Hi. Now there were quite a lot of people who wanted me to take them through my PCB layout of this power supply board. and that's exactly what I'm going to do here. while I was laying out this board I did, actually, uh, capture it in real time.

So what I plan to do here is actually play that back the complete recording of laying out the board at uh times 10 speed and adding some commentary on top of that of how I was laying it out, what I was thinking and the processes and things like that. So let's get on to it now before anybody asks. The package I'm using here is Altium Designer. Okay, so no more, that's the package I'm using.

Yes, it's very expensive I'm aware of that, but that's the tool I've used for 20 years. So uh, here we go. now. the board.

um itself. When I'm actually uh, setting this up I've already done the outline of the board. that is actually the first step I'm going to do when I start laying out a board is to do the outline of it and this is based on the box I know I haven't done a video, uh, outline the system design and the case that's actually going into, but the template of the PCB uh that you'll see here in Black the um, the black background that is already defined as the outline of my board with the little cutouts required and things like that. So uh, that's the first step you're going to want to do to aboard as well as setting up your uh placement grids.

Now I've already uh done this because this is a through hole design instead of surface mount. most of my components are on an Imperial uh 0.1 in uh grid. So what I'm going to do is set my Uh grids both uh, a component grid and a uh snap grid as well. I'm going to set the snap grid to 50 mil or 50 thou.

it's the same thing thou means mil Mil I'll probably use these sort of terms interchangeably throughout the video. I do tend to uh use both, so mil is not millimeters Mill is th 1,000th of an inch. So because the components are things like dip packages are on a 100 TH or 0.1 in uh grid, I'm going to set my snap grid to half that value when I'm routing. maybe drop that snap grid down to 25 thoul or something like that.

And the reason you want a multiple of this is so that your tracks uh, when you take them between pins of your IC go smack bang through the center. and if you try and lay out uh, an imperial board like this a instead of a metric board which is what new surface mount components use. If you used a metric grid with Imperial components, you're going to end up with the tracks, not go quite going through the Cent. All going to get a bit messy.

but um, I when I'm designing and laying out a board like this I you have to, you're forced to use both Imperial and Metric uh Dimensions because I will use Metric for things like uh hole sizes I'll use 0.8 mm hole instead of Um x amount of uh th. So I will also use metric for the dimensions of the board and possibly uh, plac in components and the center of components and things like that. So when I'm dragging around my components, I will actually um I might switch to a metric grid instead of my Imperial grid so that, uh, a lot of the Uh components themselves, especially on the front panel uh components. when you're lining them up, they will be on a metric grid.

So I've already set these things up in the background and I've dumped all my components down because it's a very important step to get your schematic and all your Footprints correct in your libraries as a first step and then dump them all onto your board. So that's what you'll see here. I've started off I didn't capture this Uh process on video unfortunately. but what you'll see when I start out here: I've got a blank board that has the outline already done I've placed some of the components around the edges because it's very important.

The first thing you want to do is Place those fixed components that poke out your front panel on the edges of your board, your connectors, your switches, your you know all sorts of things like that. You want those to be Um, exactly where you want them on the edge of the board and then you fix them, you lock them in place and then your components can. That's when you start to get to the art of PCB designers. Where do you put your components? How do you lay them out? How do you? which area of the board do you put them in and so on.

So I've already done that I've placed the components around the outside, so let's get into it all right? here we are. We've got our main schematic of course and I've dumped down all the components as I've said, and uh, you'll see the menus are flash up sorry I can't actually slow this thing down as I'm actually recording this um, uh, audio narration on top of it. But as you can see what I'm doing around at the top of the screen, there is I'm moving the heat sink around now I'm playing and uh, at the moment I'm getting that uh Power connector. there's that uh, 2.5 mm, um sorry, 5 mm uh um uh DC power jack and I'm just mucking around that top area of the board there just to uh, make sure I've got that uh Power connector on the side I want and I'm also thinking about the system design at this point because I still don't have a a complete idea in my mind about um, where everything's going to go and how it's all going to work and this will actually um, evolve as I lay out the board.

Uh, because a lot of this might be dependent upon you know things I see when I'm laying out. So what I'm doing now is I'm placing down the Uh Power traces there from the Um there I think close to 100 th wide, 80 th really big beefy uh Power tracks from the DC uh input jack and you'll notice all these Uh wires actually connecting all the components that I've dumped down there. the alium designer: the program's just done this for me. it's it's dumped all the components down and they're actually netwise.

they're called uh from twos in uh Altium Speak in other packages, they might be called, you know, rubber Nets rubber banded Nets highlights like that. Now what I'm doing here. This is a key part of laying out a board. You'll notice that I've started to group together.

Functional components are functional block and if you got the schematic and you're playing along at home here, you, you'll see that um I've divided the schematic into these functional blocks and that's what I've started laying out here is: I've started laying out just that functional block I've moved in the components I'm doing this outside of the area of the board. That's another key thing. I'm doing this out in the dead area and when I've laid out this little subsection of the circuit, then I will take that, highlight it all, and then drag it into the board somewhere as a little module. So I'm developing this thing as a module.

You'll notice. Uh, the one I'm laying out now is actually there's the mosfet that this is the microcurrent. uh, part of the circuit So that's its own little module. And there's the Uh Drive transistor.

And there's the uh base resistor for the or the pull-up resistor or whatever for that. uh, that little microcurrent part of the circuit. And if your circuit is modular like this, then that's what you're going to want to do. And here are the current shunt resistors: all 10 of them in parallel there.

and once again, uh, you'll notice that uh, the location of those 10 parallel resistors will change later as the board evolves and I move things around. but that's where I put them for uh starters. Because it was, it seemed like a convenient location. It was down near the power switch on the front uh panel.

The front panel is actually the bottom of the board to give you some orientation. The front panel, the lower, uh, the bottom section of the board is the front panel. The top half is the heat sink that's going to be the back of the project. And if you're not that familiar with Pie Ofb, you always do it looking down from the top or through the board.

So even when you're laying tracks on the bottom layer uh, which I'm not actually the tracks I'm laying down at the moment are on all on the top. So red will be the color red. Uh, traces will means the top layer and uh, any traces you see in blue will be on the bottom layer. Now, my goal is to actually with a double-sided board like this, there's only two layers on this board.

What? I Want to do what I'm trying to do here and what you'll see is all the traces are in red. You won't see me for quite a long time in this video? Actually put any traces on the bottom layer because I want to try and add all of these traces uh, onto the top layer of the board. So I'm effectively routing this board as a single side layout at the moment. and uh, and just, uh, keeping that bottom side free for possibly any last minute tracks, power tracks, and a big ground plane that I can put all over the bottom of the board.

and ideally for a double-sided board like this. Um, you'll notice that I've dragged I've dragged and dropped the uh, that subsection up in the top left hand corner of the board. There, there we go. I Just moved the power.

I Just moved the um, sorry, the current uh, shunt resistors. Those 10 current shunt resistors. there. There's my current amplifier U7 which is going to be right next to the current shunt resistors because it's the current sense amplifier so it has to be right next to the resistors.

You can't have those tracers going all the way across the board. Uh, the bypass caps are going to be near those caps this uh PL one I'm placing at the moment that's the output of my voltage regulator. I'm trying to get that down to the front panel somehow so there's less wiring inside the unit, but you'll probably see that uh Trace change further along in the design process and you'll see quite a few pauses in the video here. and that's just me just sitting in the background thinking maybe sipping some water, having a scratching my head, and just having a general think about the system, design, the layout, and and remember I don't have a clear idea of how this layout's going to go.

In fact I have really no idea. Apart from that the that the regulators on the heat sink at the back and the Uh switches and and pots and and uh and and connectors are mounted on the front and that's about it. Um so but see because I've got those fixed voltage Regulators at the back mounted on the heat sink. It makes sense to put the circuitry around the voltage Regulators up near the top of the board there or the back um, the back end of the board which is the top edge up there near the heat sink because you don't want to have to run Trac all the way across the board.

That will kill your layout completely dead. So the goal of any PCB layout um is to, uh, try and get functional groups of components and keep them together nice and tight. So that's why I lay them out functional groups often on the side of the board outside of the routing area. I Sort of.

Uh, route them and then move the entire routed block into the board. Uh, you might a little bit of that here. Today, you've already. um, seen some of that up there.

but uh, there we go. that, um, that big circle there with number three in it? That's actually one of my mounting holes. That's a PCB mounting hole. Once again, that's a fixed.

Thing Once You place down those mounting holes and connectors. You want to lock those in place so you don't accidentally move them. Um, that's a very important concept. When you're routing out boards, you're doing a lot of stuff.

Lot of things happening. You're editing things, moving stuff, and you don't want things to get automatically pushed and shoved or accidentally moved so that that mounting hole there number three will be, um, will actually be fixed in location. Now here it is: I'm concentrating on the top, uh, the upper left, uh, corner of the board here and this is where all my analog stuff will go. This is all my uh, low power, um, analog to digital converter, uh, digital to analog converter and the Op amps and things like that.

I've shunted all those up in the one corner of the board because um, that's I want that to be the quiet section of the board so I don't want to have them on the opposite uh side of the board and run traces all the way across and it can cause, um, all sorts of issues with um, just uh, ground noise and EMC and all sorts of stuff I won't I don't have uh, the capability to go into all that, uh, detail today I'll have to do separate videos on, uh, actual each element of uh PCB design. This is just me just giving you a general um overview of what I'm thinking about. When I'm laying out this board, there's my 3.3 volt voltage regulator I believe it is there. So I've moved that up in the top Corner up there because all that analog, a lot of that analog circuitry is powered from that uh, 3.3 volt voltage regulator.

My voltage reference will be up there as well. the 2.04 uh volt voltage reference and oops, what am I there? I'm dragging in my microcurrent. There you go. that microcurrent circuit I routed before I'm actually dragging that I've dragged it from the outside into the board there so it's already partially uh routed and there we go.

I'm moving my Power Trace again to fit that down because the trace was in the way and I'm just uh, sort of. You'll notice there will be a lot of shuffling in this. There we go. I've decided to Route out that hole area because now I want to drag in I believe my micro controller.

Well, that's what I thought about there by moving that Power Trace I thought my microcontroller would fit in the center of the board there. but now I'm wiring in the USB connector. Um, just to get that over and done with CU There's four resistors that are associated with that. so I put them near the connector, down the bottom and here I am.

Um, this is the micro controller. the AVR and I'm wiring in the ISP connector. and of course I'm going to put the In Circuit programming connector right next to the chip because that's where it needs to be. It needs to talk to that chip.

I'm not going to put it all the way on the board. Now here's an interesting thing: I'm actually changing my schematic uh on the Fly here I can't remember what I've done oh I added an extra bypass cap or I did uh something there I've modified my schematic uh design and I've pushed that through to the PCB Any changes I make in the schematic I pushed them through. Uh, that's right I added a second bypass cap because there's power on both Um sides of the chip. so I added an extra bypass cing there I am attempting to rotate the chip around.

You'll find that that's probably not the uh, that's definitely not the final orientation. I will end up rotating that chip again so as you'll see, pin one is on the right hand side at the moment U6 directly in the center There and that connector I just placed. Um, that eight pin connector. that's the Uh serial interface connector? No, sorry, it's the LCD connector.

There we go. It's got LCD WR on it. and because, um, that talks to the microcontroller? Um, then I want it very close to the microcontroller. I'm not going to shove it on some side of the board somewhere where I've got a route over eight traces from the microcontroller right over to the other side of the board.

So naturally, I'm going to put something like a Serial or that, um, that LCD connector close to its source which is the microcontroller and uh, I know things are happening a bit, uh, fast here. I don't have the capability to really, uh, slow this thing down I've just got it in 10 times. uh, speed. but as you can see, it is actually taking shape and uh, once again, I must have been having a a breather here and uh, maybe I've gone for a drink or something like that and or just, uh, generally, maybe I'm measuring some stuff because I will have the components and the box and things next to me.

uh, right here while I'm actually uh, doing this here you go I'm back into it. so I'm making um, a lot of system changes as well. There you go. I Just moveed my voltage regulator there too because I decided that I wanted my serial connector that's Cn3 there I wanted that over that side of the board because I thought I would make like a little Riser board little daugh board that rises up out of that at right angles and then goes out the back of my case to avoid the uh heat sink.

So that's why I added the serial connector over in that corner on the Rev B uh part of the board. You'll see that I' I actually changed that but uh, we're only doing the Rev a board at the moment which is not the one that I actually built up. Um, if you've watched the previous videos, you'll see that I didn't actually end up I got this rev a manufactured but I never built it up I Um, went went directly to the uh revb and there you go. I mentioned before how I might rotate the microcontroller again and I've done just that there.

So now I've got the ISP connector on the right hand side of the microcontroller and uh, there we go. I'm just shuffling around like that, highlighting a bunch of components, moving it around and you can see I can. If you've routed things in blocks like that then, and you keep them isolated until later in your layout process, then you'll find that it's far easier than to, just, you know, shuffle around a bunch of components. you can highlight them, including all their traces and Shuffle things around.

Now you'll still still notice that it's all the traces are red I'm still on the top layer of the board and that's that's very important when you're doing a double-sided layout like this to try and do as much as you can on the uh top side of the board. and there's lots of stuff going on in my head which I can't really. uh which I don't really have the capability to speak about here a lot. Some of it's even not subconscious things like that, but when I'm laying out aboard I do find that, um, some.

it just magically works. In the end, where almost the last Trace after laying out hundreds of components, thousands of traces that last Trace just sort of magically fits into place. And that's part of the art of PCB design. And it's actually quite difficult to, uh, teach because a lot of it is a lot of experience.

a lot of innate ability to think about the entire system and how things fit together. And um, this is one thing. if you're laying out a board which you didn't actually design, then uh, it's going to be harder than if you actually design the whole thing. But because I designed this I have the circuit in my head or I've got it next to me on paper I know exactly everything's modular on the schematic I know where the modules go and I sort of have an idea of the system design as far as the case goes and where the connectors go and and uh, things like that.

So now I'm uh, working on that uh, microcurrent part again. I've got all the resistors associated with that uh, Max um, chip there, the uh U2 One along with the a couple of transistors there, the mosfet and the drive transistor and the bypass cap and I've routed that and Bam I just I'm dragging that in I tried to drag it in and I found it didn't quite fit. Oh, it's a bit. it's a bit tight there.

the uh, but I managed to do it. It just fitted in there. it squeezed in below the LCD connector. uh, there on the top top.

uh, part of the screen there and the connector in the bottom. and um, because I'm laying out a single-sided board. it's going to be a kit and uh, you know it's fairly important to get the silk screen designators as well visible, so you'll notice like r18 R17 things like that I've got those outside of the component instead of on the inside where, um, they're only visible um after before you place components. So um, I if you've got room, then you can actually put those silk screen designators next to the component that you're actually doing.

But sometimes if you got a really tight layout, you can't afford to do that or you might have to get rid of the silk screen designators. You might have to ignore them when you're placing components like this. If the silk screen designators are overlapping other components, you'll take care of that later as a final pass at the moment. I'm not really caring about the silk screen designators.

Um, as such, I might shuffle a fewer around, but generally, um, I would do that as a last pass. So now I'm I'm sort of starting to join all these modules together now because I'm now starting to think that you know I'm I' this is looking good. It's looking like it's going to fit I'm always looking at how many components are left over, how much area I've got left. So I've decided at this point that it looks like it's all pretty much going to fit.

um as I expected. So I'm starting to get a bit more confident I'm joining the modules together, doing a bit more fine layout there. I am mucking around with a few traces, trying to keep them nice and tight. So I know there's going to be more traces through that area Later there you go.

I've laid a couple more so I I know intrinsically how many more traces that I've got to sort of join those sections together and you can see by those uh, rubber band Nets as well. there you go I needed to create a bit more space, ran out a bit of room I highlighted a bunch of components, shifted them across a bit I've made a little bit more room there What am I doing there I'm changing the USB uh layouts there Shuffle you saw a little slight Shuffle there in a cou in like four traces I just pushed them all down and there we go I managed to fit in another trace or not quite I ran out of room there right in the center so there you go I decided to take that around the top instead of it. It's hard to sort of, uh, explain where I'm placing Tru es and why. it's because I have a lot of the information up in my head about where I think they should go where you know I'm going to know Okay, I know I need to at at least allow another couple of traces through here.

so I better route I better not take one Trace through there and then have to use a jumper or you know, jump to the other side of the board for two traces. So it's a uh tradeoff about how if I know one Trace has to go from one side of the board to the other just because it has to, there's no other way around it then I'm not going to do that now I'm going to leave that until last or I'm going to take it right around the edge so it doesn't interfere with all the other traces which are close together and have to join modules together. So there's a there's a bit of an order about how you do these things. You're going to uh, do your modules first, keep them as tight as possible, route them as fully as possible, and then drag them into the board as a complete routed module where you need it.

and then you start. Once you're happy with that, you start tentatively joining the modules together, and then you start uh, thinking about uh Power tracers As you'll see I haven't really done I've done a few key uh Power traces there. and by the way, my power traces are going to be uh, fatter than the signal traces I'm using um I didn't mention it but I am using uh 10 th uh traces here. So um, all of my traces.

all my signal traces are 10th hour with my Uh Power traces and they might be 50 or 30 or something like that. they're fatter, um, lower impedance and just to designate that they're actually power tracers. Um, that's just a good thing to do. Now it looks like I've used my first VI there.

There we go. I've run out of room routing into this microcontroller and I've determined that I need to now jump to the bottom layer. But with this, the key with Uh making jumps to the bottom layer is to keep them as short as possible. Once again, I'm not going to want to use uh on the bottom layer to roue a trace from one side of the board to the other.

CU you've just split the board in half and you've completely ruined your routing space for all the other traces on that layer. So you'll notice those blue tracers under the microcontroller are as short as I could possibly. uh keep them so they don't take up too much room on the bottom layer they don't split. There's another one uh, which was quite short I'm Shuffling a future tracks to actually get it a bit shorter.

There we go. you'll notice that I um changed a few traces there just so I could save a few millimeters extra on traces on the bottom layer. so I don't cut up my ground plane as much I mean this is not a highspeed controlled impedance board, so cutting up the ground plane isn't really a big deal. Um here.

But if I'm laying out a much more critical board then those little aspects of just saving a couple of millimeters of of Trace length just to so you can get a slightly bigger ground plane on the bottom. and those sort of things can be uh, very important in Um in highspeed designs where those sort of things matter in terms of maybe EMC uh compliance as well. The ground plane's a big thing and you want to chop that up as little as possible. So here you go: uh, laying out the output track there, there's the Um J2 as my output connector there.

that's my output mounting point and that looks like the constant current Source u4 there I've sort of tacked it around. It's a low current so it has a 10th hour Trace going to it. uh, and I'm mounting a few I'm placing a few resistors associated with my Um output Uh current sense they're my output current sense resistors and j4 uh, I believe is the Um is the current sense input connector I've decided to move, move a few more resistors over to this corner and I'm slowly dragging components from outside of my board into the board so you'll find um, if you can see, you might see a wide shot. Um, soon of how many components I've got, uh, left, and uh, there will be very few actually left outside of the board.

So I'm slowly bringing them in one by one and there we go. I shuffled those around, put them vertically and you'll notice I'm lining up all of the resistors nice and straight as much as I can because that's a good. it just looks good. Um, to if your resistors are just odd.

Bold everywhere, at all sorts of weird angles and spacings. and it doesn't look like a professionally laid out board. So you want your components to be nicely grouped and this is where your, uh snap grids come in. If you're not using a snap grid, well, you're crazy.

You should be using a snap grid, but if you're not, or using a very small uh snap Grid or component uh, snap grid, then your component's going to be slightly out of a alignment with each other and things like that, and your board just ends up looking pretty horrible and amateurish. But if you, um, keep them, you know a big nice line of resistors will be lovely. Things like that. it just looks aesthetically pleasing.

and uh, it. It just shows that you know what you're doing when you're laying out a a professional board like this now. I This is actually the first uh, through hole board I've laid out in many years I think um, because I'm so used to doing everything uh, surface mount these days. that uh, a through hole board like this is quite a novel uh thing for me of late.

So um, it's it's a different mindset. SMD will be uh, different again because you can't use resistors to jump things. One of the key with through hoold designs like this: because these resistors are so long they are4 uh, inches across, you can fit many traces underneath. so you can use resistors to actually jump other traces.

you know four, five, or six other traces at at once and that's very handy. Um for routing uh, ability and routing density on a uh double-sided board like this. If you've got eight layers or something, then H it's things are much going to be much easier. Your options are much greater but uh, if um, but you'll see with this double-sided layout.

I could almost have done it on a single sided board. In fact, if I put a bit more thought and effort into it, it almost comes down to I could have done it with maybe you know, a dozen jumper links or something like that. but uh uh, these days there's really. Unless you're manufacturing a million of these things, then uh, there's not a huge cost advantage to go into a single sided.

PCB So I'm using the double I tend I plan to have all ground plane on the uh bottom as as you can see, there's a few little traces on the top there and now I'm I'm on the bottom again because it's blue and I'm routing uh looks like my 5V rail so my 5vol regulator is at the top of the board or the back of the board. um and I need to route that 5 volts through to other parts of my circuit and as you can see, I'm trying to take it around the outside of the board there in the top on the top of the board. I'm trying to route that 5 Vol So I'm think I'm going to drop through to another layer here. possibly I'm thinking about it.

Maybe I'm having another drink or something like that. There we go. I'm dropping down and I'm using more than one. uh VI there because uh, that 5 Vols um carries a significant amount of current.

or it can do so. you're going to want to use more than one. uh VI there. As a rough rule of thumb, um, roughly one VI for every half amp.

But if you got some serious current, you're going to want at least a minimum of two uh vires there. and I've used two or three uh vires there for routing the 5V rail and you'll notice that this board is really starting to come together now. and uh, I'm probably at this point. uh, thinking to myself, I'm pretty darn uh, pleased with this and uh, I don't think I actually have uh, any, or, uh, very few components left on the outside of the board to actually drag into here.

So now I'm doing a bit more fine detail up there. I'm doing some bypass cap work up the top I'm oh what am I doing? I'm down into design real checking. There you go. I have actually finished the basic layout so I did a basic design rule check to find what the errors is.

that will find uh um, uh, points that aren't connected actually you know uh circuit Nets which aren't connected and they might be a dozen or two uh, left in there. so I will I'm now starting to lay out those and I'm starting to connect the uh Power now I think the 3.3 volt rail because once you finished what I would typically do when I'm laying out, um, pretty much any board is that, do all the signals first and then once you do that, then you start work on the uh power rails, It it. It depends though. it depends how power Centric um, how important the power, um, the power distribution is to that design.

but uh, in in general I'm going to on a board like this anyway. I'm going to leave that power supply until later and uh, hopefully if I've given enough uh thought and it's up. I've considered this when I'm laying out the board either subconsciously or semic consciously. I Guess you could say then, um, the power shouldn't be too much of a struggle to actually uh Route Around the board.

There we go. I've done another design real check. I'm looking through the errors. There might typically be a whole bunch of Errors for silk screen spacing and things like that, but I'm not too concerned with stuff like that.

It looks like that. Uh, I've just had a couple of breaks in my power uh rails there and it's told me that you know I might have five un unrouted power Nets or something like that. So I'm just tidying those up, adding in a 3.3 5vt rail. Nets try to Now my goal pretty much at this stage is to reduce my uh error net count to zero or uh, well, zero for all traces and all power signal traces and power traces.

And the only errors I have left are ground cuz you'll notice I've routed no ground connections at all. maybe the odd one on the top layer or something like that. but because I'm going to put all of my ground uh on the bottom I'm going to flood fill my ground in there and this is what I'm doing now. Here we go was coincidental: I'm now placing the outline of my polygon around the outside of the board.

This will be my ground polygon. So I'm placing that on the bottom layer and you'll see it. So I'm defining the outline and then the program will automatically fill in. Uh, the ground layout.

Now, what I'm doing going down the center of the board, there is I'm going to split this ground um, basically into power and Signal side. So all of my uh Power there we go I just filled in the flood I got the flood fill there I can edit that later I'm I can uh, tweak the Finer Things later, but there you go. I've basically created a split ground plane there in my board and the part on the right side of the board that ground is all power ground. so it goes from my Regulators at the top right down to the um regul down to the output connectors at the bottom and things like that.

So um, all of my heavy current is going to flow through the right side of the board and all the stuff my that uh ground plane, the blue ground plane there on the left hand side. that's all signal ground so there's no real current flowing through that so there's going to be no voltage drop through that and therefore all of my um sensitive signal stuff. My adcs in the Dax will be at the same potential because they're at the same ground potential because there's no current flowing through that leftand blue part of the ground trace and way. here we go.

I'm doing some 3D model time sorry um, my video capture program didn't capture that. It looks a bit, uh, dodgy. but what I'm doing now is looking at 3D mode and well, no I'm going the silk screen layer now and I'm Shuffling my silk screen. So I'm going through do doing my final pass.

my design will check I'm happy with it. It passes, There's no Nets left over my board is effectively routed and finished and now I'm going through and uh, just shuffling all of the component designators. There you go. I'm moving around, rotating them and putting them next to the particular component, making sure they don't overlap any of the pads because you don't want the silk screen um, overlapping any of your pads that can affect you generally doesn't affect your shouldering, but it's just not good.

You want your screen designators all the right orientation, all the right sides, so it all looks neat and professional. Um, I'm going to add some labeling. There we go. Avrisp I added a label right next to the connector and I did it as an inverse.

I'm McKing more around with the ground plane here I've probably uh, decided that I found a bypass cap not going to the right plane or something like that. So having a little muck around and I'm uh, as you can see, I'm continually checking the top layer. ah that purple one there. That purple Trace was a keep out now cuz I didn't want ground to touch those two pads there because I was doing a star ground system back to uh, it's you'll have to look at the microcurrent circuit to to figure out what I'm doing there.

but I didn't want the ground even though those tracers were. Ground I've created a keep out there which stops the flood, the polygon fill actually joining. Now what? I did just there is I joined that's the star ground point I joined my two ground planes in that bottom left hand corner down there. that's the point at which was my star Point around the microcurrent circuit so that's where I split and I joined the ground uh planes via the top layer there and I've added some.

Oh there we go. added some nice labeling evev blog.com micro Supply I've added a cereal top. left there another label cereal I'm label in things out I'm mucking around and now, aha, what I'm doing now is doing a pass for, uh, whole sizes. So um, oh, there we go.

I'm going in checking a footprint to make sure I've got a footprint right? Maybe There was some doubt in my mind that I might have, uh, goofed that up. So there you go. I jumped over to the net, opened the data sheet, did a double check. I'm now, um, modifying whole sizes here just to consolidate them.

So this will be a last part. Um, I'm doing a 3D uh view here. Not very few of my components actually have 3 real 3D models in them, but if you did go to that trouble, then you can get a very accurate representation of what your board is looking like. I'm checking my solder mask expansion there.

that's the Uh Pink sold to mask expansion to make sure that there's um, that they're not going to break. There's enough clearance between each of those pads in this case for the transistor. There you go I Just narrowed my pad on the transistor I wasn't happy with that footprint, wasn't happy with the uh solder mask expansion on that it would have broken through solder would, uh short out between the pins during during hand soldering or uh, wave soldering manufacturer. So I'm just making sure a good thing you know, four or five th uh gap between the solder mask between pads.

that would be good enough. um, anything less you get down to a couple of thousand. They're not going to be able to manufacture that just like they can't manufacture a 2our trace reliably, or if you want them to, it'll cost a fortune. So really, this board is very, uh, coarse.

It's in terms of you know, it's like 1010 design rules. Forgot to mention that before when I'm design rule checking I set uh 10 th traces minimum 10 clearance. So all of my rules and all those polygon pores, they will have a 10 uh spacing to them. So this is a very coarse board I could make this at home easily.

Um, so any PCB manufacturer in the world could make this. Any backyard manufacturer can easily meet 1010 uh rules and I'm checking my bottom solder mask there, checking the top layer. I've added the Open Source Hardware symbol and bingo there we have it is that that's our final board and uh, pretty darn happy with that. I'm not sure what I'm doing now I'm just mucking around more with 3D View: You'll notice the top part of the board that sticks up that's had the solder mask removed from it.

um, the reason I did that is just cuz I like it. It's just a different look, it allows you to Mark the bottom of the board. Um, something like that. I'm checking the copper layer silk screen layer, individual layers in 3D View and here's the real power of 3D view.

It shows you exactly what the board is going to look like when you get it manufactured exactly how the silk screen looking. you can see if you can get very high contrast in this mode. uh, to see that the silk screen doesn't overlay any pads or something like and bingo There you have it. there's my final laid out board.

I'm feeling pretty chuffed about myself. so I added a little platypus there on the uh right hand side. Why? well why not? and I was quite happy with this Uh layout is pretty pretty pleased. There's quite a bit of um, especially on the right hand uh side of the board.

You'll see there's quite a bit of uh area left. and in the next video I'll actually show me uh, editing this board from Rev to rev B to show you how I took a completed board and then changed things around, ripped up the uh ground plane, modified a few things, squeezed in some more circuitry, and then uh, redid it. So I'll do that as a separate video I Just wanted to mention um, one of the final passes here I didn't uh, speak enough about was the drill hole size consolidation there I I would have spent maybe you know, 10 or 20 minutes going through uh, the drill size hole table just to consolidate and make sure um, all my footprints um, actually have or how many drill hole sizes I'm actually using in this design and actually consolidate them because you might find that some libraries in your Uh component Library might use a they might use a imperial drill size instead of a metric drill size so it might be 795 mm instead of8 mm that you'll use on other ones or something like that. So you want to go through a final step.

you drill whole size table, just consolidate all those ho sizes into one. Even if they might be near enough, you might go. oh okay, I'm using 50 uh, 1.2 mm holes for example and I've got two that are 1.25 Well can I just you make those uh two holes 1.2 mm and that will in theory make your PCB a bit cheaper because there's less tool changes required. It's just a nice professional final step to actually do that and and check those sort of things.

and uh, and once again, you'll do I'll do a more detailed design rule check if I do care about silk screen over pads I'll be checking for things like that Electrical uh clearances of course is a big thing. maybe component spacing clearances, but because generally I I know the size of components or the silk screen outline defines the size of the component. Not too concerned about uh components touching each other. um cuz I I know what? No, exactly what I'm doing here.

You'll notice that the heat sink up on top of the board or the back area of the board. There has a silk screen extending right out, um, outside the board and is that a problem? Um, no, not really. The PCB manufacturer just chops that off. It's just chopped off in the process of manufacturing the board, but maybe as a final step I might go in and trim that uh silk screen just so it doesn't go off the board.

but I keep it there cuz that is the actual size of the uh heat sink that I'm uh using the outside. Dimension So that helps me when I'm doing a bit of system engineering. so I'm going to leave that silk screen outline there outline there I could have done it on one of the mechanical layers or something like that and that would be a more professional step if I was doing a really professional level board. I would have other other mechanical layers um, that I'm specifying dimensions and uh, engineering notes for manufacturing the board that it's 1.6 mm and it's um, you know it might be gold Flash finish and and where the routing areas and the routing paths and things like that are.

But because you know this is not a really complex, uh, comp, complex, professional uh level board. There's a few, uh, extra steps I wouldn't do there, but in general I'm quite, uh, quite pleased with that layout. How long did it take? me? Well, how long did this video go for? Multiply that by Uh 10 and that's roughly how long it took me to uh, lay out, um, this board and there was a lot of thinking and other stuff in there. and maybe if I uh had the libraries better sorted out before I started.

Could have saved some extra time and things like that. So um, uh, sometimes it you know a board might uh, take a lot less time because you're using all existing components that you guaranteed all the footprints are right and everything like that. Other times you might be doing a lot of interactive processing I might be even going through and changing. um, some components in the middle of the design process here.

I might find. ah, you know I might have been mucking around and thinking oh, I might have found some other device in some other Uh package or something like that and and changed on the Fly I might find oh I can eliminate that bypass cap cuz they're so close to each other I don't need that I can drop one of the bypass Caps or in the case you saw on there I think I added a bypass uh cap in there. Just the nature of the layout that I didn't think about when or I didn't uh uh, get that right, when I was just laying out the schematic. So um, you might find that when you're doing stuff on the board, you might have to go and uh, back annotate the schematic and make some few, make a few changes and things like that.

But as you can see I think it's a neat layout. It's got the cutouts for the case that it's going to fit into neatly and have to do a whole separate video on that cuz there's quite a bit of uh effort which went into actually figuring out where all the components went and what components I used like the inter user interface components like the knobs and the switches and uh, the power connector and things like that and the heat sink went into this system design before I even started laying out the board and that constrained a lot of uh things. and if this was just a board that was sitting in the middle of a case and then I had wiring going out to the front panel and the back panel, then it would have just been a a simpler Uh design even from a system and a PCB point of view because it would have just been a square board, there would have been no fancy cutouts. the uh whole, the mounting holes wouldn't have to be in specific locations to meet the supports in the case.

and uh, a lot of stuff like that would have been a lot easier. But when you're trying to integrate a PCB like this like I am that fits a specific uh case, then there's a bit more engineer. and if you've got a custom case, you might have to worry about the 3D aspects. Uh, the height of components, will it foul with the case and things like that? In this case I didn't have to worry about that I Put a bit of thought into it.

The case is big enough. It's not a custom molded thing, but if you're doing a professional uh PCB layout to fit into a custom molded enclosure, really, you've got to think about the whole 3D aspect of the mechanical packaging. thermal performance comes into it, and uh, things like that you don't want stuff to overheat. Uh, if you're doing highspeed signal design, there's lots of stuff um, in there to do with, uh, you know, transmission lines and controlled impedance.

uh stuff. EMC requirements and all sorts of stuff. But this was just a fairly simple board with a simple split ground plane. I Probably didn't have to split that ground plane actually.

if you're asking exactly why, there's probably not a real genuine electrical reason to do that, just good practice. Uh, really, that? I just wanted to separate the right hand side uh Power which can carry you know, several amps or something like that and it maybe switching and doing all the load Might be that because this is a power supply Supply and an unknown load so you don't know what it's actually going to be powering and that could be doing all sorts of, uh, putting all sorts of um, uh, strain on that uh, ground system. and if that's you have one big flooded ground plane, then it might in theory cause an issu. So I just decide to split it out, separate it into low current and high current.

uh stuff effect. not really analog digital. um in this. although I guess you can make the same, uh, call that similar to an analog and digital split uh plane or something like that.

but anyway, uh, there you go. That's the complete layout of the board. I hope you found that interesting. I'll do another video showing the changes from Rev A to rev B Catch you next time.