Layout of a Low EMI DC/DC Converter in KiCad

welcome back on this episode of everything embedded we're continuing with our low emi regulator series in this episode we're going to be doing the layout portion the layout for a voltage regulator is absolutely critical if you get the layout wrong you'll have noise problems stability problems the noise will couple elsewhere into the circuit and things are not going to work quite right so this is a critical step the key things we have to focus on with the regulators there's a couple of things that are called hot loops and so these are areas where the current density is really high so you have a lot of current that's switching fast going around these and so the first one is the input voltage through ground around here so we have these v in and the power ground so the as the switch turns on and off this has a lot of current going through this capacitor and there's this on this side as well the other high current path is around the switch node so we want to keep the switch node really small so we don't have much parasitics otherwise the switch node can radiate like an antenna into other circuits and into the surrounding environment so in order to get the layout right we need to start by getting the parts placement right laying out the traces is the easy part once you get everything laid out in a way that makes sense so we want to make sure that we have all the parts near to where they need to be to make the routing and layout as simple as possible to make seeing the layout a little easier i've gone back to the schematic and added some net labels so i added a v out label a switch label and then a v in label this will help us to keep track of the traces once we're in layout and make finding the nets a little easier so i'm going to save that now we can see on our pads here things are labeled so we have the v in pads ground we have the switch node and and v out is labeled over here to make things a little easier while i route i've turned off the fab and silkscreen layers just to help see the pads a little better i also don't want to be clicking on things i don't want to be moving so i've turned off some of the things in the selection filter the other thing we can do to make these easier to see is assign some different colors to the nets so for our v in net i can go into the nuts panel here and usually for vn i'll use kind of an orange color and then for my v out i'll use a more red color and so that now highlights the rat's nest and that'll highlight the traces in that color as well so now that we're set up we can start moving our parts around so this being one of the input capacitors it's important that this one ends up right next to the in and ground pins this is the other one this is going to be a pretty symmetrical layout the way this part is set up i did forget one other color i'd also like to set up ground as a green on here so here we can tell this is that critical v in current loop i talked about and so we're keeping it really small with this capacitor so high frequency currents will only move over this little tiny loop which will reduce how much they radiate and then for the inductor we want this to be as close as possible to the switch output so this way we'll have a a plane that we'll be able to put through here and capture the switch then we'll go place our output capacitors very near the v out here so now i've placed these three output capacitors right here so we'll be able to have a plane for the output here and then these can tie right into these grounds that will be nearby at this point i'm just grabbing all the other passives around and using the rat's nest to see where they need to go and putting them as close to the pins as possible for this bootstrap capacitor it's a little tricky because we need access to the switch node but this part actually gives us access we can poke it through here and come out over here and then this can tie through through this resist with the resistor for the bootstrap okay since we have these ceramic capacitors nearby the inputs this large electrolytic capacitor really it doesn't matter where it goes it just needs to be on the board to provide us some bulk capacitance for this design this capacitor is a little too large however it's one i already had so i'm using it if i was doing this design on a board where i was actually space constrained i would probably use a smaller tantalum or ceramic capacitor instead of a very large electrolytic but these can be very cost effective if you're not very space limited so that we can hook these banana jacks up using standard test connectors we're going to use a 0.75 inch spacing between them which is the standard that like most multimeter plugs will have on them i'm going to go into inches and set my grid to be on a inch grid of a quarter of an inch and then we'll move the plugs until they're on the grid i can then center the rest of the layout between the plugs so with this we've got a pretty good start we may have to make a few tweaks to some of the parts over here as we get routing but this should let us start routing the first thing i will do is go add my board outline so to do that we will go on to the edge cuts layer and go draw a rectangle on it the next thing we need to do is set up our board stack up by default kycad only gives us the front copper and the back copper to modify that we go into file board setup and then we can go to physical stack up and select four layers if you're doing a critical stack up board you could go set all of your spacings and everything in here we're just going to let the board shop choose that for us a four layer board for a converter like this that we're trying to have really low emi is pretty critical a two layer board has too much spacing and we will have slots in our ground plane we need a really good ground plane underneath our converter in order to keep all of the return currents under control so first we're gonna go on to layer one copper and we're gonna go create a zone so we'll click on the zone tool and then we're on layer 1 copper and we're going to make a and we're going to select the ground net the name of this will be the ground plane we do not want thermal release on this since it's an internal zone and we don't have any through-hole components if you wanted just for through hook mode you could do relief for plated through holes but we're not soldering to any of our through holes and then we can click around our outline if we hit the b key it will fill in that zone for us one other setting that i'll point out i already have set i have the zone set to be somewhat transparent here in the object so you can adjust this slider to control how transparent the zone is this helps make it easier to kind of see where your zones are at without them getting in the way as much i'm going to use layer 3 for our voltage planes so on one half of the board we'll have v in on layer 3 and on the other half of the board we'll have v out so on this side will be v in we're on layer three it's going to be solid release so we're going to want our v in to go over so we make sure we pick up all of the v in and then we leave a little bit of a gap before we pick up where we'll have v out present on the board but i will start all the way up in this corner and then we can see we need to cover at least about to the edge of the ic so we can capture these capacitors for that we'll close that one up and hit b to fill again finally for the zones we'll add v out same settings as before and this one will cover the right half of the board now even with those zones on the internal layers in the areas where we have those high current loops such as around our v in and our v out we're still going to want to connect all of those together with larger planes so for that we'll go to our front copper and grab the zone tool just the same and we'll start drawing a shape that gives us our the vn that we need here we'll extend it a little bit out beyond so that we have some space to put some vias down to those internal planes it doesn't matter if our zone overlaps some of the other pads a little bit the clearance settings will take care of it the clearance for these zones looks a little large right now so i'm going to go edit that zone and change the clearance down we'll now go on the other side and create a similar zone for this side's v in so next we will create some ground zones to capture the ground pads on all these capacitors on both sides we'll extend this one out a little ways as well so we have room to put some vias on here doesn't quite behave and it's not leaving a gap between these zones like we need it to the way to set that is you change the priority so if zones are of the same priority unfortunately it doesn't change this but if we increase the priority of the ground zone then now it'll push away that v in zone and give us the clearance that we need next we need a zone for our switch node and i'm going to set the switch node to be a higher priority than the ground node so that switch node is pushing the ground out just a little bit down here and that'll give us a nice short low inductance path for our switch finally for the zones we're going to tie our v outs together with a zone so so next we're going to start adding vias to get these planes stitched together so there's this freestanding via tool and we can simply grab that and start adding vias in and these will take the class of the zone that we're adding them on to here at this point we can see we've stitched all of our vias down from these planes so that we'll have nice low inductance paths from these outer planes down to the inner planes in the board at this point we can begin routing the feedback network and the other supporting pieces for this design to make routing easier i turn off my inner plane layers so we can see just the top side and then we can just start routing traces for routing we i typically shrink my grid down to a much smaller grid size of a couple mils this spot's gotten a little tighter than i want coming through here so i'm just going to scooch this piece over just a little bit i okay route this down here when a route comes out a little messy like this we can use the d key to drag the route and kind of clean up that trace so this one i'm going to pull back down since it got scooched a little bit and then that'll let us pull this one back down and that cleans that up since this one's ground we're going to tie this straight down to the ground plane underneath and we'll put a ground via on this side as well it's generally a bad idea to share ground vias since the return currents can cause a voltage drop across the via that can interfere so for each ground pad i try to use its own give it its own via this trace doesn't have a great way to come through so we're going to put it on the back side so we'll hit v transfer over to the back side and then we'll be able to put another via right in here and then connect that up back on the top side same thing for this v out it's a bit congested through here so we're gonna pop a via through and run this v out signal on the back side that will also make it easier because we need to connect that over to the v-out over here so we can drive this underneath here and connect it through one of these vias to hook up this capacitor we're going to use zones and vias again so i've switched my grid back to a larger grid and i'm going to draw some zones on this guy and with that we've connected everything on this board as a final check we'll want to run the drc design rule check to make sure that everything is connected and there's no issues so we run this design roll check and we get one unconnected item here so we can go highlight that and so here we can see we did miss a connection here so we can close out of that we can delete the markers off so we can see better and then close out of that so we miss this guy to right there we'll rerun the drc we have no unconnected items and all of the violations on here are silk screen and text variables which we will clean up next just as a status check we can check out what this is going to look like in the 3d viewer so if we go into view and we look at the 3d viewer since i've pulled in or kai-cat already had 3d models for all of our components we can see what this will look like in 3d and this is a handy way to kind of check everything out see where we're at obviously there's some silk screen to clean up but this is what our board's going to look like we also can go into the settings and turn off the solder mask and then that'll let us see the copper one more thing that i'm going to do on this board looking at this is add a zone to the back as well that'll help with thermal it'll help pull heat out of the regulator so we'll go to the back copper and we'll just make this a ground plane to clean up the silk screen i like to turn off all of the copper and then just turn on my fab layer and the silk screen layer although first we're going to clean up the fab layer because we have some reference designators that are not correct so for some of these it has the dollar sign ref and instead it needs to be dollar sign reference and then that will fill in correctly now if we rerun the design roll check for that we've gotten rid of everything except for the silk screen overlap and solder mask so we'll clean that up next since we're dealing with silk screen i'm going to turn off my selection filter for everything except for text one thing that's important with silk screen i like to make it so it can be red either all in one direction so it either be right side up here or turn to 90 degrees you don't want any silk screen that's upside down from one angle that head does give you these little lines that indicate kind of which component the silk screen goes with so if i just start clicking on these i can pull them out figure out which component they go to and start placing them i am going to go back into drc and delete all of the previous markers so we can see a little better right around the part it may get a little tight so for something like this we can place it off to the side and as long as we have that layer connected we can go draw a line from it and point over to the part and now if we go rerun our design roll check we have zero errors and zero warnings to ensure we'll be able to hook everything up to this i am going to go add some text kind of describing what this design is and then also labeling the inputs and outputs so the last thing i want to add to the board is just some test points that'll allow us to probe this with an oscilloscope each more easily later on so i've added these sets so we'll have two ground and then v in and then two ground and v out and so i'm going to place these to add these i just went into the schematic and added some 1x4 connectors and these will make it pretty easy to get scope probes onto this board so on the layout we're just gonna move these into a spot where they're accessible i will also add some silk screen to identify the pins on these do and with those test points added this board is complete and ready for fabrication i'm going to order a few of these boards we'll build them up and then we can test them out and compare them to some other regulators you

Channel: Everything Embedded

Views: 7,245

Keywords: EMC, EMI, electrical engineering, kicad, pcb layout

Id: jV7KUufkmso

Length: 28min 8sec (1688 seconds)

Published: Sun Jun 27 2021