#transcript #kicad #phils-lab #youtube # KiCad 9 Hardware Design Tutorial (TI MSPM0) (2/2 PCB) — Phil's Lab #166 Auto-generated YouTube captions (yt-dlp, `en` auto-subs), collapsed into ~30 s paragraphs. Caption errors are left as-is ("Keycad", "poparad", "VA" = via, "rooting" = routing). Distilled in [[KiCad 9 MCU Board Design Workflow]]. Source: https://www.youtube.com/watch?v=igQWdVGZGpI · Phil's Lab · uploaded 2025-11-28 · 02:31:45 # Chapters - [0:00:00](https://youtu.be/igQWdVGZGpI?t=0) Introduction - [0:01:41](https://youtu.be/igQWdVGZGpI?t=101) JLCPCB (Ad) - [0:02:53](https://youtu.be/igQWdVGZGpI?t=173) PCB Set-Up - [0:14:16](https://youtu.be/igQWdVGZGpI?t=856) Component Import - [0:16:01](https://youtu.be/igQWdVGZGpI?t=961) Net Colours - [0:18:33](https://youtu.be/igQWdVGZGpI?t=1113) Rough Layout - [0:33:21](https://youtu.be/igQWdVGZGpI?t=2001) Board Outline - [0:40:19](https://youtu.be/igQWdVGZGpI?t=2419) Refining Layout - [0:42:37](https://youtu.be/igQWdVGZGpI?t=2557) Layout for MCU Supporting Components - [0:54:46](https://youtu.be/igQWdVGZGpI?t=3286) Layout for USB-UART Supporting Components - [0:58:14](https://youtu.be/igQWdVGZGpI?t=3494) Layout Accelerometer - [1:01:38](https://youtu.be/igQWdVGZGpI?t=3698) Remapping MCU Pins - [1:05:46](https://youtu.be/igQWdVGZGpI?t=3946) Layout Accelerometer (Continued) - [1:07:19](https://youtu.be/igQWdVGZGpI?t=4039) Power Layout - [1:15:49](https://youtu.be/igQWdVGZGpI?t=4549) Layer Assignment & Polygon Pours - [1:20:30](https://youtu.be/igQWdVGZGpI?t=4830) Via Pre-Planning & Placement - [1:24:53](https://youtu.be/igQWdVGZGpI?t=5093) Routing Decoupling/Bypass Caps - [1:31:45](https://youtu.be/igQWdVGZGpI?t=5505) Routing Crystal & ROSC - [1:35:35](https://youtu.be/igQWdVGZGpI?t=5735) Routing SWD - [1:38:28](https://youtu.be/igQWdVGZGpI?t=5908) Routing I2C & UART - [1:45:09](https://youtu.be/igQWdVGZGpI?t=6309) Routing USB - [1:51:15](https://youtu.be/igQWdVGZGpI?t=6675) Power & Ground Routing - [2:05:42](https://youtu.be/igQWdVGZGpI?t=7542) Teardrops - [2:07:18](https://youtu.be/igQWdVGZGpI?t=7638) Design Rules Check - [2:14:53](https://youtu.be/igQWdVGZGpI?t=8093) Silkscreen - [2:17:02](https://youtu.be/igQWdVGZGpI?t=8222) Manufacturing Files - [2:24:04](https://youtu.be/igQWdVGZGpI?t=8644) Ordering - [2:31:00](https://youtu.be/igQWdVGZGpI?t=9060) Outro # Transcript **[0:00:00](https://youtu.be/igQWdVGZGpI?t=0)** In the last video on this channel, video number 165, we started out with a Keycat 9 hardware design tutorial looking at creating a project and creating a schematic for Texas Instruments MSPM0 microcontroller. This video is then the second part and the final part of this series other than of course a firmware video in the future where we'll go through actually creating the PCB in Keycad and I'll show you how to order this printed circuit board with assembly at JLCPCB. The board itself is very simple. We looked at the schematic in detail in the previous video, so we won't cover that in this video. This **[0:00:31](https://youtu.be/igQWdVGZGpI?t=31)** will only be to do with the PCB design and then manufacturing and ordering. We had an MSPM0 microcontroller, a fairly generic low power microcontroller, its peripherals and surrounding circuitry as well as a debug programming header. And we have a USB toart converter as well as a USB C type connector just for power and also the USB UART data transfer. This image you're seeing here is a version I created previously just to test the design. In our design, we don't have the head on the right hand side. We'd rather we've replaced that with an I squed C based accelerometer just for **[0:01:04](https://youtu.be/igQWdVGZGpI?t=64)** the sake of having something different. But of course, feel free to use whatever your design actually needs. This is just a very simple demo board. The board you're also seeing here is a two-layer board and we'll very likely be just using two layers in this design. Feel free, of course, to go to four layers if you want to try that out. I have several videos on my channel that show you how to do a four layer board. But for something as simple as this, there's not terribly many components. We can get away typically with a two-layer board, as we'll see. Again, I'd strongly suggest checking out part one of this series, video number 165, to learn all more about the schematic and circuitry involved. Again, I will not be covering **[0:01:36](https://youtu.be/igQWdVGZGpI?t=96)** this in this video. A huge thank you to JLC PCB for sponsoring this video. I've had these MSPM0 PCBs manufactured and assembled by JLCPCB, and they did a fantastic job. As usual, I'll be guiding you through the ordering process at the end of this video once we've completed this design. And you'll see they're super easy and affordable to use. If you'd prefer someone else to do the layout and PCB design, JLC PCB actually currently offers layout services that help you through the PCB design process. various different types of boards, high-speed, highdensity designs. And it's ideal for people who have a **[0:02:09](https://youtu.be/igQWdVGZGpI?t=129)** schematic but lack the time or interest to design PCBs, engineering teams that want to focus on product development and leave layout to experts and anyone else looking for a fast, reliable, and time-saving one-stop solution. It's very easy to get a quote. Simply click on place orders, fill out the various information that you know about your PCB requirements, and you can very quickly get a quote back from JLCPCB. JLC PCCB's layout service provides a skilled engineering team with experience in high-speed high density and mortai designs. Their seamst integration with JLCPCB manufacturing and assembly of course full confidentiality for all of **[0:02:42](https://youtu.be/igQWdVGZGpI?t=162)** your projects. I strongly suggest checking them out. JLCPCB also often has coupons available and I'll leave links to them in the description box below. Assuming you followed along, you will have Keycad 9 open and this is what our schematic looked like at the state of the last video. After uploading, of course, I detect a small little correction we need to make, and that is the USB D minus and D plus lines are connected correctly, but of course, the net labels, you probably noticed in the previous video, need to be flipped at the USB UA converter. So, USBD minus needs to be moved to USBD plus and vice versa. So, I'm going to click on that, **[0:03:13](https://youtu.be/igQWdVGZGpI?t=193)** Crl X, Ctrl +V, just paste that somewhere else. And I'm just going to move these two around. There we go. And now, actually, the net labels match up with how everything is routed as well. But other than that, we are now ready to move over the PCB design. Remember last time we also had assigned the footprints and we've done the electrical rules check. So unless you spot something else, the schematic in my eyes looks pretty okay for now. So to move over to the PCB design, we go to the top toolbar. You can see the far right button is switch to PCB editor. If I click on that, a new window will open. This is going to be our view for the next remaining part of this video, at **[0:03:46](https://youtu.be/igQWdVGZGpI?t=226)** least for a large part of it. We have our main PCB editor, and the controls for moving around are fairly similar to the schematic as well. We can hold the middle mouse button and then move around to drag the PCB design, zoom out with a middle mouse wheel, zoom in with the middle mouse wheel. We also have a rather than just this 2D view, we have a 3D view. If you go to the top left, view 3D viewer. We can also press Alt + 3 as indicated by this shortcut info here. And so far we have a pretty undefined, pretty poorly defined PCB. That's why you're not seeing any shape or anything. And we can see the board outline is missing, but we'll get to that later on **[0:04:18](https://youtu.be/igQWdVGZGpI?t=258)** once we've added some components onto this. On the right hand side we have our layer view. So we have a front copper, back copper, various paste layers, silk screen and so on. And we won't be using all of these. We only need a certain subset of these specifically also just for a two-layer board. Tool bars on the right, tool bars on the top as usual, but we'll go through this as we need when we progress through this design. The first thing before we import any components, what I do is set up my PCB design and my board. The way we can do that is go to the top left and click on board setup. We'll go through this board setup bit by bit. We might not go through all of it, but I find it's **[0:04:51](https://youtu.be/igQWdVGZGpI?t=291)** important to set up your PCB, your PCB design constraints. For instance, how narrow you can make your traces, how nar how small you can make your drill holes and so on. I strongly suggest you do that before you start laying out routing or anything else. You want to make sure your design is manufacturable. And by going through the board setup initially, you can ensure that you don't have to change anything later on once you notice, oh, actually it isn't manufacturable. So, we want to stay within certain constraints. But first of all, the board stack up looking at the board editor layers. They're only certain layers we need for us. I will not be using the fabrication layers. We don't need adhesive layers. This is not **[0:05:23](https://youtu.be/igQWdVGZGpI?t=323)** part of this specific PCB design. So I can click on these little check boxes to remove those layers just to give ourselves a far clearer view of the PCB as well as the PCB layers. Paste is important. That's our solder paste. Silk screen at the front. Solder mask is important. Of course, our copper and our front copper back copper. And you can for copper layers on the right hand side change what type of copper layer it is. So if it's a signal to power plane mix for us we're really going to estimate that our front layer or our top copper layer is going to be predominantly signal and power routting and our bottom copper layer we want to keep as much as **[0:05:55](https://youtu.be/igQWdVGZGpI?t=355)** we can a solid ground plane. So that's why the bottom copper layer I'm just going to change to power plane. Now there actually isn't very much of a significance here other than just for completeness sake but it doesn't actually change terribly much. Turning off all of these other layers just to make this clean. These are the sets I want. I just want copper. I want paste, silk screen, and mask layers as a bare minimum. Then the physical stack up going on the left hand side. We can change how many layers you want. Keycadly supports up to 32 layers. Impedance control as well. And this is just information for you and also later for your manufacturer to tell them how you want your PCB stack up. So what **[0:06:29](https://youtu.be/igQWdVGZGpI?t=389)** materials you want to use, what thicknesses, what copper files and so on. A lot of this you can keep as standard. So for the two-layer board, we can see the overall board thickness. If we look at the bottom, Keycad has calculated this as 1.6 mm nominal. And that's typically what a two-layer board thickness will be at. So for us, we can just keep this as as this is board finish. We can change what type of copper finish we want. Again, this is just for completeness completeness sake. And when you create manufacturing drawings and assembly drawings, this can be very helpful to tell the manufacturer exactly what you want. For us, we'll just go with a hot air surface leveling **[0:07:01](https://youtu.be/igQWdVGZGpI?t=421)** lead free finish for now. This is a fairly simple board. Would have had very fine pitch components. So, let's just go with hot air service living lead free. This isn't terribly important if you don't set this up for now. Solder masking paste is the first actual parameter we really need to change. Solder mask expansion. We can go to the JLC PCB site to see some some examples of this. Typically, your top and bottom layers will be covered with solder masks except where the areas are where we have exposed pads. So that's why we don't want want any solder mask because of course you want to solder components to those areas and to those pads. So therefore the solder mask is actually a **[0:07:34](https://youtu.be/igQWdVGZGpI?t=454)** negative or rather an inverted layer. Anytime you see something on the solder mask layer that's where there is no solder mask. You don't just want to have the solder mask opening exactly fit the shape of the pad with essentially zero solder mask expansion. You want it slightly larger cuz there are misregistrations, misalignment issues with solder mask. Of course you can't have a perfect 100% accuracy of alignment of your solder masks. So that's why we have this solder mask opening. Still a very small amount and that depends on what your manufacturer is capable of doing. If we'd go to the JLC PCB manufacturing assembly capabilities section and every PCB **[0:08:08](https://youtu.be/igQWdVGZGpI?t=488)** manufacturer will have this on their website or you can ask them to send this to you. Scrolling down to the solder mask section. We can see the solder mass expansion capability can be actually 1:1 which is pretty good. But typically I like to keep this at for simple design something like 0.1 mm or slightly below that. We also have some other parameters we have to stay within. For example, minimum solder mass bridges or slivers. So, how narrow the webs can be. And you take all of that from your assembly and manufacture house. Then going back to keycode, I'm just going to type in 0.1 mm for my expansion, 0.1 mm for my minimum web width, and 0.1 mm solder **[0:08:44](https://youtu.be/igQWdVGZGpI?t=524)** mask to copper clearance. Solder paste settings we can just leave as default. Text and graphics, you can change your default line thicknesses, widths, and so on, but we'll get to that a bit later as well. What we want to jump straight to is the design rules and the design constraints. This is incredibly important to set up again because we want our PCB design to be manufacturable. We don't want to have minimum clearance of 0 mm. That's impossible. Minimum track width of 0 mm. You really, really have to set this up. And again, you set this up by going to your manufacturer, checking for instance traces, what they can do. They can do for two layer boards minimum track width **[0:09:18](https://youtu.be/igQWdVGZGpI?t=558)** and spacing of 0.1 mm. And that's very very very narrow and very thin traces. That's what they could theoretically do for 1 oz copper on one or two layer boards. However, you always want to stay away from manufacturing minimums. The more strict you make your design rules, that is you go further away from the manufacturing minima, the easier your design will be to manufacture. And that's what you want. You want a higher yield. you want most of your PCBs making it through the manufacturing process without having to be scrapped because there will of course be manufacturing deviations and tolerances. So that's why **[0:09:50](https://youtu.be/igQWdVGZGpI?t=590)** we try to stay away from these minimums. I have because I've done this quite a number of years and I've done many many PCBs. I just have certain minimums I have in mind. If I go for a two-layer board, for a simple four layer, for an advanced four layer or multi-layer boards, this kind of comes with experience the values we'll be entering here. But they're also based on minimums that your manufacturers and also really affordable manufacturers can do. Minimum clearance I'm going to do 0.152. And these weird.152 numbers or 0.254 come from mills and millimeters these conversions. So again we talked about in the schematic section that we try to **[0:10:23](https://youtu.be/igQWdVGZGpI?t=623)** keep things with mills. So 100 mil grid but when we come to the PCB we typically use millimeters or at least in Europe we do. So therefore you could type in 0.15 but.152 translates to 6 mil and that's about 0.152. That's why I take that number and that's still a very very small number. Same for track width.152 and we'll try and keep away from this. This is just the absolute minimum when we do our design rule check later on. Connection width same minimum annular ring. If we look at drills our annular ring is essentially the copper that's left over after drilling through the pad. So the outer diameter minus the **[0:10:56](https://youtu.be/igQWdVGZGpI?t=656)** inner diameter divided by two. However, when you're drilling a hole, manufacturers typically drill plus or.1 mm larger and then plate down to the final drill size. Minimum annular rings, therefore I like to keep at at least 0.15. Minimum V diameter I will go with 6. Copper to hole clearance I like to keep at.254 and copper to edge clearance. So essentially to the board clearance.5 is a good value. You can go down to 04 for V-cut and 3 for cutting typically but.5 again staying away from manufacturing **[0:11:28](https://youtu.be/igQWdVGZGpI?t=688)** minimums. Minimum through hole.3 whole hole clearance 2554. We'll not be using will not be using microv. Minimum text height 8 is kind of pushing it. That's okay. Minimum text thickness I'm going to go with 0.1. Predefined sizes. This is the way Keycad works. We can predefine track sizes, via sizes, and then scroll through them when we go to the PCB design. Rather than entering specific values every time we route a trace, we can just enter predefined track widths. And I have my set of track widths that I like to use. For instance, I like using.3 mm traces for two-layer boards if they're signal traces and **[0:12:03](https://youtu.be/igQWdVGZGpI?t=723)** anywhere for instance.5 and 1 mm traces for power. For VAS, my standard via is a 7 mm diameter with a.3 mm hole. We do also have differential pairs because of our USB D minus and D plus nets. So we should fill in that information as well. Now typically for USB 2.0 we want a controlled impedance differential pair. But we're using USB 2.0 full speed. So essentially as slow or as quick as SPI we're using very we're going to have very short traces. So actually the control impedance doesn't really matter. And the actual **[0:12:35](https://youtu.be/igQWdVGZGpI?t=755)** way we root our differential pairs for this design really does not matter. However, we should enter a value because Keycad assumes it wants to root a differential pair and we need to provide it with some information. Trace width might be.3. A gap might be.3 as well and a V gap of let's say.5. I'm just guessing these values just for now. We can adjust them when we come to the USB differential pair later on. But again, these are some typical trace values you might use.3 for a good signal trace. And again, not controlled impedance. Power trace is larger. my standard via. You can lose larger VA, but I'd strongly suggest not going with smaller VA unless **[0:13:09](https://youtu.be/igQWdVGZGpI?t=789)** you have a good reason to. And differential pairs, just a value to get started, but we'll adjust this later on. Teardrops we'll look into later when we clean up the design. We have net classes, and here these were taken over from the schematic. So, we have our crystal, we have Vray, 5 squed C, and so on. And for these different net classes again why I like to do them also like to define them in the schematic is because they one carry over to the PCB design but we can segment the way we route into different classes. So for instance we might want to route power and ground structures different to our sensitive crystal structures or for example to **[0:13:43](https://youtu.be/igQWdVGZGpI?t=823)** USB. You could of course just stick with the default net classes but it depends on certain scenarios. You might want to have increased clearance or greater track widths, greater via sizes and so on. You can set custom rules as well. You can set violation severities for the design rule check. But for now, this is the bare minimum setup I would do for typical PCB design. Click okay to save. Now that we set up the PCB design, we can see on the right hand side the layer count has shrunk significantly. Again, this is still a two-layer board, but we don't just have copper layers, we have other layers as well. With the PCB now set up, let's go to the top toolbar. You **[0:14:17](https://youtu.be/igQWdVGZGpI?t=857)** can either press F8 or click this little button, update PCB from schematic. So, we want to pull everything we've done from the schematic, including all the footprints, and now put this onto a PCB. So, let's click this button, click update PCB. The changes have been applied. Click close. And I didn't press anything yet, but again, zooming in, moving around with my middle mouse wheel. We now have all these components grouped together and already selected. And this is all the components we had on the schematic. And I'm just going to place them somewhere around the center on the PCB. We haven't defined any PCB outlines yet. We'll do that once we **[0:14:49](https://youtu.be/igQWdVGZGpI?t=889)** place some components. and we know a rough structure of our board. But we can see because we've linked all of the footprints to the schematic symbols. For example, connector J1 has the specific USB type-C connector. We have all our mounting holes. We've got our main microcontroller and so on. This was all pulled from the data we provided Keycad initially. Again, pressing Alt 3 or going to view 3D viewer. We've moved some components around. We've imported the components and Keycad has automatically adjusted the board outline to just about fit all of our information on this board. Again, our board outline is missing. We'll do that later on. But **[0:15:22](https://youtu.be/igQWdVGZGpI?t=922)** we can see that all of these parts not just have a 2D representation in terms of footprint, but also a 3D representation in terms of a 3D model. And I think it's incredibly important to have 3D models in place. Especially when you come to mechanical design, it gives you a different view of the board. It helps you check things easily. For example, if silk screen is overlapping, if your components are too close, I use the 3D view a lot of times, and you should not just stick with one view. Different views refresh your mind in some way, and you can see things much better. So, I strongly suggest using this 3D view a lot and assigning to your own custom footprints if you make them. Always assign a 3D model. I never use a **[0:15:56](https://youtu.be/igQWdVGZGpI?t=956)** part which doesn't have a 3D model in place. Back to the 2D view, we also saw in the schematic editor that we assigned various colors to the different nets in the PCB. And as we see here, once we've imported the components, we don't really have various different colors. Depending on what layer we're on, that color will be highlighted. So, typically a top copper layer or front copper layer F.CU CU on the right hand side that will be a red color. If we're routing or routting on the bottom layer then that will be a blue color. So as you can see on the right hand side as I click next to the color box we can see different parts of the PCB get accented or highlighted and **[0:16:29](https://youtu.be/igQWdVGZGpI?t=989)** that's the current layer we are then working on. I don't like the default color view and again this is why I do my schematic colors and then transport them over to the PCB because it makes everything far clearer. With everything red or blue here, we can't really tell the difference between powers, grounds, high-speed signals, and so on. So, you might have already noticed, but if you go back to the board setup in the top left of Keycad, then going to net classes under design rules, there's a button which is import colors from schematic. So rather than having to reassign the colors once in the schematic, then once in the PCB design, **[0:17:01](https://youtu.be/igQWdVGZGpI?t=1021)** we can just import them to whatever we set up in our schematic editor. Once I click that, I go to the right hand side. We can see the PCB colors are now assigned. And we also have a default net class on the PCB design. Depending on what we're rooting, if we're rooting USB, if we're rooting power signals, we can give these net classes default track widths, via sizes, and so on. So you might want to have a control impedance net class if you're rooting USB or you might want to have wider traces for certain powers. For now, we're going to leave everything as default and just work with the predefined sizes we defined earlier. But now we have the net **[0:17:34](https://youtu.be/igQWdVGZGpI?t=1054)** close in place. So if I click okay, nothing has changed except you can see the rat's nest which are these essentially air wires which show connections that are still to be made have changed color. I would also like to have the pads and traces and tracks and everything else change color as well. The way we can do that is go to the right hand side appearance then click on the nets tab in the bottom open the net display options drop down and then change the net colors from just the rat's nest to all. And here we go. This is the kind of view I want. It is quite colorful but this is I find super helpful when I'm rooting. I can quickly jump to okay where's the USB it's these **[0:18:07](https://youtu.be/igQWdVGZGpI?t=1087)** green patterns where's ground that's everything that's gray where's power that's pretty much everything that's reddish so that's why I find it immensely useful not just for the schematic but also for the PCB design to label my nets and to color my nets the net labels are great as well we know okay this is I squed C1 SDA this is SCCl this is power this is ground this is the reset signal I'd strongly suggest doing this for every single design no matter how small or large the design is with all of this in place we are now ready to lay out the PCB and layout for PCB designs in my opinion is and should be the substantial part of any PCB design. The routting once you've done a good job **[0:18:41](https://youtu.be/igQWdVGZGpI?t=1121)** of layout will for the most cases fall nicely into place. If we do a rubbish job at laying out, we're going to have a much harder time. We might need more layers. We might need more view transitions and whatnot if we don't do our layout properly. So lay out properly first. This is a large part of the work. And then we can simply connect things together. Often times you will of course have a predefined board outline that you might get from a mechanical engineer which are based on certain enclosure dimensions where you need to put the mounting holes, what the board outline should be, where you need certain keepout areas. And of course, you have to keep all of that in mind originally also through the layout phase as well. **[0:19:14](https://youtu.be/igQWdVGZGpI?t=1154)** For us, this is just a simple death board. We have none of these requirements. We're just going to make it, I guess, as small as it's somewhat feasible. We don't want to cramp things together. Components should be accessible. We should be able to add in test points, add in probe blades, and so on. We don't have particular conraints, but keep that in mind when you're designing for a proper product. With that being said, let's get over to doing the layout. And layout is very much, in my opinion, about sectioning. We have a microcontroller section where we have the microcontroller as our centerpiece. And we have various bypass decoupling capacitors and maybe pull pull down resistors, configuration resistors around it, and that forms its section. **[0:19:47](https://youtu.be/igQWdVGZGpI?t=1187)** We've got USB with the USB connector. We have the ESD protection and some filtering that forms its little section. We have a power supply with the LDR regulator in this case. input out capacitors those all form sections we put those sections together and then we put the whole PCB together very simply speaking the way I typically do that is take the center piece of the section and for this particular board we are working rather simply just with a microcontroller and it has its peripherals so what I'll grab is I'll take the mic controller click on it and press M to move then I can freely move if I press escape I can cancel command and it's important when you're doing **[0:20:20](https://youtu.be/igQWdVGZGpI?t=1220)** layout and also in my opinion when you're doing routing is to stick to fixed grids same as we did with the schematic where we used 100 mil grids for the PCB design. Now, if you're working in the US or if you're working other parts of the world, you might be using mills, but we're going to be using millimeters. And the grid selection drop down is at the top. My ass cursor is just circling this, and it's currently set to 0.25 mm. For rough layout, typically I would not go below 0.25 mm grid for laying out. Typically, I might even go to 0.5 or 1 mm just to get a rough placement. We can always fine-tune later, but I find it very important to **[0:20:53](https://youtu.be/igQWdVGZGpI?t=1253)** always stick to grids. Even when you're placing smaller components such as bypass decoupling capacitors, I would never really go to 0.025 mm grid. There are of course accuracies and precisions of the various assembly pick and place machines and so on. So 0.25 or 0.1 as an absolute minimum is typically sufficient, but I would suggest going with 0.25 as the absolute minimum. So I'll select 0.25. If I don't want to use my mouse to cycle through the various grid sizes, I can press N on my keyboard to cycle down and shift N to cycle up. So, that's a quick way of cycling **[0:21:26](https://youtu.be/igQWdVGZGpI?t=1286)** through the grids. So, I'm going to start with the 0.5 mm grid. Click on the component or just hover over it and press M. And we see we snap to the component center. Let's just move that somewhere on the grid. You can see the grid lines on the background and key card just somewhere away from the other components that we have some space to place components around it. Now that we have a component placed also if you hover over the component or select it press M and then R we can rotate the component by 90° counterclockwise. But with the component orientation as we had before let's have a look at the pin out because the pin out at least for this particular board we don't have **[0:21:58](https://youtu.be/igQWdVGZGpI?t=1318)** particular other constraints will determine for a large part how we place the surrounding components. If we zoom in we can see that pin one and pin 2 as we designated in the schematic belong to UART TX and UART RX. UT TX and RX go to the USB UAD converter IC which then subsequently goes to the USBC connector. So it might make sense given the pin out of this microcontroller to have on the left hand side the CH340 as well as the USBC connector. Now of course we can move the pins to other locations as we saw with code compar studio. So we could move them to the top, bottom, right, **[0:22:31](https://youtu.be/igQWdVGZGpI?t=1351)** wherever we can find a UR peripheral. And often times it really pays off to move pins around because microcontrollers and FPJs are very flexible in terms of their pin out to locations that make your PCB design life easier. For us, it'll probably be okay at the top left pins. It could be that later on as we progress through layout and routing, we say actually it's a bit cramped on the left hand side. We've got a lot of free free pins on the right hand side. So it could very well be that we want to move some components around. If we move on, we can also see that we have the crystal pins, pins 11 and pins 12. So we want that crystal probably on the bottom left of the microcontroller. **[0:23:04](https://youtu.be/igQWdVGZGpI?t=1384)** We have I squed C on the bottom. So we might want our little accelerometer at the bottom here. On the right hand side, we can see we have the serow wire clock and serow wire debug pins. So we might want to have our tag connect TC2030 programming header on the right hand side. Scattered around. Again, we have some free pins. So we could move things around. We can't move pins 34 35 around. Certain pins are fixed of course such as also the power pins. So we have 1.35 volts. We've got a VF plus those pins will be fixed for most part but do keep in mind microcontrollers are flexible. Adjust your pin out. Don't just stick **[0:23:37](https://youtu.be/igQWdVGZGpI?t=1417)** with the first thing you said in your schematic. If you can move it around if it helps you with the PCB design. So an approach now could be that we have the microcontroller placed in our current center. We can of course move the grid origin and then place components around this microcontroller. for example, the decoupling capacitors, the ROS resistor, the peripherals we need for this mic controller to even boot up. And then we do the same thing for other sections. An alternative approach might be that okay, we've placed our centerpiece. Let's not worry about the surrounding local components for now. Let's just get a rough idea of the other components we **[0:24:09](https://youtu.be/igQWdVGZGpI?t=1449)** might want to place. So, we might want to take U2, which is our U to USB converter. Press M. Move that to the left hand side. And we can see already the rat's nests seem to line up quite well. So I can just place it somewhat to the left of it. We can see ULTX seems to flow nicely and U RX seems to flow nicely as well. And on the left hand side of the USB to U converter you have the D minus D plus pins which then go to the left hand side to the SUV connector. So that would be one approach of doing it before you start placing local bypass and supporting components around these various centerpieces let's call them. **[0:24:42](https://youtu.be/igQWdVGZGpI?t=1482)** Another point is that here you can see I only have the PCB design window open. What I simply do is I have one screen which has the schematic view open and one screen that has the PCB window open. Of course, I'm recording this on a single screen at a lower resolution. So, everything would be rather cramped. But let me just show you quickly. This is a split that could look like this. Of course, it's rather cramped because this because the resolution is fairly low again and is a single screen. But on the schematic, if I click on one component, for example, click on J2, our programming header, there's cross referencing built into Keycad. So **[0:25:15](https://youtu.be/igQWdVGZGpI?t=1515)** immediately in the PCB window, we jump to the relevant component. And this works both ways. If I click on, for example, C3 on the schematic, it jumps to show us that this is the input capacitor for the LD regulator. And this is a super useful feature that I suggest you keep on pretty much at all times. And if you have two screens available, put one screen the schematic and on the other screen, put the PCB design. Then you don't have to always all tab or switch between windows to see what you're actually rooting. Now for us, we have a very simple PCB. We've colored and labeled our nets fairly appropriately. So, we can probably get away with just looking at the PCB **[0:25:49](https://youtu.be/igQWdVGZGpI?t=1549)** window. But imagine for larger schematic, multi-page schematics, it's it's really good to have these various windows open at all times so you can quickly cross reference. But in our case, again, this is a very simple board. I'm just going to go with placing the components as they are because we know the structure of the schematic quite well. We know that for U2 on the right hand side, same as on the schematic, we connect to the mic controller. On the left hand side, we go through some ESD protection to us to a USB type-C connector. And the same thing we can then reflect on the PCB design because things seem to flow quite **[0:26:21](https://youtu.be/igQWdVGZGpI?t=1581)** nicely. We take D1, press M to move, and move it just to the left hand side. We won't worry about exact placement just now. We can tidy things up as we go. It's an iterative process layout and routing. So, we can take this. Of course, we'll have to take care of the orientations and alignments. You can see for instance, the minus and plus terminals seem to be flipped. at least if we we can't read them just directly. So, we might have to sort something out later. But we can take the USB type-C connector, M to move, R to rotate, and just place it all nicely aligned on a grid. And you can see everything's **[0:26:53](https://youtu.be/igQWdVGZGpI?t=1613)** aligned on this X-axis in one line. I find this very visually appealing as we'll see later on. Sticking to a grid, aligning things that there's some sort of symmetry if possible, of course. Doesn't have to be, but I find it quite nice. Now, we're just starting with a rough layout. We might want to of course reduce trace lengths and we can do that by placing placing components closer together. You don't want to place them too close as you can see kit get will show you that they interfere but you don't want to place them too far away either. There's always going to be a happy medium. Keep in mind we have to fan out and route out a lot of these pins. We might have to place some filtering and bypass capacitors around these components. So you don't just want **[0:27:27](https://youtu.be/igQWdVGZGpI?t=1647)** to scrunch all of these components together like this. You still need to leave space for surrounding components. So I can control Z to undo all that. Again, this is just a very rough layout and placement. From that, we can then define a board edge. We can put down the mounting holes and then we can get into details of the layout. We only really have the tag connect programming header on the right hand side. That's this component. And you can see here as I hover it over and I hover over a pad. If I press M, it'll actually snap to the pad. And the pad isn't the component center. You can see the component center is indicated by this little plus, this little cross in the right in between pin **[0:28:00](https://youtu.be/igQWdVGZGpI?t=1680)** four and three. So, I actually want to hover over that and then press M. And now we can see we're snapping to the component center. That's why we suggest you do that. Keep in mind, don't hover over pins. Hover over component center before you press M. And you can see here that a rat's nest in blue are moving around as we move the component. And this is a great visual indication of where approximately we should be placing our components. Over here wouldn't terribly make much sense unless you have a mechanical reason to do so or you don't have space. For us, we want to put the component again in line but on the right hand side maybe. Again, while you're doing your layout, keep your rooting in mind. you want to make your **[0:28:32](https://youtu.be/igQWdVGZGpI?t=1712)** own life far easier. So I could also take this component rotated by 180°. Okay, layout wise it look might look very similar. But now you can see pin 35 the clock pin has to route a longer way into pin 4 and pin 34 serow DIO has to go all the way around into pin 2. So as we had it before, let's rotate the component back. We have a shorter distance like so. We can immediately see we have probably easier ways of routting this if we keep it like so. Again, pre-plan, pre-plan, pre pre-plan. For a board like this, it's very simple, but **[0:29:04](https://youtu.be/igQWdVGZGpI?t=1744)** for more complicated boards, you might want to write this down some or sketch it out on a piece of paper or whatever your preferred method is. We have a crystal. I'm going to take the crystal, and we already saw at the bottom left of the microcontroller. This is somewhat where the where the component needs to be. I'm just going to put it in the vicinity. Again, rough layout first. The last two major parts are the I squared C accelerometer. That's U4. And we saw the I squared C pins currently are and the interrupt pins are the bottom of the microcontroller. Again, we can move them around. For instance, we might want to put them at the top on the right hand side. But for now, let's just place them somewhat centrally below the **[0:29:36](https://youtu.be/igQWdVGZGpI?t=1776)** microcontroller. You can see this part is actually rather small. So, that's going to be interesting to fan out and route out as well, but not terribly difficult. Finally, we have U1. And remember, U1 is our LDL regulator. And it has these various surrounding components. It gets fed from our 5V supply coming from Vbus from the USB type-C connector and then feeds our various other IC's on this board with 3.3 volts. So it might make sense to take this LDO regulator and not put it on the right hand side anywhere. We could put it just above D1 as we're getting our power from the host that is **[0:30:11](https://youtu.be/igQWdVGZGpI?t=1811)** connected to J1, our USB type-C connector. So a rough an incredibly rough layout might look something like this. From this, we could do a quick measurement. If we go to inspect and then measure tool, I'm just going to click and just do a diagonal measurement. If I click again, I can see, okay, the board might be around 55 mm in width and the height might be around 20 mm. So, this could give us an estimate. Okay, we might only need a 50 mm wide board and a 20 mm m tall board. But, of course, we also have our mounting holes. And these are fairly **[0:30:42](https://youtu.be/igQWdVGZGpI?t=1842)** chunky M3 mounting holes. If I click on this and press E, I can open the properties and we can see yes, as we wrote in the schematic as well, this is an M3 mounting hole. For this board, it might be overkill. I quite like M3 mounting holes. This is a fairly common size. And we can move those in, for example, the four corners of the PCB. Again, fairly rough placement. It could look something like so. And you can now imagine we could draw a rectangular board outline around these mounting holes and say, okay, for this very, very simple demo board, this is a rough layout and outline. Again, it's you have **[0:31:14](https://youtu.be/igQWdVGZGpI?t=1874)** far more freedom, which sometimes can be a good thing, sometimes can't, to define our board outline and move our components. We could also say, "Yeah, this is actually far too long. I want to make this reasonably smaller." So, what we could do is just move all of our components by clicking, dragging, holding the left mouse button and say, "Actually, we might only need something like this amount of space." And again if I do either inspect measure tool or press control shiftm on my keyboard we can see okay now because the mounting holes we've increased in the height height of the board or width whatever you want to call it and the length but **[0:31:46](https://youtu.be/igQWdVGZGpI?t=1906)** is reduced to 45 mm if that's this important for this board probably not I'd rather have the board slightly longer wider desk makes that it makes our routing and layout life easier we don't have a particular constraint to make this board as small as possible so I'm going to press escape a couple times to cancel the command and control zed just to space out the board as we saw fit. What I would like to do is align the mounting holes so their centers align both horizontally and vertically. So I can control shift M, click the measure tool. We can see it's 45 mm center to center for this one. It's 19.5 mm center to center for this one. I typically prefer round numbers. So 20 **[0:32:20](https://youtu.be/igQWdVGZGpI?t=1940)** mm, 30 mm, 40 mm, something like that, not these decimal places, so integer numbers. And we can measure M2 to M3. And we can make sure that our hole centers are aligned and symmetrical. To move the mounting holes, I can either hover over these, press E, and then select the footprint, and then change the XY position in this pop-up box, press okay. Or I can just change my grid by pressing N. So, changing it to 0.25, selecting both, pressing M, and I can just press my arrow key one up to move them 0.25 mm up. Do the same thing for the bottom two. Press M, arrow key down. And now, if I do control shift M, center **[0:32:52](https://youtu.be/igQWdVGZGpI?t=1972)** to center, I now have 20 mm. And I have 45 and 20 placements like so. So, something like this could be okay. And from this then we can draw our board outline. Again, you might come up with a completely different board outline, different positioning. And I'd strongly suggest spending more time on this, seeing if you maybe optimize a tiny bit more. Again, we will probably optimize the layout a tiny bit before we add in the other components on the right hand side. You can see we still have to fit all of these in the space we then define. But I'll show you how to create the board outline because now if we go to view 3D viewer or press all three again, the board outline is missing. And **[0:33:26](https://youtu.be/igQWdVGZGpI?t=2006)** Keycad has just stretched out the board outline to contain all the components and also the silk screen on the board. And of course, we just want to define it around these mounting holes. So, close that view. Go on the right hand side appearance. Click on layers. And then we want to go to the edge cut layer. Edge cut layer is our board outline layer. And for this, we will be drawing lines on the board. I'll show you first of all how to do rectangular corners. And then we'll do rounded corners. So, I can press control shift L on the right or all on the right toolbar. Just click on this draw lines tool. Again, I might want a larger grid. So, I'm going to do shift N to increase the grid to 1 **[0:33:59](https://youtu.be/igQWdVGZGpI?t=2039)** millmter. And I can just click on one point and start drawing around these mounting holes, for example, like so. Double clicking to end, and then press escape, escape to cancel the command. And now I can press alt3 again to open the 3D viewer. And we can see now this board outline error or warning has disappeared. And we actually have a board outline that follows what we defined with these straight lines. Now this board outline again is somewhat arbitrary. It's just based on a very very rough placement. There's no particular goal here other than making a dev board. No particular minimum size or **[0:34:32](https://youtu.be/igQWdVGZGpI?t=2072)** mechanical constraints. That's why you might think okay yeah there's quite a lot of space. It's quite empty. But for the sake of our videos, for the sake of demonstration, I think this is this is sufficient. What we can also do is of course make rounded corners. The way we can do that is not by using the straight line tool. We can use the draw arcs tool. If I click on the draw arcs tool or I can press control shift A or I can for instance go to the center one of these mounting holes and click once click twice to define one vertex and then I can define the angle 90° in this case. Press escape. Then I can take my straight lines and just drag them to the **[0:35:06](https://youtu.be/igQWdVGZGpI?t=2106)** edge points of this 90° arc. Press Alt 3. And now we can see we have a rounded corner on one of these on one of the corners of the boards. And of course we can repeat that. We can simply copy that corner, that rounded corner over to all of the other corners. There's some things to keep in mind, however. Rounded corners require a routing tool rather than uh rather than using Vcuts or Vcoring for when depanalyzing or panelizing the PCBs. Sometimes Vcuts can be cheaper, less work inensive and but in any case for Vcut or Vcoring as well **[0:35:39](https://youtu.be/igQWdVGZGpI?t=2139)** as routing, you will have to keep a certain distance clearance away from the board outline. That's for any components, that's for copper and so on. So that's why for instance here if I use the measure tool again ctrlM just as a crude measurement tool from about the copper to the board edge I have about8 mm and I'd suggest for most boards unless you have very very tight constraints keeping at least about 0.5 mm of board 0.5 mm of clearance to the edge that's for components that's for copper that's for silk screen things like that we want to keep this kind of area of 0.5 mm around the perimeter of the board clear from component silk **[0:36:12](https://youtu.be/igQWdVGZGpI?t=2172)** screen as we said before and this again just ensures manufacturability. So let me copy over these corners just by Ctrl + Cing by selecting the corner Ctrl Ctrl +V press R to rotate and I can move them to the centers of all my other mounting holes and do exactly the same thing by dragging these lines around. So I'll see you in just a second once I finish that. So this for instance is what the board would look like in its very rough state just with rounded corners. And again for now it's just a visual aesthetic preference just to show you how you can do that. And of course, you can make fairly arbitrarily shaped board shapes using these simple primitives on the **[0:36:46](https://youtu.be/igQWdVGZGpI?t=2206)** edge cuts layer with a very rough outline in place. The mounting holes placed somewhat sensibly. You might also want to adjust the outline to have nice round integer numbers. You know, in the steps [clears throat] of 5 mm, but of course that's not an absolute must. Again, we are very free in the way we define our board outline here. But what I have now is a board of around 53x 28 mm, which for us is completely fine. I've moved the mounting holes to be nice and symmetrical around the board. But what we also have to take care of is of course now the grid placement. So the grid placement is something you could do right at the start. We could have said **[0:37:18](https://youtu.be/igQWdVGZGpI?t=2238)** okay the grid we originate at our microcontroller and that's our center. But it often times makes sense and also the IPC recommends that the grid origin is at the bottom left of the board. So that would be essentially the intersection if we extend the vertical and horizontal lines. That's where we want to place our grid origin. The reason for that is that if we go up or right, so anything that's on the board or within the board within the board area has positive x and y coordinates. We have no negative x and y coordinates. If we want to move component more north, **[0:37:51](https://youtu.be/igQWdVGZGpI?t=2271)** we simply have to add. If we want to move it to the right, we simply have to add a number and so on. So that's why you would typically choose the bottom left as your grid origin. So the way to place then our origin if we want to place at the bottom left is go to place grid origin at the bottom and we can just place that right at the intersection of the horizontal and vertical lines like so. And now we can see the grid is realigned to that point bottom left. So that is our grid origin. You might have already seen if we go to the place drop down again there's also a drill and place file origin and that I'd suggest also putting on the same origin **[0:38:23](https://youtu.be/igQWdVGZGpI?t=2303)** as the grid origin. So I can place that here and we can see now in red we have the drill and drill origin aligned there as well. So everything is referenced the bottom left corner we have positive x and y coordinates for all the components. Now this is great but if when it comes to alignment especially if you want to for example align components distribute them distribute them equally across the board align them horizontally vertically having the grid origin bottom left isn't particularly helpful. So often times I might start out and say okay I'm actually going to have my grid origin in the center of the board. that allows me to do symmetrical placements. So, we could do that because we already **[0:38:57](https://youtu.be/igQWdVGZGpI?t=2337)** know the dimensions of the board. So, it's 53x 28 mm. So, we need to do half of that and place our grid origin there. We can see on the bottom as I move my cursor, the x and y coordinates change. So, if I hover over the grid origin, that's 0 0. And as I move to the right and top, we can see the grid origin change. But we also have the dx and dy. dx dy tells us the relative or the deltas between wherever we set a starting point. And the starting point we set by tapping space. So we want a starting point or reference point to be on the grid origin. I can hover over that and press space. And you can see the dxdy at the bottom has reset. And **[0:39:30](https://youtu.be/igQWdVGZGpI?t=2370)** now I can do it relative to a certain position that I designate by pressing space. So if I want to go if I want to do it relative to the center of the board, I can go to position 26.5 and 14 because that's exactly the center of the board. Press space. And now our deltas are relative to the board origin. Or of course you can set the grid origin there which we could do now. But this might be sufficient for us. So I can take for example the USB connector. Press M and we can see it's already aligned centrally with the board because our DY is zero. If we do the same thing for the microcontroller, we can do that and so on. Of course, it might be easier just **[0:40:02](https://youtu.be/igQWdVGZGpI?t=2402)** to place the grid origin because then you can press E on the component and we can simply change the XY position relative to a centered origin. But at the end of the day, you should have your grid origin, your draw file origin at the bottom left of the board. That is my suggestion. Now that we've got a lot of the basics out of the way, we can fine-tune our layout a bit. We can see there's some components where the courtyards, you can see this kind of pinkish box hanging off the board and these courtyards shouldn't overlap and they should be away from the board outline as we spoke about before. We tie up this place and then we can start adding in all of these relevant components around the board before we **[0:40:35](https://youtu.be/igQWdVGZGpI?t=2435)** then move over to routing. We also have these fidial markers and these help the pick and place machines and the automatic optical inspection to find their bearings relative and absolute position. So I take the fiduial marker and I want to place them across the board. So we typically have a minimum of three fedio markers. Typically I will have I'll put one top left, bottom left, and bottom right for instance. But you want them spread as far as you can across the board. So I might just place one next to the mounting hole like so. Take the second footed marker. Press M. Move it next to the bottom left mounting hole. Take the third marker and move it next to the right mounting hole like so. **[0:41:09](https://youtu.be/igQWdVGZGpI?t=2469)** And clean all this up a tiny bit. If I go to 3D view, this also helps me a lot. Sometimes you want some overhang on the USB type-C connector, even though there is a tiny bit of distance between the actual shroud of the USB type-C cable or plug that goes into this connector. So, you can actually arrange that the connector edge is flush with the edge of the board. But for now, I'll keep it like so. We also want to make sure that these mounting holes are sufficiently far again from the board edge. And we here we have about a millimeter. And that's okay. For through hole through holes I like to have a bit further away **[0:41:40](https://youtu.be/igQWdVGZGpI?t=2500)** from the bolt edge than for example SMD components. So a millimeter seems to be around fine. Our ESD protection we typically want a bit closer to our USB type-C connector. Again leaving space so we can fan out the part, but we want to have it fairly close so we can shunt ESD pulses essentially to ground quickly close to the source. You want our power regulator. We might want to move a bit further away up here so we can fit the supporting circuitry around it. The USB connections you want to keep short as well. So that's why I might want to move U2 a bit closer to D1. I want to move U3 and its fironic circuitry. So I can drag **[0:42:15](https://youtu.be/igQWdVGZGpI?t=2535)** and hold over it and move it a bit more to the left as well because we do have some supporting components around it. And that also gives me then room to move J2 just a bit further away from the board edge like so. So again, it's an iterative process. You might want to clean things up just a tiny bit before you start adding in the smaller components. And you'll do this repeatedly for your boards. After having adjusted the layout just a tiny bit as we just saw again as we add in more and more components we might have to move things around. We might have to adjust the pin outs just to make our routting life easier later on. We're now ready to move over adding in the smaller **[0:42:47](https://youtu.be/igQWdVGZGpI?t=2567)** components. And typically for PCB design I'd suggest going in order of criticality. You might want to do slower speed connections last. You might want to do critical components such as the mic controller and crystal USB connections first. Prioritize those. Prioritize those components before you put in less critical components. For example, capacitors on reset lines, pull-up resistors somewhere. It really depends on criticality. But of course, there's always going to be a compromise, always going to be a trade-off there. There's not going to be a single opt most optimal design. There many paths that lead to Rome as they say. For us, what I'd like to start with is the micro **[0:43:21](https://youtu.be/igQWdVGZGpI?t=2601)** controller. This has the main bulk of supporting components. We have various bypass decoupling capacitors. We've got the whole crystal circuit. We've got these trimming resistors, Reref connections, and so on. Once we have all those around the microcontroller, the rest is actually fairly straightforward. A couple bypass the coupling capacitors, some filter networks, some power, and so on. So, let's just get started with that. What I'd suggest doing again is an order of criticality. The pull-up resistors for the I squed C accelerometer aren't that critical. Similarly to the end reset pullup resistor as well as this filtering **[0:43:53](https://youtu.be/igQWdVGZGpI?t=2633)** capacitor. Okay, we might need it for this device to work. But in terms of proximity to to the device, what is most important? That's typically the bypass decoupling capacitor. It might be keeping the crystal oscillator loops short and small or trimming resistors. So those are the components we should be prioritizing. And again, it's an iterative process. So for instance, we have C12, which is our Vcore capacitor. I can take that and just by looking at the rat's nest, I don't even have to have the schematic open. We can see at least for this case, we only have one Vcore net. We want to have the Vcore capacitor fairly close. We don't want it **[0:44:25](https://youtu.be/igQWdVGZGpI?t=2665)** too close that it interferes with the courtyards. That our copper clearances are too small. We want it reasonably close. Close enough, but not too far away. Somehow, this might be okay. Something like this might not be. It really just depends. We want it as close as is feasible, but also not to interfere with any future routting and future component placements. For instance, if I place this capacitor like so, let's say we had to route out signals for for pins 47 down to 44. we can't really get past this capacitor. An option might be, okay, let's rotate this capacitor like so. Now, we can at least fan out pins 47 to 44 if we need those **[0:44:59](https://youtu.be/igQWdVGZGpI?t=2699)** pins. But it's not just the connection between, for example, this forward power path, this 1.35V signal. It's the overall loop area that matters with bypassing and decoupling. We have to take into account also our ground pad. And our ground has to go from pad 2 somehow, and we'll see later how that some is to pin 7. That is the ground. the only ground connection actually for this microcontroller. So this entire loop area could be critical. So a way maybe to optimize that to also help with if we route out pins 47 to 44 is take this capacitor, press R to rotate and move it like so. Now the ground and **[0:45:33](https://youtu.be/igQWdVGZGpI?t=2733)** 1.35V nets are fairly close. And I'll show you how to connect all the ground pads later. And actually just as a little hint, we'll be using the bottom copper layer to facilitate that with a large hopefully solid ground plane. For this board, of course, all of the components are on the top layer. And that's what I'd strongly suggest doing unless you have a reason otherwise too is if you can use one primary layer for all of your components and that's exactly what we're doing here. So for instance to start off with a capacitor placement like so might be okay. It's reasonably close to the 1.35V pad. The ground connection we will see is probably as short as we can get it. **[0:46:06](https://youtu.be/igQWdVGZGpI?t=2766)** Okay. We we could move the capacitor in like so. But if we look at the 3D view in terms of assembly, if we want to get to this component, it makes a bit harder because of the LQFP edge at the top left of this package. Therefore, let's say let's keep the component like this for now. We of course also have our 3.3 capacitor. Going back to the schematic, that's C11. If I click on this, go back to the PCB design, we've already jumped to it. And this is a larger component package. It's 0805. Press M. Move this to 3.3 volts. So, this already is a bit maybe, let's say, a bit more challenging. If I press R to rotate again a couple times, ideally the **[0:46:40](https://youtu.be/igQWdVGZGpI?t=2800)** connection would be something like this. Let me just click on this silk screen designator. Move this a tiny bit of way so we can see it a bit better. We want to consider both the forward and the return path. So 3.3 volts. We could think of a nice short connection between these two pads and pins 2 and 7 is our ground connection. Again, a short path. Now, while this would be great in theory for bypassing the coupling, how are we going to get our osque pin 8 out to a resistor down here? How are we going to get reset out? N reset. Okay, it might be a bit easier because we can slip out of the top here, but ours is going to be difficult. So, we probably have to move this capacitor away a tiny bit. This **[0:47:14](https://youtu.be/igQWdVGZGpI?t=2834)** way, we can come out of pin 8, move past the capacitor down to the bottom. Again, thinking ahead to your routting, your layout choices will significantly impact how you route out this PCB. So, something like this might be okay. In case you're rooting out pin 5, you might have to rotate your capacitor like so. Again, not entirely optimal, but it could be an option. But for us, because we are not that constrained in terms of how many pins we're actually using, some placement like this might be okay. Bypass decoupling capacitors as close as is feasible to the relevant power and ground pins. Other than that, C11, C12. What's also important, ROS, and of **[0:47:46](https://youtu.be/igQWdVGZGpI?t=2866)** course the crystal oscillator because we just saw the ROS pin. Let's just do that. R4 M to move. And keep in mind again, we're still with these fairly fixed grids. So, we can't place it terribly close to pin 8. Ideally, we want something like this. But of course, our capacitor is in the way. So, we might want to put our ROS resistor somewhere like here, which means we have to carry out of pin 8 into pin 2 of the ROS resistor. And it looks like we should be able to fan out pins 11, pins 12 of a high frequency external crystal oscillator, which sits down here. So, again, we might have to move these **[0:48:19](https://youtu.be/igQWdVGZGpI?t=2899)** capacitors and resistors out a bit further, but this might be a good starting point. If you can, and if you want to while you're rooting, of course, we'll have to adjust the silk screen later on. I always like to also move the silk screen out of the way just to make things a bit easier to see, a bit easier to read like so. But of course, we'll adjust that later on. These are fine tuning things. They're not terribly important for now. That being said, we have our osk in place and now we have our crystal that we need to put in place. Now, ideally, our crystal, we are missing the load capacitors for now. Should be as close as is feasible to the pins. So, something like this might be okay. But keep in mind, we still have **[0:48:52](https://youtu.be/igQWdVGZGpI?t=2932)** load capacitors left and right of this. And also we want to keep our crystal and crystal oscillator circuitry away if we can from other aggressive signals. Aggressive signals might be fast rise and fall time digital signals. For example, we wouldn't want to put our crystal oscillator far away from the component next to these USB signals. That wouldn't be great. So we want to keep the distances reasonably short. It doesn't have to be terribly short. There are somewhat forgiving, but maybe a component placement like so might be right. We will looks like we have fairly short traces for HFX in and HX out. We have place for our load capacitors and we can route our I squed C lines **[0:49:26](https://youtu.be/igQWdVGZGpI?t=2966)** somewhat away from the crystal. So picking up C8 and C9, I'm just dragging over pressing M to move both. What I want to do is place my load capacitors fairly close. If I place them close like so, this still looks okay that I could, for example, desolder C8 and replace it with a different capacity if I need to tune the load capacitor values. So keep them close, not too close, not too far away. Something like this seems okay. And again, I'm relying on the grid settings to make sure I'm vertically aligned. But for instance, also X1 to R4. I quite like when the components are also aligned horizontally like so. So, **[0:49:59](https://youtu.be/igQWdVGZGpI?t=2999)** always checking with all three looking at the 3D view. Again, this comes from experience, just seeing just by visually being able to tell, is this close enough? Is this is this too far? And so on. Is it away from signals? An iterative process. And of course, it takes some time to get familiar with how these circuits work. But somehow this might be okay. If you want to live a bit more aesthetically, you could of course move down X1 and C8C9 to be in line with U4. Now, that's a sacrifice that the pins 11, pins 12 have a longer trace length to go in here. So, it might not be reasonable to do so. So, that's why you might want to keep your crystal oscillator section just a bit closer **[0:50:32](https://youtu.be/igQWdVGZGpI?t=3032)** like so. Other than that, what's left in terms of critical circuitry? Well, I would immediately jump to the VRF minus VF plus pins. If you are using the integrated or an external voltage reference, you will have to place those. So C10 and R5 would be the next critical components. And after that, we can then finally move on to the end reset. And by that time, we've pretty much done a rough layout just for the microcontroller section. So you can see just following some basic simple rules, it isn't that difficult, at least for of course a very simple demo board like this. C10 is our VRF capacitor, and I'm just following the rat's nest. You can **[0:51:04](https://youtu.be/igQWdVGZGpI?t=3064)** see the rat's nest are twisted. That's our crossing. That's why I have to rotate the component by 180°. Let me move the silk screen out of the way because it's a bit irritating. And now we can see okay maybe we want to place it centrally between pads 43 VF plus and pad 39 VF minus. And I'm also placing it in line with my 1.35V capacitor. So we have nice short distances to VF plus VF minus and our bypass decoupling capacitor. And now we can also grab that grounding resistor. And again if you're using VF minus you should in theory tie this directly straight to ground. We've just used this 0M resistor as a short **[0:51:37](https://youtu.be/igQWdVGZGpI?t=3097)** link. So I'll take this resistor press M to move as usual. Rotate it 180 degrees by pressing R and place it close again. Not too close that the courtyards overlap, but just that the courtyards align like so. And I can move the silk screen just to make it a tiny bit neater like so. Crl S to save. Alt three to view in 3D. And you can see like so this is a pretty nice tight placement of decoupling and bypass capacitors. Again, C11 is a bit further away because it's a larger package and because we have pins to route out and past these components. That's why we place C11 a bit further away. In any case, this is a rough **[0:52:09](https://youtu.be/igQWdVGZGpI?t=3129)** layout for our mic controller. Very simple, and we've already thought ahead to the routting stage, which will make our lives quite a bit easier later on, as we'll see. Of course, now we can't forget the end reset lines. So, we have this pull-up resistor and this filtering capacitor, C14 and R8. So, we are going to do C14 first. Take C14 and let's see where this needs to go. C14 looks like it has to be here at pin 4. Now unfortunately if we place for example our reset and reset capacitor like so when we place iron reset pull-up resistor left of this for instance our URX RX lines will have to go over this **[0:52:43](https://youtu.be/igQWdVGZGpI?t=3163)** capacitor over the resistor and into our U2 USB to UR converter not great and also the actual location of the N reset capacitor resistor doesn't terribly matter at least it doesn't matter as much as for instance the bypass and decoupling capacitors where else does this N reset signal go to well following rat nest it goes to our serial debug our tag connectet connector so we could say okay the location of these components isn't terribly critical let's place it if in the vicinity of something that belongs to this component group so I could move it like so close to the tag **[0:53:17](https://youtu.be/igQWdVGZGpI?t=3197)** connect connector that means later on we'd route out of pin 3 through this spacing into the reset capacitor and then we'll route into our in reset pin like so again for something that's less critical this placement might be okay we of course also need the restor That's R8. And we'll just place that adjacent to our capacitor. Something like so. Now, for my liking, we're getting a bit close to the mounting hole. So, if we go to all three again, 3D view. Okay. This pad for the mounting hole is fairly generous. So, it's probably still okay, but you might want to move these **[0:53:49](https://youtu.be/igQWdVGZGpI?t=3229)** components a bit further away given that we have the space. So, for instance, we could take this grouping of components and we could move it like so. for instance, we still can route out in a nice clean fashion to the end reset pin and this still gives us some space away from our mounting hole. Keep in mind also now the T connector footprint and actual connector is fairly small even with this legged version. But you will have these prongs for lack of better word that have to go through these mounting holes. So that's why you might also want to keep clearance away also indefinitely on the bottom side. Keep clearance away from these holes for the **[0:54:21](https://youtu.be/igQWdVGZGpI?t=3261)** legged version of this connector. But again, just to show how you can be fairly flexible or more flexible by not with these less critical components. Again, just moving the silk screen out of the way, clicking on it, making sure it's highlighted, and pressing M to move. Making sure the order is right as well. So, something like this, for example, and I've just aligned it also on the X-axis, horizontal axis, like so. All right. So, this is the main part of our microcontroller. What we want to do now is maybe move to the next critical thing. Of course, power is critical as usual, but that's something I might do a bit last unless I have a lot of, for **[0:54:55](https://youtu.be/igQWdVGZGpI?t=3295)** example, switching converters or high frequency switching converters. A lot of them, lot of different rails. I also have to pre-plan that a bit better. But for now, the next critical thing seems to be U2, which is a USB to converter because this has a somewhat fast USB interface and it has a various different connections. Going back to the schematic, looking at U2, what does it need? Okay, it's got power and ground connections, but expounding circuitry, it's only really C6 and C7. And the way we place these capacitors is again because they are decoupling capacitors. We want to place them close to the **[0:55:26](https://youtu.be/igQWdVGZGpI?t=3326)** relevant power and of course ground pins. That's pin 7. And that we want to have adjacent to C6 and pin 10 is what we want to have adjacent to C7. There's a reason why I've placed my capacitors like this on the schematic. And this is an indication to whoever does the PCB design, this is the order I want them. I don't want C6 next to pin 10, and I don't want C7 next to pin 7. I want C6 next to pin 7 and C7 next to pin 10, just as it is with the schematic. It's delivering design intent. Now, you might say, okay, this isn't really important. They're both the same voltage. They're both the same capacitor. It doesn't really matter, which is in this case absolutely correct, but it's a matter of **[0:56:00](https://youtu.be/igQWdVGZGpI?t=3360)** principle. It's a matter of following through even in the most basic of boards that you can do those for more advanced designs as well. So, with that being said, take C6 and let's put it next to pin 7. Pin 7 of U2. And that happens to be right here. So this is a bit of a squeeze at the moment. I could rotate the capacitor like so. Means we have a fairly close connection to pin 7 which is exactly what we wanted. However, our ground needs will need to be connected somehow and we're interfering with UR0 TX and UR0 RX. Before we could simply route out pins 9 and 8 into pins 1 2 of the mic controller. But placing this **[0:56:32](https://youtu.be/igQWdVGZGpI?t=3392)** capacitor here, yeah, that isn't that great. What we could do instead is take this capacitor and sacrifice do a compromise and move the capacitor for instance somewhere like here. We would then route power through the capacitor and then neck down the trace into pin 7. This then gives us clearance to route out TX and RX pins. Okay, it's less optimal than the closer connection. But in this case, this is also a reasonable attempt of doing this connection and it means we need less VS or jumps or hoops to route out TX and RX. Again, this is a matter of experience knowing when and **[0:57:04](https://youtu.be/igQWdVGZGpI?t=3424)** when you can't do these things. But the simpler the circuit, the lower the speeds in your design. Typically, you can get away with this more and more. Now, we had the other capacitor that was C7 and we said they want that next to pin 10. Let's take C7 and we can move that next to pin 10. Again, we have various options. We could place like so where we have the same problem as before. We can place it like so, which gives the shorter connection, but we also have to keep the ground connection in mind. So what we could do also for the sake of symmetry is take that capacitor and have it symmetrically similar to C6. Again, we still have a fairly short connection between pin pad **[0:57:36](https://youtu.be/igQWdVGZGpI?t=3456)** one of the capacitor and pin 10 of our USB to converter. And we've made it look a tiny bit aesthetic. Not that that's terribly important, but I find a nice PCB layout is something very nice to look at. And in any case, this might be an appropriate positioning of these decoupling and bypass capacitors. So let's just move the silk screen out of the way as usual. Something like this might be completely fine to do. Again, keeping in mind current loops, power paths, short connections, as we'll see later. And we're just trying to facilitate an easier time when it comes to routting later on. We don't have terribly many components left. Let me just drag all of these over just a tiny **[0:58:08](https://youtu.be/igQWdVGZGpI?t=3488)** bit just so I don't always have to scroll to the right all the time. Looking at the schematic, what do we have left? We have our accelerometer, of course, so that might be the next critical thing. Then we have some filtering networks, the whole power section, and the USBC pull down resistors. Let's keep the power section, the pull down resistors for the end. And now let's look at the accelerometer briefly. There's not terribly much. We've already placed the accelerometer itself. We need the bypass capacitor. That's our first order of criticality. And then the pull-up resistors. These are of course important, but they're not as critical as the bypass and decoupling capacitors. So clicking on C13, moving to the PCB design. We want to take this **[0:58:42](https://youtu.be/igQWdVGZGpI?t=3522)** part and see where it needs to go for our accelerometer. Now we can see we've got three different pads. And this can of course be misleading. Which which pad do we place the capacitor closest to? pin four, pin 7, pin 8. Well, if you remember back to the schematic video, pin four is the chip select pin. That definitely does not need a decoupling capacitor. VDDIO, if we looked at the data sheet again, this did not need a decoupling capacitor. That simply sets the IO logic level voltage. What needs a decoupling capacitor and where C13 needs to be closest to is pin 8 of U4. So, **[0:59:15](https://youtu.be/igQWdVGZGpI?t=3555)** that's where we want to put it. And again, that's why you should always cross reference back to the schematic and see where to actually place components. Similarly for all the ground pads, we've got pin 3, 9, 10, 11, 12, 13, 14, and all ground. Which one is the actual power ground? Back to the schematic, it's pin 9. So ideally, we want to short connections between pin 8 and the capacitor and pin 9 and the capacitor. Luckily, pin 8 and pin 9, as their numbers suggest, are right next to each other. So it would make sense to have our capacitor placed somewhat symmetrically. And of course, the grid isn't aligned to these pads. But something like this might be reasonable **[0:59:48](https://youtu.be/igQWdVGZGpI?t=3588)** because now we can route out pin 9 through the capacitor and pin 8 through the capacitor coming from a power source. And that might look something like this in the 3D viewer like so. There's two things I don't like about it. One, which might be more critical than other. I think for my personal liking for this board, we've got a bit more space that C13 is a bit maybe too close. Let's say we want to resolder or refflow U4 because some connection didn't connect properly when when soldering. If we try to hot air U4, C3, C13 might come off as well. It might be more difficult to access the pads of U4. So therefore, I might want to move C13 a **[1:00:23](https://youtu.be/igQWdVGZGpI?t=3623)** bit further away. Give myself some clearance. You don't have to pack components that tightly. Another thing is again just for the sake of aesthetics and satisfying my OCD, I probably want to just center C13 with U4. Again, if I center this, it's only one click up. One click in this case being 0.25 mm based on my grid settings. It's a small enough change that is absolutely going to make no difference into the decoupling performance of this, but it just satisfies my need for making things nice and symmetrical and aligned. Then moving the capacitor also one unit out, that gives me just a tiny bit more space between U4 and C13. It might not seem **[1:00:56](https://youtu.be/igQWdVGZGpI?t=3656)** like much, but when you actually come down to having this under microscope, trying to reflow, resolder this, it could make a world of difference. So that's the easiest way we can then place C13 and U4. The next thing are the I squed C connections. And for I squed C. Now we could think about, okay, we've got the UART RTS CTS signals. We're going to have to figure out how to route them past the crystal oscillator into the pads of U2. And these of course will be crossing with the SCCl SDA connections. So we could go to code go back to code composer studio to see can we maybe use pins 18 to 24. Are there **[1:01:30](https://youtu.be/igQWdVGZGpI?t=3690)** any I squed C pins we could use there? That might make our lives quite a bit easier. So just having a quick look at look at code composer studio. I've just got the pin out view on the right hand side open. If I just hover over some of the pins, so we're looking at the bottom side, of course, we can see actually pin 18 seems to have I squed C0. SDA and pin 19 is I squed C0.CL, which actually might be a good thing because then we can simply route out pin 16 17 to the left of the accelerometer and we move pins 14 to the right hand side and we don't have that awkward crossing which we have to sort out with **[1:02:02](https://youtu.be/igQWdVGZGpI?t=3722)** layer transitions and jumps and all of that nonsense. So let's actually make that change. So I squed C, we're not going to use I squed C1 anymore anymore. We're going to use I squed C 0 on pins 18 is SDA, pin 19 is. So let's make that change in the schematic. Okay, I've made some changes in the schematic to reflect the changed pin out of the microcontroller as we just figured out from Code Composer Studio. Because I ran out of space on the right hand side, I would have had to increase the schematic page sheet. I thought I'd show you something different. And I moved the accelerometer which is previously in the right hand side of the schematic to the **[1:02:35](https://youtu.be/igQWdVGZGpI?t=3755)** bottom left. And to indicate that I'm jumping within a schematic or across schematic pages, what I typically do is do global labels as they're called in Keycat. So for instance, we have now pin 18 is SDA, pin 19 is. And I've hooked these up with global ports. On the right hand side, I can pressR plus L, place global label. You can give the label name just like the net, but also a shape. So it's input, output, birectional, whatever. And that's what I put for pin 8, pin 19 to indicate that I'm jumping somewhere else. If I just had a net label there, it looks like, okay, I've labeled the nets, but actually it's not connected to anything **[1:03:08](https://youtu.be/igQWdVGZGpI?t=3788)** else. By placing a global label or one of these ports, I can indicate, at least to me, a jump. I also like to place some text around those ports or labels and say where's it coming from? Where's it going to? So here I'm saying two from accelerometer. This is I squed C0 SDA, I squed C 0Cl. And that indicates, okay, we have to look for the same color, same net label. And we can see bottom left the accelerometer. That's the remaining space I had. Of course, you could could clean this up quite a bit. And here I have the same thing. I have the ports. I have two from MCU. And I've also changed the port directions appropriately. So SDA is birectional.Cl is from the **[1:03:42](https://youtu.be/igQWdVGZGpI?t=3822)** microcontroller to the accelerometer. The mic controller is the master in this case. Similarly for the interrupt signals because I've moved the accelerometer away. I have my interrupts which are two output pins, pin six and five, which go to the MCU. So we just have to look on the schematic. Uh-huh. They're in the same place as before. They ain't one and two, but these are inputs to the microcontroller. And I'm writing here from the accelerometer just to make the schematic a bit more clear. And I didn't didn't want to cramp anything as much as it was before as well. You could also add, you know, some graphical elements, some boxes, labels around all this to make it a bit neater. But just to show you another schematic drawing technique also because this **[1:04:15](https://youtu.be/igQWdVGZGpI?t=3855)** accelerometer and parts of the schematic have changed, moved around. I've also changed my annotation. Previously, I believe these pre-op resistors were R six R7. The bypass capacitor was C13 rather than C14. So I've adjusted my designators to fit the flow of the schematic. So it's left to right, top to bottom. That's why the accelerometer and its panic components are last. Now if we go back to the PCB, I haven't imported those changes yet. And what we have to do is either press F8 or go to the top toolbar and click update PCB from schematic as we did to get the components in in the first place. So **[1:04:48](https://youtu.be/igQWdVGZGpI?t=3888)** click on that update from schematic. Update PCB. And we can see here our changes are now reflected on the on the printed circuit board. Now we can see our 16 1617 signals RTSCTS. We can route through this passage here. I squ C SDA and SCCl look easier to route out as well. It looks like actually we don't have to do any crossings anymore. And our int one and in two we can just come around the C14 decoupling capacitor into the pins of the microcontroller. So this already seems a lot better. And this is again trying to emphasize the point that a microcontroller is a flexible thing. **[1:05:20](https://youtu.be/igQWdVGZGpI?t=3920)** If you have free pins, if if you have free peripherals, don't just stick to whatever you chose in the first place when you are creating the schematic. The schematic in a loose sense isn't terribly concerned with the actual physical placement. Of course, you can think of that ahead of time and derive that from the schematic symbols, but it's something you can adjust and should adjust on the fly. Also, when it comes to PCB design, this is why I suggest doing it like so. Now, after all of that talk of adjusting pins and pin outs, we also have to, of course, add in the pull-up resistors. And because our colors are all nice, we can see that our polar resistors are R7 and R8. And these **[1:05:53](https://youtu.be/igQWdVGZGpI?t=3953)** should be in the vicinity of the I squed C devices. So I'll move them together first of all. So a thought could be that we either route into a U4 then out and into the polar resistors or we do them somewhat in line. So for instance, I could move U4 and C4 down a bit. So I could place my polar resistor somewhat in line that I route into SDA into the SDA pincccl through the polar resistor into U4 for instance. It it doesn't really matter in this particular case. I could even have for the pull-up resistors over here route into U4 first and then to the pull-up resistors for I squed C such a slow bus such a slow **[1:06:26](https://youtu.be/igQWdVGZGpI?t=3986)** interface it isn't critical but of course you should make a reasonable effort reasonable attempt of making your routing layout fairly clean and fairly sensible. If we place U4 and C14 that far at the bottom it's quite close to the board edge and also we'll probably have difficulty rooting out in one and in two. You might want to move U4 and C4 up a bit or moving your pull-up resistors up a bit as well. We're iterating again because now UR RTS CTS will have difficulties passing past R7, R8 and C9. So that means we might have to move our crystal section just a bit **[1:06:59](https://youtu.be/igQWdVGZGpI?t=4019)** to the left to make sure we have a channel for RTS CTS to route past the crystal. Now again, it might not be as aesthetic as before, but we want to prioritize the actual function over the aesthetics. So something like this might be in a reasonable first attempt at the layout for these particular components. Finally, we really only have things that are to do with the power section. We have the USBC pull down resistors as well as a filtering pi network and the input output capacitors for U1, which is our LDO regulator. So you could start left or right. You can say, okay, let's **[1:07:31](https://youtu.be/igQWdVGZGpI?t=4051)** put R2R3 down. Let's do a PI filter that goes into our LDO regulator. But again, in terms of order of criticality, R2, R3 aren't as critical, for instance, as the power path. Again, of course, they're needed, but in terms of placement, we could place R2, R3, as a joke, on the moon, and it would probably still be okay. But, but our our power line is more critical than R2, R3, for instance. So, we might want to do our power rails first before we then put on R2, R3. So, let's just start, for instance, with C1, which is our input capacitor from the **[1:08:03](https://youtu.be/igQWdVGZGpI?t=4083)** USB connector. And the USB connector of course has two orientations rotated 180 degrees. So we always have the double double sets of pins. We have double sets of D minus D plus CC pins VUS and ground. So we could place C1 down here next to V bus and ground. But actually we've placed our U1 regulator at the top. So it makes sense to place it on the opposite side because our power path is going to be from the USB connector through a Pi network into U1 and out of U1 for 3.3 volts. I would suggest placing C1, R1, C2, our pi filter up here somewhere. So that's why we would **[1:08:37](https://youtu.be/igQWdVGZGpI?t=4117)** take an R1 which is our our placeholder series element and I'm going to make it align with D1. This C1 R1 C2 isn't any bypass decoupling. It's simply a filtering network which is a placeholder. It should be close to your power source of course but and it shouldn't be too far away but it doesn't have to be as close as for instance you know our bypass and decoupling capacitors. So something like this might be okay. And then symmetrically we can take C2 and put it on the other side. For instance, that would look something like this. So that's one method of doing a PI filter. What I prefer, which is a slightly bit more compact version, is **[1:09:11](https://youtu.be/igQWdVGZGpI?t=4151)** actually this structure. To me, in this scenario, this is of course just a tiny bit more compact. We have to keep sure now not that it makes terribly much of a difference that we route from the V-bus power into the C1 capacitor pad first then into R1 out of R1 into C2 and then only into U1 through the capacitors as well rather than going from USBC jack USBC connector into R1 then C1 and so on but it's a minor difference. We'll come to that when we get to the routing later on. So again closeish to Vbus not too far away and not too close that become we have difficulties with soldering and **[1:09:43](https://youtu.be/igQWdVGZGpI?t=4183)** assembly. You could also line this whole structure up like so say that R1 is aligned with C7 for instance might make it a tiny bit neater. So something like that might be a good starting point. This also keeps the Vbus connections then short between Vbus of the R1 network as well as Vbus of the ESD the TF TVS diodes on the USB line. So we want to keep that connection short. So this this is why this placement might be favored as well although the components are quite close. In case now we've done our PI filter, C1, R1, R2. Let's move over to the audio regulator. Now, all of these components are of course **[1:10:15](https://youtu.be/igQWdVGZGpI?t=4215)** important, but the most important components are C3 and C5. C4 is an optional bypass capacitor, which which can help to reduce the output noise on the 3.3 rail, which in our case isn't that terribly critical. So, let's start off with C3 and then C5 and then place C4. Taking C3, this is a larger 0805 capacitor. Again, now we have the issue of is pin one the power pin or pin 3 the power pin. They both have the same net label. Looking back, pin one is the power input, and that's where our input capacitor should be. Pin three is simply just an enable input pin. A high impedance input pin. So, we have to **[1:10:49](https://youtu.be/igQWdVGZGpI?t=4249)** rotate our capacitor by 180°. Place it close to U1. Move the silk screen out of the way. Like so, might be a good starting point. We also have to think about where we're going to place VAS, our ground connections later on. So, we might want to keep a bit more space to be able to fit a via in. But, as an initial guess, this seems to be okay. Now we need the output capacitor and that's fairly unambiguous. It's C5 placed close to the output. So we have this kind of symmetrical layout. Input capacitor LDO output capacitor. You could of course place the out capacitor also like so. And this could work as **[1:11:23](https://youtu.be/igQWdVGZGpI?t=4283)** well. Of course, you're still giving a very short connection between pin one and pin 5. And your ground loop, your overall current loop is also quite small. But in this case, this layout is in my eyes preferred because it's more symmetrical. And our power ground loops are very similar between those two scenarios as well. Lastly, then we have C4, which is our optional filtering capacitor. And depends on what regulator you choose, you probably won't have this. I'm just going to place this somewhat symmetrically close to the device. You want to keep the connection between pin 4 and pin one short and reasonable. Not too close, not too far away. Again, always checking in 3D view if it looks reasonable to you as well. **[1:11:57](https://youtu.be/igQWdVGZGpI?t=4317)** So, something like this might be an okay starting point for layout. We have plenty of board space to move things around. If we feel like things are getting too tight with rooting, we need to give a bit more space. We can relax our initial layout a bit more as well. But you saw as we progress through the schematic, we did things fairly logically based on criticality and then section by section and then stitching those sections together. We of course still have the pull down resistors on the CC lines pin R2 and R3. And these need to be placed somewhat sensibly as well. So we have CC1 and CC2. Now CC2 is **[1:12:31](https://youtu.be/igQWdVGZGpI?t=4351)** easier to access which is R2. We could place it for instance somewhere like so. Keep in mind we still have to route out Vbus and ground and all of that. And ideally we would want to just place C1 symmetrically at the top maybe like so. But now CC1 CC1 interferes with Vbus and that's what we just spent a bit of time on getting the PI filter somewhat right. So that might not be great to have there and probably isn't great to have there. If we go to 3D view, some USB connectors have their shell resting directly on the board. Now, of course, it's kind of eyeballing it with this USB connector, **[1:13:04](https://youtu.be/igQWdVGZGpI?t=4384)** but the shell here is actually lifted off and doesn't make direct contact with the solder mask or the top layer of the printed circuit board. I bring this up because often times you will not want to, for instance, root underneath the USB connector because you shouldn't be seeing in the solder mask, that is that top surface covering which protects the copper layer underneath. You shouldn't be seeing that as an insulator. While it is an insulator, it's not a particularly great one and solder mask can fail and I wouldn't rely on it as an insulator. For our case, for sake of simplicity and also because this actual USB connector, the shell is raised off away from the **[1:13:37](https://youtu.be/igQWdVGZGpI?t=4417)** solder mask. I think it's okay to route underneath in this particular case. So, what we could do is just place R2 and R3 somewhat symmetrically. And that means we can then simply route underneath. So, out of pin B5 underneath the USB type-C connector into CC2 and similarly and symmetrically for USB CC1, pin A5 into R3. And that just makes our lives easier because now it doesn't block VBUS. At least outside doesn't block VBUS. We'll see. We'll have to do a jump for VBUS anyway. But this makes it maybe a tiny bit nicer and cleaner. With that being said, this might look like an initial **[1:14:10](https://youtu.be/igQWdVGZGpI?t=4450)** layout. Okay, there might still be things to clean up. We have silk screen, which is superolous. For example, for the mounting holes for the fidial markers, there's some silk screen hanging off the board which you need to clean up. But the main point I'm trying to illustrate is that we should spend a fair amount of time doing a proper layout. It'll make our lives a lot easier when it comes to routing later on. We've really thought ahead of what connections need to go where. We've really done some pin mapping, pin swapping based on what we think our routing is going to be like. We've placed components as we think would be optimal, also considering power, decoupling, bypassing, signal length, and so on. And all of that without doing **[1:14:44](https://youtu.be/igQWdVGZGpI?t=4484)** a single route. It's all just essentially visually doing the layout. Again, all components on the top side, no components on the bottom side. A fairly arbitrary shaped board outline just to make our lives a bit easier, make this board fairly simple. We can add some graphics later on and various information that is typically necessary on a printed circuit board. For now, the last steps I would like to do, clean up the mounting holes. So, I'm going to click double click on the reference properties and or the silk screen and uncheck visible. do that for the fidutial markers as well. I can also click and press E. It's the same thing. **[1:15:16](https://youtu.be/igQWdVGZGpI?t=4516)** And of course, you can clean up the rotations of the silk screen with placements on. I wouldn't spend too much time on that. I usually do this kind of clean up right at the end of the PCB before I'm about to produce manufacturing files because there is a high chance that our placement layouts will change. Things will interfere. So, don't worry too much about silk screen, but do keep it out of the way so it doesn't interfere with you being able to see net names, pads, and so on. For now, this seems like a fairly sensible attempt at an initial layout, which means we can move over to rooting very shortly. With this hopefully somewhat sensible layout in place for this rather simple **[1:15:49](https://youtu.be/igQWdVGZGpI?t=4549)** board, we can move over to rooting. And there's a couple things I would like to talk about before we begin routting. That's first of all, of course, the stackup of the board. That's something you can decide beforehand and you might adjust during your routting process. Depends on the amount of components. It depends on the type of components. If you're using just standard through VAS or if you're using blind buried VAS, microv, that'll all influence how we route things. But this board is incredibly simple. It's going to be a simple two-layer board. Our front layer, front copper layer, just has all of our components on it. And we'll be using this predominantly for signal and power routting. The bottom layer, where there **[1:16:22](https://youtu.be/igQWdVGZGpI?t=4582)** are no components, we will do a single large polygon pole that spans the entire area of this board. This will provide a fairly nice low impedance ground reference that we can connect all of our ground pads to with shortwire connections and VA that we can then just drop down to that layer. And that's a pretty standard practice to have your primary layer single power and your bottom layer ground for a two-layer board. And this is going to be pretty much sufficient for this type of board. The way we can create a polygon pole is on the right hand side draw zones. And you might want to increase your grid size by pressing shift N or just selecting the toolbar. So I'm just going **[1:16:55](https://youtu.be/igQWdVGZGpI?t=4615)** to 1 mm grid. Click on draw field zones or control shift zed. And I'm not going to bother with following the contour because keycad will automatically fit the polygon paw to the actual outline. I just leftclicked and now you get this copper zone properties. I want this for now just on the bottom copper layer. And our net I want to be ground. So I can just type in G and ground. Zone name. I like giving my zones names cuz they're easier then to find. So I'm just going to call it layer two ground. My second layer or my bottom layer ground. You can change various parameters here such as the solids or hatch fill if you want to remove islands and that's pretty much **[1:17:28](https://youtu.be/igQWdVGZGpI?t=4648)** always the case as well as electrical clearance. Now this is a very very generic electrical clearance. This is a clearance to anything. This is a clearance to holes. This is a clearance to outline. This is clearance to traces which isn't terribly great because there are different design rules for different copper to feature clearances. A fairly reasonable number is 0.3 mm. That's a kind of catch all case and that's pretty much produced by about any manufacturer. Keep in mind this will also be the board auto polygon pore clearance. So let's increase that a bit to 04. Minimum width that's the minimum copper feet width **[1:18:01](https://youtu.be/igQWdVGZGpI?t=4681)** which also should relate to your trace width minimum. And for PCBs that's for two-layer PCBs you can go down to something like 2 or even 0.15. Pad connections for a large solid ground plane or any polygon pore we have to worry about thermal imbalances. one for small components and also two that for instance if you solder a through hole pin to a large copper mass it's going to take a very very long time you have to heat up the board and that's why we might want thermal relieves pad connections and that's what you can define here size of them IPC has some various standards and suggestions of how **[1:18:33](https://youtu.be/igQWdVGZGpI?t=4713)** to do that but typical values might be 3.3 for the relief gap and the and the spoke width and these are just fairly generic numbers for now corner smoothing I would like to implement as a as a fillet and now I can click Okay. And we can start actually drawing the outline. So, we clicked on the bottom left. I'm going up and I'm just going to follow this outline. And you can see this polygon shaded area start to appear. Click on the initial starting point. And that closes the polygon. Escape to cancel. And now nothing's really poured. I can press B on my keyboard and that repor the polygon on the bottom layer. **[1:19:07](https://youtu.be/igQWdVGZGpI?t=4747)** If I go to the right hand side, right click and hide all layers and then just enable the bottom copper layer, we can see we have a large holog that fits the outline with a certain clearances we specified. And we see we have thermal relieves on, for instance, the USB mounting hole, the shield connections, which is what we specified. But also, we have thermal relieves on our mounting holes. And we're not really going to solder anything to the mounting holes. These are mounting holes for screws. So that's why that doesn't really make sense to have thermal relieves on these. But that's the default property of these footprints. So I can hover over one of these, press E, and then go to the connections tab on the pad properties. **[1:19:40](https://youtu.be/igQWdVGZGpI?t=4780)** And here we can see connection to copper zones. And currently the pad connection is from parent footprint. And we don't want that. The key to put footprint has thermal reliefs. We want this to be solid. Click okay. Press B again to repour. And now we have a solid connection to our mounting holes, which makes sense. And we want to do that for the remaining three as well. And that's exactly what we've done. And here we go. We've got a polygon pole on the bottom layer. And that's going to be our predominant ground connection. So anytime we want to connect ground, we go to the top layer, route out a bit, drop a via, so Zaxis connection, and that then links up to the bottom layer to our **[1:20:14](https://youtu.be/igQWdVGZGpI?t=4814)** ground plane. In 3D view, we can see on the top layer, we don't have anything other than components. But on the bottom layer, now we now have this polygon pore with the relevant clearances to all of the features because of this rather generic electrical clearance rule. with our polygon paw on the bottom layer in place which is connected to the ground net or assigned to the ground net. What we can do and what I typically do generally and this is not just for ground nets. This is for power or anywhere where I might think I I might need a via is I do my via pre-placement. If you just start routting right away laying down tracks and whatnot you'll **[1:20:47](https://youtu.be/igQWdVGZGpI?t=4847)** very quickly see once you need to start adding vas later that there going to be loads of issues. You're going to have to rearrange tracks, rearrange components, rearrange VAS. So that's why as far as I can, I also try to pre-plan my VA before I lay any traces out. A rule of thumb is that if we have for instance a ground plane as we do here on the second layer, that for every ground pad we see here, we want at least one via very close to that pad, not in the pad, but adjacent to the pad that goes to ground. Later on we will then link that up either with another polygon paw on the top layer or **[1:21:20](https://youtu.be/igQWdVGZGpI?t=4880)** with wide short traces that we have nice low inductance low impedance ground connections. The way I can place a via is either go to the right hand side click on that little place icon or press control shift X on my keyboard. You also have to of course choose your correct via size and I'll just choose our standard or our predefined 7.3 mm via. Then click on the V tool and you can see our V is now free to move. I want to change my grid. It's a bit large at the moment. So I'm going to press N and move down to 0.25 mm. So for instance for C12 I definitely do not want to place the VN **[1:21:55](https://youtu.be/igQWdVGZGpI?t=4915)** pad. There are very good reasons for doing so, but typically that requires a different PCB process manufacturing process or rather an additional PCB manufacturing process which you should avoid for most boards unless you have very good reason to do so. So the ground via I like to place just outside the copper pads area. For instance, here would be a good spot or even just below. Remember our ground of pin 7 is down there. So I kind of want to have my ground connections facing the shortest loop area. So in this case I would probably place my ground V like so. It's not connected yet but it's just in a way **[1:22:28](https://youtu.be/igQWdVGZGpI?t=4948)** a symbolic representation that we need to connect this and I'm pre-placing my VA. Same for the ground here. I'm just going to place it slightly outside of the pad like so. And I'm going to repeat that process with a minimum of one ground via per ground pad. Ground v in parallel assuming the correct connections can reduce the impedance. So that's why often times it can pay off to actually have multiple ground v around the pad. for instance, like so. But as a bare minimum, I'd suggest just doing one grand via per pad just to start off with. And if you have space later on, add more in. Now, of course, **[1:23:00](https://youtu.be/igQWdVGZGpI?t=4980)** [clears throat] for higher power designs, higher current designs, you will have to use multiple VA. If you need to transition through layers or if you need a low inductance, low low impedance ground connection, then of course you will have to use parallel VA. But for a simple board like this, a simple design, go with a rule of thumb, one ground via per pad. Place close to the pad, but not in the pad. So, let me just add the remaining vas. And I hope you do the same on your end. And here I've now placed at least one via per pad fairly roughly. You might have to move these around as we get through to routing, of course. But again, just slightly outside the pad for the most **[1:23:33](https://youtu.be/igQWdVGZGpI?t=5013)** part. Sometimes I've just, you know, gone a bit crazy and added a few more just around. And we'll come to stitching v later on when we do a top polygon paw. But for instance, for example, for power components, I typically add even more than one via again just to reduce the overall inductance of that connection. The VA is in place, they actually can strain how we route out as well. This will block off some areas which we can't go through. We have to go past. So that's why I pre-place my VA. If you had for example a four layer board or power on a different layer, for example, 3.3 volts, you would do the same process **[1:24:06](https://youtu.be/igQWdVGZGpI?t=5046)** also for the 3.3 volt VA and nets. And this could also be for signals. If you know you have to do a jump somewhere, I might pre-place some VAS before I do my routting. You might even have to root out tiny bits of section to see how the signals might flow just to get a feel for where you might need the VA. But in any case, this seems kind of all right for the most part. One VR I might not be too happy with is I placed one V directly under this tiny accelerometer part. And not my preferred method, but I've done this a couple times with okay results. Ideally, you don't want to really have VAS underneath these small **[1:24:39](https://youtu.be/igQWdVGZGpI?t=5079)** components. But here, it's just so I know lucrative in a way because then we can just route all the ground pads directly into that central via. We could of course also scatter ground v around here for all these pads. Again, only really pin 9 is a is a proper in quotes ground connection. So, we'll see about that V if we needed later on. I'm just placing it there just to prove planet. Some components for instance sensitive magnetometers or certain components I think uh certain accelerometers as well actually explicitly tell you the data sheet to not put any copper underneath or at least on the same layer underneath **[1:25:13](https://youtu.be/igQWdVGZGpI?t=5113)** these components. For this particular data sheet I didn't see that. So that's why I just put a via here in case with all these vis. We're not going to hook them up yet. I typically do my ground and power connections right at the end. Again as it did with the layout process my routing process is also in order of criticality. So I might do the short connections for my decoupling and bypass capacitors. I might do my crystal oscillators first and then I might do USB and so on. And only at the end I will then hook up all these ground connections and also the overall power routting across the board. And that's a method that's worked fairly well for me. **[1:25:45](https://youtu.be/igQWdVGZGpI?t=5145)** Again, order of criticality I think is important to keep in mind. So with that being said, let's actually start with rooting out. And the first thing I like to do as we just talked about is do these bypass decoupling capacitor connections. And for this ideally you want the shortest lowest impedance that is widest shortest lowest impedance connection you can between the power pins of these of the capacitor and the relevant device that needs to be decoupled or bypassed. I can choose my track width at the top left with this drop down and this is where we can find our predefined sizes. So for instance 0.3 mm and then I can hover over a pad **[1:26:20](https://youtu.be/igQWdVGZGpI?t=5180)** and press X to start routting. And you can see why I chose 0.3 millimeters because this is exactly the width of one of these MCU pads. So I could simply start on this pad, go into this capacitor and call it done. What I prefer doing, however, is necking down rather increasing the width as soon as I can to meet the capacitor pad width itself. And that way I increase my trace width or the or just slightly. But that gives me a slightly low impedance, slightly low inductance connection. So for instance, I could cycle through my track widths. So for some reason, keycat **[1:26:53](https://youtu.be/igQWdVGZGpI?t=5213)** is being a pain in the neck. For example, if I do a trace width starting at 0.3 mm, route out a tiny bit, then press W to increase the trace width and try and place that. That is I'm necking down or necking in and up to that capacitor pad. So increasing my width, then key card for some reason will make the entire trace that last width. Whereas if I route up here, then press W to increase my trace width. Everything seems fine. So, you see what I'm trying to do? The way I'm going to get around this for now is change my trace width back to 0.3 mm mters. Root out a tiny bit. I'm going to copy that segment, **[1:27:25](https://youtu.be/igQWdVGZGpI?t=5245)** rotate it, place it, change that segment to 0.5 or 0.6. And this is now how I'm going to do it for now. And I'm just going to trim that end. And you see what I'm trying to do. Maybe there's someone who knows why this is happening. Keycad only in certain areas. It's incredibly irritating. it. Anyway, just to illustrate the point, as I come into or out of the pad, I want to maximize the width as far as is reasonable to a wider trace width to meet in essence the capacitor pad width. Later on, we will also be adding teardrops, which helps with this this kind of necking down. But **[1:27:57](https://youtu.be/igQWdVGZGpI?t=5277)** for now, this is what I kind of want to achieve. Now, for these short distances of this particular board, it doesn't matter terribly much if we do this. For instance, I could just route out a 0.3 mm trace width, go directly into the pads of VREF. If you want to make it slightly nicer, again, we'll add teardrops later on. Or we can do this kind of adjusting track width idea that I just showed you. Similarly, for the 3 and 3 volt net, I want to do something similar. So, ideally, I want to come out here. Really, I want to increase my trace width. Now, keycode won't let me for some reason. This is the kind of shape I would want to do. So, as soon as I come out of the pad, I want to widen **[1:28:30](https://youtu.be/igQWdVGZGpI?t=5310)** the track. So, I'll see if I can do this. So, after some manual readjustment and dragging, this is what I came up with just again to illustrate the point. this kind of structure. We also need to keep this widing away a bit from pin 7 because we also want to have this connection, this ground connection which we'll be doing later on with a polygon pore on the top layer. We want to make sure that the polygon pore can connect pin 2 and pin 7. Yes, we do have v left and right of these pads but ideally we want a solid straight connection here as well. Now whether we've rooted out at least the critical bypass decoupling capacitors, we want to do that across **[1:29:05](https://youtu.be/igQWdVGZGpI?t=5345)** the entire board as well. So ideally short wide connections increasing in trace width as you can. So I'd strongly suggest now following this along for all the bypassing decoupling capacitors doing that on your end as well. I've added some more of these bypass decoupling capacitor connections for the USB to odd converter. And here I've actually decided to move C7 and C6 not centrally but to the right because we also have the USB D minus D plus lines that look like they need to be flipped and I'd like to avoid using VAS. So one way we can do that is simply route around underneath the component and into the pads from the back side and the C7 **[1:29:38](https://youtu.be/igQWdVGZGpI?t=5378)** was in the way and just to make it symmetrical I move C6 to the right hand side as well. And I'm doing exactly the same tactic if I need to come out left and right for example pin 7 I'm starting with a narrow track and then widening out widening out coming in to the decoupling capacitor here at the top. I've simply choose a wide trace and I've just adjusted the trace length to meet the end of the pad here pad 10 like so. So this is a nice short wide connection. I did have to adjust my track size here. I actually had to start out with a 0.25 mm track based on our design rules. Otherwise, Keycad wouldn't let me root this out. So, I added some more **[1:30:10](https://youtu.be/igQWdVGZGpI?t=5410)** predefined sizes such as 0.15 and 0.25 in the predefined sizes for the IMU at the bottom. These pads are very very close together. If I try and route out, if I press X above the pad, you can see here tells me the routting starting point violates DRC. Now, you could go back to the board setup in the top left hand side. go to constraints and check the constraints and these constraints actually seem in order. What the actual issue is is if we go to net classes and scroll down the default clearance track with via size and so on those are **[1:30:42](https://youtu.be/igQWdVGZGpI?t=5442)** somewhat different at least the clearance is different to our design rule. So actually we need to match the clearance to the constraints or we actually need to fill in this information for example for the power nets and so on. But for now I'm going to do it very quickly just change the clearance to.152. Click okay. And this now lets us root out of that pad and we don't get that DRC error anymore. We do have to use a fairly small track width. So if I use 0.25, you can see I can't route out. So that's why I also added it to 0.15. Again, pin 8 is our main power pin. So that's what we want to root out. And we do the same procedures before. Short **[1:31:15](https://youtu.be/igQWdVGZGpI?t=5475)** segments widen out as soon as we can. And I believe the issue was why Keycad wasn't letting me actually increase the trace width. If I just go straight into the pad, it suddenly snaps and makes all traces the same. uh width of that segment. If I stop just before, you can see it actually doesn't do that. So, for some reason, only when snapping to a pad, it'll be annoying and uh try and make all the traces the same width. So, not the prettiest, but a structure like this might be okay. It's the general principle of widing out. Once again, having done these somewhat critical power decoupling caps first, we of course want to do the next critical **[1:31:47](https://youtu.be/igQWdVGZGpI?t=5507)** segments. And for instance, for the microcontroller, we talked about previously that we have this trimming resistor, which is fairly important, and of course, our crystal oscillator. We can do the trimming resistor first. And typically I will stick to one unless I have unless I have specific requirements. I for PCB design will try to just stick with one trace width for my signals. If it's controlled impedance then of course I'll adjust that. But typically to make something fairly manufacturable that fits most pad sizes unless you need to go very small. At 0.3 mm track is pretty good. So I selected 0.3 mm. I'm going to start on pad 8. Go out. I've changed my grid to 0.25 mm. **[1:32:22](https://youtu.be/igQWdVGZGpI?t=5542)** keeping clearance away from all of the pads and components and going into the pad like so. You see, I was very deliberate of how I did my pad entries. Keycad tried to suggest different pad entries, but I would strongly suggest entering your pads at 90° angles rather than doing something like this. You don't want these kind of sharp angles because in manufacturing, many people say they aren't an issue, but I've spoken to several manufacturers that acid traps are still an issue. So, overetching of certain areas by having these rather sharp angles. So that's why I try to avoid that by having nice clean pad entries and exits like so with these **[1:32:56](https://youtu.be/igQWdVGZGpI?t=5576)** 90° angles. We'll add teardrops later which also smooths out these sharp 90° angles. But for this this this could be an okay starting point. We also have to route out pin 11 and pin 12. Now pin 12 we can break out quite easily. Pin 11 looks like we're going to get into problems with this iros trace. So what I can do I can select one of the segments and hold my mouse button and press shift sometimes also helps. And then drag this trace up a bit. Now I've got the right angle here and I can just fine-tune manually my traces like so. I still have a somewhat okayish pad entry, but now I've given myself space to route out pin **[1:33:30](https://youtu.be/igQWdVGZGpI?t=5610)** 11. So I've made a short ROS connection. Now I can do HFX in. I come [clears throat] out of the pad. Try to stay away from other components. Click to set certain points. Go around into the capacitor and then straight into the crystal. And I do something similar for pad 12. HFX out again. Forward slash to change the routing direction into the capacitor first, then into the crystal. Again, I can drag the traces manually afterwards. I can also hold shift to change the grid a tiny bit. Just making sure I'm staying away from any digital **[1:34:03](https://youtu.be/igQWdVGZGpI?t=5643)** signals. The crystal oscillator is a fairly sensitive circuit, so you don't want to route it and hug it next to, for example, USB or UA or something. So, just an additional starting point, this might be okay for this fairly sensitive area. What you can also do and in certain cases this can help is do a bit of via stitching in terms of guard traces. So I can place a couple of vas around this fairly sensitive section. This can help as long as the stitching is close enough. So the via spacing is close enough for the aggressor signals. So you could add that in place. The issue is we'll have to be rooting the **[1:34:35](https://youtu.be/igQWdVGZGpI?t=5675)** RTS CTS signals next to the crystal anyway. So here we can't really add these VAS for the most part. So that's why I'm just going to add them vaguely around this area. And I do do this ahead of time because then I know I can't get close with my RTSC signals close to this signal. So for me, this is also visual indication of okay, stay a bit further away from this crystal because I've already put this kind of guardish fence up. Now, is this needed? Probably not. But I think it's a nice addition to this and also just a visual addition for yourself to say, okay, stay away from this crystal. You can remove these VAS later on. Not a necessity. But in any **[1:35:08](https://youtu.be/igQWdVGZGpI?t=5708)** case, now we've rooted out the essentially sensitive components around the microcontroller. We still have this VEF connection up here. For this, I'm going to go with a 75 trace width. Just make this nice and wide because essentially this is a ground connection. So, we want to reduce the inductance. So, for these power connections, decoupling connections, we want to have as wide as is reasonable. But that's pretty much it for the microcontroller. Again, ground connections we'll be doing later on. We now can go to the actual signal connections. for example, our debug connections or our UARD connections and so on and fan those out and route those out to the relevant **[1:35:40](https://youtu.be/igQWdVGZGpI?t=5740)** peripherals. What springs out immediately is we can just go on the right hand side. So we can do the serial wire clock serio and for that I'm just going to insert my 0.3 m trace width to start with clock. We can start on the pad. Press X go out and as soon as I'm out of the pad I don't want to go straight to the right because my serial wire debug connection will be below it as well. I want to come out of the pad and then immediately give myself space. So come out, go up to the top, past here, and then I need to fit through. And because this is a 0.3 mm trace and as I try to come through here, you can **[1:36:14](https://youtu.be/igQWdVGZGpI?t=5774)** see key cut is not letting me of course because of the design rules. And this is exactly why you set up design rules before you start any routting. Cuz if we didn't, we would have basically unmanufactured board. But this is no issue because we can simply place a track as far as we'll go. Click. And then I'm going to change my my routing width to something a bit smaller to get through that gap. Escape that gap and then change back to my larger width by pressing W. So something like this might be in order. We come out of the pad with our standard trace width 0.3 mm. As we have to only we neck down in the areas where we need to. Once we've escaped **[1:36:47](https://youtu.be/igQWdVGZGpI?t=5807)** those neck down areas, we try to increase our trace width again because this just improves manufacturability. We will then do the same thing for serial DIO. So, we'll go back to 0.3 mm trace width. Press X on the pad. We don't want to hug the serial clock pad, but we can already escape a tiny bit below because we're aiming for pad 2 of the tag connect header. We go in, we neck down a bit by pressing shift W, go through, and then we neck up again and go back to 0.3 mm. For example, something like this. Not maybe the entirely the prettiest, but of course, you can fine-tune this a bit later. For **[1:37:19](https://youtu.be/igQWdVGZGpI?t=5839)** example, we can just use Keycad's drag mode. I'm just clicking and dragging with my left mouse button to just move the tracks and make them a tiny bit nicer. But of course, you can fine-tune as much as you want. But that's the general idea. We also have the end reset signal. And this end reset signal looks like it just needs to travel underneath the mic controller. And that's typically pretty fine, pretty okay to do that. If you have other options, if you go around, then that's probably better as well. But if we went around, we have a pretty long path to get there. So for us now, we're just going to go under the mic controller. There's no other signal, at least for now. Of course, we still have to come to power routting later on. **[1:37:52](https://youtu.be/igQWdVGZGpI?t=5872)** That has to go underneath. So now we can just route the end reset signal again with a 0.3 mm trace width. We just go between those pads. We escape. I could go straight into pad two here, but that for me is a bit close hugging pad 25. So that's why I'm just going to go out a bit, up a bit into pad two, into pad one of the capacitor, and then out of the capacitor again these 90° sections. And then we do the usual necking down procedure as before. For instance, something like this might be okay. Not the prettiest again, but this is just a simple demonstration. We have the I squed C connections and we **[1:38:27](https://youtu.be/igQWdVGZGpI?t=5907)** have then the UR. So why don't we do the I squed C connections first and as well as the interrupt connections because then we can start moving, you know, from right to the left hand side and finishing up with USB and then doing the power. So it's the same procedure as before. Again, because we've done a fairly good job at laying out this board, the routing is fairly straightforward. It's just connecting dots, connecting colorful lines, and so on. So, I'm going to do the I squed C lines first. I'll come out with I squed C at 0.3. Go into the pull-up resist. I'm going to do the same for I squed C SC. Now, we could of course drag the track up a bit. That gives us a tiny bit **[1:38:59](https://youtu.be/igQWdVGZGpI?t=5939)** more clearance away from the SDA line that they don't run in parallel for too long. Will it make a difference in this case? No. But it's generally good practice. I can't pull the SDA line up too high because remember we have the UARD CTS line there and the RTS line as well. So that's why I'm deliberately keeping the dent in this line, keeping this 45° segment in this line a bit further down so I have space to escape with RTS and CTS out of the pull-up resistors. Then we need to go into the accelerometer pads. I can already see this V is going to be a bit too close. So let me just move this out of the way for now. I'm going to move this V a bit **[1:39:32](https://youtu.be/igQWdVGZGpI?t=5972)** to the right to give myself a bit of breathing room for SCL. Let me just move it down a tiny bit. We can fix all this later. X to root. Come out. And you can see we're going to have to neck down again as usual. Now Keycad is actually letting me go in. So I guess this could be okay because we're not overextending the pad. I'm just going to drag this move this segment from the track away from the V a bit more. And then we can do something similar. Then we do something similar for SDA. Come out. Give myself a tiny bit of space. But here we'll have to neck down. You see keycat is not letting me go into the pad straight away. So again this is just a quick effort. Something like this might **[1:40:06](https://youtu.be/igQWdVGZGpI?t=6006)** be as an okay starting point. You can still fine-tune quite a bit later. Now we have the interrupt connections as well. So I'm just going to you can either start from the IMU or from the MCU. I'm just going to start from the MCU route out giving myself a bit of clearance. Coming past giving myself clearance from the 3.3 W connections like so. And then of course we have to neck into this again. And for the in two pin we also do the same thing. I don't want to hug the traces like so. I don't want to do something like this. Just using the absolute minimum clearance. I do want to give myself some clearance. Again will it make a difference in this case? Probably not. But cross talk can **[1:40:39](https://youtu.be/igQWdVGZGpI?t=6039)** and is a real issue in PCB design. So that's why the the number one thing you can do to minimize cross talk is actually increase spacing. So that's exactly what we're trying to do here. And then we have to neck down into that pad again. For instance, something like this. Now I also want to move my int 2 trace up a bit this horizontal segment because you can see the ground plane underneath. It's pretty close to the edge for my liking. So, you don't want your traces to be close to the edge of the reference planes because then you get kind of field spread extending beyond the board. That isn't great for EMI. So, I'm going to move it a tiny bit up. Now, there's not terribly much we **[1:41:12](https://youtu.be/igQWdVGZGpI?t=6072)** can do. Of course, we could move all of these components up a bit more or move this whole segment up a bit more, but for now, this is okay. We will have to find a way to jumper the 3.3 volt nets later on, but just as a simple example of what you could do to fan out and route out this I squed C connection. They're not terribly critical sections, but we because of the way we've laid this out, we can keep these connections fairly short, fairly simple. We don't really have any crossings we have to do with VAS, at least for the moment. So, we've pretty much done all of the MCU part. All that is left signal-wise are the UA connections. And hopefully, we've **[1:41:45](https://youtu.be/igQWdVGZGpI?t=6105)** done a fairly okay job again for layout. Because here, URX, U RX, we can simply route out with a 0.3 mm trace width. I'm going to go up a bit. I'm actually going to give myself a bit of space away from the 3.3 volt pad because I'm probably going to want to place a V here because I can't really get to this capacitor any other means. I could go under the MCU, but we'll see later how to properly route power. And we we want to go through the decoupling capacitor first before we go into the MCU pad. So, I'm going to route this way. I'm This is just indicative that I need to properly put a via here. UX I'm going to do as well. And I'm not going to hug the **[1:42:17](https://youtu.be/igQWdVGZGpI?t=6137)** traces again. I'm going to come out and try and break away quickly. give myself some space and route into the TX pad. And again, I can always make adjustments later simply by dragging. Make sure to keep fairly nice pad entries like so. Give yourself spacing between the various traces as well. So, you know, something like this seems to be fairly in order. A possible option for the 3.3 actually might be through this capacitor, through the pad, then into this capacitor for the MCU. But that's just thinking ahead a tiny bit. Okay, so now we have CTS RTS. Let's see how we **[1:42:51](https://youtu.be/igQWdVGZGpI?t=6171)** need to connect them. And it seems actually fairly straightforward. I don't think we actually have to do any crossing. We just come RTS out here below the crystal up into RTS and CTS. We can come out the left side and then go under the RTS trace. So that's exactly what we're going to do. Let me just drag this SDA trace down a bit. Press X 0.3 m trace width. Come out past these pull-up resistors. Give myself ample space away from the crystal oscillator. And I'm going to come into let me just move this grand via a tiny bit. We we'll probably move this around a bit more afterwards as well. It's just I didn't have really space to move the CTS signal in properly. Now for the RT **[1:43:26](https://youtu.be/igQWdVGZGpI?t=6206)** signal, very similar. Come out, give myself space immediately when I come out of the pad. I don't want them hugging. Now I can either move it close to the crystal or the crystal capacitor here or I can move it closer and kind of hugging the UR connection. In this case, what do you do? You can place it centrally and that's kind of the I don't know worst of both worlds. I prioritize that I want to stay away from the crystal. That's why I'm going to move the trace closer to the CTS line until I can break away and have ample space from the crystal. That's a exactly the reason I place this via fence for lack of a better word around the crystal to tell myself, okay, **[1:44:00](https://youtu.be/igQWdVGZGpI?t=6240)** I can't go close to the crystal here. I'm going to go around and I'm going to have a nice pad entry like so. I could also come into the pad like this. I prefer having this kind of horizontal entry like so. For RF designs, that can sometimes make a difference how you enter the pad, but for us, it doesn't really matter terribly much. I do want to give myself a tiny bit more spacing because we have fairly long parallel runs. Again, will it matter? Probably not, but it's a matter of doing and following good practices. Again, staying away from the crystal and just adjusting and correcting a tiny bit. For instance, something like this. I'm giving my space **[1:44:33](https://youtu.be/igQWdVGZGpI?t=6273)** when I can have space. I'm trying to stay away from the crystal, but I'm also trying to minimize or reduce the length of trace I have generally because you want to reduce the length of traces. It reduces the chance of this becoming an unintentional radiator, also known as an or an antenna. And the way we can do that is by keeping our trace length as short as is reasonable for this board design. But this seems fairly good. The nice thing is we still on the bottom layer have an unbroken for the most part solid ground plane. We try and only route on the top layer and only do small jumps. So we might have to do some small jumps on the bottom layer later on. **[1:45:05](https://youtu.be/igQWdVGZGpI?t=6305)** We've connected up most of the MCU connections, of course, not power and ground, but now we can move more to the left hand side and finish off essentially with the USB signals before we move over to the power routting. And then we're really pretty much done and ready to check the board of course and then produce manufacturing files for ordering. And I'll show you of course how to do that as well. But for now, we've so far just considered single-ended signals. So for example, URX, RX, and so on. But now we're moving over to rooting a differential pair. Now there's not terribly much to this other than using a different rooting command. So far we've been pressing X to root. If **[1:45:39](https://youtu.be/igQWdVGZGpI?t=6339)** I press X here, I can route each of these parts individually. But we specifically told Keycad or rather implicitly that with these minus and plus symbols that these same net names form a differential pair. And the way you do that is actually going to root and then root differential pair. Or we can press six on our keyboard. And if we press six and hover over either one, either over minus or plus, you can see keycad now because we've named this appropriately starts routting out a differential pair. And we can see the track width at the bottom and also the differential pair gap is at the bottom because it's assuming the default **[1:46:11](https://youtu.be/igQWdVGZGpI?t=6371)** differential pair net class. So I press escape to cancel. Go back to the board setup. We can see that actually for the default net class, we can see there's a differential pair width, DP width, and DP gap defined here. Now, because we've already defined our USB net classes, we could also define that we want a differential pair width and differential pair gap. Now, typically for USB, you want controlled impedance. However, for short segments, and especially in this case, we're only running USB full speed, which is up to or even slower than SPI, we will not worry about controlled **[1:46:44](https://youtu.be/igQWdVGZGpI?t=6404)** impedance. We're just going to take a somewhat standard track width and track spacing, something that works for these short segments that enables us to route in and out of these rather small pads here. So, we could just route with a default differential pair net class. But the trace width is a tiny bit small for my liking. So, I'm just going to change that to 0.25 rather than.3. The reason being we need to get in and out of these rather narrow pads given our design rule constraints. So, I've just slightly relaxed the constraints here. I can hover over either one of these differential pair parts. Press six. And **[1:47:17](https://youtu.be/igQWdVGZGpI?t=6437)** you can see now because we're using the default net class, we're not doing any controlled impedance or different differential pair parameters. I've simply updated the track width to be 0.25 and the differential pair gap to be 0.25. And I can start routting except now I have a diff differential pair rather than a single ended signal. But there's nothing really to be worried about. You can see here I'm having a bit difficulty getting past the ground via. So I'm going to press escape and I'm just going to move this via up and out of the way. and press six again on the end of these tracks to continue. I'm going to move away this ground via for now as well. We'll rearrange this a tiny **[1:47:50](https://youtu.be/igQWdVGZGpI?t=6470)** bit later on. And I want to route out of this pair. And you can see I'm rooting underneath the component because we need to do this little flip in D minus D plus. And this is one way we can achieve that. So once you've rooted out the tracks, it could look something like this. We have really short connections. We've used fairly generic differential pair parameters. It really doesn't matter in this case as long as you can do the routting. And we've kept clear of other signals. We've kept clear of the VA. Given ourselves ample bit of space and we've avoided using any V, any crossings on the left hand side, this D1 diode, these sets of diodes within this **[1:48:24](https://youtu.be/igQWdVGZGpI?t=6504)** D1 component actually they have connections internally between pin one and pin six and pin three and pin four. That's why we don't actually have to route underneath and through this component. We can simply come out of simply speaking pins one and three and go into the USBC connector. The USBC connector itself again has two sets of differential pairs, two sets of differential pair pins because again we have this 180° shift in in plugging in the cable. These two options again this is USB full speed. It's really not critical. I'm just going to click on pin one and I'm going to go into the top set of pins B7 and A6. And unfortunately you **[1:48:59](https://youtu.be/igQWdVGZGpI?t=6539)** might end up with something like this. It's not the prettiest. It's not terribly differential but again we've kept these trace length these distances so short. This is USB 2.0 full speed that this really really does not matter for this particular scenario of this development board. This will work completely fine. We don't have to do any delay matching between the D minus and D plus pairs. We've kept our trace length short. This is a very slow interface. This is a comparatively slow interface. So you can avoid this differentialness of it. You can if you want of course try and make it prettier on your end. But for now this will absolutely do. What I **[1:49:32](https://youtu.be/igQWdVGZGpI?t=6572)** can then do rather than rooting a single-ended pair because we have to connect D minus and D plus. A simple trick is to route them single-ended. So I'm going to change to 0.25 to match my differential pair width. But I'm going to route a single-ended signal. So I'm going to hover over B6 and press X. And I'm just going to meet this A6 connection like so. And I'm going to do the same thing for A7. I'm going to come out the back side like so. And this is how I then connect my D minus D plus differential pair pins like so. It's okay. Not terribly pretty, but it's very convenient, very simple for what we actually need this to do. And this **[1:50:06](https://youtu.be/igQWdVGZGpI?t=6606)** actually even works also for USB highspeed as well, as long as you keep these stubs, these segments comparatively short. We only have two of the USB pins left before we can move over to power, and that's CC1 and CC2. For this, I'm going to go back to 0.3 mm track width. These are again single-ended signals. And keep in mind, we talked about this previously, but we're going to actually route underneath the USB connector. In this case, this is okay for reasons we talked about earlier. Come out and into this resistor. We're going to adjust the traces in just a second. I'm going to do the same thing on the bottom side. Like **[1:50:38](https://youtu.be/igQWdVGZGpI?t=6638)** so. I don't really like how close we are to the mounting hole. Again, we have some clearance because this is a fairly wide pad, but I'm just going to drag this a bit. Give myself a tiny bit of space that we're not too close with these traces from the mounting hole. Something like this seems okay. I guess this looks fairly symmetrical. But here we go. We've rooted out pretty much all of the signals. Now what is left is simply just to do the power connections as well as the ground connections. Then we can clean up the board a tiny bit. We'll add some silk screen. We'll add some text, maybe revision ID and so on. And then we can get this ready for **[1:51:10](https://youtu.be/igQWdVGZGpI?t=6670)** manufacturing. After having completed essentially all of the signal routting, let's move now over to routting the power. And we'll first do the more straightforward route and we'll add in V jumps as we need to going on the bottom layer with small cuts as is appropriate. And we'll just follow the path of power flow simply speaking. Essentially we have our host connected via the USBC connector which provides the power. We go through our Pi filter into our LDO regulator and its appropriate capacitors input and output which forms our 3.3 volt net. And that then needs to **[1:51:43](https://youtu.be/igQWdVGZGpI?t=6703)** distribute through essentially the right half of this board. For power routting for these types of boards, having wide traces is pretty much sufficient. We don't have particularly fast switching frequencies in this design. We don't have particularly high current draws in this design. So fairly beefy trace widths are sufficient. You could of course also do this with a polygon pore, but we will be doing this with trace widths. And I do do this in a lot of designs unless they're very high speed, very high current designs. So somewhere this is completely fine. We will start off with pin A4 of our USB connector. We of course have pin A9 as well, which we'll take care of just a bit later. We **[1:52:15](https://youtu.be/igQWdVGZGpI?t=6735)** could go out with the 0.5 trace width. Typically for power routing, I like to make the traces as wide as the pads themselves. So the B9 pad happens to be 0.6 mm. And these 0603 pads have a width of 0.8 and a height of 0.95. So we could go with a 0.8 mm wide pad and always neck down to whatever pad widths we need. So let's add some more predefined track widths. So we come out of B9. I'm using 0.6 mm track width. I'm going to go to the capacitor first of this PI filter. Then through my series element out of my series element into the second part, second capacitor of this PI **[1:52:49](https://youtu.be/igQWdVGZGpI?t=6769)** filter. From this PI filter, I come out. I'm just going to go with a 0.6 mm trace width. This is sufficient. We could also go with 0.8 to match the width of the pad. But from that, then we go straight into our input capacitor. So not into pin one of U1 first. We want to go through the input capacitor first. So input capacitor first. C3. And from the input capacitor, we then neck down a tiny bit to go into pad one of our regulator. And pad one actually happens to be 0.6 as well. And remember, pad 3 is actually our enable signal. We'll take care of that in just a second. So we can go back to 0.3 mm trace width and **[1:53:23](https://youtu.be/igQWdVGZGpI?t=6803)** try and squeeze past into our power net here. Just cleaning up the connection tiny bit. Remember pin 3, it's enable pin. It's high impedance. This trace doesn't need to carry any power or any current. And that's why we give this a smaller trace width. And we're just about to squeeze it past these two grand pads like so. We could of course move the capacitor left a tiny bit, give ourselves a tiny bit more clearance, but this seems okay for now. Before we do our 3.3 volt net, we'll just quickly do this pad 4. And this is just a bypass pin to reduce the noise by attaching external capacitor C4 in this case to that pin. And for this again, we can **[1:53:57](https://youtu.be/igQWdVGZGpI?t=6837)** just use a 0.6 mm trace width. This is going to be nice and short like so. That's really all we have to do. We could also make the entry maybe a tiny bit cleaner like so, but that's okay. Then the output of our LDO, that's pin five, then feeds into the output capacitor C5. From C5, now we have to distribute all across the board our 3.3 volt net. So there's many ways of doing this. We can try and move components around a bit more to make it easier, but the general idea for rooted power for these types of board is you want to come from your power trace for instance like **[1:54:29](https://youtu.be/igQWdVGZGpI?t=6869)** so. We we have our power trace which is a fairly wide trace. We route our trace. We go through a capacitor first and then through the capacitor into the relevant power pad. We don't want to go from our trace into the pad and then into the capacitor. That's a slightly unoptimized filtering element. We want to use the inductance and resistance of the trace in combination with the essentially shunt capacitor to form a filter that then feeds our reent power pin. Otherwise, we have worse decoupling. And that's the strategy we're going to use for the rest of these components as well. So we need to try and get to all **[1:55:02](https://youtu.be/igQWdVGZGpI?t=6902)** of these power pins. So similar to the strategy where we have trace, capacitor, then input power pad, I'd like you to try on your own, I suggest pausing this video trying finishing the routting of the power yourself and see how our solutions compare. So for instance, a possible way of connecting up the 3.3 volt nets would be like so at least for this rooted power very simple board. We started off coming out of the LDO regulator with a wide trace about 0.6 mm and then rooted in for instance to C7 which was one of the decoupling **[1:55:35](https://youtu.be/igQWdVGZGpI?t=6935)** capacitors for for U2 our USB to UD converter. However, we also of course had to supply the MCU and this MCU 3.3 volt net was a tiny bit hidden. Okay, we could of course come through pin 7. So for instance an a possible option to routting out 3.3 volt power would be like so we started off coming out of the output capacitor of our LDO regulator using a fairly wide trace about 0.6 mm rooting into our first decoupling capacitor into the power pin and this network then distributes out. We're necking out, necking down as we can. **[1:56:08](https://youtu.be/igQWdVGZGpI?t=6968)** Again, going into capacitors first and into the relevant power pins. And every time we can, we'd widen out our traces and follow the same pattern of trace, capacitor, pad all the way through. If I do have to do jumps, and I do have to do a couple of jumps, I could have, of course, also rooted around, maybe made it a tiny bit better rather than rooting through all of these pads. There, of course, many options, but this will work sufficiently fine for this case. But when I do have to do jumps, I try to do as little jumps as I can. So you can see my bottom layer is still predominantly just a ground plane. I do have about four cuts in it, though. And I try to **[1:56:42](https://youtu.be/igQWdVGZGpI?t=7002)** keep those cuts as small as reasonable. The way I do my cuts is, for instance, if I look at this one here, I route with X and I press V on my keyboard to jump to the next layer. And then Keycat already automatically roots on the next layer. I keep my track width, route over, press V again to get to the top layer. And then I can continue rooting on the top layer. So that's how I would do those jumps. The via nets are then automatically assigned to the net you are routing to. And this way we can connect up all of the 3.3 volt nets. I still have to connect these imu nets here. And for that I will just use a narrow trace because these are just **[1:57:15](https://youtu.be/igQWdVGZGpI?t=7035)** essentially logic level signals. Something as simple as that will do for these 3.3 volt nets. Remember the large wide pads and traces are only for actually the power and current consuming nets and pads. But this is one way of doing it. This is completely fine. You could of course pour polygon paw over the top layer and have the polygon pore do this for you. But we will actually be pouring a ground polygon paw the top to actually do all these ground connections. Now you've probably already spotted it, but we still have the VOS connections left. So for example, to the ESD protection, it's the same principle as before wide trace going to the pad. And here I'm doing this kind of 45° **[1:57:48](https://youtu.be/igQWdVGZGpI?t=7068)** entry, which is also fine for the most part. So what we could do for the Vbus pin A9 to A4 is we could of course route out, jump to the bottom layer, jump to the top layer up here, connect together, but that then creates a cut under a somewhat critical USB differential pair. An alternative is we route back and just do a cut under the USB CC1 pin. We do also have a fairly narrow area at the back of the A4 pin because of this mounting pin, but we could do that. That of course destroys the symmetry of this a tiny bit. We could rotate R2 for **[1:58:21](https://youtu.be/igQWdVGZGpI?t=7101)** instance, come out of R2 and just route USBC like so. Move my VA around. And then I that means I can escape B4V bus, drop a V and go to A4V bus for example. Then I don't have to do a cut under the USBC differential pair. That would be an option. Both are fine to be honest. Could look something like this. It's not the prettiest. These are not the prettiest pad escapes either, but again this will work just fine. The key concepts are for this rooted power is fine. Widen your traces when you can. Shortcuts on the bottom layer and try to **[1:58:55](https://youtu.be/igQWdVGZGpI?t=7135)** keep the bottom layer as a solid ground plane as possible. And this is done by thinking a bit more about the layout before you go over to routting. Again, press B to repour all of your polygon pores. And that would then show all these clearance areas on the polygon paw on the bottom side. With that being said, we're nearing completion. All we have to do now is also add a polygon paw on the top layer and that's also assigned to ground. The way we can do that is select the polygon pole and double click on it on the bottom layer and simply check top layer as well. Click okay. Press B to repool. And now we can look at the top layer as well. **[1:59:26](https://youtu.be/igQWdVGZGpI?t=7166)** And we can see we now have a ground polygon pole on the top layer as well. And for us this has made quite a few of the ground connections. But we can see we probably have to move some VAS around because of our clearance constraints. So either we could change our clearance constraints to make our thermal relieves smaller. That's one option. So I could double click on the polygon paw and change the thermal relief gap to let's say 0.25 mm. Press B to repour and that improves at least the connections that the VA are kind of outside of the thermal relief zone. That improves that a bit more. That would be an option. Or **[1:59:59](https://youtu.be/igQWdVGZGpI?t=7199)** I can simply take my VA and just move them out away from the thermal relief zone manually. And that's typically what I would do. So changing my grid now going to a 0.1 mm grid. I want my VA just outside that thumb relief zone. So you can adjust your VA as necessary and make sure they are all within the polygon pore is also what I'd suggest doing and then go around and fixing all of that. Now I've moved my VA outside of the regions of the thermal reliefs, but there are still areas which aren't connected or not optimal. For example, looking at the pin 7 of the MCU, this is **[2:00:34](https://youtu.be/igQWdVGZGpI?t=7234)** actually not connected. the rules we set up for the polygon pause and our design rules are not enough to make this connection. So we could also just do that manually. So we can just do a track X connect that up and we can also connect that up for instance on other side of the capacitor just to complete these connections that are not reachable by the polygon pore for instance. Keep in mind we can adjust our clearances and trace width and so to make this a type optimized but this is the general principle. Sometimes also we have these kind of poorly paused polygon regions, let's call them, where we actually don't **[2:01:07](https://youtu.be/igQWdVGZGpI?t=7267)** have too much of a thermal mass imbalance. For instance, pin one doesn't have a lot of copper connected to it, but pin two doesn't either. And normally we would use thermal reliefs to improve the copper balance and improve the solderability at least for through hole parts. So here we actually might want a a solid connection rather than a thermal relief spow connection. So I can click on the pad, press E, go to connections, and we've seen this before, and change the pad connection to solid. Click okay. Press B to repour. And now I have a solid connection, which for this part here doesn't change the thermal mass differences between pad one and pad 2 **[2:01:40](https://youtu.be/igQWdVGZGpI?t=7300)** considerably. So this is what I'd suggest doing when you don't need those thermal spokes. You can go in individually and change specific pads to solid connections. And I'll just go through and do that. And I'll also connect up the various unconnected pads that haven't been addressed by the polygon pore. That's exactly what I've completed now. But there's still some optimizations we can do. First of all, you can see here, for example, we have this one singular via. And this via is just connected to this tiny tiny little island or this little planelet. So this acts basically just a tiny little antenna, a very high frequency antenna. But this isn't great. We don't really **[2:02:12](https://youtu.be/igQWdVGZGpI?t=7332)** want something like this. So what we could do is either join up this little segment under the MCU or let's just get rid of this via press B again. That gets rid of this island as well. We also have these little necks of polygon paw that kind of just float off. And again, these can create high frequency antennas as well. And for that to get rid of those, I know this is terribly manual, but what I typically do is create a rule area or a copper polygon pore clear out where I just define a little box segment on the top copper layer, for example. So, I'm going to give this a somewhat sensible name. I'm going to select keep out zone fills, click okay, and start drawing **[2:02:47](https://youtu.be/igQWdVGZGpI?t=7367)** just a little box. Close the box. Press escape. Press B. And you can see now we've cut away this bit of essentially an unnecessary segment of ground film. I can take that rule, copy that and then move that wherever I need to. So for example here I could just do it the same thing. Press B and this how I can then chop away. I know a terribly man manual procedure how I can chop away these little unused segments for segments where I have a larger area where I could use some vas. This is where I can then do via stitching. So I can take one of these vas, copy it, paste it, crl +v, **[2:03:22](https://youtu.be/igQWdVGZGpI?t=7402)** and just stitch this whole plane to the bottom polygon pore to make sure this little plane that doesn't resonate at too low frequencies that we fail EMI testing, for instance. We don't want to turn all of these structures into little antennas. And that's what I typically would do all across the board. Now the the spacing between these VAS depends on the maximum frequency content or the bandwidth of frequency content within your PCB design. And you want to then space the VA based on a certain fraction of the wavelength. For example, a 10th wavelength or 20th wavelength. And this **[2:03:56](https://youtu.be/igQWdVGZGpI?t=7436)** is what's known as stitching VA. And it really depends on the design. But for us, we are just going to spread these VA around to make sure we don't have any loose ends simply speaking. So one here, one here. And I'm doing it just by eye, just eyeballing it for now. There are far more scientific methods of doing this, but for a board like this, I just simply like to stitch for example the corners. Make sure I have stitching v all across the board that tie the top and bottom polygon paws together. Not only does this help with EMI, but it also can help because a two-layer board actually has a very comparatively very **[2:04:30](https://youtu.be/igQWdVGZGpI?t=7470)** wide distance between the top and the bottom layer. So often times if we pour a co-planer ground a polygon porn adjacent to our signal and power traces this actually this adjacent ground paw actually could serve as a better reference. Again stitching helps with lowering the inductance. So that's exactly what I'm doing. I'm just stitching around the board. And for example this is then what a stitched board could look like. It's fairly arbitrary in this case. I've eyealled it based on previous experiences. This seems to be fairly reasonable for this board. VAS are essentially free for PCB design. And of course, you shouldn't go **[2:05:02](https://youtu.be/igQWdVGZGpI?t=7502)** overboard and completely make this border to Swiss cheese. Of course, this comes with experience. And of course, you can calculate and simulate exactly what the stitching via placement should be. For other e-cut tools, there are actually stitching tools that you can use that simplifies this process. And I believe there probably are plugins for key cut as well. But with that being said, we are pretty much at the end for the main part of the PCB design process. What we need to do now is clean up. We need to do a design rule check to make sure the way we've rooted this board actually follows our design rules and can be manufactured. We need to add some text, clean up the silk screen, and so **[2:05:35](https://youtu.be/igQWdVGZGpI?t=7535)** on before we can proceed to generating manufacturing files. before we run a design rule check. And it's incredibly important that you do run design rule checks. And typically, it's also a good idea to run design rule checks as you progress through a board, especially if it's a more complicated board because that lets you pick out errors early and solve those errors early before at the end of the board, you might have 200 hundreds of errors there which you have to figure out. But in any case, for a simple board like this, it's fine the way we're doing it where we're just doing a design check right at the end. One optional item which also plays into the designer check is adding teardrops. **[2:06:09](https://youtu.be/igQWdVGZGpI?t=7569)** There's probably a plugin for adding teardrops to multiple pads at the same time. I couldn't see anything in the board editor or anything. You can add teardrops by for instance going to a pad. Let's say this VRF plus pad, pressing E when you selected it and going to the connections tab and clicking add teardrops on pad tracks connection. You can change the various teardrop settings. We're just going to keep the default. And you can see here a teardrop as the name implies it's just necking down of the track or going widening up into the pad. So this is something I quite like doing especially on through hole components. It improves **[2:06:43](https://youtu.be/igQWdVGZGpI?t=7603)** reliability, manufacturability. So I would suggest doing that on at least these kind of boundary interfaces where you're going from a wide pad to a narrower feature such as here. For example, adding a teardrop to this pad doesn't really make terribly much sense, but these kind of boundary interfaces, let's call them, I'd like to add teardrops. So that's an option you can add on if you want to. For the sake of simplicity, we are not going to proceed with teardrops, but keep in mind that that is an option. It's fine to leave the board as is for now. Tear drops are very advantageous in certain situations, however. But for this design, it we don't really need them. What we need to **[2:07:15](https://youtu.be/igQWdVGZGpI?t=7635)** do now is assume we finished the board. At least we can with a naked eye, we can't see any remaining connections. We need to run a design rule check, which will also tell us if there are any connections remaining. The design rule [clears throat] checker is on the top toolbar under design rules checker. If we open that, we want to keep refill all zones before performing DRC checked just in case we haven't report our polygon pors after editing them or after laying new tracks and vas. We want to show both errors and warnings. Then click run DRC and this checks the way we've rooted and laid out our board with the design rule setup we did right at the start of this **[2:07:48](https://youtu.be/igQWdVGZGpI?t=7668)** video. So click run DRC and don't be shocked there are a lot of errors and warnings. certain errors here. We can see there's a clearance violation between netclass default clearance 0.152 and actuals 1.52. And if we click on these various design rule errors, we can see on the right hand side, Keycad is actually jumping to it and showing us with a little red arrow where these errors are. We can see we have a couple of clearance violations. We've got a whole clearance violation because of this rather peculiar footprint. more of these clearance violations, incomplete **[2:08:21](https://youtu.be/igQWdVGZGpI?t=7701)** thermal relieves. And the majority of these errors are front solder mask aperture bridges between items with different nets. And for instance, those are the bulk of the areas. So we can see most of these red arrows are because our solder mask expansion. If we go to the front mask layer, keycat is complaining saying this is an error that our solder mask openings are so wide that they span across pads of different nets. And for components such as this one, fairly fine pitched LQFP packages, you can't really get the solder mask to be just around the pad due to manufacturing constraints. So your solder mask **[2:08:53](https://youtu.be/igQWdVGZGpI?t=7733)** openings for these type of components. Also, for instance, for the IMU or fine pitch components such as U2, that's pretty much unavoidable. So in that case, I see this not as an error, but rather as a warning or just a completely ignore. And we can change the severity of these errors. The way you can do that is either in the design rules check window, right click on one of these errors and just say ignore all of these errors or edit the violation severity. So I click on edit violation severity and we can see under the design for manufacturing section right at the bottom solder mask aperture bridges **[2:09:26](https://youtu.be/igQWdVGZGpI?t=7766)** items with different nets. That to me we want to ignore. Click okay and then run DRC again. And you can see we have significantly dropped the number of errors. We do of course have to take care of all of these. You should when you're done with the board and you've really checked it, you should have zero errors and ideally zero warnings. Quickly just looking at the warnings themselves, the warnings are actually fairly simple. We can see why. It's because I changed some of the properties of these pads manually to not have spokes as thermal relieves and just do solid connections. And that's why we can **[2:09:58](https://youtu.be/igQWdVGZGpI?t=7798)** see, okay, the footprint does not match the copy in the library. So, this is fairly safe to ignore. So, I'm going to do the same thing. I'm going to ignore all of these and get rid of my warnings. So now we just have to take care of these various errors and clearance violations are of course concerning but you can see actually the difference is 0.152 mm to 0.15 mm. So we need to see what's going on there. So let's close that. Go to the board setup again and in our design rule constraints we said our minimum clearance is 0.152. But if we go to the neck classes 0.152 and this is because of this weird mills to **[2:10:32](https://youtu.be/igQWdVGZGpI?t=7832)** millimeter conversion. So actually we can drop that to 0.15 also in the net classes default net class just change that to 0.15 and that's completely fine. That's the simplest way of fixing this because remember at the start of this video we actually define the design rule constraints to be well above the manufacturing minimums. So going down by 0.02 mm is completely fine in this particular scenario because we already have that buffer in place. So click okay. Let's just press B to rebuild all the zones. Go to the design rule checker. Click run DRC again. And we've already gotten less errors here as well. **[2:11:08](https://youtu.be/igQWdVGZGpI?t=7868)** So we have a couple of these thermal relief incomplete. Let's check those out first. So again, we can click on this and then see what's actually going on. So this seems to be these connections. We can see here, yeah, this thermal relief connection is not complete. The way we can change that here, because we don't have terribly much of a thermal mass, it's probably okay just to make these solid connections. Alternatively, we can just do polygon port cutout in this area. and then just do manual connections. So we could just do that. So I can take one of my predefined cutouts we created before, move that over here, and then actually change the **[2:11:40](https://youtu.be/igQWdVGZGpI?t=7900)** dimensions of it. So I can get rid of this polygon pole just around this component. Press B to repaw. And now we just have to do manual connections. I've added that polygon pout, done manual connections. I've rerun the design rule check, but we still have two of these issues. And that's actually a J1. So, we have to seem to have a similar issue right here of pad B12 and pad A1, it seems. So, let's try and fix that. The way I'm going to do that is actually I'm going to change this to a solid connection because the connection width is pretty small anyway. So, I'm just going to change that to solid. Also for **[2:12:13](https://youtu.be/igQWdVGZGpI?t=7933)** B12 because that's right underneath. And also do the same thing for A12 and B1. Open the design rule checker. Click run DRC. There we go. We've gotten rid of those thermal relief errors. Now we just have these whole clearance violations. And we can see the whole clearance violations are because of this slightly awkward footprint for this USB connector. So actually this mounting pin is too close to these pads both for the top here and for the bottom here. So one option would be okay let's just check our manufacturing guidelines from the manufacturer. Could the manufacturer **[2:12:45](https://youtu.be/igQWdVGZGpI?t=7965)** even manufacture this? Do we just have to relax our design rules or do we actually have to adjust the footprint to make sure that these pads for example B4 A9 and and A12 B1 are further away or shorter that they're further away from this mounting pad. Both are of course viable options. Let's go with editing the footprint. So I can click on the component J1, press E, go to general, and we're going to edit the footprint but not the library footprint. We want the library footprint to stay the same. We saw this in the schematic editor. We can do the same thing. We just want to edit this one instance of the footprint. **[2:13:18](https://youtu.be/igQWdVGZGpI?t=7998)** And this will also show you the footprint editor. So what we want to actually do is make these two pads, the power and ground pads shorter and move them up, but still that the edge aligns with the edge of all these other pads. And we'll do the same for A9 A12. So one option of doing that is selecting the pad, pressing E, going to general and the pad properties. We can see the pad length is 1.15. So we could change the pad length, let's say, to one. So, we're taking off.15 mm, which means we need to move this pad up by half of that by 0075 mm. Click okay. And you can see this is **[2:13:51](https://youtu.be/igQWdVGZGpI?t=8031)** exactly what it's done here. We've taken off.15 mm, moved it away from this mounting pin, but still aligned the top edge with other pads. So, let me do that for the rest of the pads. And that's now what I've done. So, now we should hopefully have gotten rid of that design rule error. I've saved the component. And again, this is just saved for this particular PCB. And we can see it's updated in the board as well. So I can go back to the design rule check, click run DRC, and we have zero errors and zero warnings. But keep in mind, this might have seemed like a bit of a cheat, **[2:14:23](https://youtu.be/igQWdVGZGpI?t=8063)** relaxing the design rules, moving the pads. There are, of course, other options. You could use a different connector. You could check your manufacturer capabilities. We could really move the design rules, relax them down to the absolute minimum the manufacturer can produce and hopefully it'll go all right. I try to sort out these design rule errors fairly logically, fairly systematically based on experience. We pretty much have a finished board now. You could go ahead and just produce the manufacturing files, produce the Gerber files, pick and place and bill of materials. That's the bare minimum. Ship them off to your preferred manufacturer of choice and be **[2:14:55](https://youtu.be/igQWdVGZGpI?t=8095)** done with it. However, there's a couple things I would like to add. For example, we might want to clean up the silk screen a tiny bit. Some of the silk screen is on holes, which might not look great. We should add maybe some text on it, revision, things like that you can add to your board and you should add to your board if you want to. The way you can do that is simply go to the silkcreen layer. I'm actually not going to be using the bottom silk screen layer because that gets rid of one process step. The manufacturer now doesn't have to print any silk screen on the bottom layer in volume and that is in large volume. That can make things cheaper. But I just like if I don't need it then I won't use the silk screen layer. But **[2:15:27](https://youtu.be/igQWdVGZGpI?t=8127)** we will be using the top silk screen layer. And here I can also place text. You can choose whatever font you want. You can choose the position and you can place this kind of sure on your board. Make it look nicer. Add revisions, date codes, and so on. Very simply, not to spend terribly much time on it, I simply just added a title of the board, a name of the board, what revision this is, my initials, and the month and year that I finished this board or this revision. And, you know, company name and things like that. Depends on what your company implements. There are certain mandatory markings you might have to do for certain products, but for now, this is the simplest. We have all the pin one **[2:16:00](https://youtu.be/igQWdVGZGpI?t=8160)** indicators. is we've got our component designators. Although they are not terribly required, we've got a bit of silk screen text around it. This looks fairly okay. Now, of course, there's certain improvements you could make. You could try and move these holes away from silk screen to make it more legible when it gets manufactured. We could try and move some of these silk screen pin one indicators further away from the exposed copper openings because if we get silk screen on top of the exposed copper and the manufacturer actually goes through with this that of course can worsen the solderability of the board. So these are certain things you can pay attention to. **[2:16:33](https://youtu.be/igQWdVGZGpI?t=8193)** Trust me you can spend hours and hours just cleaning up a board. But for now we'll call this done and we can move over to generating manufacturing files. Of course before we generate manufacturing files it's incredibly important that you triple check the schemata. your triple to check the pin outs, your routing, that everything's been connected, that you've chosen the right components, and so on. To generate manufacturing files, the bare minimum are three sets of files we need. One are the gober files, which essentially export all of the layer information. So, the front copper layer, bottom copper layer, the paste layers, silk screen, solder mask, outline layers. that will **[2:17:07](https://youtu.be/igQWdVGZGpI?t=8227)** be typically in a Goba file format, although that's kind of outdated these days, but a lot of the more affordable PCB manufacturing houses don't really support OW++ or the IPC based file format just yet. So, we'll just stick with Gerber. That would be enough to get your board manufactured. If you want to assemble it at home by yourself, that would be all you would need, but we would like to get this assembled. In my particular case, I'd like to go with JLC PCB where I had the actual demo boards manufactured and assembled. So, we also need a bit of materials. So what components are on this board? Where can we source them from? What are their **[2:17:40](https://youtu.be/igQWdVGZGpI?t=8260)** names? What are the manufacturers? And we need a pick and place or component placement file. And that tells the the assembler relative to a certain origin. In this case, we have the bottom left. What are the coordinates of the centers of the components for the microcontroller center, the diode centers, the capacitor centers, as well as their relative orientation. So rotation. So these three files or sets of files is what we need to produce to get this board manufactured and assembled. Now the process is fairly straightforward specifically for Gerbers. We can just go to the top left file fabrication outputs Gerbers. Here **[2:18:13](https://youtu.be/igQWdVGZGpI?t=8293)** we want to select the output directory and I'll just select my root directory of my project. Then create a new folder and just call it manufacturing or MFR for short. Choose this folder. We can use a relative path. That's okay. Then we need to select what layers we want. We definitely want the front and bottom copper layers. We want the front paste. We are not using the bottom paste. There are no components on the bottom paste. We want the front silk screen. We have no silk on the bottom. We want the front mask, solder mask, and we the bottom mask. And we want the edge cuts, which is our outline layer. We want to use the extended X2 format. We want to use the drill place file origin. And we're going **[2:18:47](https://youtu.be/igQWdVGZGpI?t=8327)** to uncheck indicate do not place on fabrication layers. Not that for this project, this actually means terribly much. We don't need a go job file for this particular manufacturer. So, we're going to uncheck that. Once we've selected these options, then we can just have to click on plot on the bottom right that button. We can see the exported files in our manufacturing folder where we have the front copper, bottom copper, front mask, bottom mask, a front pace layer, silk screen, and of course, our outline, which is our edge cuts layer. Other than those Gerber files, we of course have drills in our design. both plated throughhole drills, PTH, and non-plated throughhole drills, **[2:19:20](https://youtu.be/igQWdVGZGpI?t=8360)** which happen to be part and loose in this design of the TAC Connect TC2030 programming header. To plot those or generate those drill files, we just click on the generate drill files button on the bottom right output folder. We select the same as we do with the Gerber files under manufacturing. I'd like to use a pretty standard format for this is the Exelon drill file format rather than Gerber, but check with your manufacturer what files they would like to see. We can leave these options as default on the right hand side. We would like to use the drill place file origin units millimeters in our case and we'll stick with the decimal format for the amount **[2:19:54](https://youtu.be/igQWdVGZGpI?t=8394)** of zeros. Then click generate. We can close that and we can see in our manufacturing folder again we have now in addition PTH plated through hole and NPTH non-plated throughhole drill files. And these sets of files compromise the Gerber files. In our case we just need to zip them up into an archive. So zip or raw archive. And that's exactly what I've done here. just created a simple zip archive and that's going to be our gober archive. The GABA files are of course enough if you just want to have your PCB manufactured without assembly. For instance, if you want to assemble the parts at home by yourself. If you do want assembly, we do need to provide two **[2:20:28](https://youtu.be/igQWdVGZGpI?t=8428)** more files as an absolute bare minimum. And this is the component placement file or pick and place file which tells the manufacturer the assembler relative to a given origin where are the centers of the various components where the X and Y coordinates for example for the microcontroller. What's the rotation of the microcontroller? All of that is contained in the pick and place file. Other than that, we of course also need a bit of materials which tells the manufacturer what components are on the board, what their reference designators are, where to source them from, and so on. First of all, while we're still in the PCB design view, we can export the pick and place file. If you go to the **[2:21:00](https://youtu.be/igQWdVGZGpI?t=8460)** top left file, fabrication outputs, and then component placement file. We'll do units, millimeters, format CSV, and we can keep the rest as default and click on generate position file. This really depends on your manufacturer and assembler. But for instance, GLC PCB can be very picky of what their automated system detects as a an adequate pick and place file. For instance, they provide this reference here. So you need a designator mid X, mid Y, layer and rotation and the format pretty much identically to how it is here. This could be an Excel file, it could be a CSV file and so on. You have to have the **[2:21:33](https://youtu.be/igQWdVGZGpI?t=8493)** right columns however and the right structure for the system to detect it unfortunately. So this is what Keycad exports. You can see it's not entirely the format that JLC PCB wants. So I've adapted it to the format JLCPCB wants. It's pretty much just changing the header to designator value, footprint, midex, bit, y, rotation, and layer. And sometimes when JLCPCB throws an error, you might just need to put quotation marks around the various fields in your CSV file. I know it's irritating, but unfortunately this has to be done to work with the JCPCB assembly. Then to **[2:22:06](https://youtu.be/igQWdVGZGpI?t=8526)** export the bill of materials, we move back over to the schematic. And remember for all of these schematic symbols, we while we were creating the schematic, we entered the relevant information as symbol fields. And we can check that by going to the top in edit symbol fields. We can see that we have the reference designator. We have the quantity value, what footprint we're using, but also the additional fields we added such as manufacturer, manufacturer part number, various distributor links, as well as the LCSC part number, which comes into play if you'd like to get your boards assembled at JLCPCB. And we filled in **[2:22:39](https://youtu.be/igQWdVGZGpI?t=8559)** this information as we went along. And I strongly suggest you generate your libraries with this information in place so you don't have to keep re-entering and re-entering it. Also from the last video um while I was going through also a comment by Derek also highlighted that I picked out the wrong package type at least the part number for the 470 nanopharad 063 capacitor I actually picked at 085 then selected a different manufacturer part number just to correct that which is an 063 470 nanofharad capacitor. So hopefully all of this should be okay but please keep in mind we all need to check our bill of materials. There's a lot of human error **[2:23:11](https://youtu.be/igQWdVGZGpI?t=8591)** that can come into this. In any case, once you have the information in place, all you have to do is click export and it's actually written to the root folder. And this is what the bill of materials export then looks like. I did adjust the top header designator used to be reference with the Keycat export and quantity used to be QTY. So I've just expanded that just to make JCPs be happy. The rest is exactly as Keycat exported it. So these are the three folds we then need as an absolute bare minimum to get our board manufactured and our boards assembled as well. If you just want to get your boards **[2:23:43](https://youtu.be/igQWdVGZGpI?t=8623)** manufactured, again, you just need the Gerber archive. If you want them assembled on top of that, we need the bill of materials as well as the pick and place file. So now, let's move over to JLCPCB and see how we can order these. Here we now are at jlcpcb.com. And all we have to do is click on instant quote. Then we need to upload our Gerber files. So click on add Gerber file. Select our Gerber zip archive. Then we will upload the files to JLCPCB and the automated system should extract the number of layers as well as the dimensions for this board which it looks like it has. We have this simple board **[2:24:15](https://youtu.be/igQWdVGZGpI?t=8655)** preview. We can check just very roughly if the holes are in order, if the silk screen, solder mask openings, copper top and bottom have been exported correctly. And we can also use the Gerber viewer to double check that. And I'd strongly suggest checking that because it gives you yet another view on the PCB design, which is always a good thing. In any case, we're using a simple F FR4 two layer board. The dimensions have been correctly identified as 53x 28 mm, and we're just going to get five produced. That's the minimum amount, at least from manufacturing. We're going to use a standard 1.6 mm thick PCB. That's the default or very common for two-layer **[2:24:48](https://youtu.be/igQWdVGZGpI?t=8688)** PCBs. Green solder mask color and white silk screen. Those options are the quickest, most standard, and cheapest. Surf as finish, I typically at least go with lead free hot air surface leveling. For more complicated boards, if you maybe need a longer shelf life, if you need a flatter surface finish, then you might want to go with enigm nickel gold. The highspec options we can just keep as default. What I do like to check, however, is the confirm production file option. I want to be in control of what is produced. And the way I can do that is by asking my manufacturer to send back their actual manufacturing files **[2:25:21](https://youtu.be/igQWdVGZGpI?t=8721)** that they're going to be using in production. And the way I can do that is by clicking yes on here and checking do not confirm automatically. That'll add a small $1 search charge, but I definitely think that's worth it. That would be then enough. You would just have to click on save to cut to get five PCBs that we just designed manufactured. And excluding shipping, tariffs, customs, and so on. That's just over $4 for five PCBs, which I think is incredible. But we would, of course, want to have our PCBs assembled as well. So, very easily, we just check the PCB assembly option. For us, we just want the top side **[2:25:54](https://youtu.be/igQWdVGZGpI?t=8754)** assembled. There are two different PCBA types, economic and standard. Standard includes more advanced options for assembly and also includes finer pitch parts. Now, we could use economic in this case because most of our parts [clears throat] are very simple. However, because of the addition of U4, our accelerometer that has a very fine pitch small part, we actually have to use standard assembly. So, you could in your design, if you want to use an accelerometer, maybe choose a package that's easier to assemble and economic PC PCB assembly is a bit cheaper than standard, but standard is pretty **[2:26:26](https://youtu.be/igQWdVGZGpI?t=8786)** affordable as well. So, we go with standard again because we have this fine pitch component. I would like to just have the top side assembled and that's cheaper, of course, and that's also what we have on our board. We don't have any components on the bottom layer. So top side and we can go anywhere from two to five boards at least. That's because we set five as a maximum because that's what we set for how many boards we want manufactured. We could of course change that by changing the overall PCB quantity, but for now let's just get five PCBs manufactured. Edge Rails will let JLC PCB add and I would like them to confirm the parts placement with me as well. That's similar to the confirming **[2:26:58](https://youtu.be/igQWdVGZGpI?t=8818)** the production files. Click confirm. The rest we can leave as standard for now and then just click next. Here we get a little board preview again where we can have a quick look and then click next. Now we need to add our assembly files. So the blue materials in the JLC required format and the component placement or pick and place file again in the JLC required format that we just saw. I selected the blue materials and the component placement file. Now click process and very quickly JLC's automated system brings you to this page. On the left hand side we can see what was extracted from the blue materials and on **[2:27:31](https://youtu.be/igQWdVGZGpI?t=8851)** the right hand side we can see what the automated system has figured out what we want to have assembled. So we need to go through row by row check is the component on the left actually matched with the component on the right and of course in most cases it is. But I strongly suggest going through line by line checking is this the component we actually want assembled in the right package and so on. Sometimes there might be not a check mark next to the component. For instance, here we get a little notification that a special component fee of 3 cents per piece will be charged because the processing of this USB connector happens to be difficult. We can agree to that by just clicking the little select check box on **[2:28:05](https://youtu.be/igQWdVGZGpI?t=8885)** the right hand side and make sure to go through this in detail. But once you're happy with that, we just have to click next. Then we get led to what I think is one of the best parts of using JLCPCB is that we get our footprints are shown to us and we can visually check if the footprints look in order. We can check the rotations, orientations, placements, and so on. Now, you will already have noticed that some of these components aren't rotated correctly. And this is because every manufacturer, every assembly house, every ECAD tool uses a different orientation standard. So, where is 0°? Is that north, south, east, **[2:28:38](https://youtu.be/igQWdVGZGpI?t=8918)** west? And that becomes of course problematic if everyone uses their different standards. So pretty much in any case, every time you use a different ECAD tool, depending on how you set up your libraries, you will have to rotate your components in this view. But that's very straightforward. I'm just going to go to 2D view. If we zoom on a component, for example, U1, I click on this and press spacebar and rotate it by 90° each time until it's in the correct orientation. And I'll just do that for the rest of these components. And that's very quick to do, but that's something I would suggest verifying as well. But again, I really like this view because it lets me check at least very roughly **[2:29:11](https://youtu.be/igQWdVGZGpI?t=8951)** visually that the footprints look somewhat in order. I can do that in 2D, but also in 3D view just by moving my mouse around here. So, I think this is a very cool feature of JLCPCB. You might have also already spotted on the left hand side this little checker chest box mark is because JLCPCB hasn't got the 3D model info there yet. But once you actually place the order, they will typically generate that info that you can then use for the next time as well. Also, once you've checked the check parts placement, you should get an image or an interactive viewer that actually shows this missing footprint or 3D **[2:29:44](https://youtu.be/igQWdVGZGpI?t=8984)** model. I did notice one thing here. So, this footprint has two pin one indications here, which aren't an alignment. And that's again another reason why I always check the confirm part placement button because this was probably generated by an automated system at JLCPCB. So, there will be some human involvement to actually check this part. Just make sure you always check that option because things like this can happen. For instance, if you've checked this and everything looks in order, all the pin one indicators are there, all the footprints look all right, we can then scroll down and click next. But that's pretty much it. Now we get a list **[2:30:16](https://youtu.be/igQWdVGZGpI?t=9016)** of all the charges that are required to produce the printed circuit board as well as to do the assembly. And overall for five boards excluding shipping, we are just below $80, which I think is pretty incredible because you don't have to do any of the soldering yourself. none of the PCB manufacturing yourself. So I think that's pretty good. We do also have to select what this device is going to be used for and that's just for shipping and customs. So in our case that would be research education and it's just a development board or DIY for instance. Then you can save to cart and check out using your preferred shipping and payment method. So I think this is pretty good and pretty straightforward. **[2:30:50](https://youtu.be/igQWdVGZGpI?t=9050)** Thank you very much for watching this video and well done for making it through these two videos. I know it's been a long series, but hopefully it's been useful showing you the whole PCB design and schematic design process for simple MSPMO microcontrollerbased board using Keycad 9. If you'd like to support me and like to support the channel so that I can provide more of these free tutorials, please do consider signing up to one of my hardware design courses on Federville, which is Robert Ferinex platform. I have two hardware design courses there, mixgore hardware design with keycat as well as advanced digital hardware design. Well, leave links in **[2:31:23](https://youtu.be/igQWdVGZGpI?t=9083)** the description box below. Thanks a lot for watching this video and supporting the channel in any way you can. Leaving a like, a comment, subscribing really helps me out. I have many different videos on embedded systems design, hardware design, firmware, digital signal processing, and much, much more on the channel. So, please do consider subscribing. Thanks again for watching, and I hope to see you in the next video. Bye-bye.