Hi and welcome to this webinar about high feed milling. My name is Antti Wikström and I'll be hosting this webinar here from Sandvik & Center today. But as always safety first, so we ask you to make sure you're in a safe location and know safety routines in case of an emergency. As I mentioned my name is Antti Wikström. I work as a training specialist for Nordics and North Europe and today we will be talking about high feed milling. So looking at milling we have of course different milling applications. One would be phase milling. Basically milling your phase, often without any particular relation to other phases. other phases in the process. Another one shoulder milling. Milling two shoulders, usually 90 degree. Then we have a groove milling for instance. Milling groove with for instance disc cutter. And then high feed milling. So what's high feed milling done? The other ones explain themselves quite easily, but high feed milling, we'll show that by a demo of what you can do with high feed milling. So we will be running a demonstration with the high feed milling cutter in 2541. It's 300 Brunel hardness. Using MH22 with diameter 50 first and then we will run diameter 25 after that. And insert, we start with 4340 grade with M50 geometry. So we'll start with phase milling. We'll run this at 200 meters per minute. To feed of one millimeter. And radial engagement of 35 millimeters. That's the cut 1.3 millimeter. Now we move over to pocket milling. So we do a helical ramping. Still at 200 meters. 0.7 millimeter in tooth feed. AE of 44 millimeters and pitch on the ramping of 1.3 millimeters. I can hear it's not the nicest pocket. We have a quite tight corner radius compared to the milling diameter. So it increases the engagement quite a lot there. But no problem handling it. Now we do a plunge milling. At 250 meters. And now we have dropped the feed to 0.12 millimeters per tooth. And we'll come into this a bit later. But when we change the direction that we're moving in, we get different entering angle. Entering angle is in relation to feed direction. And that then affects the feed we can use with the same thickness. The step over for the plunge is 5.5 millimeter. And we do this on the ramp or slope. And after that we will do a ramping cleanup for this. And this is not really the suggested process for plunge milling. Normally you would do this step by step. Side by side. For each increment inwards. To open up the pocket gradually. This is more challenging for the tool. To do it this way. To do a full full diameter plunge straight in. And then we do the ramping. Now we move over to an open pocket milling. Starting with the full slot. And then removing the corner. So we run this at 200 meters. One millimeter in tooth feed. And AE of 44 millimeters and 34 millimeters. That will cut 1.3 millimeter. And to show a bit of the benefit with. The high feed milling concepts. We have this a bit extended. The tool. It's a bit longer than it needs to be for these operations. And we'll come into that a bit as well. But that's also one of the benefits with. The high feed milling cutters. That you can use longer tools. And still get rigid setups. Now we do full slot milling. At 200 meters. 0.7 in tooth feed. And we get the full diameter engaged. And one millimeter depth of cut. Is 15? Hellenic. Now we move to a smaller diameter cutter, a 25mm, still an MH20. We have a different grade here as well, 1130, which is a PVD. And we start with an open pocket milling at 250m, 0.80 tooth feed, radial engagement of 17mm and depth of cut of 1.3mm. And in general, moving to a smaller cutter or smaller engagement allows us to use higher cutting speeds because we get shorter contact time for the insert. So now we do full slots. Here we also use straight entrance into the workpiece material. Same as before, which is also more challenging, but not the ideal way of programming. Do plunge milling of 250m and 0.12 in feed here as well and the step over of 5.5. Pocket milling. Ramping down and running is at 250m, 0.18 tooth feed and radial engagement of 18mm and depth of cut of 1.3. It's really high tooth feeds in all of these applications. And that's, I mean, that's the reason why it's called high feed milling. It's not 0.08 in tooth feed, but it's 0.8 in tooth feed. helical interplation. Helical interplation, 250m, 0.4 in tooth feed and diameter 38 on the circle milling here. The step down or the pitch of the helical interplation is 1.2mm. So, in summary, you can do a lot of different machining with high feed milling. Lot of different features and a lot of different machining types. And can be a really efficient way for roughing. But as you saw on the component as well, we get a bit rough surfaces. So, usually it's needed a finishing operation afterwards. So, why can we go at this high feed then? Well, as I mentioned, it's related to the entering angle. So, if you look at the 90 degree cutter, the hex maximum ship thickness for a cutter is equal to the tooth feed if we are machining at the center line of the cutter. If you are at the side, we get the ship thinning there as well. But if you are using the center of the cutter, then hex is equal to tooth feed if you have an 90 degree cutter. So, a hex of 0.1 gives us a feed of 0.1. But if we change the entering angle, keep the hex, it affects the tooth feed. So, if we have a smaller entering angle, in this case 75 degrees, hex is now 97% of the tooth feed. Really close. So, a 0 .1 hex gives us a 0.1 tooth feed. 0.15 hex, 0.16 tooth feed. So, we didn't gain so much by changing from 90 to 75 degrees in feed. But moving to smaller and smaller entering angles, gives us bigger and bigger advantage in feed capacity, which remained ship thickness. So, if you are at the 10 degree cutter, the factor is close to 6, 5.8. So, 0.1 hex, we need to use 0.58 tooth feed. So, to make this a bit clearer, we have an animation here. Where we have the ship thickness here in, or the ship here in red. When we move to 45 degree, ship thickness is 70% of the tooth feed. And moving down to 10 degree, the ship thickness is now 17% of the tooth feed. That means we need to increase the feed to get the ship thickness back again. We can't do machining with success if we have two thin ships. We need a certain ship thickness to get good machining. So, we need to increase the feed when we have smaller entering angles. So, we need to increase the length of the insert. We need to increase the cutting depth. So, we gain in table feed and in tooth feed. But we lose in cutting depth for the same length of engagement of the insert. And then, if we would like to increase the cutting depth, we need a longer engagement of the insert. Of the cutting edge. And that will then draw more power and more torque. So, that's something to consider and something we'll come back to a bit later on. Looking at round insert. Here, the maximum ship thickness and the entering angle is dependent on depth of cut. So, moving to a small depth of cut. Ship thickness is decreased. And we need to increase the feed to compensate and get the ship thickness back up again. The same here. More shallow cut allows us to go with the higher feed. But then, you need to go to a bigger insert, if you say, to get small entering angle and depth of cut capacity. And then, we'll get longer edge line in contact and draw more power and torque. And we can, of course, make calculations on this as well. So, general recommendation is to never exceed 25% of the insert diameter, the IC. But to get real high feed milling benefits, you need to go lower than that as well. So, around 10% or even lower than that to get the entering angle down to a level where you can really increase the feed a lot. So, entering angle. So, we state entering angle on our concepts. So, we have 90 degrees as long as we have feed direction here. So, as soon as we start to do rampings or as you saw in the demonstration, plunge milling, we get different entering angles. So, the 10 degree will get 100 degree entering angle if you are doing plunging. The entering angle that will then be between here. If you get new feed direction. The entering angle also decides the force direction. And that's, as I mentioned, one of the benefits with the high feed milling concepts. The high feed milling concept in having common that they are having small entering angles, which allows them to use high table feeds. Small entering angles means we get a lot of axial cutting forces instead of radial, as with the 90 degree cutter. And this then reduces the complication of having long tools. A long tool with a lot of radial cutting forces gets a lot of bending. And then you can get a lot of vibrations. But with the smaller entering angle, we get more axial cutting forces and in the more stable direction basically. So, I mentioned power and torque. This is an example of a power and torque diagram for a machine. We have the torque here on the left with some curves here. And we have the power to the right with some additional curves here. And these can be a bit complicated to read and we will not go into the details of power and torque diagrams this session. But you have several lines. In this case, the blue line is the continuous load. So, that's what you can expect from the machine to cope with on continuous duty cycle. But then we have some additional lines. And temporarily, the machine can handle more load, both in power and in torque, than the continuous. So, if have a high load, even after it will take longer time to recover. But in this case, we have a low alloy steel, 127 millimeters, five pitch cutter. Length of the cutting edge is four millimeters. And we have a cutting speed of 274 meters and hex of 0.178. This gives us a RPM, 688. A power requirement of almost 17 kilowatts and a torque of 233 newton meters. That puts us here on the power. So, the power is slightly above the available power in this machine. And the torque here is slightly above the available torque capacity for continuous action. So, this could be run temporarily in this machine. if you are machining continuously at this load, you will overload the machine. If you move to a smaller cutter and lower pitch. same length of the engagement of the insert here. You will get a higher rpm and different power requirement of 10 kilowatts and different torque requirement of 88 newton meters. Putting us here on the power and here on the torque. So now we are within limits for this machine. But as you see these curves aren't constant. I mean we don't have 190 newton meters all over the spectrum of rpms and we don't have the 25 kilowatts all over the board either in power. So depending on the rpms you will have different availability of power and torque in your machine. And that's something that you might need to consider and especially machining at higher rates of Q. And using high feed milling you can your machining at higher metal removal rates and you can expect that to draw more power. And you might not be able to use as big cutter as you're used to. Depending on the depth of cut for instance. So something to keep in mind when you are increasing the metal removal rates in your machine. Have we got any questions? No? No questions? Then I'll end off with the summary and perhaps just adding that the high feed milling concepts are available in different entering angles. So that gives you slightly different balance between depth of cuts and feed capacity. And also force direction. So that's something perhaps to consider for instance choosing between a 20 degree cutter and a 10 degree cutter. Which one will be more suitable for job you're doing. But with that I wish you all a nice day and until next time. Thank you. Bye.