Hello and welcome to this solid round tools knowledge session. During this series we will cover features, strategies and products relating to solid round tools. As always we start with safety. Safety is our top priority at Sandvik Coromant. Please ensure you're watching this in a safe environment. Be aware of the safety procedures, exits and assembly point of the building that you're in. My name is Ben Lodge and I'm the solid round tools product specialist and I'm joined today by Paul Lugton. Thank you Ben. Yep, my name is Paul Lugton. I'm the CAM specialist. So today we're going to be looking at slotting. So here we're going to be looking at the strategies and best practices of producing slots when milling. So see there's lots of different techniques for creating a slot when we're milling. Obviously if you start sort of on the first slide, obviously we always prefer nowadays to do down milling. Some of the other strategies are rolling high feed face milling to corridor high feed side milling. The ramping and the plunging will go over those in more detail in the coming slides. But that's just an overview that sort of different methods of slotting. We're covering today mainly Ben that has solid round tools, but we also have a good selection of indexable tools as well. Both sort of end mills, but also side and face or slitting source, which can be useful in some applications, especially for really narrow deep slots. OK. And the next slide just gives you a sort of a general overview of our sort of slitting or side and face products. The sort of the width range and the depth range that those are all capable of. So there's a good selection. So if you need more information on those, you've got sort of the product family there. Now go onto our website and have a look. So what we're looking at today could lend itself to both an indexable solution as well as a solid round tools when it comes to the slotting applications. Indeed, yes, indeed. So obviously as we covered before, we're going to talk about, we're going to split the sort of slot up into sort of main, two main subjects really. Entering the slot and obviously the actual slot in itself. So first we're just going to talk about how we enter the slot and obviously how you enter the slot is different for sort of open slots or closed slots. When we talk about open slot, we mean entering from sort of an open face at the Zed level and coming in at that level. Closed slot is what we refer to as, you know, it's actually closed into the material. So you've got to sort of plunge down into Zed to get into the material. So that's how we sort of differentiate between an open and closed slot. So first we'll go over how to enter an open slot and generally obviously open, open slot is, as you can imagine, quite easy. But obviously there's still some good recommendations and the best recommendation is to roll into cut. And this is something we recommend for all sort of milling, solid round tools and indexable. And the best way with your face milling, slot milling, it's the best way to enter the material. It gives the tool a really kind entry into the material. You keep the fit chip exit and you always keep that down milling. We'll cover it and it reduces the vibration. It gives you much better tool life, especially in these challenging materials. And the more challenging material, the bigger the difference you'll see with sort of rolling cut. And I'm right in thinking that the side that we enter from is important as well. That's right. So what we're talking about rolling in, this is obviously, as you can see on the screen, the video animation, you can see that sort of red shaded there. That's what we call a fit chip exit. And that's what you get when you just go straight into the material. And as the insert breaks away with that fit chip exit, it damages the edge of the cutting edge of the insert. So you can see when we're rolling in the correct, as you said, Ben, we need to roll in the right way. Obviously the wrong way will make it doubly worse. And when we're rolling the right way, you can see that that green shaded area, we get that thin chip exit. So as the cutting edge exes material, it's got sort of virtually no load on it. And that just gives us a much smoother cutting action, much better tool life. And it's just preferred for everything, you know, face milling, slotting, you know, everything. Only solid round tools and indexable. So it's about producing that thick to thin chip. It is. Yeah, it is exactly that. So that's obviously talking about sort of open slots. Now we obviously close slots. I suppose in a way, really Ben, close slots is a little bit more challenging. We've covered some of this perhaps in our previous pocketing, but obviously it's slightly different sometimes with slotting. Because sometimes you've got less room for the tool to maneuver around. So obviously we're going to talk about mainly sort of ramping. So obviously this is good method for sort of entering a slot. We just sort of ramp down. So the tool will be going X, Y and Z, but obviously the Z is much slower, lower angle. It eliminates the need for a pre-drill. And it's obviously, but the problem is it is quite a demanding cutting action. As you can see on the video animation running, you get sort of a full slot in cutting action. But you also get a lot of back cutting as well. So you get it's quite a demanding. You've got swarf coming from the bottom of the tool and the silo tool is quite demanding cutting application. So you just need to bear that in mind. And generally we have some recommendations perhaps to reduce the feed and speeds by 20%. Our CoralPlus tool guide will give you general recommendations on that sort of cutting data for that. The helix ramp on the ramping and there you can see on the screen just some general guidelines of ramping angle. But again, we use the tool guide. It gives you that sort of recommendation or ramping angle. Every tool, every tool diameter has its own effective ramping angle. So it's a good thing to use that tool guide. It always gives you the recommendation. There is also the option to use a helix ramp. Obviously doing a helix, so just going round and round in a circular motion. is a much kinder cutting action. Not always possible. Normally with pocketing, it's normally the first choice, but it's not always possible with slotting. But if you can, there is enough room. It's always preferred method still to do that helix. There is the other option to do what we call like a profile ramp. So the tool begins around the profile of the slot and gradually going down in Z as it enters into the slot. The drawback to this is I'm sure you hopefully you can see on the screen. You can see that that sort of profile ramping gives you a sort of spike in loads. Each time the tool approaches the corner and switches direction, you get a sort of a peak in the load. So we do just to be a little bit more kind or careful, I suppose, with the cutting data we apply to that. So then we make kind of a reduction then in the data to try and counterbalance these forces. That's right. Yeah. Yeah. So that's where in that previous slide we talked about at 25% reduction. Sometimes with the helix now we use this two degree ramp and we can run sort of full data. But obviously with that profile ramp, we would definitely need to reduce the cutting data a bit on that. So yeah, we've mentioned about getting this helix cutting data and all your recommendations are from our online nowadays. So tool guide, if you put in there you want to do a closed pocket or a closed slot, it will give you a recommendation both for the angle and also the cutting data. And it will reduce the cutting data if you're doing that sort of full helix angle. So you can see it's just a general recommendation on the screen. What's highlighted in the red boxes. It will show you how to reduce the cutting data and what sort of ramp angle the maximum ramp power that tool is capable of in that application. But of course, as we said before, two degrees can be a really good rule of thumb and you can generally use much higher data. perhaps the actual slot or pocket data will give that two degrees. So once obviously that's how we enter our open or closed slot and once we're at that Z level to create our slot, either we're doing it in multiple depths of cut or right to the bottom. We're going to look now at perhaps different options for how we actually create a slot itself. So we just just to give you a little bit because we're going to talk with some terminology today just to give a sort of exploration around the cutting process itself. So you can see on the screen we've got number one, which obviously as the cutting edge enters the material we got number two, which is what we define as the arc of engagement. So that's how long the tool is engaged into the material. So that sort of arc of engagement and then we got number three, which is obviously how the tool exits the material. So we just sort of just keep that in mind while we're going through this. Arkham engagement is one thing we'll talk about a lot and it's obviously very important with all sort of machine, especially high feed machine. So we can see on the screen there Ben, we've got different cutter positions, both from full slot to both to sort of 25% high feed side milling. Full slot and we will show full slot today in our demonstration, but obviously generally it's something we don't recommend. Because it's quite a challenging process and the problem that can happen is you get a lot of heat generation. Because if you think about as the tool enters the material, we start with a zero chip thickness and then we gradually build up the chip thickness to reach that center line. We get full chip thickness and then we gradually. So you get what you tend to get with a full slot is quite a lot of rubbing action as it tools trying to get into the material. So you get a lot of heat and also when you're slotting full slot as you'll see in our demo is quite challenging to get the swarf away from that cutting action. So and the other things I look at there, 50% engagement is something we always try and avoid. It's a problem with 50% engagement is the tool that enters the material at maximum chip thickness. The maximum chip thickness is at the center line, so we always try and avoid doing exactly 50% so always do try and sort of 60 or 40. Don't try and do six and this applies to both index for obviously solid round tools. It's just a good generation 70%. Access there, I suppose this is probably more for index one of solid round tools, but we've shown in our previous demo. Some of our tools are capable. Some of the solid round tools are capable of 70% engagement. Yeah, with the Plural HD with the pocket in. That's right Ben, yeah, that's right. So they are capable of and you get really high metal removal rates if you've got the stability. But obviously generally for an index for that's something that's probably quite common with 70% engagement. But yeah, solid round tools can still perform in that area with the right tool. But generally for solid round tools and to be the most sort of reliable and effective process, we generally nowadays look at very small radial engagements. High feed side men is what it's sort of termed as. So we talk about high feed side men and I suppose modern slotting techniques that are perhaps terminology. I suppose this is more about terminology in the process than anything else. We have what I suppose has been around for a good number of years now. Most people have probably heard of tracoil and willing. So obviously this is this is a very good reliable process. It's I would say it's simple because they're basically just concentric circles going around. Right? So it's very simple. They are good in older machines because it's it's simple short NC code because it's just continuous circle. So it's quite a short G3. The problem with it is it's inefficient because obviously you imagine keeping a consistent circle. Both is is it's will show through the next couple of slides how it's inefficient in cutting. But obviously you can imagine it's doing the same circles is out cut as well. So spending a lot of time out of that's not in contact with them. Exactly. Yeah, we're spending half the time in the material and half the time out the material. So really it's very inefficient in that way. We've also got like a I suppose a modified version of tracoidal called pill milling, which is like a tracoidal, but like a stretch, which is a good option for wide slots. So it's basically taking the tracoidal milling, stretching it and putting two curves in between. It's slightly more efficient because the actual process between the exiting the material re-entering it is a little bit shorter. Still not as efficient as some of the techniques we will show in a minute. But the problem with it is you can get sort of high peak loads, high arc of engagements on the entry because it's quite a short radius. Right. So it's okay. It does the job. So hopefully we'll show through the rest of this presentation that there's better techniques nowadays. So I suppose what's certainly our preferred technique and what our tools are sort of designed for and how we get the best out of our tools. So it's called some people refer to it as D-slotting because it looks like a D. It's also called non-linear because it's generally unlike tracoidal, it's lots of circles. Generally, this is more linear. So it's non. And then, but there again, it's also referred to by sort of sort of the cam companies names of sort of dynamic milling, which is master cam waveform, which is edge cam. And obviously all the cam companies have their own sort of terminology. And we can see that on the screen there. So a lot of these cam companies have their own name, but they're all following this same sort of high feet side milling technique. So we'll cover first for a coil machine, because this is, I suppose, what most people are used to. So this is really good for narrow wide slots. So say for the wide slots, you can sort of use this stretch coil or peel milling. It's a two times D method, high feet. It uses the principle of high feet side milling. So we do doing small radial cuts in just a circular motion. And it does keep, as opposed to sort of full slotting, you have much lower cutting forces, as you can imagine. And our general rule of thumb is that you take your slot width times it by 0.7 and that will give you your sort of tool diameter size. And obviously you do need to try and match that also with your flute link. But we also have different times D tools, Ben, don't we? Yeah, exactly. Obviously we've got the two, four, five times D available to us. So we've got a lot of options available in certainly in the length ratio. And I suppose that rule of thumb is really important as well when we talk about this arc of engagement and not trying to reduce the contact. And keeping with this high feet side milling method. That's correct. Yeah, that's where that sort of 0.7 comes from. It's the sort of ideal relationship. You know, it's the most efficient. If we go wider and the tool smaller, it's less efficient. And obviously if we go slightly tighter, we'll get a really high arc of engagement, which can obviously have a negative effect on tool life and stuff. So this is just the basic calculation of how to work out sort of to cord and wheeling. We won't go too much over here today because obviously there's calculators. Most CAM systems, you can put this data in it. It will give you that data out. The important thing to bear in mind is that what we call a step head, the W, isn't necessarily like the AE. It's not a true. So if you put in there like a 10% at all, you actually get much higher value than that in effect. So you do need to perhaps bear in mind and perhaps use some form of calculator or just use a conservative cutting data. Know the fact that if you put in there the W is your step over, it's actually going to be higher arc of engagement and it would be a straight line. And the same with this sort of wide cordial milling. Yeah, it's still very good. You get a very small contact area. It's still if you've not got a complex canvas system, you're an older machine tool. This can still be a really great solution for creating slots and wide slots. I suppose we're talking about that when we talk more and more about sort of high fee side. Me and later on we get to the demo net, but there are some other other options for creating a slot on there. Yeah, and we can see here with obviously the high fee milling tools. Not only do we have them in indexable solutions, but we haven't been obviously a solid round tools portfolio. You know, in solid and also in the 316. So you know we can we can utilize these cartway to form the slot. No quick tool paths going across the surface and small engagements. That's right Ben. Yeah, generally a very small depth of cut but a very high feed rate. And I understand these are also available in ceramic tools. Yeah, we have ceramic tools with the high feed profile on as well. So, you know, if we're looking at nickel based alloys, then we can certainly utilize those as well. Yeah, good. As you just mentioned, we also do obviously high feed indexable tools. We do lots of sort of index or high feed tools, but one we'll just mention today is what we're going to use in the demo. And we mentioned this because it's more in size with perhaps solid round tools because it's a tool that's available with very small diameter. So perhaps it's more comparable to solid round tools. But we have our sort of 415 and this has unique eye lock. So the actual inserts got like a V on the back. So it's actually locked into the pocket very securely. And we have these available. We have an 05. Insert and we have an 07 insert and they're sort of available from diameters 13 to 32. And because of that small insert size, we get quite a high density of inserts. Not as many as obviously perhaps a solid round tool, but you can certainly get a lot of. Inserts per cutter there. And these are available on the EH Kaplan, which is we've covered before. Yeah, yeah. And obviously that's a really good solution for different back ends for different extensions and uses and stuff like that. So that's a really good, really good option there. Yeah, definitely. So I think one thing to just be mindful of when you're doing high feed million when you're full slotting is obviously the first pass is OK. And obviously subsequent passes, as you'll see from the second picture down on the right, we get a sort of a wrap around effect because we're dropping. This is if you're just going straight down into a slot. You get a wrap around effect more on the walls and you lose some of that. You get a higher hex than what you would have used just going in a straight line. So hopefully you can see those two sort of section views of the tool. You can see their comparison between the blue shaded area and the gray shaded area. So we just need to be mindful that you can still use them in full slotting applications and going down sort of vertical walls. But we just need to be mindful of the fact we're not getting the true chip thickness as we would if there's using just a facing operation. OK, so I mean a general rule I use is just to half the depth of cut, but obviously we could also just reduce the feed and do the full depth of cut. But in my experience, I generally find reducing the depth of cut is a better way of taking the load off the tool. If it was just doing a straight pass or he wasn't cutting down the vertical wall, we could run full data. It's just because we've got that extra wrap around as we're dropping down into a slot as I hope you can see from the pictures there. Yeah, so demo. Yeah, so now we're going to look at different techniques when it comes to producing slots. So we're machining 316 stainless steel. This is on our DMU 60 EVO machine and we're doing both open and closed slots with this. Wherever possible, we're trying to not use coolant so it is visible, but there was some times that we had to certainly when we're doing the ramping applications. So we've tried to replace them with some Mastercam simulations. So let's have a look at the demonstrations now. Sure, good. So here we're using this 415 cutter that we spoke about before, the 20mm diameter. Yep. So you can see here, we're just doing just simple straight, you know, the first pass is at full depth of cut and then the subsequent passes, as we said before, because you get this wrap around, we're doing half the depth of cut. But as you can see, that's a very high metal removal rate, you get for that tool. Obviously, the other thing to bear in mind is you'll see as we go through, Ben, obviously, because of that high feed, the angle at the bottom, we are going to leave a little bit of excess material in the floor, in the corners. So you'll see at the end, towards the end of this video, we just bring up an MBL just to clean that corner out and get it ready for your sort of finished pass. But this is a really good productive method, just roughing out material really. So you can see we've roughed the slot out and now we just, as we've said before, we're just bringing that MBL in just to clean those corners out with a high feed sort of angle. of the tool, just left a little bit of excess material. This might not be needed in all applications and you might be doing a semi-clean sparse anyway, you can clean for that. But this is just to give a sort of as true a comparison as we can give really. So now we're looking at a Pluda HD product. And this is this trichoidal milling method that you were talking about. That's right. So this is just using trichoidal milling. We're doing sort of a 0.53 step over, which gives us an effective 10% AU as we were doing in a straight line. Like I said before, you need to be careful with trichoidal because the step ahead you put isn't true because it's not allowing for the arc of engagement, that tighter radius. So yeah, this is just, it does the job really. I mean, it's quite, it seems quite slow, but it's very stable. And we're talking about giving processes here that are reliable, consistent, the sort of thing as we said before, you can shut the door, push the button and know it's going to work every time. So you will see through some of these demos, you will see obviously we're running the stainless dry. So we will see some swarf problems. We did have problems getting swarf out of the pocket, but obviously ideally all of these tools will be run with food coolant and that age that stops the sticking effect of stainless, but also flushes that swarf out as well. And now we're going to use the same product, but obviously with a dynamic method that we spoke about. That's right. So this is the dynamic method. It's the same tool as the previous one, then, as you said, and when we're using the same step over 10%, but obviously because the cam system keeps that continuous arc engagement, we can be much more reassured that it's doing that 10% all the time. And you'll see through some of the slides later on, how much more consistent it is doing that, keeping that arc engagement. So, I mean, it's called deslotting because if you, if you analyze the actual slot itself, it enters on a big arc and then it exits on a tire arc. So, I mean, that's why it's so much more efficient. But again, it's comparable. It's still a good process. But we'll have less time kind of cutting fresh air. Yeah. Yeah. I mean, the other thing this does, it doesn't show up to well in the slotting, but when it's actually doing non cutting, it would do what they call a micro lift and a fast feed. Okay. So it actually travels back at more or less rapid rate. And now we're going to do exactly the same, but we're going to use the very quick force optimization as well. That's right. So we've taken the ENC code from the previous slot and we've done this very quick force optimization, as you say, Ben, and this we've based the actual force loads where we've used this before. It's all on the pocket. So on the pocket side, we've done before, we took the max force, max chip, thickness loads, and we've optimized this slot based on that. And we've got some really good cycle time for that because obviously the very quick force makes a really big difference on entry and exit, where obviously the cam system keeps the feed rate. It doesn't mean no need to, or not quite as intelligent as it could be sometimes, but it does a really good job, but the very quick force is almost like the cream on top. It just adds that extra little bit of, you know, goodness to it. And then lastly, full slotting, you know, the Pluri HD, you know, specifically designed for this kind of application, you know, heavy machining, heavy duty cuts. That's right. That's right. So yeah, this is a 10mm tool doing two times D. I mean, the tool we had got a little bit more fluting than that, but we're doing sort of full slots. So we're doing one full slot down the center. We're doing two 50% up each side to open the slot out to that 20mm. But you can see as the video is run, because this tool really should have run the coolant, we shouldn't have run. But you can see there we're having a lot of problems getting a swap out of the pocket. But yeah, with coolant and the tool, the fact this tool has got a free coolant that would have aided that a lot, but obviously then we wouldn't be able to see anything in the recording. But this is a really strong, robust tool, isn't it? Absolutely. And you know, we can see obviously we're re-cutting the chips there as we're passing back through, but we're still able to do that because of the strength that we've got, you know, the optimized flute design that we've got to give us that space for the full slotting as well. That's correct Ben, yeah. That was very impressive, you know, given what the tool was put from it, it's doing it really well. So I mean this is, if you've got a really stable setup, a really stable machine, this is a really good way of getting material out of the slot. Now these PlurHD tools as you just said, Ben, are really good metal removals. So we'll just go for a quick summary. So obviously you can see on the summary slide there we've got the high feed when we did the 415, and we obviously we did, we cleaned out the corners with the corners. You can see there that obviously that the actual 4 slow, you can see in blue the 4 slow from the very cut there, is actually quite a lot higher than some of the other processes. So you do need to bear that in mind. You know, that is that high feed tool is a roughing tool really, you know, so it does support. You do need that stable setup there. But you can see there that we've included the total cycle time for both of those, both of that and cleaning out the pocket. And then we move into the middle with a high feed side, meaning so we've got those different techniques in there with the quad or million, the dynamic million, the slot free, and obviously then the same dynamic million, but with the force optimization. And you can sort of see this all times. You can see there's quite a big difference between the quad or million and then the dynamic million. And you can also see hopefully that even though the dynamic million is faster, it actually gives less load on the tool and it's using this getting more consistent chip load, which we'll see in a minute. So you should get better tool life still from that, even though it's faster. And of course, then we use that dynamic force and that just optimizes it and gives us a little bit extra on top of that efficient dynamic million. And you can see on the right hand side before start, we did that sort of at that 10 mil plura full slide two times. That is again a very fast process. But again, look at the force loads. If you've got that set up to do it, it's great. Obviously you do need to have that stable setup. So I suppose you need to be aware of what the limitations might be with your machine and what the power you might have at certain points. Exactly. Yeah, yeah. Power stability of the machine, but also also the fixture in the set up and apart as well can have a, you know, so it's there. It's good, but just need to have the right process and set up for it. So on this slide, Ben, we're just going to, we're just comparing sort of using the force again, but we're just comparing both with cycle time and giving a comparison between, I suppose, the traditional corner milling and the modern dynamic nonlinear D slot milling. So you can see there it was just a comparison because some things you need to bear on. You can see the difference in cycle time is quite sort of, it's quite considerable. There's nothing to be sniffed about if you like, but so you can see there the path length, obviously the trachoidal milling actually, because it's doing that continuous arc, it's actually traveling a much further distance than the D shape because the D is flatter. It's like a squished circle. But the important thing to bear in mind, I suppose on newer machines is the NC code length. Obviously the trachoidal milling is quite simple NC code. We just continue circles, but obviously dynamic milling is made up of a lot of G1s or G3s. So there's quite a difference in the code size of the NC code. Modern day machines, not a problem. Older machines might be something to consider. But you can see there what's interesting if you look at the max chip thickness and the force, that again, even though the trachoidal milling is slower, it's actually, we have a higher force and a higher chip thickness with it, because it's not controlling this arc of engagement, like the dynamic milling is. And what shows it really well is this sort of the very cut force can do like a starting of nothing and the maximum chart, which you can see right on the bottom. You can see there that there's sort of the, the, um. On the trachoidal we've got sort of 50% cutting nothing and you can see that the blue line gradually increases. So that's all the entries and exits are very slow and you know there's only one point in the trachoidal milling we're actually getting a full engagement. The rest of the time it's gradually building up and gradually exiting. You can see that on that chart. As you compare that to a dynamic milling, we're sort of we're up cutting sort of just over 35% of the time. We're cutting so much more at a time, but we're also utilizing that load more. So we're more in cut and we're more loaded up, which is obviously people might think that loading the tool up is actually bad, but actually it's good. Yeah, that's in it because you keep the consistent chip load on. Absolutely. Is what you get the best, best tool life and best productivity. So now we're going to look at some closed slots. So we're going to start off with a zigzag method. Yep, that's right Ben. This is just quite similar. 10mm tool zigzagging left and right, gradually going down his head into a 10mm slot. We had to run this with coolant because we've got that sort of high arc of engagement. So once the tool got into cut, we lost sort of because of the coolant. So we just got a sort of master cam simulation in there. But you can see the tool is just literally zigzagging backwards and forwards. It's quite rudimental, simple. And then we move on to this, the helical strategy that we've got here. So we're using a small diameter tool with this, a 6mm. That's right, yeah. So again, this comes back to a 4 perhaps. We use a more economical, we use a smaller diameter tool. So we're helixing down into the pocket and then once we hit the bottom of the pocket, we'll be doing a dynamic sort of deslotting out from that sort of pocket. And with this we use the 2 degree ramp angle so we can keep that same data? We did, yeah. We did use the 2 degree ramp angle and get the salmon cut data. So again, you can use the data from the tool guard and use that sort of 2% and keep the same pattern data. And then lastly, we're using the same tool but this time we're doing the profile ramp. That's right Ben, yeah. So again, we're using that same 6mm tool. We'll be just following the contour of the slot and sort of running around the slot, gradually dropping in Z or ramping down in Z until we hit the floor and then we do a sort of final finish pass. So again, it's a really good method. So, you know, both are really good methods to creating that slot. So here we can just see a comparison between the three different methods. So you've got the zigzag ramp using that 10mm tool. A really good method, perhaps not the most stable but it can do. You know, it's simple, you've got a robust, strong tool there. You might have to do a finish pass because the profile pocket might be a little bit deformity, especially in the ends when the tool deflection changes. But again, for basic slotting, perhaps is a really good technique. Then we've got in the middle, we've got this sort of the helix high feed side milling. So a slightly longer cycle time we're using that 6mm tool. So we're using a smaller tool, so perhaps that might be more economical. You know, smaller tool, we're using more of the flute length. We're using more of the tool in this case. And again, on the right hand side, you've got the profile ramp where we use that same 6mm tool. And we just profile ramp down. And again, we're not using perhaps so much of the flute milling. We're more using the bottom couple of millimetres tool. So perhaps the tool life with this won't be quite as good as the helical ramp dynamic milling. Because we're doing most of the work on the actual flute to the tool. But you can see we've got sort of good cycle times for most of those. Most people will be happy to see those results. Yes, certainly. And again, just a comparison using this, the Vericut force chart. You can sort of see on the zigzag ramp. You can see how sort of spikes. Now that force is, you can see each corner change. We get a really big spike in the load. We're getting a lot of changes in forces there. So maybe not as a consistent or robust process as we've seen. Certainly when we look at the helix entry in the dynamic. Yeah, it can be quite a challenging process with that. So as you can see the helix one is very consistent on the load. And the chip thickness. And again, the profile ramp is pretty good. We are getting a slight peak of load as it's going around each of the corners. But obviously nowhere near to the effect of that zigzag ramp. And I guess we need to, we've talked a little bit about machines. We obviously need to consider the machine when we're selecting the process. And selecting the tools. And there are some things in the machines that can affect both your selection. But also the performance of how things work. Obviously the machine alignment, the run out of the tool. And the chip evacuation can all have a good or a negative effect on the actual process. And obviously your machine, especially your machine sort of spindle size. and the power of the machine and your fixture. Your setup can obviously affect the size of the tool and the type of tool. And obviously the type of tool holder you'll be selecting for the process. And again, it's quite important. As we covered before with pocketing, sliding swarf evacuation could be quite challenging. Especially with closed slots. So obviously you've got, you know, if you've got a horizontal machine. You're quite lucky because the swarf and the coolant will naturally fall away. But obviously with these vertical machines. Good swarf evacuation is very important. Either with air or through coon. So that's quite important. And we saw the effects of not utilizing something like that. When we did the full slotting. Obviously we had a bit of a chip jamming within there. But you know, because we've got that robust tool. We were able to do the process. But in an ideal world, obviously we'd try and use the coolant for that. To ensure that we get those chips away. Yeah, if we had to turn on the coolant there. Because that tool has got through coolant then. And so we're going to flush that swarf out nicely. So very important to bear in mind. So obviously tool selection is also very important. Generally use that. We recommend to use our 930 chuck. It's got this fulcrum technology. You can see that bottom picture in the middle. So you know, gives them the highest clamping forces. At both ends of the sort of clamping shank. And you got the HD chuck for the biggest rigidity. And we've got our standard chuck. Which is quite good sometimes for dynamic. For light machining. And obviously we're also available in a good selection of sleeves. And you know, we're talking about full slotting. Now see, you see that mechanical. We do mechanical sleeve. Yeah, so obviously that helps to reduce the pull out. Or zero pull out in all honesty. We set mechanical locking. You know, it engages with the weld and shank. And then obviously as we put that into the 930. You know, we ensure that there's zero pull out. Because of that. So you know, that's a really good introduction. Certainly when we're looking at applications like this. That's right. Yeah. I'd say if you're doing those full slotting applications. That's really good. And that tool sleeve also comes with the CF. So it's got the coolant channels and a silenus sleeve as well. Yeah, exactly. And we also do obviously CF sleeves. And sealed sleeves as well for the fruit tool print. So a good selection of both collet sleeves and. Obviously chip evacuation. You know, we saw in our demo we had some problems. With some of the chip evacuations. So chip evacuation is really important. for keeping a reliable process. Is that right Ben? Absolutely. And this is one of the things that you know is really important. And while we have different designs of tools. You know, we spoke about. You know, the through coolant options that we have available. You know, and also these, you know, specific sleeves. Where we can get the coolant coming down the side as well. So it's really important. Certainly in these kind of applications where we, you know. We don't want to recutting those chips. We want to make sure we've got a nice clean process. to have that in place. That's right. That's right. And one, I suppose, obvious thing. Is obviously if you're on a horizontal machine. Try and come from the bottom up so the swarf is falling away. And obviously if you're on a machine that hasn't got. Perhaps through cooling, you've got a cooling jet. Try and cut towards the cooling jet. So the cooling jet is washing the swarf out of the pocket. Not towards the tool. So maybe some obvious things, but some things to consider. When you're setting up your process. So your program. And also we do it. We also do our 2P370. the large chip divider. Which obviously breaks up the chips last this morning. But so I suppose when you're talking. When we especially we're talking about really high engagements. or full slotting. It's quite a balancing act. Is that right Ben? Between the core strength from the. Yeah, absolutely. I mean, if we look here, you know the different types. On number of flutes that we have, we can see there. You know the the two flute cutters that you know traditionally that we'd say for. These full slotting applications. You know we've got this large chip space. But we you know we have. A small core because of that. OK, so we have to bear that in mind when we're doing this. But you know we've seen obviously the developments of products going forward. And then like we saw today, you know that the plurihd in full slotting. You know we see there this this high rigidity that we've got. But we may have a small chip space because of a four flute. If it was a standard one. But when we're looking at things like the plurihd. You know we've got this specific specific design. Of the flute this open flute geometry in there as well. So you know it helps aid the chip evacuation. So we're able to full slot with a four flute. But we also have five flute. You know options available in that as well. And we can full slot with that as well. So it is it's you know it's changed quite a lot. From from where we were you know. And the traditional method of two flute slotting. You know to where we are now with the kind of application. Specific products. That's right. Yeah. I'd agree with that tool technologies come on a long way. In the last couple of years. And then we have something cool. We call our VFD wearable flute depth. But yeah, this is a really good tool in this sort of. All round tool in the event. Yeah, so I mean it's a fantastic tool. You know we have this large core diameter. So we've got to go up to approximately like the 0.9. Times D of the AP Max. So we can see there as we go up. You know we see a larger core above there. So we've still got the ability to full slot. But we have that strong core available to us. To give us that stability. So we saw a really good all round tool in full slot. And then we come to our, I suppose, that conical core. Yeah, the conical core, you know. It's probably the most common design that we see. Nowadays on our newer products, you know. So we have this improved improved chip flow. As it says there, you know, we have this smaller core at the bottom. And as we go up to the diameter, we have the large. The AP Max. So you know it's similar to the VFD. But you know it is a little bit of a different design. But again, we're utilizing this chip space. Making sure we've got enough room for these kind of applications. And that concludes our knowledge session on slotting for today. If you'd like any more information about the topics that we've covered, then please either scan the QR code or follow the link on the screen. Thank you.