Gustavo Blando: “A ground via next to a differential pair can reduce the amount of crosstalk”
During DesignCon 2018, we met with Gustavo Blando, Senior Principal Engineer at Oracle. We discussed material characterization, transmission lines, differential pairs, how placing vias can reduce crosstalk… among other things!
0:08 What are your thoughts on this year’s DesignCon?
DesignCon is great. Great conference, great people. It’s great to come once a year and meet friends. Certainly, every single time I leave DesignCon I feel invigorated with a bunch of new ideas. I think it’s a great place for people to join and learn from each other. That’s the most important thing.
0:28 Can you summarize your presentation?
I presented the paper this morning and it was more about some of the pitfalls when you take some of these measurements. Some of the things that are not obvious after you take the measurements, but after a bunch of post-processing you can observe. Hopefully, people have learned something and take better measurements in the future. That’s the whole idea.
0:53 Why are these measurements are so critical?
Sometimes we look at losses, particularly at very high frequencies, that’s one of the limiting factors to be able to accomplish transmission from driver to receiver. Other times we are trying to characterize materials and so precise measurements of these traces allow to get you good material characterization. So if you do it wrong, you are going to be simulating with the wrong values and hence you won’t be able to properly simulate your channels. It could lead to problems in the real operation of the channels. I think it’s very important to measure properly because that’s the way you gain understanding. By measuring, simulating, and correlating, right? And particularly at high frequencies. This is extremely important to be able to accomplish high data rates.
1:52 What is material characterization?
There are a bunch of different ways that we characterize materials over the past years. But basically the parameters… Let’s start with the parameters that we should characterize, every single integrity engineer should characterize our basically like electric material properties. Like electric lost engine versus frequency, copper losses, skin effect, DC losses and all those things. Cross sections of the board to get an idea of the stack-ups. And all those things are going to basically be the number one factor for the losses of your transmission lines. And it is very important for simulations in terms of passivity and things like that. I mean, many people know how to do these characterizations, but also when you have good models, you can use the massive black box. So not everybody needs to definitely know all the ins and outs.
“Rather than characterizing every element individually, we characterize and we measure the transmission line as it’s supposed to be.”
The way that we like to characterize materials, rather than characterize just the dielectric, we want to characterize the press stack, such we can see everything together. And that’s why rather than characterizing every element individually, we characterize and we measure the PCB transmission line as it’s supposed to be. And that’s probably a little bit of the difference.
DOWNLOAD OUR PCB TRANSMISSION LINES eBOOK:
3:14 What kind of coefficient of coupling range is more reliable for a differential pair?
So you have the coupling between the differential pair. And the coupling on a differential pair is rather low as compared for example like to an X. It’s like a five percent range, three to five percent range. The big things are how will you minimize the coupling to different differential pairs and how will you control the impedances within the differential pair. And that’s kind of where you need to look at the stack-up and you need to look at all the variables in your design. Because some people like to do loosely coupled differential pairs. Some people prefer tightly coupled differential pairs. Basically claiming tightly coupling differential pairs will have less amount of crosstalk to a differential pair. But that has to be looked at the same time of impedance because the moment that you put your two transmission lines closer together, your impedance will go down. So if you want your impedance to come up, you have to lift the planes. The moment you’re lifting the planes, now you have more crosstalk to your other differential pair.
So there is always kind of a sweet spot that you have to analyze. And in order to analyze crosstalk, you can not only do it just by looking at the crosstalk. You have to look at your whole channel. You have to look at the losses. Perhaps you have a situation where you need to tightly pack a lot of differential lines and by doing that you can shorten your length by two or three inches. So in which case, it might be okay to sustain a little bit more crosstalk because you’re reducing your length. So the crosstalk and the stack-up have to be seen, in my opinion, more as a holistic view of the whole loss margins that you have in your design.
I would say somewhat in between is kind of a good compromise solution. It’s really a ratio of the separation between the differential pairs with respect to the separation to the planes. So that’s the ratio that you have to be looking at.
You will see sometimes people cannot have too many layers in the wall and they have asymmetrical stack-ups where they put the differential traces really close to one plane and the other plane really far away because sometimes they have to cross and split or things like that. So it’s really the ratio to the closest plane because you can imagine us doing impedances in parallel from the bottom plane up to the top plane.
5:43 Any tips on good design practices a designer can adopt to have the minimum amount of distortion?
So that’s a problem, when you go from one layer to the next, you need a via, I mean unfortunately, you need a via. And really the way that I think about this, I think about all the return currents more than anything. So I want to make sure my return currents have a uniform path to come back. So if you can go from one layer to the next sharing one of the ground planes, for example from layer three to layer five, being layer four the plane. Now even though you are crossing, you are still using at least one of the references doesn’t change. So you facilitate your currents to return. Often times you cannot do that so you have to go deeper into the board or cross many, many different layers. In which case we try to put vias to allow the current to come back.
“Having a ground via right next to the differential pair would completely reduce the amount of crosstalk coming from mid-frequency signals.”
The reality is this via have two functions, really. Function number one, it helps you control the impedance of the transition, which is really important. Because ideally if you have let’s say a 50-ohm or a 100-ohm environment, you want to control your trace all the way through so you have 100 ohms. And by putting ground vias you allow for that to happen. And the second reason is to shield for interference from other circuits. We’ve seen problems where lower frequency circuits get into our differential pairs. Having a ground via right next to the differential pair would completely reduce the amount of crosstalk coming from mid-frequency signals. We see that with power supplies, for example. Sometimes it’s not easy to put ground vias everywhere. And the way that we like to put ground vias is on the outside of a differential pair because really, when you look at this differential signal, most of the energy is contained between the differential pair. And that signal kind of goes nicely. One of the signals is the reference on the other. The problem is the common mode signals. The common mode signals tend to spread away and that what is crosstalking other signals. By putting ground vias outside where the common mode will go, you’re catching those currents. And you are improving the isolation to our differential pairs or crosstalk to our circuit.
So there are two things for the vias. One of the things for the vias, as I mentioned, is the impedance of the via. And the other thing is the staff of the via. Sometimes when you are doing economical designs, you don’t want to back drill your boards. So the stab will generate a big dip, which is a quarter resonance of that stab. So the longer that stab is, the lower the frequency of the resonance it is. So you want to make sure you try to minimize that for higher frequencies. Now, that’s a first-order effect type of a situation.
A little bit of a secondary effect that you would see clearly on the s-parameters is an impedance of the via itself. You will see on the s-parameters when the impedance of the via changes, you will see a very flat profile and then going into a dip. Or you will see as the impedance of the via is smaller, that flat profile will dip a little bit more. So there is kind of a profile on the s-parameters before you head to the dip and the location of the dip that is going to impact dramatically your insertion loss. So you definitely don’t want to have a big stab, you want those stabs to be minimized as much as possible. And with back drilling technologies these days, you can do that rather easily. You want to sometimes remove the path. The path by itself without back drilling the via is a big capacitance to the first plane and that by itself generates a big capacity stab that would create a dip at lower frequencies. So just sometimes by removing the path by itself, you can improve dramatically your channel.
“If you’re running a signal at like 100 megahertz, you won’t even see the via.”
9:49 Can the amount of disturbance in a via be catastrophic?
It will depend on the frequency that you’re running. If you’re running a signal at like 100 megahertz, you won’t even see the via. The via is related to the wavelength of the signal that you are sending through the circuit. Now if you are sending a signal that is 20-picosecond long, now suddenly a 150-mil via is almost like 30 picoseconds of delay or something. So it’s in the order of magnitude of the signal that you are sending. So that is the problem. It’s not related so much to the length of your channel but rather to the frequency content of the signal that you’re sending.
10:30 What is the frequency threshold in which the via can become an important parameter?
When we look at vias, we look at vias with stab. You can create a via without a stab and you can basically match the impedance on the via, such the via is transparent, it won’t be an issue. It just won’t be an issue. Now, it’s all degree of grace. I mean, depending on how high of the frequency and how well matched is the impedance, you’re going to see an issue. And it’s going to be independent case by case, I guess that’s the best way I can answer the question.
I used to create a calculator by which I modeled the via very roughly. But there are formulas, there are close form solutions where you can estimate the impedance of the via. But what I would recommend for particularly people here at DesignCon, if they are working at the higher gigahertz frequencies, the best thing they can do is try to model the vias and not only a couple of vias, but many, many vias to look not only for the vias itself and the impedance of the via, but also the crosstalk to other vias in a 3D field solver.
11:41 Do you have a simulation with and without the via?
Yes, so normally the model is generated in different ways. But the model is generated for the via by itself or for a set of vias. And in there you extract these parameters; just by looking at the via itself, you can see the insertion loss of the via has. And then, you have to know how to split the via, where to begin and where to end. But then, it’s kind of like a block process. You can connect your traces with your vias and it’s very easy to remove the via from your circuit or not and you will understand basically what the via will be impacting in your channel.
12:18 What kind of software do you use to calculate these simulations?
I’ve used many, many different simulation softwares, I’ve used CST, I’ve used ANSYS, I’ve used HFSS, I’ve used Simbeor, I’ve used ADS. Really, we like to look at different softwares, compare results one to another to make sure our simulations are solid and it does not just result from one single tool.
“I wouldn’t only trust simulations to give me absolute values.”
12:45 How do you verify that the simulation is near or exact to the results you are trying to achieve?
We have to do measurements. Simulations, in my opinion, are good guidance, but I wouldn’t only trust simulations to give me absolute values. I really need a measurement stake in the ground at some point during the same process to determine if the simulation is accurate or not. So, that’s a way I view simulations. I view simulations more like a guidance tool, comparative analysis between two different strategies. But not necessarily as an absolute measure of the results that I would see without having a measurement right next to it.
13:31 What kind of instruments are used for these measurements?
We have like Agilent Keysight 50 GHz VNAs. We have high-frequency scopes. We have TDRs of different brands.
We can use the via measurements using TDRs or using VNAs. I mean, one is the best forward in terms of the other. The only difference is the noise floor that different instruments have. So we tend to use VNAs through this passive channel characterizations, we graph the data from the VNA and convert it to the time domain. But there are times where a simple TDR measurement can really help you divide a problem or analyze something.
14:08 Any general guidelines you think PCB designers should know about?
Oh, we’re full of those design guidelines. I mean, you can go in here and you can see all this different rule of thumbs and all these different things that people talk and those comes from measurements and experience and sometimes people agree with those rule of thumbs, sometimes people disagree. Sometimes there are little times where the rule of thumbs cannot really apply. So it’s not so much of all the rule of thumbs, it’s really about the knowledge to apply those rule of thumbs when they should be applied.
14:40 How important is DesignCon to you?
It’s a great opportunity for me to really present some of the work that we are doing, but mostly to learn from other people and to invigorate myself and the team to create new work. Moving forward in terms of research. I would encourage attendees to basically go to as many presentations as they can. I would encourage them to be extremely curious and humble and try to learn as much as possible from the experts. I think that’s very, very, very important. And that would be my advice to them.Tags: controlled impedance, crosstalk, DesignCon, TDR, transmission line