 Hey, what's up, folks? Welcome back to another layer by layer in today's tutorial. We're going to take a look at making some shapes using LED noodles. So this is a 3D printed holder for these LED filaments. Adafruit calls them LED noodles, and you can get them from Adafruit. So the LED noodles can be press-fitted into these little 3D printed holders. I have a couple different shapes, and I'll show you, folks, how to design different letters and different shapes using Fusion 360. But first, I want to jump into our learn guide that really takes these shapes to the next level. So if we go over to the learn guide, we created an LED noodle lantern. We basically took one of each color of the noodles, and we mounted them vertically in this cool sci-fi-inspired container. And all the noodles are, you know, press-fitted into these 3D printed holders. And then the 3D printed holders are kind of arranged in these mounting brackets that allow them to be, you know, vertically mounted. They look really cool, and you can do lots of things with the LEDs, like fade them in and out, create different animation patterns, that sort of stuff. So check out this learn guide, and for getting the Adafruit noodles, adafruit.com, search for nudes is what we call them for short, and there's different ones. Be sure to sign up to get notified when they're back in stock. I used all of my noodles up, and I actually only have this one on hand. So this is 130 millimeters long in length. But one thing to note is when you're designing a holder, it's actually, you don't want to create your holder to be exactly 130 millimeters long. You actually want to go under a bit. So I definitely recommend calipers, measuring them out. If you just measure, you know, from here to this end, without the metal contacts, you'll actually get somewhere around like 110, 115 millimeters, which is enough to make or break a design. So just measure that out, and we'll keep that in mind. And I'll also show you some tips on keeping track of the length of your shape when you're designing it in Fusion 360. So let's go ahead and jump into, well, yeah, we'll jump into Fusion, but take a look at neon letters, like the alphabet. You notice that to do an alphabet with neons, you kind of want to have a shape that doesn't close in on itself. So for example, if you want to do like a spelled out word, you can see that it's doing like discursive writing, and it's just a single line. So keep that in mind when you're trying to make a shape is like, how do I make a shape where it doesn't close in on itself, because it can become difficult to do. There's various techniques to do it, but we're going to keep it simple and just make a shape that just doesn't close in on itself. For example, when you saw the R, the R doesn't close in on itself, it just kind of wraps around. So you know, you can do some Google searching and search for different fonts that might inspire you. Reading letters, if you're doing different shapes, like the heart, you can see you want to be careful with how close these ends, you don't want them to touch. So something like this, you want to either use some sheathing to avoid a short circuit. So that's one thing. Another thing I want to note, this feature is there is a little bit of a kind of a covering here, and that allows the doodle to kind of stay secured, so it won't pop out. So that's kind of a nice little feature, and we'll do all that stuff in Fusion, and you can print this without any support material, it prints flat on the bed, and they print pretty quick. This took like 10 minutes to print. So with all that, let's go ahead and jump into Fusion 360. So here's the letter in Fusion 360, it's the R, and we also have that heart shape. So what I'll do is I'll make a new letter, and I'll probably make like a Z. I think a Z, the letter Z would be kind of easy. So I'm going to start out with a new sketch, and I will draw on the floor here, on the floor plane. I want to have it be about the same height. So let's just bring out our line tool, and we'll start making our Z shape. I'll start somewhere over here in the bottom, and just kind of draw it out, like that, and then hit escape to stop. So there's our Z shape. When you double click a line, if your line is connected to other lines, at the bottom here you'll see that the length of it is 100 millimeters. So we can make it a little bit longer. Let me start adding some dimensions, but before I do, I just want to note some of the automatic constraints that were added here, notably this one here, it's called the parallel constraint. You can see down here what it is, it's the parallel constraint, and it's basically saying this shall always be parallel with that one, and then this right here is a horizontal constraint that just says that this line should always be horizontally or vertically set up, so it can't do an angle like that, like this line that I selected that has an angle. So let's give this a length, let's go with 30, and then I want this line up here to be the exact same line as this one down here, so let's use the equal constraint. So I'll say this needs to be equal with that, and that's okay, that looks good. Next thing I want to do is I want to add a, I want to select this line, hold down shift and select that line, and then hit D, I'm going to keep it for a dimension, and then I'll let me do an angle. I want this to be 45 degree angles, so I'll just type that in, and that looks good, and the next thing I want to do is kind of give some height from this to this, how much height I want to do, probably about 40, hit okay, and then that's kind of it right there. We can click and drag it to move it around if we want, but really I don't think that's anything else I want to change. You know, I'm not liking the shape, what I want to do is I'm going to delete the 40, and I kind of want this to be lined up with this line here, so I'm kind of struggling to do that. So I'm going to use another line, and I'm going to kind of connect these two dots here, this dot with that one, and you can see that it's not a straight up and down, so I'm going to add a horizontal constraint to it, I just brought up my sketch shortcuts window, you can do that with the S key on your keyboard, and then just click that, and then click that, and then now it's straight, so that'll always be straight. But the next thing I want to do is hold that line, like click on it, and then hit the X key on my keyboard, and that makes it a construction line, so I have to worry about the construction line closing the path. So now I can select this bit, and it tells me the length, it's 102 millimeters, so I can go a little bit taller now. I think what's making the shape a little bit hard is the 45 degree angles, so let's change that to something like last, like 35, or more in this case, let's do 50, let's try 60, that's too much, to 55, 52. Let's get rid of the, who cares, about the, you know, having a thing. Let's make the height really what we want, 40 degrees, or 48 millimeters, and now you can see it's pretty much locked in there, that's good. I'm pretty happy with that, it matches up with the length here, maybe 42 would be better. There you go, that's a little bit better. So I'm just referencing the size of this, and then when I double click on that line, it gives me a length of 111, you know that's going to be about fine, because what I found is that when you start creating the extrusion for this, your length never is the same because it's just the nature of it, so let's go ahead and say we like that, hit OK, and then the way to extrude this out is with the extrude, but you want to change the type from extrude to thin extrude, so you just select that, and now you're able to select that line, that path that we created, and the first thing I'll do is I'll change the distance, so let's make that, the distance is how thick you want, well not how thick, but how tall you want this thing to be, so I want it to be three millimeters tall, and then the wall thickness, this is how thick you want it to be, so I'm going to make it four, and that is really the number that you want to do, four millimeters, and you can see here the wall location, you can switch that around, you have three different options, so play around with the options, I think the center option works the best for us, and you can see here it's already bigger than our R, so I already know I'm going to have to change this dimension here of the construction line, because it's kind of defining our height, and then the operation is set to new body, so hit OK. Now right click on the sketch, and then say show dimensions, so that way we don't have to go inside the sketch and have to edit the dimension, we just edit it here and see our changes apply, so let's change that 42 to 40, and that looks good, looks better. It's still a little bit tall, so let me make it maybe 38, yeah, and then maybe move it up a bit, it doesn't matter where it is, because we'll just center it in our slicer program, but I just want to line it up, be as kind of accurate as I can, and you could also make this thinner if you want, so maybe instead of 30 we do like 26, and that just looks, to me this proportionately looks better, but it's up to you however you want to do it, so let me double click that line again, and see it's about 98 millimeters, so you can decide what you want to be bigger, if we had it be taller it wouldn't match our R, so maybe this is good at 30 millimeters in length, and then we can see it's about 100, maybe we want it even more, but like I said, it's all about testing, so let's leave it at that. Now the next thing I want to do is actually round out these corners, you'll notice that we have some really nice radiuses here when you're bending your thing, and there's also a note here in the learn guide for the noodles, under physical properties there's something called bend limits, and you really want to be aware of your per axis bend radius, so you can read through this, but basically you can't make a super sharp bend, it's just the nature of the thickness of the filament won't let you do that. So I'm going to add some fillets, and I found that these internal corners here are really sharp, so I'm going to give them a 0.25 millimeter fillet, and hit OK. Actually you can go back into the fillet, hit the plus sign, and then add these sharp corners on the outside, and because we hit plus, it's a different fillet, so instead of having to create two fillet features in your timeline, you can just do it all in one fillet. So what I'm going to do is I'm going to add the thickness of our wall, which is 4, plus the 0.25 radius that we applied to the internal corners, and that'll just give it a really nice tangent shape, so let me hit OK. And now we're ready to start sweeping our channel, so to create this internal channel for our filament to press fit into, we will go on one of these edges here, one of the end caps, have it selected, and then just create a sketch in there. I want to bring in the geometry from this, so I'll select it again, and hit the hot key P on my keyboard, and that'll project in the edges from that surface, so hit OK, and you can see it shows a kind of pinkish-purple. And then the next thing I'll do is I want to create a rectangle on the inside of this, so I've got my rectangle tool, my regular two-point rectangle, I'm just going to draw a rectangle freehand like that, and what I'll do is I'll select this top edge, this top line rather, and then hold down Shift and select that top line, and then I'll bring up my sketch model toolbox, and I'll say I want those two to be midpoint constraint, so it'll always be in the center of that line, and then I'll select this line over here and apply a dimension to it. I want this to be two millimeters in length, and then I want this line to be one millimeters in length, so it's a two by one. Next thing I'll do is I'll grab my line tool, and here's a cool trick to create a curve. If you click and hold down your mouse button and start moving, you'll start creating a curve here. You see how that curve is affecting where I am, where my cursor is. So I'm still holding down my mouse button, and I'll hover over this corner here, and then you can see that there's a square icon. If I let go of my mouse button, now it's applied. This is really easy, very tangent. You can even see that there is a tangent constraint, so that says that this will always be tangent with this, which is really cool, which is what we want. And then to kind of close this out, I'll select this line here. I don't want it to separate my shape, so I'm going to hit the X key on my keyboard, and that makes it a dotted line, which means it's just a construction line, and it won't intersect my path here. You can see that there. Yeah, and the next thing I want to do is I want to create a shape so that I can have something that covers over. You see kind of how this one is? So it's kind of covering it over, and that's going to allow our noodle to thread in, and it won't pop out, because this top cover here, this top roof, will keep the filament, you know, in place. So to do that, I'll just create another rectangle, two-point rectangle, just like that freehand, and then you can just click and drag the corners, and just drag and drop them on the corresponding corners. Sometimes fusion will be like, I don't like you. I think it won't move right now. It really is annoying sometimes. I really can't move it, so I'm going to double-click it, delete it, try again. You know what? Let's use our shortcuts, because clicking and dragging sometimes freaks out fusion. So let's try this method instead. I got my sketch shortcuts open, and click on coinciding, and that's what we're doing. We want this corner to be coincident with that corner, and we want that corner to be coincident with this corner, and that's done. That works better. Now, the only dimension we want to apply is to this line. Let's make it one millimeter. Actually, sorry, two millimeters. And then what we want to do is grab our line tool again, and we'll do that same trick to create that curve like we did down here, up here, so click, hold down the mouse button, start curving out, and then just drop it here. And that's it. There's our shape. Now we can create our top roof, and then we can use this shape to do a sweep along our shape. So let's get out of here. Let's say we finished the sketch, and I'll bring up the sweep feature. So let's select sweep, and then for the profile, we'll select our internal thing here, and then for the path, it'll be either this one or this outer one. Let's click the outer one to see what happens. Right away, you get a really nice preview of what it's going to do. So it's wrapping around those corners very nicely because we did our fillets here, and we were, you know, we thought about the fillets. They look good. I'm going to hit OK. The operation is set to cut, so that's all good. And that's pretty much what we want to do there. Now we can start creating our roofs for the end caps. So I'll select the profile, start extruding. I need to go the opposite way, so I'll put negative, and I found two millimeters of distance works well here, so I'll hit OK. Now unfortunately, we can't like mirror that. I'd love to mirror it, but I really can't, so we'll have to create the same stuff on this cap, on this opposite end. So again, select surface, create a sketch, select the surface, project it in. And then really all we need to do is that rectangle again, so let's make a rectangle. Let's not bother with dragging and dropping the corner. Sometimes it works, sometimes it doesn't, so we're going to do the method where we hit coincident. Click on the, ooh, click on the corner if I can select it, and then the second corner where we want it to glue to this corner and that corner. And then with the dimension, we can apply a two millimeter dimension there, the line tool, and then we'll do our trick where we click, hold it, start curving, and then let go where we want it. Hit E on your keyboard to start extruding. Again, we've got to go negative two, and that joins it automatically. And that's kind of it. That is our shape. The next thing I'm going to do is show you folks when your, let's name it, call it Z, Z letter. When you right click on it, save as a mesh. I like to do it STL because I'm old school, so let's try it 3MF to be new school. Hit OK. I'll save it here as letter Z. And then I'm using Cura. This is my STL. Let me delete that and bring in the 3MF. If I can find it, under shapes, 3MF. Oh boy. So let's right click on it, center selected. That's good. Now real quick, I'll take a look at my slice settings. You see my line width is set to 0.4. That's sort of a default thing, but if you don't have 0.4, your toolpath might be different. So I'm going to leave it at 2.4. Let's slice it and then go to preview. And take a note of the path here. The walls are super thin. They're just two perimeters thick, which is what you kind of want for something this small. And you can see here, it looks great. The radius, if you were to see some infill in here, then maybe your radius isn't as tangent as it could be. Now that's okay, but I just wanted to show folks, like taking a look at your toolpath and seeing if it's clean or not or if it has extra infill. You can just play around with a fillet amount and you can get rid of some of that material and make it nice and smooth. So this takes about seven minutes to print, which is great. I haven't tested it out, but I have the R, which you can see. So that's just kind of some of the techniques you can use in Fusion 360 to create these holders. Yeah, you'll definitely want to test print them out and see if it fits within the length of your project. Looking at the overhead again, you can see how much access I have here. And you can see it's not a lot, but it's better to have some access, I think, than no access because you wouldn't be able to bite onto the thing. But you can play around with it. So let me disconnect this and then kind of pop it out just to show how easy it is to pop it in and out. You're just threading it through that little kind of closing there. And when you're bending it, it only kind of bends, it only wants to bend one way. It's kind of hard to see, but you can sort of see the wire and the LEDs in there. And you'll see that it only wants to bend about right there where that internal line is. I think that is what's kind of bridging them all together. And then you have this side here, which is kind of the diffuser end and it doesn't really want to bend. It wants to just bend like that. So just keep that in mind when you are kind of manipulating this shape here. So yeah, this is the new Inca twist too, which is crazy. It doesn't seem to break, but be careful with it. There's some notable things like knowing what the anode or the positive end has a hole in here. It's hard to see, but there's a hole there. And then over here, there's no hole. You always want to use a choke resistor. This is 220. If you have a different LiPo battery, then you'll want to adjust accordingly. You can use an LED calculator to figure out what resistor you want, but this is a 3.7 volt battery pack. Wired up to a breadboard. We've got a choke resistor. The resistor can go on either end. If you want more information, like I said, go to the Learn Guide, but let's wire this up again in free form. So just making sure that the hole is visible for positive lead. No hole for your negative lead and it should just power on automatically. There it is. It looks really nice. The LED noodle that you can eat. And very flexible. It looks really nice in person. All over the camera you can kind of start seeing the individual LEDs. But yeah, that is a little demo of the LED noodles. That's going to do it for this tutorial. Don't forget to check out all the links in the description. Sign up to get notified when these are back in stock. They come in different colors. Different lengths. Really, there's just two lengths. 300mm in that 1.30mm. Check out the Learn Guides if you want to build this very cool LED lantern. Or just check out the Learn Guide for the noodles if you want to know more about it. There's some example code here too if you want to animate them or what not in CircuitPython or do we know you have control to do that. That's going to do it for this one. Thanks for watching. I'll see you guys in the next one. But until then, remember to make a great day. Bye, folks.