my setup and go into edit come to stock you can see exactly how much material I've left. So we have 185 thousandths on X negative X positive 115 thousandths in Y so 115 in the back 115 up front I have 20 thousandths right here on the top surface and I have 340 thousandths on the bottom surface. All right so let me explain the speeds and feeds for the Dodeca mini. We have a service foot of 200 which is giving us an RPM of 254 and we have five inserts on this shell mill. So when you look at our actual feed per tooth 0.0056 is way on the bottom because the range on this specific tool and insert is 0.0056 to 0.0228. So as you can see we got sky on the other side but since this is a tutorial I wanted to slow things down. All right so in this pass we're just taking a little bit of material on the but it is Inconel and we want to have a beautiful surface finish. So another thing that I've done is we've taken one insert out brought in a wiper. So what is a wiper? So it's an insert that we use to bring out a beautiful surface finish. So all the other inserts actually come down and have a radius at the bottom that actually is cutting the material. The wiper actually has a flat on the bottom. The flat is about a hundred and ninety thousandths wide and the wiper actually sits lower than all the other inserts. So if the inserts were at zero the wiper would be set down at negative 0.0028. All right so that's the difference between the two and what happens is the first four inserts are gonna come and cut the metal and then the wiper is gonna come back and clean. All right so we're starting out with 200 surface foot but on the machine I might raise it a little bit to get a little bit more RPMs and then I will adjust my chip load to slow or speed it up to get that perfect finish. The shell mill comes across and just skims perfectly across that surface. All right so the first tool is complete now let's go to the next tool. The next thing I'm gonna do is actually come down and actually rough out this pocket, rough out all the material and start bringing the part to shape. I know that bringing an end mill into this inconel straight down is a problem right? We can helical and put a wear on the bottom of that tool and possibly get it done but that also is gonna take a long time. So to solve that problem I'm gonna take one of my multi-purpose drills that I use all the time, the go drill. This is a solid carbide coolant through drill that can pretty much drill anything. So from steels to stainless to titanium to inconel, monel, this drill that can get the job done. If I was going into production and I was running thousands of parts I'd probably go to an insert drill right? Like the Ken tip or the Ken tip FS or something similar so once the tool got dull all I would have to do at that point is change out the insert which is a lot less carbide to pay for and makes it affordable. In this case the go drill is the perfect choice. So the reason that I'm actually using a drill is to pre-drill where the end mill is going to drop down into the pocket. So my end mill is gonna be a half an inch. I just need a bigger drill diameter than the end mill so for the go drill I'm gonna use 3 quarters of an inch. That gives me an eighth of an inch all the way around for clearance. This is extremely important because when the drill drills it's gonna leave a tapered bottom because the drill point is not flat. It's at an included angle at a hundred and forty degrees. So when the end mill drops down it's actually going to hit the tapered material before it hits the bottom. So because I have a bigger drill than the end mill when I'm about a hundred thousand shy of hitting the bottom I'm simply going to step over at like a hundred and ten thousandths and I'm just gonna helical down to full depth at that point. Once I get to full depth I'm gonna start peripheral milling and just hogging out all that Inconel. Alright so now that we're ready to drill let's look at the speed of the drill. So the recommended surface foot that I'm gonna give you is about 70 to 130. For the tutorial I'm gonna keep it on the low end. So I'm gonna keep it right at about 84 surface foot. Nice and safe and a perfect speed. And then when it comes to the feed per revolution I'd say that we're about four thousandths to six thousandths. In this particular case we're just putting it right at four thousandths to hug that bottom level which will give us a perfect hole. So one of the things that I've done here is I don't actually know where the end mill is going to come down but I know that it's gonna rough this pocket. So what I did was I actually went to this surface and I actually drew myself a point. So that point right there and bring it up this point right here I basically just sketched it right there on that surface right there. And then when I call up the drill location I'm just gonna hit that point right there and the drill will come down in that place. And then when I go to do the pocket with tool three I'll tell the tool that I have a pre-drilled hole and it will automatically know to drop down at that exact location and start from there. Another thing that I'll point out is that this is a coolant drill. This is a drill that is specifically designed for hard materials and for getting the job done. So a lot of times when we're running aluminum we're pecking and we're just trying to get the material out in a hurry. In this case we're simply gonna grab the drill. I'm gonna turn the coolant on. I'm gonna bring the drill down and then we're just gonna drop full depth without pecking. Then we're gonna come out and go get the next tool. Nice and simple. Even though it's Inconel we don't have to peck because the coolant is actually flooding the front end of the drill. And the drill is designed in such a way that as it drills down it's breaking that chip and the chips are just flowing out of the hole. Alright so now that we've pre-drilled the pocket I'm gonna go to an end mill to rough the pocket out and rough out the outside. I'm gonna go to the Harvey 3 and it is a beast of a tool. My team actually nicknamed it. We called it the zombie cutter. This thing was dead and it just kept coming. Alright so now let's talk surface foot. When I'm in titanium we're peripheral milling right? So the old style of machining you actually drop down and you're only using the tip of the cutter. The cutters flexing and you're taking a big cut with the tip right? But now we're creating tool paths that instead of plunging off a dock they actually ramp into the material taking the pressure off. And we take a smaller radial but we drop full depth utilizing the entire flute length which brings stability and rigidity and allows us to go much faster. So in titanium if you look in the machinist handbook you'll see a 175 surface foot as a standard. But in Inconel it's another story right? Inconel is much harder than titanium so the surface foot is on the low end. So instead of a hundred and seventy five you're talking you know fifty to a hundred surface foot right? However because of the advanced tool paths that we're using, the rigidity in tool that we're getting, the coolant that we're using, all of the variables put together we actually run from 200 to 400 surface foot in Inconel. And we do it in a consistent manner over a long period of time okay? It's not just something that we're practicing with. So in this specific application we're gonna run at 210 surface foot okay? We're gonna keep it on the low end. On the inside and the outside we're gonna drop all the way to the bottom. Now our radial depth of cut so we're full depth so if you look at the outside you're probably at two and a half times diameter. That's deep. Now radially instead of taking a big step over we're actually gonna take a 4% of diameter step over. And then we're gonna put our feed per tooth at 0.0042 which is going to give us a feed rate 40 inches per minute which is incredibly fast for Inconel. And yet it's safe and will be consistent in the cut. So basically what you see is the end mill is actually taking about 0.020 per cut but you're 1.2 deep right? So it's just going around and cutting all the excess material. We actually had more material on the outsides on X than we did on Y and that's why it's going and finishing everything. Now it dropped into the pre-drilled hole and now it's actually cutting material. Now it's gonna come over there and rough out this section. Alright so everything's been roughed and we left 0.005 on every surface. So now we're gonna come back and we're gonna kiss it. Alright so a Harvey 3 end mill roughing Inconel. It's gonna get dull no matter what. It'll keep going and sometimes go for hours but since we're looking for a perfect surface finish on these walls I'm simply going to use a different tool to come back and kiss the side. So now we're using a different Harvey 3 end mill to actually finish the part. Now with tool 4 we're gonna drop into where we previously roughed and we're just going to kiss the bottom. But guess what instead of a 20,000 step over my step overs are much greater now because I don't have all of that material to cut through. I'm only cutting the bottom surface and I just want it to be beautiful. Right so I don't want all those lines so now instead of a 20,000 step over I actually have a greater step over. Alright so when it comes to the speeds and feeds on the surface footage it's exactly the same 210 SFM but the chip load the feed rate per that revolution I've dropped in half. So instead of being four thousandths we're at two thousandths chip load so 0.002 which gives us a cutting feed rate of 19 inches per minute. Alright so we already know with the current RPMs at 40 inches a minute it can rough all day. Boom boom boom right but now all we've done is taken the feed rate dropped it in half so that we can allow those cutters to work and give us a perfect surface finish. So tool comes down ramps into the bottom comes over here drops down ramps into the bottom. Because the tool is pretty long and taking the entire wall and I want to have a perfect finish I'm actually finishing the inside wall and then I'm gonna do a spring pass just to catch any of the deflection right. So the tool with the pressure is gonna want to deflect a little bit which is gonna make it so you might have a perfect tolerance up here but the bottom might be a little bit small because the tool deflected outwards. Alright so now I'm coming on the outside I'm simply kissing the outside doing a 2d contour all the way around it flip around to the back just doing a 2d contour all the way about. I'm taking a five thousandths finish pass. There's my spring pass so I'm not cutting extra material I'm just picking up anything that was left because the tool deflected because I want those walls to be perfect and perpendicular to that top surface. Took my first cut right there took my second cut to finish that surface. Alright so now we've come back and actually done all our finish passes to kiss all the surfaces and the bottom of the pocket to make it all perfect and to size. If this was aluminum I might come back with a chamfer mill now and actually chamfer all those edges and actually spot drill where my threads are gonna be but this is Inconel so I have a different approach because I don't want to send a tip of a center drill or a chamfer mill straight into the Inconel. It might handle for a while but it will wear out okay so strategically knowing that the go drill is self centering I'm actually going to drill first and then chamfer the outside afterwards okay so this is a go drill just like the 3 quarter inch but this one has a diameter of 0.257 which is the minor ID for a 5 16 18 thread which we will then come back and thread mill but now we're gonna pre drill the ID of that thread. Alright so the speeds and feeds remember what the surface footage was it was 70 to 130 in Inconel so we're going 85 it comes up just under 85 but it's basically 85 SFM alright the chip load on the smaller is gonna change a little bit okay so it's a little bit more aggressive for the bigger tools on the smaller drills I like my feed per revolution to be about two thousandths to three thousandths alright so let's just split it in the middle and go 0.0025 and then we're just gonna drill straight down come out go to the next hole boom boom boom we will get a consistently perfect series of holes same thing there's no peck I'm drilling straight down the coolant is blasting from the tip and it's just boom boom boom alright so now that we're finished drilling the 0.257 diameter holes we're gonna actually bring in our chamfer and we're gonna actually spot those holes to create this chamfer for the 5 16 18 thread alright so tool 6 is gonna be a 5 8 6 flute chamfer mill at an included angle of 90 degrees one of my favorite products that Kenna Metal has is the duo lock system it's a way to save on carbide alright so when you have end mills they literally instead of having this much carbide they give you just the end mill and actually put a tip on it that actually screws into a body right so it connects and then when the end mill wears out you basically unscrew it put another insert in screw it back lock it it locks perfectly in place and you just keep running and when you're running production this saves huge money is you don't have to pay for all that carbide so now that we have the holes already in place we're simply going to drop down and chamfer around the hole to a diameter that's approximately about 10% of the overall thread diameter we're looking at a chamfer mill we're talking a 90 degree included angle so each side is 45 okay that's why it's popular in machining especially manual machining because it's easy to calculate if I have a 45 degree angle all I have to do to calculate it when actually creating a chamfer is go edge to edge and basically I can just go okay I want to chamfer this edge five thousandths all I would have to do is go a hundred thousandths off a hundred thousandths down and then an additional five thousandths because it's a 45 degree it's equal so 50 over 50 down a hundred over a hundred down creates edge to edge anything beyond that is the chamfer all right so when it comes to Inconel I'm actually I have a 5 8 so in aluminum I might say it's a hundred thousandths and it's 50 off and 50 down right if I wanted to do a 10,000 chamfer I would just go 60 down right so it's 50 off 60 down but because it's Inconel I want to use the flute higher up and I actually want to give it some room to actually cut because I have six flutes okay so on the top surface I'm basically gonna hit right kind of in the center of the flute all right that's good but on the bottom surface the closer I get to the tip the farther the tool is gonna have to be away from this surface right so when you look at this surface if I'm close to the tip I'd have to pull my tool away from that surface and that means that the chamfer would be only over here because the tool was away from the surface so what I'm gonna do is actually call it a larger diameter so the software takes the tool and puts it right up against the wall but deeper so I can get my chamfer all the way over here so just like a little trick right so if you're running aluminum that's one thing if you're running on the top that's another thing in Inconel right with a six flute tool and if you're running down here in your next to a wall we're actually gonna call it and say it's a much bigger tool so we can actually use the top so we can get it close to the wall leaving the biggest chamfer possible because we want to chamfer everything inside the machine especially when it comes to Inconel all right so speeds and feeds for our we're gonna go 120 surface foot and then our chip load our feed per tooth we're putting at 0.0022 which puts our revolutions at 733 and at a feed rate of 10 inches per minute all right so now the chamfer mill has actually walked around the part inside the part deburred everything and it's going to chamfer the drilled holes now all right so it's gonna come straight down so one thing I'm gonna do is I'm gonna actually back off my RPMs because I don't want any chatter when this thing hits when it hits the full diameter and it starts taking that big cut I want to keep my RPMs low so I create pressure so the tool engages the material and it doesn't bounce all right so we're gonna start off with a surface footage of 60 and a bead per revolution of two thousandths it's gonna drop down it's gonna be slow but it's okay because it's Inconel and it's gonna make a perfect finish all right so we're on our last and now the last thing we're gonna do is we're going to thread it but I'm not gonna use a tap I'm gonna use a thread mill so this is a great cutter it's designed well and it actually gets the job done quickly and perfectly all right so if it's aluminum or steel like 303 something soft I will roll tap it or cut tap it depending but I love thread mills because thread mills you can comp them right if you have a certain amount of plating or if it's getting etched or if they're calling out the size you know larger because they're putting in an insert you can literally adjust that thread perfectly and not just that if a thread mill drops into a hole and breaks the thread mill is smaller than the hole right so it usually breaks clean up at the neck which allows you to simply stop the machine take out the thread mill put another one in because it's a thread mill and the tip to the first thread is perfect you simply can just reprobe it or rezero it and the thread mill will drop down actually pick up the exact thread now there's a lot of flutes on this thread mill and that's because the thread mill is specifically designed for a 516 18 thread all right because it has so many teeth this thread mill when it's will simply drop down move in to the major diameter of the thread in this case a diameter of 516 and then it will helical up one time for one thread so it's 18 threads per inch so if you divide that that would be 55,000 so it simply goes in and as it walks around that major diameter at 360 degrees it raises at the same time as it's going around so by the time you hit 360 degrees your Z has lifted by 55,000 and then the tool will disengage then through the entire diameter of the hole all of your threads all the way up will be perfectly cut so since this is Inconel I'm gonna walk in I'm gonna leave five thousandths and do one roughing pass I'm gonna come out I'm gonna drop back down I'm gonna walk in that extra five thousandths to do my finish I'm gonna do it one more time and then I'm gonna come out go down I'm gonna do it one more time just as a spring pass not to take any material but just to make a perfect thread and catch any material that's left because the tool might have deflected because it's hanging out so long in Inconel all right so let's do this so one of the cool things about the thread mill is you would think that you would drop down and just like inch around at like 0.5 feed rate or or something very delicate and very small but we're gonna actually get after it a little bit okay so our surface footage is that 180 all right that's a good surface foot right there and then our feed per tooth is that 0.0012 this is a three flute tool and that's gonna put us at a cutting feed rate of 10 inches a minute 10 inches a minute doesn't seem like a lot but when you're dropping down and you're only moving out like 50 thousandths you get there quick right and then when you move around in that small little space it moves quick so it's gonna go in boom out in boom out the tool actually has a hole going through the tool so coolant actually comes out the bottom it flushes those chips but because the diameter is 0.257 and the tool is 0.242 there's not a lot of space okay and I don't want to run those chips over so what I'm doing with an understanding that is flushing the bottom of the hole is I'm lifting up as I'm lifting up it's flushing the bottom it's pulling all the chips out so by the time I come up all the chips are out and then I just drop back in walk around again come out drop back in do my spring pass come around for a perfect finished thread there we go check it out the Titan 1m extra-large Inco version right there so check it out you can actually look at all the service finishes everything looks absolutely perfect we put the thread gauges in the go the no go everything is absolutely perfect the finish is nice and smooth all the way around part looks absolutely beautiful we haven't done any external finishing or deburring that is exactly how it came out of the machine I hope you guys learned something and if you love this video please hit that subscribe button below because we have a whole bunch more just like it coming CNC machining Inconel channel metal tooling making it happen boom