KEYNOTE: Where High Speed Meets High Frequency - AltiumLive 2022
As many design teams may have experienced, high-speed designs are confronted with many of the signaling and layout challenges seen in high-frequency designs. High-speed interconnect design should take a similar approach seen in high-frequency design with respect to losses, impedance determination, and analysis.
In this technical session, I'll explore some of the correspondences between high-speed PCB design and analysis as they relate to the fundamental concepts in high-frequency design. Topics like interconnect design, measurement, and analysis will be examined while comparing the design approaches in high-speed and high-frequency PCB layout and routing. The goal is to help high-speed design teams become more familiar with the conceptual explanations for why very high-speed signal integrity problems occur and how they can be overcome with some smart design and layout decisions.
Hello everyone, and thank you for attending my session. I'm very happy that Altium asked me to present at this conference. And I think this is going to be a lot of fun, especially now that it is a virtual format. My name is Zach Peterson. I run Northwest Engineering Solutions. You've probably seen me on the Altium Academy YouTube channel talking all things, PCB design for new designers. I also work with some external publications producing similar types of educational content. And the topic for today that I want to address is the correspondence between high speed and high frequency design. Both topics that are near and dear to my heart. For those of you that know me, you know I have a background in optics and lasers, and that really primes you to work in high frequency design because many of the concepts and of course the mathematics are all very similar. So, that's what I'm going to be talking about today.
On the agenda, the very first order of business when we start talking about this type of topic is to provide a very rigorous comparison between digital and analog signals, specifically within a PCB. And I think that's the first place to start because it reveals some of the justification for various design choices and why when you look at a digital board it looks very different from a radio frequency board or even just a lower frequency analog board. Then what I want to talk about is materials and PCB stackups. Materials are very important for RF design. They're important for high speed design too, but they're typically the cornerstone of RF design, and we'll see why that is the case. And I'll actually provide some examples that are fun to look at.
And then I want to discuss probably the most important part of RF design, which is impedance and propagation. And impedance is certainly a topic that is near and dear to my heart. If you've seen any of my videos on my personal channel or attended any conferences with me, then you know I often talk about impedance, and specifically models for impedance. And so we'll actually dig a bit deeper into the standard transmission line model, because I think this is something that most designers, whether you're a digital or RF designer, really don't get exposure to. It's one of those things that's buried in the research literature. And so my hope that I can help designers understand a bit more about where that formula actually comes from.
So first to really start is to compare digital and analog signals. And I've listed millimeter wave here on the right, but the same kind of ideas could apply to any analog signal. So first with digital signals and analog signals, when we compared them, the first order is to compare the bandwidths. And when I talk about bandwidth, I'm not talking about data rate when I'm referring to digital signals, I'm actually talking about the frequency components that make up a digital signal. So I'm sure if you are a digital designer, you've seen a Fourier series representation for a digital signal, which is basically a bunch of frequencies that add together to give you the time domain representation of that digital signal. Digital signals are very poorly defined bandwidth, because in theory, the bandwidth extends all the way to infinity. They have infinite bandwidth.
Now, only a portion of that bandwidth actually matters because what really matters in the digital channel is what the receiver can actually receive and interpret. So the receiver as well as the structure of the channel itself actually limits the signal bandwidth, or limits the signal to only transfer power to a component within a certain bandwidth I think is the right way to think about it. Now, millimeter wave, microwave, really any analog signal has a very well defined signal bandwidth. The bandwidth is just the carrier plus whatever the modulation is that's applied. The carrier just carries the wave, and that's really the wave that you use for analysis, and then there is some modulation that's applied that carries the frequency. Contrast this with digital, you actually don't really know what the frequency you should use for analysis is. That is the eternal debate that comes up when I'm talking to newer designers, is do I use the clock frequency, do I use something with the rise time?
Really the answer is none of it. There is no specific frequency that you have to use. You have to consider all the frequencies. And so there's some tricks to doing that. The signal level also carries the information in a digital signal. So obviously with binary signals, you know signal is off, it's a zero, signal is on, it's a one, unless you're active low and it's reverse, and so on and so forth. You can extend that all the way up to PAM4, where you basically have four signal levels. So you're carrying two bits in a single unit interval.
And then there's something important that happens when you start dealing with high frequencies, which is dispersive losses. And so when there is any signal content at high frequencies, there will be some dispersive losses. And what I mean is that the loss depends on frequency. So different frequencies will experience different levels of loss. Now, in a millimeter wave channel, or just really in an analog channel, you probably won't notice a difference because you're only working at one frequency. You don't have any other frequency around to really compare, okay? Or you're just working in one frequency plus a very narrow bandwidth. So, really take any analog signal, the bandwidth is very narrow around the carrier frequency. We're only worried about that narrow bandwidth. But with a digital signal, we have to consider the entire bandwidth. And so, I've talked about this in some other presentations. I'm going to focus more on the millimeter wave in this presentation.
So digital signals are also analyzed in the time domain. And the typical way you do this is either with simulations or measurements, sometimes with an eye diagram, sometimes with spice if you're designing just circuits, really depends what you want to design and what you need to look at. But generally you look at the eye diagram and how the eye diagram becomes corrupted, let's say, as signals travel through PCB and then eventually reach their destination. And there's all sorts of metrics that get used. Inter-symbol interference, insertion loss deviation, channel operating margin are all popular for various high speed protocols. But S-parameters are actually a frequency domain analysis that are actually very useful and the standard for analyzing a channel, which you can then apply to a digital signal if you like and figure out a bandwidth limitation in the channel.
And basically as long as the channel has enough bandwidth such that the signal needed by the receiver can reach the receiver, then the channel should work. Now, obviously you want to test this more deeply, but that's the high level of what we care about when we talk about bandwidth in a digital signal. With a digital signal, the bandwidth and of course the reconstruction of the signal and the time domain during a measurement is related to this rise time. So this should not be new to the audience. And of course the rise time determines all of these other effects. And so I mentioned Gibbs when I just started with this slide, but of course it also affects crosstalk, radiated emissions. You can see this transient phenomenon here.
And then in some cases you have resonant phenomenon. And this is really where there's a powerful correspondence with RF design, because RF design really relies on propagation and in some circuit elements that you create resonance. And so we'll talk about that more later in this presentation. Now, with digital, I love showing this particular slide in presentations because it really does show how far the bandwidth spans and how much of the bandwidth matters. And even though the bandwidth spans out, well, here we're going to like 500 GHz on this readout that's been computed with Symbio, really a portion of this is what matters.
And it still goes up to high frequencies as you can see here. However, this portion that really matters you can see is up to the Nyquist. And then everything above that causes interference and signal integrity problems elsewhere in the board. So this particular power spectrum is just the power spectrum density of this pseudo random bit sequence being fed in. And then you can calculate the power spectrum from this. And so, of course the magic question here is, what is the bandwidth? And this is really what is the frequency that you should use for analysis. And the answer is, really it's the maximum frequency that matters here and which I would say is the Nyquist frequency for this particular signal.
Now, with an analog signal or with a wireless signal, whatever it may be, we have really just one frequency that we worry about, which is this carrier plus some small bandwidth rounded, as I mentioned before. And so if we were to take this signal, put it into the PCB, and then maybe read it out with a spectrum analyzer, something like this at the receiver, this is what we would see on the right, so on the lower right side. And this is important beyond just wireless. I mean, I mentioned 5G and upcoming 6G deployments here in the examples.
However, quantum computing uses not horribly high frequencies. I mean, Intel's quantum computer operates at 20 GHz signaling, not very high. Short range radar and long range radar are both higher than that. And I'm sure there's someone in the room that's worked with one of those products. There's also very fast multiple gigabit wireless systems. So this is 211 standard up to very high frequencies. And so there's all sorts of other examples that you can pull out. Most people just focus on something like wifi or Bluetooth, which is fine. I mean, that's so many products work with that. But the same principles are really universal.
So to get started with a design where you need to ensure that you can transfer a signal across the PCB from a transmitter to a receiver, where do you start? Well, my process beyond just figuring out the topology or the circuits that are going to be needed is really to think about a material, because whatever you want design has to be fabricated, and you need to make sure that you select materials that are compatible and that you can actually get produced somewhere either because they're number one in stock, obviously that's important, but also that the fabricator that you like to work with actually can get them, or has them, or they have a process that accommodates them, and you can do it in a cost effective manner.
So here I've listed some particular materials here that are either marketed as high frequency materials or they fall within I think what most designers believe to be an acceptable range of values for a high frequency material, okay? So up at the top, just for comparison, we have FR4. And then we have the set of Isola and Rogers laminates listed down here. And I particularly like some of these. One, the laminates that I tend to like for this, but really will depend on what the circuit needs to do. And so this is very important because if you ask somebody what is the best material out of this list for an RF design, probably everybody will say, "Oh, well, it's going to be the one with the smallest DK value, probably this Rogers 3003." Most people will say that.
And this material has its uses. What's really important here is to take both the DK value and the loss tangent. And most people just focus on just the DK value or just the loss tangent. And they'll say, "Well, I'm just going to go with the Rogers 3003, because it has this very small decay value and a very small loss tangent." Now, the low loss tangent is important, but it's really important to minimize loss tangent when you're propagating a signal over very long distance, because those losses add up over distance. And so if you want to minimize loss, well you then have to focus on minimizing the loss tangent in the material, and then design the channel to also have minimal loss.
So that's an acceptable application of a lower DK material. But what's important to note about the DK value is that it will actually determine the size of the signal, meaning the wavelength of the signal in the PCB. So that's very important because RF circuits rely on the wavelength of the signal that you actually want to put into that printed circuit element. And I'll show some examples here in just a moment. But if you have a larger DK value, you actually get some benefit in radio frequency design if you want to minimize the size of that design.
So if you want to make your RF circuits smaller, you actually want to use a larger DK value. This totally goes against conventional wisdom. Most people would say you should never use a large DK value when you're doing radio frequency design. But you have to really think about what you want to do with the design. And if your design needs to have minimal footprint, then you should actually go with the larger DK value because the larger DK value will correspond to a smaller wavelength for a given frequency.
Now, just for a moment, let's compare the loss tangent here. If you're familiar with the definition of loss tangent and how that relates to actual losses, you'll know that the loss tangent is the ratio of the imaginary dielectric constant to the real part. And so if I factor out the real part from the loss tangent, I actually see that I still have about a factor four lower losses compared to FR4, even with this RT Druoid 6010.2 material. So even with a high DK material, I can still get to a low loss situation and do better than a standard FR4 laminate.
So how do we represent dielectric constant? This is really the important parameter that you will typically look at when you're selecting materials and then send a stackup off to your fabricator. We model the dielectric constant using something called a Kramers-Kronig relation, which I mean, if you've never done this type of integral, it's ugly, it's the type of thing you'll probably do in an optics class. So I won't show any of the mathematical details here. But the important point is that it produces this standard model called the Wideband-Debye model. And commercial field solvers, impedance tools like Polar, as well as the Altium Layer Stack Manager tool include this model or some version of it, some closely related version. And if you graph out the values for a typical FR4 laminate, it will look like this lower right graph. And this lower right graph shows you the real part and the imaginary parts, and generally how they will behave as a function of frequency.
And so you don't necessarily need to calculate this on your own. If you are using the right impedance tool, it will include this for you and run that calculation for you. So, now that we know how the material or how to select the material, you need to put them into a stackup. And then obviously with stackups, they need to be producible. So I like to show this example because this is a stackup that we've actually done for radar boards for little radar modules several times throughout 2021. I don't know why so many people were coming to my company requesting radar modules in 2021. That's what they did. This or some version of this was a pretty common stackup. And this stackup is actually a hybrid stackup. And so this is one way to integrate RF circuits onto some other type of board and put all of this into one stackup. Instead of going all Rogers throughout every single layer and every single area of the PCB, you can actually just put Rogers on one layer or some other laminate on one layer.
Now, obviously you want to check with your fabricator to make sure that this type of thing can actually be produced and then it can be produced well really anywhere. However, there are reference products or evaluation products, I should say, from certain semiconductor companies that use either this stackup or a very similar stackup. So this type of six layer stackup. And so, obviously is producible somewhere. And it's a good choice if you just want to have RF routing on one layer. So in this case, it would be the top layer, and then we have our ground plane to set the impedance, and then we have our other layers that are useful for other types of signals. Maybe on this layer four, we do something with low speed digital. Maybe we do high speed digital on the back side. Whatever the case may be. But this is a good example for a radar board with some digital sections.
So, you can also take this and invert it. So this stackup that I'm showing here with three dielectric layers, it basically takes the typical four layer board and inverts the thicknesses. And by that I mean instead of putting a thick core layer and then thinner outer dielectrics that actually turned this around, and we've taken the thicker dielectric layers, put them on the outside, and then put a bond ply on the inner layer. Now, you might ask, well, why would you do that? The standard four layer board has the very thick core, and then you go maybe seven mils or something on the outside layers.
Well, the reason you might want to do this is because you can actually produce wider traces on the outer layer. Those wider traces can have lower inductance, they can have lower skin effect that can be beneficial for losses. In addition, you can get a standard low loss laminate, in this case it's Rogers 4350B, in this somewhat thicker dielectric and put it in on the outer layer. So it's readily available. So this is also a good type of stackup to use if you need RF on two layers. So here we can do RF on the outside and we can do RF on the bottom layer. And we have two ground planes to provide some nice separation.
So, the next aspect to consider when selecting materials, particularly glass weave materials, should you choose to look this deep into your laminates is the potential for skew. And this is really where we like to compare what happens with digital and what happens with RF. So in digital, skew can be unpredictable. And what I mean by that is, if you are in your CAD tool and you're trying to lay out these two traces, let's say these are part of a differential pair, the skew that you actually get when you produce the board is actually relatively unpredictable if you are using a very loose glass weave. And that can be problematic if you're working at very high speeds that will then cause the two signals or the two sides of the two opposite polarity signals on each trace to become out of sync. And they may not be read correctly at the receiver. So, as a result, you would want to go with a weave that is thicker. You would want to go with something on the right which has smaller cavities or basically no cavities in this case.
Now, in the case of an RF board, if we look at the laminate on the left, what would be the problem with this? Well, there's something called periodic loading that it has been used in the literature. And what that term means is that you essentially could excite some resonant cavities or excite some resonance in these cavities, I should say, that make up this dielectric weave. And so all of these cavities that make up this weave can couple together to produce some very odd peaks and valleys in the return loss spectrum.
And essentially what you have here is when you get to very high frequencies, what happens is you then will excite some resonance and that could create these return loss peaks and valleys. So this has been looked at in literature. There's actually an article in signal integrity journal that looks at it. And this is a resonance effect that happens in RF. And so what you would also want to do is to, if you're going to go with some type of glass weave like this, you would then want to use a thicker glass weave. Essentially close up these holes like we've shown on the right. So, the problem in digital and RF is different, but the solution is the same. The solution is the same, to get rid of these cavities.
Next on the list of materials. So as you go through and you look up your stackup, the next material that is very often overlooked is the solder mask. So even at small wavelengths as well, actually especially at small wavelengths, I should say, which corresponds to high frequency, the solder mask matters significantly. And if you look at I don't care if it's stock photos of RF boards, or you look at maybe some professional RF boards, or even reference designs or evaluation products, typically what you'll see is that the solder mask is removed from elements that are carrying signal. So from the emitters, basically if it's like an antenna or if it's a receiving antenna or from waveguides.
And so that is removed because if you actually look through this list of material properties, what do you see? Well, we see down here the dielectric loss factor or in other terms the loss tangent is actually quite high. And this is just measured at one MHz. So this is comparable to your basic FR4. And remember, we typically have about 0.002. So an order of magnitude lower for RF substrate materials. So this is actually pretty high, and some would say of course unacceptably high. And so, because of that, we like to remove the solder mask from those portions of the design or from the conductors that are part of waveguides, I should say, or that function as emitters for RF signals.
So the next portion of the material system to consider is the roughness. So the roughness depends on the number of factors. And if you're just looking at the bare copper on a laminate, the roughness depends on the process. And when I say the process, I mean is it reverse treated, is it electrodeposited, is it rolled copper, is it additive? I would say one of the leaders in this area, his name is John Coonrod, he is encyclopedia of knowledge on this type of topic. And if you ever have a chance to see him speak at a seminar, you should definitely do that. The data on the right shows some of his work comparing two different types of copper, rolled copper and electrode deposited copper. And what we're looking at in this graph is the loss. And what's really different between these two coppers is the surface roughness.
So the surface roughness for the rolled copper is actually much lower and it can be measured in terms of an RMS roughness. And that can be done with a profilometer. It could also be done with an anatomic force microscope. When the surface roughness is much higher, you actually can see here in this graph, you get much larger loss. And at low frequencies, maybe you're at a few gigahertz, these curves essentially overlap. I mean, you'd want to zoom in here to see a real difference. But basically they overlap for this particular substrate. And it's only once you get to very high frequencies that you start to see a really serious difference.
Now, remember these are in loss per inch, right? So this is in DB per inch. So the longer your waveguide or your trace or whatever, your element is, the larger that circuit is, the more loss you'll see. Now, you can actually also visualize the roughness in SCM images. These were provided by Oak-mitsui. They're a maker of embedded capacitance materials. But they've provided some data here that at least shows what the surface roughness actually looks like. And it's not just these kind of peaks and valleys, it's also the particles that make up this surface roughness that matter. And so there are actually models that you can use to account for the roughness when you're calculating impedance.
So ideally we'd like to be as smooth as possible. But for those of you that are obviously familiar or more familiar with fabrication and with surface finishes, you will know that once the surface finish is applied, that will also determine the roughness or could influence the roughness. Now, the roughness is important because when an RF signal propagates along one of these circuits or along this conductor, what happens is we have a skin effect. The skin effect refers to the tendency for charge that is associated with that signal to cluster along the edge of the conductor. Or you could say along the skin of the conductor. And if the conductor is rougher in that area, then it will see more impedance and we'll see more loss. So that is the problem with roughness.
Now, obviously the roughness is not just going to be from the copper, but because of the plating, the plating will also matter. So different platings produce different levels of roughness. And so this is another material choice that needs to be made when planning an RF PCB. Same goes for digital PCBs. With the digital PCB, I think most people just default to something like ENIG. I know I do, especially if it's much lower speed. But if you're getting up to higher frequencies, you definitely want to go with something like just the bare copper plus organic solderability preservative, or bare copper plus immersion silver. And then here we're actually comparing not just the copper plus immersion silver but with copper plus the solder mask. And so we can see what the solder mask actually does at high frequencies. You can see that it actually causes increase in the losses out here at 35 GHz.
And again, at low frequencies, they overlap. And so it's not a huge change, especially if you're going to be doing small routes, probably not really going to matter. But if you're working at higher frequencies, then it really does matter. And these are not crazy high frequencies. We're not talking about hundreds of gigahertz. We're actually talking well within the purview of digital bandwidths. So digital signal bandwidths definitely span into this region where my mouse is, and that particular region will experience more loss if you're not using the right plating.
So where does this plating problem come from? Well, it's certainly a problem with nickel-based platings. And so that's one of the reasons that ENIG and ENEPIG are so low on this graph. And you can actually see how the roughness arises when you look at these SCM images. This data on the right, I believe also provided by John Coonrod. So again, go listen to John Coonrod talks about copper and laminates and RF if you ever have a chance.
Now to the fun stuff. So once you've figured out everything that you're going to use to build the PCB, all of the materials, the next thing you have to do is you have to figure out impedances. So this is important both for simulation, just for basic design, as well as if you're going to be testing your own boards for test and measurement. If you know the impedance and you know the propagation constant, if you really want to, you can calculate all of the other metrics that you would need to use to qualify your board during testing. And you have everything you need to do some basic simulations. And so that's another topic that I'll almost likely present at another seminar, hopefully at the future Altium Live. But this is really the basis for network analysis that you would do with something like S-parameters or another parameter set.
Now, what I'm showing here on this slide is at the very top, the basic equation that you get for impedance and propagation constant from the telegrapher's equation. So the impedance, it has just this really common form here. And this is universal for all transmission lines. I don't care if it's on a PCB or if it's a high tension line hanging from a power pool, this is the equation. And then there's an associated propagation constant that is related to these same circuit parameters, okay? So, the circuit parameters are further expanded as these four equations that I show here. And we have our resistance, which is actually a function of frequency, and I know they tell you in Electronics 101, that resistance is not a function of frequency. However, the skin effect does create a frequency dependent contribution to the resistance. And so that's what this RS is here. This RS value can be calculated geometrically, and it does contribute to the resistance.
The RS value also appears in the inductance for the transmission line. So the inductance is dependent on the inductance at infinite frequency, that's just going to be some number, plus this additional contribution from the skin effect. And this skin effect contribution is incomplete. And what I mean by that is it doesn't account for roughness. So I will explain what that means here momentarily. And there's also this frequency factor here. Then we have our G value, which is like a parasitic conductance. It's not really a conductance. What it really does is it accounts for the loss tangent. And we have our capacitance, which also relates to the other part of the dielectric function.
Now, this is a model that I've presented several times, and it actually does get pretty mathematically intense. So I won't go too deep into it. But the basis for bringing all of these material constants into this model can actually be found in this IEEE paper that I've cited down here at the bottom of the slide. So if you want to look at a very interesting paper that provides all the mathematical basis for this, I encourage you to go read this paper. The other piece that we have here is the dielectric constant. And you'll notice here in this definition for the dielectric constant, I've used a positive here. That is the mathematically correct way to write the dielectric constant. I don't know why engineering textbooks continue to put a negative sign here. That is wrong and I wish they would stop doing it. It has to be a positive sign here. It means we put this negative sign here in the loss tangent. So loss tangent should really be a negative number.
That's just me as a physicist complaining about how engineers write their textbooks. So ignore me if you want, or during the Q&A session, you can ask me about it further. But regardless of whether you put the plus or minus here, you need a model for the dielectric constant, and specifically you need what's called a causal model for the dielectric constant. And so the Wideband-Debye model that I presented in the earlier slide that I referenced, and that is used in programs like Altium Designer, like Polar, and some other tools, that model is a causal model. And so we can get a dielectric constant.
The other thing that we need is the copper roughness. And then we can get the electrical parameters once we have the copper roughness, because you can see here, the skin effect resistance is incomplete. It relies on this copper roughness value, and that'll give us the electrical parameters. And then if you wanted to, you could actually calculate the impedance by hand. You don't have to do this, but this is really the basis for understanding why you get more loss when you have rougher copper and things like this.
So what are the standard models used for copper? If you have read anything from Bert Simonovich, he is by far the expert in rough copper. There is also an excellent paper from Signal Integrity Journal that looks at how this model is derived. And so if you're interested in the mathematics that justify this, I encourage you to read both of these papers that I've cited down here at the bottom of the slide. Now what's important here is that when you're accounting for the skin effect and how copper roughness modifies the skin effect, you're basically just applying this transformation. You're basically saying, "Hey, the copper roughness that this K value, this factor, is just going to multiply to my skin effect to produce a larger skin effect." Okay. So when we have rough copper, we need to figure out how to do something to counteract that either by using a different type of coffer, right? So instead of electrodeposit, maybe used rolled, or we redesign the stackup in the transmission line so that we can overcome that additional loss at certain frequencies due to the rough copper.
And so this correction factor can be defined just based on these models that look like essentially just stacking spheres on each other. But the Cannonball-Huray model is one of the main models that is used here. So if you're inside the layer stack manager in Altium Designer, and you see some roughness model that's being referenced on the right side of the screen when you're using the impedance tool, this is the kind of thing that it's talking about. And all of this is built in there. Other tools I believe do something similar. They'll work in this model and they'll actually calculate the correction factor for you. And then it will get included in the impedance calculation that I showed earlier.
And basically the effect of roughness is not only to modify the skin resistance, it also modifies the dielectric constant a little bit. And this little bit that it modifies dielectric constant by, just depends on the extent of this roughness and how far it extends into the laminate. So this rough DK value is essentially just slightly different based on the difference between the nominal thickness of the dielectric minus this H10 value. What is this H10 value? Well, this H10 value is the 10 point roughness measurement. Again, this is something you can measure with a profilometer. You could even measure it using image analysis. You could measure it with an AFM. The point is it can be measured and it can be quantified.
Now, how do we actually use all of this? Well, in a digital channel, it gets really complex really quickly. And this is one of the reasons why RF designers have it easy. In a digital channel, as I mentioned earlier, we care about all these different frequencies up to some limit, Fm. So this Fm just refers to some maximum frequency that we care about within our signal bandwidth. And so we'd have to take this big, long integral. And if you're not a mathematics person, you're probably looking at this and being like, "Why? Why would I have to do all of this?" Well, these are actually specified as evaluation parameters in much faster signaling standards. So one of these being integrated return loss, essentially what you're doing is you're using the S-parameters for the channel and the power spectrum for the input signal as a way to measure and check that you are actually hitting a return loss target for that standard.
Same thing goes with the insertion loss. We have this value or this integral here that looks at the S-parameters, S21 for insertion loss. And then we have another one for integrated crosstalk. So all of these metrics are taken over very wide bandwidth when you're looking at digital channels. Talk about difficult if you're not a mathematics person. Now, RF design, we don't care about this entire set of frequencies, we only care about the one frequency that we're looking at, which is the carrier frequency. Really it's the carrier frequency plus a small range around the carrier frequency. But that range of frequencies is generally so small that we can just look at the carrier frequency and we can usually get very accurate. Obviously you want to test that, but you can usually get to very high accuracy with just looking at the carrier frequency.
So, how do we want to route things? Well, for RF we typically prefer a coplanar arrangement or a coplanar arrangement with ground, coplanar arrangement with ground is really the preferred way to do it, or a microstrip line. And so if you look at a lot of RF designs, the microstrip line is typically used, but you can do things coplanar arrangement. One of the ways that you have to try and design this, if you're going to do coplanar is to do coplanar with ground, or grounded coplanar way, God, I should say. So this type of structure essentially just applies a fence around this signal. So remember the field for this that is carried along this trace, this center trace, it exists around the trace. You're not actually worried so much about what happens on the trace except for where charge budges up.
But it's the field around the trace that gets confined within this structure. And as long as these vias that make up the structure are spaced close enough, then you can expect very high shielding effectiveness to be provided by these vias. And so this is one instance where copper pour is actually needed to set the impedance of this trace to the required value. That's the impedance of this structure to the required value.
So just some examples here of how you can route things. This image on the right is a stock image, but I like it because it has some good elements to it as far as how to route things. And you see this reflected on some of these test boards that we've built. So this top test board is for a low band filter section. These chips here are actually integrated low band filters. And then that filtering circuit is essentially being tested with this top board. Here within this section, we set the trace impedance to the desired value using this copper pour with vias. So, in the previous image where I just showed one row of vias, that's not the only way you can do it. You could actually do it with multiple rows of vias like we've shown here.
The other possibility is to use a structure like this. And so in an earlier Altium Live Talk from a couple years ago, Rick Hartley mentioned this structure on the bottom. This is called a substrate integrated waveguide, and substrate integrated waveguide that are very fun to work with. They can act as edge emitters. So basically this right edge can actually be an emitter. You basically have a big antenna here, or you can put slots in this. You can put apertures in the surface of this, and that can also make an emitter. And you could basically, if you wanted to make like a passive phase array with this emitter or with this structure. So it's a very fun structure to work with, and it provides very high isolation. So these are two other boutique options, if you will, to route RF signals.
So just an example here that I always like to show is with a radar board. And these are two different boards. These are not the same. But here on the RX and TX sides in the left, you can see this is coplanar routing going to the center fed patch antennas. On the right, we've essentially done the same, but with blind vias. Typically you would do through-hole vias. But with this you're going to be able to do blind vias and do it just fine. The blind vias essentially line against these traces. Here we've got a thin dielectric. And by doing that, we're able to set the trace impedance to the required value for this feed line.
If you're a radar person or an antennas person, you might be wondering, "Hey, why do you have, what is this, six antennas over here and these two aren't connected to anything? These are for directivity." So that's more of a point of antenna design that we won't get into. But these are just some examples for how you can actually route this stuff within a region of copper pour. And so this chip here, that's outlined in yellow, this is the transceiver chip. And you can actually see it actually comes up to a set of other traces here on the bottom side. These are all the data input traces. And so this is routed in such a way as to really section off the RF stuff from the digital stuff so that they sit in different areas of the board.
So you'll notice that there's a lot of talk on earlier slides about copper pour and RF lines. And one of the things that the astute designer should note is that there is some parasitic capacitance between conductors. Whenever you run two conductors next to each other, there will be some parasitic capacitance between them. What it will do is it will essentially modify the impedance a little bit. And the basic function of capacitance is to reduce the impedance by acting like a low pass, or I'm sorry, like a high pass filter when places a shunt element. Now, the question here becomes, is this spacing too small? That is a good question. What spacing should you use? Let's assume that you want to put a 50 Ohm line here and you have some copper pour around, but you don't want the copper to modify the impedance or propagation characteristics of this RF line. How close can you get?
Well, what we can see if we actually look at some data and look at some field solver results is, with that we can violate the conventional 3W clearance rule. So in the history of PCB design rules, a lot of rules are some number and a letter. And they're talking about a clearance. One of those is the 3W rule. And there are actually multiple 3W rules depending on what type of routing you're talking about. This is one of the 3W rules. And basically the 3W rule says that this distance in yellow should be triple whatever the width of this red line is.
Now, really the clearance that you can have without modifying this 50 Ohm impedance target for this type of line depends on the dielectric thickness. And so as you make the dielectric thicker, you can actually have a smaller clearance or smaller minimum clearance and still bring that copper close to the RF line without modifying the impedance. But then the next question, what about losses? So losses are reduced with smoother plating as we saw earlier. However, what effect does that have if we then have charge clustered along the edges of this trace, and then we have the field terminating at the nearby ground region? What happens then? So that's actually something that you can look at with measurements, and as it turns out, the same type of effect that we would expect if we had just swapped out ENIG for emerging silver doesn't change if we bring in these regions of copper, as long as we're using a smooth enough plating. So this is another reason to prefer OSP or immersion silver with RF designs.
So, the next question that often comes up is with routing. Can I route into internal layers? The answer is yes, certainly, you can definitely try to route into internal layers. Obviously, if you're going to do any kind of creating routing with the high frequency designs, you should build a small test board for that interconnect and you should actually test it, because as you go through that route, these individual sections of the via will actually have their own S-parameters. And those S-parameters can be measured and you can compare them. And what happens here is in this via barrel, this via barrel essentially acts like a small resonator. It's essentially like a small transmission line.
So, typically if you are going to do this type of transition, what you would prefer to do is actually route deeper through the via. And the reason is that you could actually get to a point where you don't need to totally back drill this. Now, 0.1 millimeter sub length, if you actually calculate the quarter wavelength or the lowest order resonance in that quarter or in that 0.1 millimeter stub, that's fine for signals up to about 150 GHz on a typical FR4 substrate. So, that stub length is going to work just fine. So if you can route all the way across the substrate and use the internal layer that way, then that's okay. And the same guidance would apply. I would give the same guidance to digital signals. If you were going to make a via transition with a digital signal, try to go deeper. So that way you don't have to do back drilling, because during fabrication, I should say, back drilling can get expensive.
So we can actually see the effects of a via when looking at S-parameter measurements. These results were actually produced for a dim connector by a friend of mine at Ansys. And he was nice enough to provide some of these results. And clearly with this via stub at about 8 GHz, you can see very clearly what happens to the signal. There's this huge dip. And so this particular stub would only be useful for low data rates, which would then correspond to lower bandwidth than the digital signal. So this particular channel would not be very useful for high speed DDR.
So, this is a case where, again, instead of routing through the via if possible, we need to redesign the interconnect. And we would get the same problems with RF. But what's interesting about this is that eventually there's this kind of mid-range region with RF where we can still use this channel even if it has the via stub. But if we were to extend this frequency graph out to much higher frequencies, we would actually see this resonance appear again, and we'd see them appear in succession. And that's because this stub is a resonator.
So all RF PCBs could have some kind of unintentional radiation. And that could arise due to unintentional resonances. And so this is why the wavelength and frequency of our signals is so important. It can interact with the structure of a PCB and produce a resonance where you didn't expect, and that can produce a lot of noise. Eric Bogatin in his really excellent talk from Altium Live 2020, he pointed out some really excellent simulation results that he did with a student that showed this type of unintentional resonance occurring with essentially a thin guard trace and a via fence. And that's a really great example of how it can arise in a digital signal. The same thing could happen in an RF system. Instead, what you actually aim for in an RF system is you want your intentional resonators to actually resonate at your desired frequency.
And so, there are some examples here of intentional resonators, which are your antennas. So your antennas are essentially going to resonate and emit radiation very strongly at specific frequencies, waveguides. Waveguides we like to set up specific wave patterns inside the waveguide, because sometimes what you're doing with the waveguide is, like I mentioned earlier, you might be using the waveguide as an emitter, or you may be coupling that waveguide to another circuit, which will then act maybe as a filter. And then that will go to an emitter or something like this. Whatever the waveguide is doing, it's going to rely on transferring a specific electromagnetic field pattern between different portions of the design. This is not something that you generally do with digital signals.
With digital signals, we want to avoid all of that stuff with resonance. And we just worry about propagating a pulse from point A to point B. Very different with the RF design. So this is really a fundamental principle, is that, with RF designs, you actually care much more about the wavelength. And so this is why I brought up the potential for using very high DK materials for RF design and how they can be beneficial. Because if we want to take this big structure here and reduce the size of it, even for a low frequency, we would have to do what? Well, we'd have to reduce the wavelength of that signal. The easiest way to do that is to go with a higher DK laminate material.
So all channels also have some dispersion. And the dispersion and the phase response will affect coupling between different RF circuits. So all channels have the dispersion means that the propagation characteristics are a function of frequency. And being a function of frequency, that means that the speed of light or the speed of the signal in one channel is not going to be the same at different frequencies. And so that's quite important if you're worried about coupling at a specific frequency into a waveguide like this I've shown here on the right or between two circuits on a printed circuit board.
And the reason for that is because, if you calculate the wavelength at one particular dielectric constant but that dielectric constant is taken at the wrong frequency, then you may not get the most efficient coupling between circuit elements in your RF board, because you actually have a different wavelength than you were expecting. And that's because you weren't using the full set of dielectric information. And you can get that information from material manufacturers. So if you're going to be doing anything with RF designs, make sure that you have accurate dielectric constant data. This is another area where John Coonrod is really excellent to listen to because he actually has a ton of knowledge about picking out the correct material, but also understanding what the material specifications mean when you look into a data sheet.
So the last points here that I want to leave listeners with is something that is a bit near and dear to my heart and inspired by RF design and the need for unique RF structures and PCBs. And I've often wondered if there's something that we can do to mimic essentially what happens with MIMO antenna arrays and MIMO radar. And that is something called aperture engineering. And so there's a very old formula that relates the current density around an aperture to the emitted wave pattern from an RF element. And I say RF element generally, because I'm just talking about an aperture here. But I think it would be quite interesting to explore more about doing this in PCBs. And so, I actually showed earlier an example of this. If you saw earlier when I was discussing the coupling to a waveguide and I was talking about [Ugi meters 00:54:31], really what we're doing is something that I like to call aperture engineering.
We have an aperture that could emit a RF signal very strongly, and that aperture has been engineered to provide a specific wave pattern. And maybe you didn't engineer it intentionally, but that's certainly what it gives you. And so it would be quite interesting with newer fabrication technologies like 3D printing of electronics to be able to fabricate some very unique apertures that could be used to engineer the wavefront for very specific applications. This is something that is certainly of interest to me. But I think the best application is for number one radar obviously but also just for wireless communications in general.
And so, the point of this is to say that, as a designer, you actually have a lot of freedom to experiment with this type of thing with emitters and with receivers in an RF design by engineering apertures in different circuit elements. So the main one that I showed earlier was the slot in the substrate emitting waveguide. There are substrate integrated waveguide, I should say. So anyone who has questions about that, I invite you to attend the Q&A session as that is certainly something you could ask me about, and I can now go into a greater depth. And that is certainly a topic that deserves really its own talk.
So, I will leave you all with that and hopefully to contemplate how you can start engineering your own apertures in a radio frequency design. Thank you everybody for attending. Please feel free to find me on LinkedIn and send me some questions. Also, as I mentioned earlier, please attend the Q&A session if you have more questions. We would love to have you and I will be there to take any questions on any of these topics. Thank you again, and thank you to Altium for having me.