Practical RF Hardware and PCB Design Tips

in this video i'd like to go over some practical rf hardware and pcb design tips in particular we'll be looking at a real-world embedded systems design which includes a gps module as well as an active antenna the board you're seeing here was developed by me in open seneca and i will be going into more detail about the various subsystems of this board in the future video but for now we'll be focusing on the rf part and what we need to pay attention to when designing these boards before we get started this board was actually produced by jlc pcb who were also sponsoring this video it's really cool to see that the jlc pcb smt parts library now actually features connectors which we also use on this board so you can find things such as hdmi connectors or usb connectors various types of wire to board connectors and so forth so that's a really cool addition and something i'll be showing in future videos as well but let's get back to the rf tips here are the topics i'd like to go through in brief detail in this video firstly i'd like to talk about when we actually need to consider these rf design techniques and when we need to apply them and this is often referred to as some sort of critical length so how long do our sections or traces need to be for the rf effects to actually take place and to mata secondly i'd like to talk about pcb stack up two and four layer pcbs or even beyond and what we need to pay attention to thirdly i'd like to show you how to calculate controlled impedance traces typically something like 50 ohms or 75 ohms the different types microstrip and strip line then the fourth point is the pad to trace or trace to pad parameters so for example when you go to a very from a very wide pad for example from an rf connector into a controlled impedance trace which typically for example for a full layer board will be much skinnier do we need to take these effects into account and what can we do to mitigate them then as usual clearance is very important also in rf design of course and we want to try and keep that separate from other for example analog or digital sections and lastly i'd like to briefly show you how we calculate values for an antenna by sd so for an active antenna we have to supply dc power to the antenna whilst not disturbing the rf part into the receiver our first point is the critical length and this is essentially telling us when do we need to take rf effects into account and when do we get phase changes across a section of our pcb essentially if traces are longer than a fraction of the wavelength of the signal of interest so for example for gps typical consumer l1 band which is about 1.6 gigahertz the wavelength is 19 centimeters so if the traces are longer than a fraction of that wavelength we need to start paying attention to rf effects and we need to take extra care this is often termed as a for example distributed element the question now is what is that fraction of the wavelength this is how we calculate the critical lengths and you can see there's two formula here first of all we have the strip line and the strip line essentially means you have an internal trace where above and below we have a reference plane a micro strip is essentially a trace on an outer layer where you have on the next layer underneath a reference plane now you can see here the formula is actually pretty similar the critical length is the speed of light divided by the frequency of interest times 1 over the square root of epsilon r epsilon r is the relative permittivity of the dielectric so for fr4 this will be something like 4.5 or 4.6 and then we divide that whole number we have here by 12 and this is then the fraction of that wavelength essentially for microstrip it's slightly more complicated we essentially have the same equation except that the dielectric constant here is called ef or rather the effective dielectric constant and this is because below we have essentially died trick of the pcb and above we have essentially air so it'll be a combination of those two dielectrics and there's calculators online that shows you how to calculate this but typically this value will be lower than just the dire electric constant of the pcb material so here i've done an example calculation for the gps l1 band now the speed of light is three times ten to the eight meters per second the frequency of the gps l1 band is centered at about 1.575 gigahertz and then i've used a calculator which i'll show you in just a second to calculate the effective dielectric content of this pcb then for a micro strip trace we can then figure out the critical length and this turns out to be just 8.6 millimeters so just under a centimeter and we already need to pay attention to these rf effects so this is something which is really good to know and really easy to calculate if you just google effective dielectric constant calculator you'll see a lot of pages where you can actually calculate this effective dielectric constant one of them is the first one here pasanak.com and we want to calculate the effective directory constant we need to know the directory constant of the pcb we needed to know the approximate width of our trace and the height between the trace and the next reference plane so the dielectric constant is easy we can just get that from our preferred pcb manufacturer a glc for this certain stack up it's 4.6 um the height between the trace and the reference plane is easy as well you can see here for a four layer board between the top layer and the first inner layer which is typically ground it's 0.2 millimeters the next thing is the actual width of the trace and essentially you need to calculate the correct impedance of the trace if you want a 50 ohm line for example and then put that width in here i already know it's about 0.3 millimeters to get a 50 ohm line so that's why i put that in here but i'll show you later how to actually calculate what you would need to do for a width for 50 ohm line or 75 ohm line and so on but essentially you plug these numbers in and this down here then tells you the effective dielectric constant which is about 3.4 and that's what i used in the previous calculations so here we are in keycad and this is the open seneca board and i'm going to show you this rf section over here effector we have a ufl antenna connector we have some sort of biasing network for the active antenna and that that then feeds into this gps module now the critical length was about 8.6 millimeters so let's measure how long i kept this rf section so i go from the ufl connector all the way into the pad and you can see that's about 7.6 millimeters which is below the critical length so here are the takeaways when we've talked about critical lengths before you start routing make sure you calculate the critical length in your design this will depend on your pcb stack up the frequency is interest if it's analog or digital and so on remember to keep rf sections and traces as short as possible to make sure that you don't get into this critical length domain if you can help it now let's look at stack ups for rf boards and we'll look at two of the most common scenarios the first one is a two layer board and this is a very very common scenario for rf boards or pure rf boards the reason being that we essentially have one layer to route our signals on and the next layer is then our reference plane which will be ground typically for two layer board for like a 1.6 millimeter board there's gonna be a large height between the trace and that reference plane this means in turn that for a 50 ohm line would generally need to have wider controlled impedance traces wider control impedance traces means there's going to be a better tolerance for manufacturing and also the trace width variations will have less of an effect on trace impedance if you contrast that to having very thin controlled impedance traces and then having the same manufacturing tolerances for those very skinny traces the alternative is to have a full layer board or multi-layer board above four layers and four layer boards are very very common in sort of mixed signal or embedded system boards which you see a lot where you might have a micro controller some various sensors and maybe a small rf section the difference to a two layer board here is that there's a very small height or much smaller height between the trace and the reference plane which means also your rf traces your controlled impedance traces will be narrower as well typically we'll probably be using microstrip lines instead of strip line because the internal layers for four layer board will be reserved for ground plane as well as sort of the power routing the nice thing with the four layers of course we have more routing layers for example the bottom layer as well also most embedded system boards the rf part is typically only a small section so for the open seneca design because it's a typical embedded systems board i chose to use four layers and that's more than sufficient you can see i have the rf section over here on mc over here and various different modules and sensors scattered around i have a routine on the top and i have rooting on the bottom and internally i have a ground plane also underneath the rf section and then i also have some sort of power distribution on another plane now let's look at controlled impedance traces and in particular we're going to look at two specific cases one of them is the microstrip line where we have a trace on an outer layer then we have a dielectric medium and then we have some sort of reference plane on an internal layer or the second layer of a two layer board this is termed microstrip the other common case is a symmetric strip line where we have the trace now on an internal layer and above and below on adjacent layers we then have reference planes for a typical embedded systems board or four layer board we will most likely go with a micro strip a strip line has several advantages over the micro strip it depends on the use case but i'd like to show you how to calculate a 50 ohm line or any impedance line with a full microstrip to be able to calculate the required trace width for certain trace impedance you need to know the stack up of your pcb you're using and this is typically given on the pcb manufacturer's website so for example for jlc pcb you can click on the control impedance pcb layer stack up in the capabilities section so if i open that up i'm using a four layer board of 1.6 millimeter thickness and here it is this stack up consists of this so we have a top layer of a certain thickness we have a prepreg in the middle then a second layer and so on and this is the information information we then use in combination with a impedance calculator to give us the required trace width so one way of calculating the trace width is going to keycad and then click on this pcb calculator over here so let me just open that then we want to click on transmission line and here we have to fill in all of our parameters so now i've put on the left side here the stack up of the pcb from jlcpcb.com and on the right side we have the keycad control impedance calculator i've selected microstrip as my line type and you can see here a diagram of the relevant dimensions first of all we need to copy over the relative permittivity of the dielectric and that is 4.6 the next important dimension is the height between the trace and the reference plane below and it turns out this is 0.2 millimeters and i've put that in here over where as well we also need to know the thickness of the trace and for typical one ounce per square foot copper that'll be a 35 microns or 0.035 millimeters and that's what i've put in here okay let's say you want a 50 ohm line and that's typical for rf systems and gps so i would like to type in z0 which is our characteristic impedance and then i click on synthesize and you can see we need about 0.35 millimeters to get a 50 ohm line based on this keycad calculator now jlc pcb also has a calculator for their boards and this is typically what i would go for because uh to me it's much quicker so i go on glc pcb impedance calculator i type in that i want a 50 ohm line a four layer board with 1.6 millimeters it's on an outer layer because it's micro strip and it's single ended click on this little arrow and i can see 11.55 mil is the recommended trace width and let's just convert that to millimeters and that happens to be about 0.29 0.3 millimeters so you can see there's a slight discrepancy between the glc pcb calculator and the kicad one they have various different calculators have different methods of solving these equations and solving for the characteristic impedance but as long as you're on the right ballpark you'll typically be fine so something around 0.3 millimeters now going back to the open seneca board and looking at the rf section again my main rf trace over here you can see the width of that trace if you look down here is 0.293 millimeters or about 0.3 millimeters and that's what we calculated using the jlc pcb impedance calculator the next topic is that of when you have a controlled impedance trace such as this thin 0.3 millimeter trace over here and that then of course sometimes has to go into component pads for example this rather large pad of this ufl connector or even this 042 inductor over here you can see there's quite a little jump from this trace to the pad or from this trace to this pad of this connector the question is does that matter because this will have a different impedance to this trace and this will have a different speed into this trace now i attended a rick hartley seminar or a webinar rather where he talked about rf design and i asked him exactly that question like do we actually need to take an account and his answer was no we don't in pretty much most scenarios especially low frequency situations like this the impedance discontinuities are so small and the critical lengths that are involved are so small so this is fine if you're not happy with this answer one way you can maybe mitigate the effects of having these impedance disc annuities in these large steps and jumps is something i've done here so instead of having a jump straight from the pad down to this trace i could start off with a slightly larger trace take it from the pad and move it in into the trace and this way we have a jump here but a rather smooth transition to the next trace and of course you can stagger these transitions so i could start with a larger trace and then this is a bit of an extreme example but then essentially carry it out like this and this way you have a as more gradual smooth transition into these controlled impedance traces but in general according to rick hartley and according to the experiences i've had you don't really need to worry about it at least at these frequencies but try to keep your pads relatively small or rather similar sized uh relative to your controlled impedance traces now of course if you're rooting on a two-layer board your traces will be much wider and then will accommodate these larger pads so there's a bit of a trade-off there a very important point when it comes to routing in general and also for rf designs is that of clearance and spacing and you can see in this board here i've tried to keep the rf section far away from the digital circuitry or any other bluetooth or wireless modules and just to give make sure to give it enough physical space so these circuits don't interfere with each other in particular that nothing interferes with this very sensitive gps section over here now the power section might be a bit close but i've tried to place the inductors which could radiate more magnetic field lines further away from this antenna section so try to keep space between the rf section digital sections analog sections so on that's generally a very important rule in pcb design and finally let's briefly talk about bias tees so typically we'll have an active antenna with a gps module to improve reception and an active antenna is basically passive antenna which includes some sort of filter and a low noise amplifier and this low noise amplifier and this filter or primarily the low noise amplifier needs to have some sort of power applied to it in form of dc and typically we want to superimpose the dc on the rf signal and the way we do that is via a bias t the bias t essentially we take in dc signal pass it through an inductor which effectively idd should block rf and then we add that together so to speak with the acrf signal which is past this capacitor which blocks dc but let's ac through and the sum of these two signals is then passed to the antenna so the antenna can receive the rf but it can also be powered by dc now the inductor makes sure that no rf signal goes back into the power supply but it lets dc through and the capacitor makes sure that no dc signal is passed into the rf receiver front end but of course that the rf signal can pass through at ac frequencies and the question is how do we calculate the values for the inductor and for the capacitor now this question unfortunately isn't quite as straightforward as i would have hoped there's three ways of going about this firstly it's simulation and this is probably the best way of doing it but that involves rather expensive rf simulation software so maybe we'll pass on that for now secondly the best option is the data sheet the data sheet from a gps module will typically tell you the values and i'll show you a second that it did in my case of what values of l and c and so forth to use if you don't have any of these of this information you can use the rule of thumb and i'll quickly show you how to do that now so here's the rule of thumb for given characters to compete in said naught so for our system that will be 50 ohms and a frequency of interest f which will be about 1.575 gigahertz for the gps l1 band we need to make sure we do two things first of all we may need to make the reactants or rather the ac resistance of the inductor much bigger than these 50 ohms at the frequency of interest so to make sure that at that frequency the inductor behaves as an open circuit the other thing we need to think of is the capacitor and we want to make that reactance of the capacitor or other the ac resistance much smaller than that impedance at the frequency of interest and that makes sure all of the ac signals pass through the capacitor with minimum loss now remember this is just a rule of thumb and in more sensitive systems you need to really take care of impedance matching and so forth but for simple systems like these consumer gps modules this is more than fine here's one of the gps modules i used and also the one i used on this open seneca board it's fairly inexpensive and jlcpcb has it in stock for only a couple of dollars and if i click on the data sheet and scroll down a bit you can see there's some typical application circuits and this includes part of the bias t so you can either have it with a passive antenna and an extra low noise amplifier or in my case we have an active antenna and we have a really simple bias network you can see here they give you the value for an inductor but they're not showing a capacitor this is because the capacitor is actually included in the module and sometimes this is the case sometimes it isn't but the best thing is to always check the data sheet to make sure they might give you the values for lnc and it did in this case and that's exactly what i did then in this board essentially i only have i copied the circuit and took this inductor value of 47 nanohenries and the circuit works completely fine

Channel: Phil’s Lab

Views: 59,248

Keywords:

Id: _Hfzq1QES-Q

Length: 18min 45sec (1125 seconds)

Published: Fri Feb 05 2021