Hello and welcome to Sandvik Coromant's Optimizing Turning Operations and Aerospace HRSA Materials. I'm Bill DeRoe, Global Engineering Project Office Manager with a focus on aerospace, space and defense. Hi, I'm Scott Lewis, the Turning and Aerospace Industry Specialist here at Sandvik. And I'm Doug Evans, I'm a Turning and Grade Specialist at Sandvik Coromant. Sandvik Coromant is a safety first company, so please be mindful of your emergency exits, your assembly points. If you're in a manufacturing environment, please make sure you have all the proper protective equipment. If you're driving in a car, please make sure you pull over on the side of the road or find a safe place to park and listen to our presentation. Today's agenda will cover materials as well as machining challenges and some cam processing. As well as heat resistant super alloy grades optimized for these areas. Core Cut 2, which is our main parting, grooving and profiling family. Core Turn 107, round insert platform with the rails. And we are also going to cover some process applications, some pocketing methods, and then we're going to have a summary at the end, and then we'll do a live Q&A. We'll first touch on HRSA materials and their machinability and characteristics. Some of the challenges we see when machining heat resistant super alloy materials. The components themselves typically have thin walls, complex shapes, deep cavities and pockets, which are hard to reach, long overhangs, which can make unstable setups. Surface integrity and finish. In some applications and materials, you have to worry about grain distortion, white layer, and actually the surface finish itself. It's difficult to change a proven process. In some applications, there's certified or approved processes that exist, and you can't just change a grade or a tool without getting recertified. We're looking at edges per part, not parts per edge. These materials are extremely difficult, and they really beat up on your inserts, so tool life is essential. The production planning, programming methods, for example. The proper choice of tools and grades is important, but the programming techniques and how to apply those tools is even more important in many cases, especially with these difficult materials. The materials are high cost, and the machinability is 10 to 30 percent of steel. So many of the forgings and castings we deal with today are in excess of tens of thousands of dollars. So we need to be very cautious and particular on how we process these parts and not to scrap the different components. So when we look at HRSA materials, we look at their machinability, but we look at some of the characteristics of how they're actually built. We look at them in three different ways. We have the nickel-based, which is mainly about 50 percent of the weight of an aerospace engine. Typically, we see materials like 718, Inconel, Waspoloids, and Udimets. They could be hardenable. Some are not hardenable, such as Inconel 625. We also have some iron-based materials. Common to the industry is Inco 909 or Greek Askeloid or A286. We also have cobalt-based materials. We see more common in some of the engines as of late, but typically we see that in a lot of also in medical industry. Common materials might be cobalt-chrome, the Hanes materials, and also stellates. Also, we're not going to so much touch on it in this presentation, but titanium. We actually look at the two a little bit differently. They have different characteristics and different tooling profiles are also used in these materials. Most common one that we see in the industry is the titanium 6AL4V. It's an alpha-beta material. So it's a combination of an alpha phase and a beta phase. Very common in the aerospace engine as well as structure. We also see some other materials like TIE 17, also in the engine area. When you look more towards the frame area, we see more of the beta type of materials like the 1023 or 5553. Very difficult to machine materials. Many of the challenges of these materials are strength retained at high temperatures. They're heat resistant. They're designed to handle higher heat applications, hence why we see them in the aerospace engines. What the challenge is, is very high cutting forces. So you need to make sure your machines can handle these types of cutting forces. Poor thermal conductivity. As I mentioned earlier, they're designed to resist heat. So higher temperatures are generated in the cutting zone. So particular care needs to be taken on your applications and also the geometries and the edge preps on your inserts. Some of these materials are actually hardenable, as we mentioned. Upwards of 46 plus Rockwell. So the surfaces are prone to work hardening as well. So high tendency for notch wear. So again, special care needs to be taken when we're actually using our inserts. Some of these actually have hard carbides in their structures, hence abrasive wear. You're going to get a very extensive flank wear on these inserts. Also prone to burrs generation. So when you're exiting the apartment, your components, you're going to get a risk of actually getting edge chipping. When you talk about the hardness, Bill, small changes in hardness in these difficult materials can make a drastic difference in the cutting data. That's correct, Scott. Even the condition of the material. A standard piece of block material is going to be a machine that's completely different as a forging or a casting. So all these things need to be taken into consideration. And with the high temps generated, the use of cooling through tools or high pressure cooling tools is critical in these areas. Another good point, Scott. So you've got to remember, these materials are designed to resist heat. Coolant is essential. And I think you'll touch on that later on in our presentation. Next, we're going to touch on HRSA grades. Grades are actually optimized for these types of materials. And we'd like to introduce Doug right back to our presentation. We have two new grades that we just introduced in March of this year called GC1205 and GC1210. As Bill mentioned, these are optimized for heat-resistant super alloy materials. So we're going to look first at grade 1205. And this is our next generation PVD-coated grades. And largely look at final stage machining with this grade. Also some intermittent stage machining. And also we look at the recommended cutting speeds of up to 328 surface feet with this. And if you notice at the finish recommendations, you know, we're at the feed rates anywhere from 4,000 to 6,000 per rev. You mentioned PVD, Doug. What is PVD? PVD is a physical vapor deposition that it's a low temperature process for coating inserts. And it allows us to keep sharp edges on the inserts when we do a PVD-coated process. And sharp edges with these materials that tend to stick on to inserts is important, I think. Yeah, very important. We want to slice that material, not push that material. Another grade we have was the 1210 grade. And this grade is mainly geared for intermediate stage machining. It can be used for finishing as well. For non-machine surfaces where edge line security is more important. Where notch wear and crater wear is seen on the insert edges themselves as your primary wear. And it's a complement grade, the 1205. The speeds in this grade, because it's intermediate stage machining, is a little bit lower versus 1205. 130 to 260 service feet, typically. And the feed rates are higher, again, because of the intermediate stage machining, 4 to 14 thousandths. And that depends on the shape of the insert and the radius of the insert you're using in this case. But this grade is also a PVD-coated grade. Here we get into the grade positioning with all of our grades. And we're really going to focus kind of on to the right side of the screen. This is where the new next generation PVD-coated grades fit into our portfolio. You have 1205 and 1210. We also have a CVD-coated grade, which we're going to talk about a little bit later on. And that's S205. And what other grades do we find in these applications, Scott? Some of the other grades you see is CBN or cubic boron nitride, which is used in nickel-based materials for high-speed finishing operations, low depth of cuts. You have your ceramic assortment as well, more for the intermediate stage to first stage machining or roughing operations. Some companies are also using ceramics with high speeds and semi-finishing. But you still need to clean up that component with carbide after the ceramic, typically. Yeah, like Bill mentioned, its surface integrity is huge in these components. You also see the 1205 and 1210 overlap each other here, as well as increase the speed capability versus the grades they're replacing. Here we have a grade 1105, where we are looking at flank wear and crater wear. Here are the speeds and feeds we've ran these inserts at. And as you can see, we have a very defined flank wear area and a crater wear area on the insert. So the top side of the insert, you're looking at it. The crater wear and the flank side of the insert, you're looking at the flank wear. And I see the flank wear is 7.5 thousandths with a max of 11 thousandths. And typically aerospace companies will have a flank tolerance on the wear on the max from 8 thousandths to 12 thousandths. Sometimes a little bit higher before they change that insert. But they usually like to change them in that 8 to 12 thousandths flank wear. And this is well within those limits. Yeah, and in flank wear, you've got to remember, creates heat. And heat's detrimental to these materials when we're machining in the final stage. Right. For surface integrity purposes, it's very critical. Yes. Then we look at 1205. So with the same cutting data at 230 surface feet, at 5 thousandths feet and 10 thousandth depth of cut, now we're achieving over 45 minutes of cut time. Everything else remained the same. We just changed the grade. And the tool wear in this example is less. 6 thousandths, 7 tenths to around 8 thousandths max. Again, well within those flank wear tolerances that we like to see. Yeah, and you can definitely see the difference in the crater wear on the top side of this insert. So in this case, this insert is worn. You can slow it down and get even longer tool life or maybe even speed it up if you don't want the 45 minutes of tool life. Correct. Now we'll cover a grade, CVD grade S205, which is a high-speed carbide grade that we came out with probably a year and a half ago. Yeah, like you said, it's a high-speed carbide grade for heat-resistant super alloys. Normally you're looking at 30 to 50 percent increase in cutting speed over a PVD-coated grade. With this CVD-coated grade, it's very unique because it's a very thin CVD-coated. And we're also able to do it at a lower temperature in the CVD process with our new technologies. So therefore, we can keep the edges pretty sharp for these materials and then take advantage of the CVD-coated process. And with CVD-coated grade, we have a greater heat barrier. So that might explain why we see excessive speeds here of over 400 surface feet, which is pretty impressive for a carbide grade. Yeah, very impressive in these materials. The main application area for S205 is intermediate stage and last stage machining. As Doug mentioned, the finishing operations typically. Pre-machined surfaces. We do offer some heavier chip breakers that can get into your first stage machining, but it's more geared toward your intermediate to finishing operations. Nickel-based materials is the main material area, but it can also be used in stainless steels and cobalt-chrome materials in the medical industry. Aerospace engine components like turbine discs, rings, and casings would be typical components to look for. Oil and gas also uses some nickel-based materials, so it's pretty common to see this grade being used in that industry as well. Yeah, and the unique thing about this grade, because of the speed that we can get out of it, it really fits between that area where we have our old legacy carbide grades at the slower speeds and where you can run the CBN at much higher speeds. So this kind of fits that window or that envelope where we can get more speed and get productivity out of the... Yeah, like you said, Doug, it's creeping into the lower end of what CBN grades can run at. Yeah. Here's S205 again. It's just some pictures we're going to show with S05F being what S205 is replacing in somewhere in the future. Not now, but it is a complementary grade right now to S05F. And you can see the distinct advantage of the S205, the new CVD-coated processes that we have. Very distinct advantage on flank wear with these inserts. And like we said, flank wear creates heat. And what does heat do, Scott? Well, heat is not good for insert tool life. It will wear down the insert. And also, we don't want to introduce heat into the components as well for the surface integrity. Correct. We also see the flank wear, as Doug mentioned, is we're saying 103 microns, which is around 4,000 flank wear. Again, well within those flank wear limits. So this insert could run a lot longer or maybe even a little bit faster than 410 surface feet. Yeah. Flank wear also size control. So if we can maintain that flank wear, we're going to maintain that size on that component for a lot longer period of time. That's correct. So grade S205, and now we're looking at an intermediate stage machining. And what we would see typically in results in this case, 20 passes running for 20 minutes of cut time on the right side of this slide. Nice, even, what I would call classic flank wear. So this insert could most likely run more than 20 minutes, but in this case we ran it to 20 just to see what would happen. And with more aggressive cutting data as far as the depth of cut at 80 thousandths with a 20,000 feed rate. And the speed is a little bit lower at 200 now because we're taking those heavier depth of cuts. Yeah. And again, if productivity is what you need and you're only looking for 8 to 10 minutes, which is the common time and cut for a lot of these materials, speed this thing up, take advantage of it. Our CoreCut2 platform we mentioned during the agenda. This is our main platform for parting, grooving, and profiling and pocketing operations. And some of the new features with the CoreCut2 platform is the, obviously, is the great technology, which we've been talking about. We've also introduced a whole new pressing technology with some of our inserts, especially in the CoreCut2 design. We hold the edge a lot tighter, a lot cleaner. It comes out post-treatment processes, nice, clean, defined edge. New grades, 1225, which we're going to talk about a little bit here on a few other slides. That's new. Obviously, we still have the 4425. We added Cermets into this. So Cermets may be more into the lesser, harder, not tie, but ink and L materials that's more metal-based instead of nickel-based. And then we also have our services here where you can go up online, get into our services that we have online, look at our cutting data, and see what recommendations we have for these materials. We'll look at the two holders. We also have some nice improvements, which we'll talk about here in that area as well. And one of those improvements is going from a V-bottom interface tip seat to a rail tip seat. Our system today for 157 wide and up is a rail tip seat. And from 118 or 3 millimeters down below was typically a V-bottom tip seat in the past. Now we have a rail tip seat all the way down to 2 millimeters or 79 thousandths. For more rigidity, especially when we're doing pocketing and profiling operations or side turning, this becomes very critical and increases the stability and security of your processes. Also, in all the inserts now in CoreCut2, we have wiper technology. And what does wiper technology do for us, Scott? Well, the wiper technology and inserts like this will improve the surface finish on the side walls as you're plunging in and creating grooves. It also enables you to increase your feed with the same surface finish. The typical rule of thumb would be to double your feed and keep your surface finish or improve your surface finish two times by keeping the feed. Yeah, and obviously if we can double our feed, we're going to reduce our cycle times. Yeah. And here's just the grade chain that we have today in this CoreCut2 platform, really geared towards the heat-resistant super alloy materials. And you can see the new 1225 grade sits right there in the middle. In the middle, so that seems to be a first choice. Also, first choice would be 1105 in these grades also or in these geometries. And 1105 will be upgraded to 1205 later this year in the CoreCut family. And H13A that you see on here, that's more geared toward aluminum materials and titanium materials, not nickel-based. Correct. Correct. So some of the tools we have have cooling through. Part-off blades now for CoreCut2 that have the cooling through from above and below, as well as the, in this example, capto but also shank holders will have cooling from above and below with a screw clamp system for better security, as well as the rail tip seat that we discussed earlier. So I like to discuss a little bit about coolants in these nickel-based materials, Doug. So it's critical to have the right concentration of coolant to get consistent tool life. And we like to see coolant concentrations in 10% or over. Over 10% is even better. Yeah. The more lubricity we can get in these materials through the coolant, the better the tool life will be. And we typically see in many customers running in 5%, 6% range. And we know it's difficult to maintain those percentages in some systems, especially if you have individual tanks and they're manually being adjusted. It's hard to keep that concentration consistent. But if you can keep it over 10%, that's really ideal. Yeah. And don't forget, when we look at our holders and we have the screw clamp design, what's the most important thing we need to do when we have a screw clamp holder? The most important thing, Doug, is to use a torque wrench and torque it to the proper torques that we have on our website and our catalogs. Yeah. We over-torque this. You're going to crack that insert. So if you're cracking inserts in half, that usually means you're over-torquing a clamp design holder. That's correct. And then here we have, again, just a S205 and the RM geometry. And again, 10 passes. We did increase the speed to eight, where we got eight passes. But you can still see a very defined edge line on that insert and some really good flank wear on those inserts. Yeah. In this case, it was the RM chip breaker, which you can see is a full-radius chip breaker that we have in a core cut family. And it's used more for the intermediate stage machining, some roughing, getting into some semi-finishing as well. Yeah. And also, you can see we used proper techniques, which you and Bill will be getting into later on. Rolling on and rolling out of cut. Yeah. Very important. Now we'll talk about Core Turb 107. This is our round insert platform with a rail interface. This animation will show the system and how it goes together and how it works and the advantages. We have a shim, which has a rail on top of the shim. It's screwed down and secured into the pocket of the holder. The inserts have serrations on the bottom. And the amount of serrations depends on the diameter of that insert and the application area that that insert is supposed to be running for proper indexes. Here we're showing, based on what direction you're turning, where the forces are being applied on that shim and the rail. Yeah. And the beauty of this is you can do bi-directional turning with this because you get no movement out of a round insert. So the old designs where you just had a screw holding it, if you went the opposite direction, you actually could see some movement. With the rail system and the screw, there's no movement in the insert. That's true. And some customers that run round inserts without the rail, they have insert movement or spinning of the insert, and sometimes they don't even realize it. Correct. And again, some of the features and benefits of the 107. The most important thing is the rail system locks that insert in place, again, bi-directional. Some of the newer geometries we have in this also, and the new pressing technologies and new grades. So there's a lot of benefits for the CoreTurn 107 rail system. We also have that CBN-topped insert with a hull, which is pretty unique. Yes. And a round insert for high-speed finishing and heat-resistant super-aller materials. And again, you and Bill is going to talk about this later, but as you use a round insert, you get that chip thinning effect. So now you can increase the feed and decrease your cycle times. The main chip breakers that we have in this offer is L3 for light, M3 for medium applications, and H7 for your heavier operations. And it makes sense that the heavier, you can go higher depths and higher feeds, where on the L3 side, you're more in your finishing, lighter depth of cuts and lighter feed rates. Yeah, it's real important to use the chip breakers in the application areas that they're designed for. They're designed that way for a reason. And the M3 probably has the widest application area. So if you're looking for an insert or a chip breaker that can cover many operations, the M3 would be the one to look at. And we'll take a look at a video showing this in action here. We're running 230 surface feet, 71,000 step to cut, and almost 24,000 speed rate. Yeah, the beauty of that was, one, it was dry so we could see what we were cutting for the video purposes. But in these materials, we recommend coolant for all these materials. Yeah, always coolant if you can. And coolant through tools, high pressure coolant, always very important, these materials. But I wanted to highlight again that feed rate in that video was around 24,000 speed rate, which is quite fast. And Inconel 718 aged at around 43 Rockwell. And we were able to do that because, as we're going to talk about coming up here now, the chip thinning effect using full radius or round inserts. Correct. And we're going to bring back Bill to help you on the application side of it. Okay. As we mentioned, we'll talk about application considerations now using primarily round inserts. And you saw in that video, again, the chip thinning effect. In that example, we're running at 15% of the diameter of the insert depth to cut ratio. And we'll talk more about that coming up. Before we do, we'll talk about insert shapes. With the round inserts being the strongest shape insert that there is out there. We're very flexible and probably still underutilized. But every shape has its place because some features or some components require the use of a D or a V to get into small radii's and corners of components. Or maybe the need because of the setup or the sensitivity of that component is so sensitive that we need less cutting pressure on that component or on that setup. So that's where these other shapes come into play. But we'll focus more on round inserts now, Bill. As you saw from the previous slide that Scott was speaking about, we talked about different types of insert geometries. And what we need to consider is actually the entering angle of the different components. When you're dealing with these types of heat-resistant materials, one of the considerations we need to worry about when it comes to our tool life is actually notch wear. And you can see that highlighted right here where a notch is being developed. That's because the notch is being developed at that depth of cut. But as we start to put that insert on an angle and as the angle starts to change, you see that start to go away. But you can see here, even on an SMG style insert with just a little bit of an edge line, you can see right here that the notch is actually starting to develop. So we need to be very mindful of that. So as we start to switch the insert more on a 45 degree, as you see on an SMG on a 45 degree entry or on our CNMX inserts, you can see now that notch is going away. We don't see that anymore. And what's happening now, we're starting to get a very nice, clear, even flank wear. Okay. And you can see here, now that we get into the round inserts, based on the depth of cut, the entry angle is around a 45 degree. You can see here, too, we start getting that nice, even, predictable flank wear. Ideally, this is what we want to see in the applications. We have HEX on this slide, which is the chip thickness. And as Bill explained, for a CDMG at a 95 degree entry angle, the chip thickness is equal to the feed rate. So for an example, if your feed rate's at 10,000ths, your chip thickness will be 10,000ths. But on the other side of the screen, using a square at a 45 degree entry angle, now that chip is 0.71. So typically around 7,000ths then for a 10,000th feed rate. So you're thinning that chip out. And if we, in this case, we probably need to accelerate our feed rate or increase our feed rates to compensate for that chip thickness. And if we don't do that, what are some of the problems we might see? Yeah. What will happen is you actually wind up underfeeding your inserts. These materials, as noted earlier by Doug, was these materials like to be sheared. If they're not sheared, what they're doing is actually rubbing, and you're actually creating more heat. And again, these materials are designed to resist heat. That heat builds up in the area, and you're not going to get a predictable situation when it comes to tool life. So be very mindful of this. I think the other thing we should mention, too, is the geometry of the inserts is also indicative of what the geometries are we're actually manufacturing. Sometimes you actually need that CNMG-style insert to go up against a wall to create that geometry. Yeah, that is true. So coming on to a part, we never want to come on to a sharp edge. It's very detrimental to the insert. You can get inconsistent tool life. So we like to roll on to the component if possible. An alternative to rolling on would be to make some form of chamfer on the edge of the part to soften that entry point. 45 degrees is typically what we'd like to see, but you can choose other degrees as well as long as you can soften that entry into that component. If you don't, again, sharp edges are going to destroy an insert over time and be inconsistent. Yeah, and I think one of the things you'll find is many times when an insert fails, it's going to either be on the entry or the exit of your component. So a lot of care needs to be taken when you're entering and exiting the components or the feature. Yeah, you mentioned the exit. The exit is almost as important to roll out of that exit as well. Correct. You've got to think of all those pressures being built up inside the insert. Once it's released, those pressures come back, and you have to worry about that. So extra care needs to be taken into that. So depth to cut, we talked about earlier about the feed. So one of the things you've got to take note of is your feed. This is actually your machine function. This is actually what you're putting into your program or your machine. But then you get your ACX. That's the function of the insert. That's actually what the insert's actually seeing. When you're going full depth of the IC of the insert in this case, what's happening is that insert is actually seeing that full load on the insert. But as you get down and you decrease your depths of cut, what's actually happening is you're actually thinning that chip. So this whole area, you're actually building up heat in that cut zone. So when you actually drop that depth of cut, you actually need to start increasing your feed to maintain that proper chip thickness. Those inserts, those geometries that Scott and Doug highlighted earlier are designed to handle certain of a feed. So we need to make sure we're in that window of that insert. If not, what's going to happen is, as we mentioned earlier, you're not going to shear that material anymore and you're going to start rubbing that material. Hence, you're going to build up more heat and you're going to get a not a predictive situation. So some of the best practices I mentioned earlier in that video, 15% of the IC, or in this case, that stands for inscribed circle, and around the IC or inscribed circle is equal to the diameter of that insert. 15% percentage ratio is usually ideal, especially when you're going into corners on a component. If you're just running straight cuts, you can get as high as 25% of the IC or diameter of that insert. But keep in mind, as you go into corners, you increase your engagement and you could get wraparound or too much contact and introduce vibrations into that component. So a 45 degree is really a nice area to be in and a safe area to be in if you can keep it there. Yeah, agreed. We found at that kind of angle, we found that you get very predictive tool life, very good predictability on your process as well. So we talked about all those different types of entry angles, and here's just a chart showing you where they are based on the IC, the insert, and then your depth of cut. And you can see we highlight, as mentioned earlier, at that about that 0.15 ratio at about 15% of the IC, the insert, we actually have a feed factor here where we can actually increase our data. So depending on your depth of cut, at this depth of cut on this IC insert, we're about that 45 degree entry angle. Ideal situation for those inserts. And what we want you to be mindful of is based on that depth of cut, you need to increase your feed. So what we have here is this really nice chart that shows these feed multiplication factors. So you basically take that factor, multiply it towards your feed based on your depth of cut, and you can see down here, it'll actually give you in this calculation what the actual feed should be based on that depth of cut to make sure you're actually shearing those materials, not rubbing that material. Yeah, in this example, that feed factor now becomes 20,000s feed rate to compensate for that chip thickness. If you remember in the video we played just a little while ago, we used a 472 of an inch diameter insert or 12 millimeter at that 15%, and we were feeding close to 24,000s. So we're even above this in this example. So look at this chart, looks a little cumbersome. Do we have anything that can help our customers? We have various calculators that can calculate this to make it easier. Also, some of the more modern CAM programs that are out there in the softwares also calculate this for them. We also have our website as well as reach out to any of your salesmen that can help you with this as well. That's right. Cora Plus Tool Guide is a good tool online for a digital service. Now we'll talk about pocketing methods and some of the CAM options that there are out there and different methods to achieve or open up a pocket or a cavity in a component. So you can see here there's various different ways to create these types of pockets. And these are kind of representation of the different types of features we see on some of the aerospace components common scene. It might be disks, blisks, even on different types of casings where we have features very similar to this. And we're going to discuss all these types of applications. The plunge turning, ramping, tracoidal, dynamic, as well as scoop turning. But before we get into those, let's like to cover machining against a wall, for example. Remember the 15% rule that we mentioned of the IC or diameter of the insert, depth of cut ratio. If we're coming down a wall and across making a 90 degree, you get excessive engagement. In this case, 100 degrees or equal to upwards of 60% of the diameter of the insert. So what's going to happen in that area with too much engagement, you're going to get vibrations. And you could ship out an insert if you're using a wear-resistant grade. In this case, if you can't change your program at all, you have to go to a tougher grade in that case versus a wear-resistant grade. But on the examples on the bottom of this slide, here we have a program radius equal to 25% of the diameter of the insert. In this case, the program is driving that insert around with a larger radius, decreasing that engagement in that corner or in that pocket. To the right, even better yet, the program radius is equal to 50% of the diameter of the insert. So even better. Here you have a bigger radius, very safe. In this case, you could probably maintain your feed rate around that whole radius and along the bottom of the component here. Yeah. The other thing you have to take note too is that heat propagation area where we talked about that heat, how detrimental it is to the inserts. That's right. A method that we're going to talk about now is plunge turning. And you see the toolpath strategy and cam simulation on this slide. This is an older method. It's been around for quite a few years. In this example, we're showing it being used with a full radius insert. But this could also be used with a square-ended grooving insert that's designed for turning operations. Some of the advantages. It's a simple method. It's very common to be available in cam softwares. It's been around. It's been improving. But as you saw in the animations and videos in the previous slide, you could have excessive engagement before you start changing directions. In that case, you're going to have those classic vibrations and inconsistent tool life. And poor chip control. Yeah. One of the things I think, too, we've got to consider with poor chip control is you could damage your parts, too. Not only do you have to worry about the vibration, but chips can get wrapped around your components and scratch and mangle up on your components and actually potentially bind a tool. Yeah. Especially in a finishing operation. You don't want to have those reworks or a scrap part. Even recutting of chips could be an issue as well. If you don't get that out of there, it folds back over itself. You're doubling your feed rate on that insert and hence have an unstable situation. So one of the techniques we look at, it was quite common and pretty easy to program, was the ramping technique. Where you come across the part in a ramping. You're changing your depths of cut, which actually helps support the situation where we get that notch wear. But one of the things you've got to make sure is, as you're coming across, then you could see it actually was going at an angle. When you come back, feed back the opposite direction. You want to make sure you're actually coming straight across, not angling. If you're angling, you're actually doubling your depth of cut and it could access the depth of cut of the insert. So you need to be mindful of that. So what's nice about this strategy, as I mentioned earlier, is it avoids that notch. So typically where you get that notch wear on the depth of a cut that the inserts were progressing through the cut, you avoid that by constantly changing that engagement as the insert progresses through the cut. And you could see here from the sketch, very simple method. You could actually do it right on the machine. Very smooth change back and forth. Various depth of cut, so you don't have to worry about notch wear so much. But the problem is that you need to vary your feed with each pass because you've got to remember, as you're coming down on that angle, that depth of cut is constantly changing. And we talked about that chip thinning earlier, so you need to be mindful of that. So good for spreading the wear out over a larger area of that insert. But on the one side of the stroke here, you could have excessive engagement and wraparound and shatter issues as well. Maybe one method or one remedy to that would be to back off on every pass by a few thousand so you're not engaging so much of the insert on the end of that pass. Very good point, Scott. And it's very similar to the situation we saw in that plunging where you're still coming up against that wall. So the insert is still seeing that engagement right there. So when you come against that wall and you go to change direction, you're still getting that wraparound right in here, whether you know it or not. You're building up that heat in that zone, and you have an unstable situation. Another method is tricoidal turning. This is a method that we came out with some years ago. Prior to the next method, we're going to talk about dynamic turning. This is a good process where you're rolling in and rolling out of the cut. And some of the advantages we see here, because you're rolling in and rolling out, that's easing the insert and increasing the tool life. But as you're rolling in and rolling out, you typically decrease that feed rate. And in those areas, you could have poor chip control or less chip control. So in this case, maybe not as desirable on entry and exit. As you travel across the bottom of this pocket, in that case, you can accelerate your feed rate to your program feed rates. And as we saw with the plunging or even with the ramping technique, that arc of engagement you see here actually decreases now because we have that radius that we're applying on the entry as well as the exit. So a smoother transition back and forth. As that insert travels along the bottom, because at that point, it's a consistent depth of cut, you could develop a notch where at that depth of cut, because we're not variating the depth of cut at that point. So it's nice. A lot of the CAM providers today actually have systems built within them. CAM cycles that you could actually implement into the operation. The one we're highlighting right now is dynamic turning, which is found in Mastercam. You could see how it actually works. It does a nice algorithm right here, which actually rolls the cutter into pass, comes back up and up again. But then it's constantly keeping that constant engagement so that feed remains the same. And also, the in and out of cut is actually rolled in and rolled out, very similar to the tracoidal technique. But as Scott mentioned now earlier, that the technique is actually built inside the CAM systems today, where years ago, you would actually have to draw all those profiles in there to create it. Today, the CAM providers actually provide that for us. So it becomes much easier to use a method like this now in today's time. It is. And we see customers using it a lot more, which gives you better predictability, better tool life on your operations. And the advantages are good chip control, decrease on the notch wear, because you're actually, as you're coming down in and out of cut and that radius in and out of cut, and you don't have as much vibration. You can actually use more wear-resistant grades, harder grades now, because it's a stable operation. You don't need the toughness anymore. You have to worry about pinching those chips and binding chips anymore. It's very easy to use now because of the CAM systems today. As you mentioned, you could use a more wear-resistant grade or a harder grade because this method is so secure and consistent. Where with some of the other methods that we previously showed, you might need to use a tougher grade and slow down your cutting speeds, which would extend your cutting time to make that feature. Correct. And as I mentioned earlier, that the different CAM providers out there provide these today, and I just highlighted a couple today. The dynamic turning and master cam waveform, nonlinear turning, adaptive turning, and value turn are just a couple out there today. So your master cams and your Gibbs cams, for instance, these are some of the softwares that are out there today that can provide this for you. Another method is a method we came out with recently called scoop turning. And scoop turning is where you're rolling in and out of the cut from two different directions. And this was more designed for seal fin production or finishing of seal fins components, which we'll show you in the next slide. But also maybe with some ceramic inserts where you have some back cutting possibilities that ceramics do not like. So this would smooth out that process for using a wear resistance ceramic, for instance. I can also see this in thin wall applications where you're coming down, you don't put that pressure on the sidewall, which actually flexes the component over. Exactly. As you see in this slide here, Bill, with the finishing portion of a seal fin, we're using the scoop turning method rolling on to the crest of that fin and down the side and out, and the same from the other direction there. So this way we're not pushing the material one way or the other. We're not flexing that material, which is very important at this stage of the component. It's usually a lot of value-added steps have been performed already. If you scrap a seal fin on a component, it's a big cost for companies. So this would be a more secure, consistent, safe process. And then on the other side, for the roughing of a seal fin, we would use a tricoidal or dynamic turning method using a full radius insert. And we have inserts that are designed for seal fin grooving that are step-down, left and right-hand versions, as well as cooling through tools to help you machine these type of features. You know, that's something good to hear. I mean, years ago, it was always a challenge to find things specific to the aerospace industry. We're seeing now more optimized, not only the grades, but now you're actually talking about inserts that are designed for specific features on aerospace engine components. Actually really good to see. Yeah, standard tools. You can't always have standard tools of everything for every feature, but more standard tools available from companies nowadays. Next, we're going to talk about slicing in the corners. So now you've actually created that profile feature, and you actually might have used an optimized insert a little bit larger to create that pocket or profile. But we know in many applications where you might have a smaller radius in the corner or a little feature you need to actually take care of, something that might even be even more sharper than what's shown in the animations. So after we've come in and we've done our dynamic or tricoidal or slicing technique where we've actually opened up the pocket as we did maybe in this application right here, we need to actually come back and finish the application where we need to actually open up these corners right here. And ideally what you want to do is you want to use an insert that's smaller than the radius of the feature and come in here and actually take small slices and actually progress down into the feature as you can see here down in the lower side here to be able to slice that material out of there so you have a controlled situation. We don't want to actually take your insert, you can see in the other feature where you come down here and plunge straight in and then come across. You can see here indicated by the red pie piece right here what's happening and you have that heat propagation area. You want to be careful with that because again, lots of vibrations, unstable situation, and you're building up heat in that cutting zone. Many times you're finishing the feature in this application so you don't want to scrap a part in this specifically. So take the time to come in here, smaller insert, optimize it for the application, and come in here and take actually smaller slices that you can see here. And you can see here from the animations what's actually happening. When that insert came down, actually almost plunged into that corner, you saw that vibration tendency in there. Bad situation. And also we weren't driving that insert. We actually came in at a 90 and changed direction. So here, good optimized situation where the insert radius is smaller than the corner radius. Good operation. Good stable situation. And you can see here using the slicing technique. Coming down again, driving that, creating that little radius that we need to do. It might take a little bit longer during the process, but you remember we're dealing with very expensive parts, very difficult to machine materials. So efficiency, optimization, productivity are important, but also stability and process security are also important as well. And that concludes our formal presentation. So we'd like to bring Doug back for a summary. In conclusion, our pocketing solutions included the rail interface with the core turn 107 insert, V-bottom carbide and ceramic options, as well as our core cut 2 family and various full radius and profiling options, including 90 degree and the seal fin option. So in summary, we discuss HRSA materials and their challenges. The machining challenges we also have when it comes to sharing the materials, the heat propagation, things like that. We talked about the cam capabilities when we're creating pockets in the different types of applications. We talked about the productivity criteria when it comes to using round inserts and the chip thinning required, and why you need to maintain that proper chip thickness. We also talked about optimized insert geometries and grades specific for these families of HSRA materials. So I see we got some questions for us already. The first one looks like it's actually going to be for you, Scott. Do you have any grades that can machine many applications and materials? Yeah, this is a question or a wish. I know that a lot of companies like to see if there is a grade that can handle many different materials and stages of machining. And I would say out of our grades, the 1125 and 1225 in the core cut 2 platform, for instance, 1125 in our turning platforms right now would probably be a wide application area grade that can handle different materials and stages of machining. But I have to emphasize your risk and optimization in those cases. So it's always better to have an optimized grade and chip breaker to handle the stage of machining or the operation that you're trying to machine. Good. Yeah. I see we have another question. I guess this one's more towards me. Do you offer any support for component processing? Yes, we do. Actually, the team that I work on, that's exactly what we do full time. We support customer projects, whether it's features, materials or components themselves. We can offer everything from full cam packages to processing components from full turnkeys right down to specific features. So, yes, it is something we can support our customers with. The next question, do you have internal capabilities to support customer testing? Again, this falls on me. Yes, we do. We actually have a lab in Meblin, North Carolina. We have actually labs throughout the world that can support customer testing, where we can actually bring in customer materials and actually test them on our machines in real time, real actually applications. And we can also work with the cam and give full service for those types of testings. Next one. Doug, this is probably more aligned for you. Can CBN inserts used in aerospace materials? I know we touched on that during our presentation. Yes. And it's something that's been being more applied over the last few years. We have grades specifically for these types of materials. We have edge preps for this material. It works extremely well. It's not uncommon to see 20 minutes of cut time in a lot of cases with a CBN finish, only used in finish applications. But, yeah, we can definitely do CBN in aerospace materials, especially the Econel side of it. The tie side of it is no. That's more of a PCD type for finishing. So we're seeing that more and more also. I have to say the programming is very critical when using CBN or PCD inserts in these areas because they are sensitive to proper programming techniques. Yeah, most definitely. Another question, I guess, Doug, for you. We are using CBN in 60 Rockwell material and 440C material. Will you be developing more CBN tooling for smaller features? We have all the way down the seal fin grooves. So we do very small round inserts, cutoff inserts, grooving. It doesn't matter. We go all the way down to one and a half millimeters. I think the CBN is probably two millimeters as small as you can get. But, yeah, we have inserts now in stock on the market and just get a hold of your frontline salesperson and we'll be happy to come and look at your application and fit the product to your needs. I know we've made some customized solutions down to 60,000 or even as low as 50,000, some widths, full radius and square ended options. So the technology is there to get into the smaller width CBN tipped inserts. Yeah, and that goes back to what you were talking about, the scoop turning. Normally, if you're a thin wall, you're a thin component with a real small, real thin insert. So that's kind of where the scoop turning comes in with the round inserts. Another question I see here, maybe for Doug or Scott, do you have anything specifically for Aramit 100 in 35 Rockwell material? I know that's a material we're seeing a lot more on landing gear parts. I know Aramit, yeah, like you said, Bill, the Aramit 100 material comes up quite a bit in different hardness ranges. In this case, it's 35 HRC. We see a lot of our steel turning grades working pretty well in here, our 4,400 grades, as well as some of our stainless steel grades performing well in that application area. Next question. Will this presentation be made available after this distribution within a given organization for those who could not attend? Yes, it will be available. I think we could have all answered that one. Yeah. I think that's it for the question. Yeah. So I think we're good. Thank you very much for attending. Thank you for the questions you posted. Hope we answered them all. If there's any other questions or you need any other things from our team, please reach out to your local sale person or distribution, and we'd be happy to help you. Again, thank you for your time today. Yeah. Thank you, everybody. Thank you, everybody.