Hi and welcome to today's webcast we're going to be looking at how to model aluminium composite material in SOLIDWORKS. Thanks a lot Charlie, good morning everyone and thank you for coming to this webcast, how to model aluminium composite material. Actually this webcast came about really from a question I had on the support desk. We have a lot of customers who use this material for architectural cladding as you can see in the image and they were asking how would we go about modelling this. So I thought I'd share information with a wider audience on today's webcast. Aluminium cladding is mainly used on the buildings such as the images we've seen here. So this is a cladding which is made from aluminium composite material. If I just move on to my next slide. These images here just show the sandwich of material so we've got aluminium on the outer and bottom of this panel and a plastic of some sort in the middle and it can be supplied in different colours and coatings and obviously there's an effect there of a wood effect on one of the panels as well. So that's typically what the composite material would look like. Moving back onto the slide I was on a second ago just looking at how we would produce this because obviously it's a folded sheet metal component but on the other hand we can only work with a uniform thickness and obviously this has multiple thicknesses and in fact it could even be multiple bodies. So how are we going to produce that in solid birds? Now one of the first things you could say is actually do we need to go to that level of detail? You could actually just model it with the outer dimensions, the bend radius and things like that in solid birds and try and maybe even ignore some of this detail. But if it is something you want and you do want to go down to that this is really where we're looking at for this webcast. How would we do that? So at this point let's go over to Solvus and to save a little bit of time I've just drawn up a panel. These two panels are typically mounted on buildings without any fixings visible so it might be some sort of hook or something like that which hooks over some sort of bracket which is mounted on the outer frame of the building. So this is a panel and we're going to just create a base flange from that initially. So if I just go to my sketch tools up to sheet metal and I'm just going to create a base flange. The sandwich material we're just going to say this is maybe a 5mm thick piece of material so it's going to probably have in this case maybe half a millimetre of aluminium then plastic at maybe 4mm and then another half mill of aluminium on the other side. So I'm just going to stick with that half mill there. I'm just going to go for minimum bend radius using a K factor but of course as you're probably away you can use bend tables and bend allowance and things. That would all be possible as well with this. I'm just going to set the relief type to auto relief and tear as well on this. So really all I've just done is taken that sketch and applied a thickness to it. It's not folded or anything at this point. So next thing I might need to consider is adding in the different layers. I'm just going to do that by creating a sketch on the inner face. I'm going to use convert entities to convert the outer edge. Actually in fact I just need to convert the inner loops as well there. So let's just add those. Let's do an extrusion on that. I'm going to make this a multi-body. So when I do this extrusion I'm going to say it's 4mm to represent the plastic core. But I'm going to untick merge results. So if I just OK that now. What we should have if I look in there is considering these to be separate bodies. And obviously I need my final skin on here. So I'm just going to do the same thing again. Let's just convert entities on that. And let's just make sure we get these holes in here as well. And then let's just do a basic extrusion on that. And this will be back at 0.5mm again. And remember to untick merge results. So then we should have our sandwich. If I zoom in there you could see our sandwich of material. So the next thing we really need to consider I guess. Is we'd have to use a router. So maybe a CNC router to machine out the grooves on here. And now I could do just an extruded cut or something. But I thought actually a good way of visualising that. Would be to use a cutter of some sort. And we do have a tool under the swept cut tool. We can use a tool body. So what you might want to do in your library. I've just added one quickly here. On the right hand side of my screen. So if I just quickly go and find. The one I've put together for this. So I've got some router bits. I've just sort of modelled up with different profiles. Maybe I'll just drag and drop one in here. Hopefully we'll just place it. And we'll take a closer look. So this would have more like a chamfered profile to it. If I just undo that. Because that's not the one I wanted. Let's go and find another one. I wanted the one which has a radius to it. So if I just drag and drop this in. Okay. Bear with me. I missed the fact that I was still in a sketch there. Just double check. I think I've somehow managed to not. Okay that last operation. So let's just quickly redo that. And take manage results. Right. Obviously hit undo probably too many times though. So if I just drag and drop this in again. And just plunk my cutter in there. So this is the profile I want to represent as being my cutter. It has to be a revolved profile for this. Now I'm just going to locate it using some constraints here. Because essentially I'm inserting a part into a part with this. So I want to add a coincident relationship. Maybe between that plane there. And that edge there. Add that. And maybe that plane and this face. We'll add a relationship there. And then I'll just do that there as well. So once I've got that into the position I want. I might just hide those planes. So it doesn't look so messy on your webcast screens. So we can see we have. There's my tool. And I want to machine that along this edge here. So because it's going to be a sweep. I have to put a path in for that. Just to save a little bit of time. I've already put some sketches in for that. So let's just show the sketch. I've already pre-drawn for this. And the features. I'm going to go to swept cut. I'm going to select a solid profile. The profile is going to be that tall body there. And the path is going to be this path here. So then I can select the bodies I want it to affect. Actually if I just untick auto select here. Really it's going to be this top body. And that body there is not going to affect the outer skin at all. I want to keep all the resultant bodies from here. And you can see what it's done. It's machined that groove all the way along that path for me. So once I've done that. I can just maybe hide that sketch. And let's move on to the next profile. Obviously as I said this doesn't have to be this method you use. It could just be a simple extruded cut you use. Just for the purpose of this though. I'm going to stick to the same method. And I've already put in some other bits. So I can only use the bit once for a profile. And if it was a circular profile I could come around in a whole loop. When I was putting this webcast together I did find for this particular operation I had to run it as four separate cuts. So let's just turn on the next profile and do the same process again. So that's got my profile going across there. And then let's come down the other side as well. So this is fairly repetitive I guess for you guys at the moment. So bear with me whilst I go through these different cuts. I think I've got everything there. Let's just go through that. And then we've got one more and that will finish off the other side. So if I'm going to go through the profile we'd use one of those other cutters for this. I just chose this rounded off profile for this particular example. Later on we will use another more chamfered example and look at a slightly different method of creating that. So let's just bring that through. OK. So we've now got our panel and it's got the different layers to it. Now I could at this point because it is a multi body and it's created a cut list for me here. I could come into here and actually set some materials. So I could come into here and pick the aluminium for that outer panel. What else have we got here? I'm just trying to round a bit so I don't need to do that one. Sweat profile. So yeah, that would probably be one of the plastics. So let's apply material to that. You can see how that's applied in. Let's just apply some material to this. I won't do all of them but hopefully we'll get the idea. Sorry, I picked the wrong one. So apply the aluminium. So hopefully we can see here that we're getting the effect of those three cores coming through the model. So what ultimately we do need to do though is we need to turn it from 2D into a 3D folded up part. And how I'd propose doing that is using sketch bends. So if we just minimise that back down. Once again, to save a little bit of time I've created some sketch bends here. So let's just pick this sketch bend here. Under the sheet metal tools we can select sketch bend. And we need to pick a fixed face. I'm going to pick the underside as my fixed face. And let me just do that again. Slight different answer to what I was expecting at the moment. Bear with me. Ah, there we go. 1.5 is using a way too big radius for that. Let me try one more time. If not, I'll go over to it. It does work. I can assure you because I've done it several times. So. I can't seem to get that. Open up my finished version of it. And I'll show you back down through the feature tree. So. This brings us to the point where I was. And what I did. I used a sketch bend here. And what it does is it just folds up that outer skin. Now, the problem with that is of course the other bodies don't follow suit. So if I do the other fold quickly. You can see obviously the other skins haven't moved with it. But luckily in SolidWorks we do have a tool called move copy bodies. Because these are considered to be separate bodies. So if I just show you how that would work. If I roll those through. In fact maybe we'll just do one. And I'll just quickly edit it so you can see. Exactly as when I inserted the tool bit in. I used the same tool. Now essentially it's like having the assembly mates tool within the part environment. So I was able to reselect those bodies. And mate them up with these edges here. And reposition them. And you can see how they're now positioned accordingly. If I roll to the end here. What it allows me to do. Is then create a configuration. So I can have a configuration. When it was flat. And a configuration when it was folded. And that's one method. Of working on. Aluminum composite materials. If I just zoom into the corner there. Actually with this particular example. I haven't followed the profile through. So we could actually see. If we didn't do the. The router cut all the way to the end. We would have an interference fit here as well. So that is an advantage. I guess I'll have modelling up the entire model. If we look at this model here. At this corner where I have applied the router. All the way to the end. You can see how we don't have an interference fit. So that is one way. We could look at doing this. If I just close that down. There is a second method. I proposed as well. When I was looking at this. So let's have a look at the method 2. So what we can do with this. With this option here. Actually I've just modelled this as a block here. I'm going to convert it to sheet metal. So I'm going to pick my bottom face. I pick my material on my bend edges. You don't have to model it like this. You could model it using edge flanges. I'm just trying to get the basic shape. As quick as possible. And then what I could do. Is an unfold operation. I'm actually in fact. What I could probably do. Is just cut those cutouts through it as well. So if I just cut those out. Like so. So what I'd then do. Is an unfold operation. So if I do unfold. Pick my fixed face. Maybe that will be the bottom face here. And that flattens the model out. So this time what I might choose to do. Is add the material onto the panels themselves. Now for time reasons. It's only a short webcast. I won't do all of it. But what we could do. Is pick that face. Create a sketch. In fact in this case. Let's do offset entities. I want to reverse the offset. And maybe just a normal amount of 0.5mm. Now when I was testing this. I found that if I converted entities. And added the thickness of material directly on this edge. It failed to fold. So I did need a slight offset. At this point. And let's just do an extrude on this. Let's just set that to 4.5mm. Now of course. On the edge detail here. We would actually have that. Maybe a chamfer detail. Depending on what tool we'd used. So let's just use the chamfer tool. On here. I'm just going to set the distance. At 4.5mm. So it's consistent. All the way around. So you can see how I've added the material thickness there. Let's just do it on. I'll just do the same on this edge here. So if I created a sketch there. Let's just do a. Convert entities on that one. I wanted to marry up with these two edges here. But it's maybe just this edge here. Which needs to change. So I'll just come in. And get rid of this relationship here. I can then move the sketch line up. Put dimension in to control what offset I want. So we'll just keep it consistent with 0.5mm maybe. And do the same with that. This time obviously I am merging results. I should point out rather than. The method I used previously. Right. So this method here. Is assuming that we're using like a V-groove cutout. The advantage of that. If I come over to my. Sheet Metal tools again. And do a fold operation. Let's all bend. You can see how it has folded it up. Using the sheet metal functionality. This time I haven't had to create two. Configurations manually here. Now. With this method. I guess the disadvantage is. I am not representing. The three layers of material. One way we could work around that. Is to do a split. Operation. Whilst it's in the flat state. And then apply different appearances. To. To it. When we fold it back up. Or. Whilst it's in the flat state. I go to my finished version of that. Because I did have to apply them. I applied. The plastic material. To the main core. And then I applied the. Aluminum appearance. To the. The finished. Outer faces. I just come in and take a closer look here. This option here. As I said. Whilst it was in the flat state. If I just roll back the tree. I've done a split operation. So all I've done here. Is I've just dragged. Two. Sketch lines. Through the model. At the correct offset values. To represent where the aluminium would be. Used the split tool. I've then done the fold operation. Which we just saw. To fold it back up. And then I've just gone through. Using my appearances of aluminium. And the black appearance. As well. To represent the. Plastic in the middle. To represent that as well. So that's sort of. Two different methods. We could employ. To. Represent. Aluminum composite materials. So really going back to my PowerPoint here. So method one. Model the outer skin. As a flat. Flat panel. And the base. Base flange. We then. Model. The other layers. As separate bodies. I machine. The grooves. In using a cut feature. In my case. I used. The tall body. Cut. With the sweep. Cut. Cut. But it could just be. An extruded cut. Didn't have to go to that detail. We can then. Create new configurations. For the folded. Unfolded version. And I used. Sketch bends. To fold up. The outer skin. We then used. Move copy bodies. To reposition. The. The internal layers. Within the folded. And flat. Within the folded. Version. So we have. Two configurations. The other method. Used more. Core. Sheet metal. Functionality. We did have. The key thing. Was we did have. To put a slight. Offset. And when. When I. Did the extruded. Feature. On the internal. Faces. And I did need. A slight offset. On those internal edges. But then. I was. Able to use. The refold tool. To fold. The material up. And then. If we wanted. To represent. Those different layers. The material. Using the appearances. So I guess. In terms of. If you were. After the actual. Mass. Of the item. You get. A much more accurate. Result. With the first method. Because we've. Actually got. The separate bodies. There. We've been able. To assign. The different materials. To it. Whereas in the second option. We're more. Graphically. Representing it. So that really. Brings me to end. Of the. Webcast. Are there any questions. At this point.