Verstecktes Juwel in Altium: ein integrierter 2D-Feldlöser – Eric Bogatin – AltiumLive 2022

Eric Bogatin
|  Erstellt: February 3, 2022  |  Aktualisiert am: September 9, 2022

Altium hat sich mit Simbeor, einem weltweit führenden Unternehmen im Bereich elektromagnetische Simulationen, zusammengetan, um einen benutzerfreundlichen 2D-Solver zu integrieren. Mit diesem Tool können Sie einen Lagenaufbau analysieren und synthetisieren, um einen Zielwiderstand an einzelnen und an differentiellen Endpunkten zu erreichen. Man muss kein promovierter EM-Experte sein, um damit eine brauchbare Antwort zu erhalten. Ich werde Ihnen zeigen, wie Sie so den Widerstand Ihrer Leiterbahnen analysieren und ein Design synthetisieren können, das Ihren Zielwiderstand erreicht. Einfacher geht es nicht.


  • Verwendung des 2D-Feldlösers für die Analyse
  • Welche Bedingungen beeinflussen den Wellenwiderstand am stärksten?
  • Analyse und Synthese in Altium Designer
  • Eigenschaften von Übertragungsleiterbahnen kennenlernen
  • Einblicke in die Signalintegrität

Weitere Ressourcen:


Eric Bogatin:

Hi, everybody. Thanks for joining me today. I'm going to walk you through an example of what I think is one of the coolest, hidden gems in Altium Designer. And this is a built in 2D Field Solver that uses the simulation engine from Yury Shlepnev's Simbeor software. And Simbeor is a full blown 3D full wave field solver, but it's got 2D capability, and that has been integrated into the Altium Designer with a very simple, easy to use front end. So I'm going to show you how you access it and how you get the most value out of it.

Now, I'm not going to go through a lot of details of who I am. I would just want to highlight three hats that I wear. I'm a professor at University of Colorado in Boulder. I teach electrical engineering classes, and one in particular is a Printed Circuit design class. I'm also a fellow with Teledyne LeCroy, and I do some webinars with them that focus on best measurement practices, and I'm technical editor of the Signal Integrity Journal.

Now, a lot of what I'm going to talk about is covered in other resources, and we just don't have a whole lot of time to go through a lot of details today. So I, instead, I'm going to provide you some additional reference material that you can take advantage of. In particular, I've got four textbooks out in this field, and two of them cover this topic of transmission lines and characteristic impedance in a lot of detail. So you'll definitely want to check out my book on transmission line design and characterization, it is a really good starting place for the properties of transmission lines and how to think about the characteristic impedance, which is the number one most important design figure of merit for a transmission line.

And then in my other textbook on Signal and Power Integrity-Simplified, I have a chapter there on transmission lines, which gives you a good jump start to think about the design of transmission lines.

In addition, I've started a podcast series with Signal Integrity Journal. And so you can check out the podcast. And while you're at it, you can check out the rest of the Signal Integrity Journal if you haven't been there before. A lot of great information on signal integrity, power integrity, EMI. We curate all the articles. And so we make sure that it's only top shelf content in there. A lot of high value content from beginning tutorial topics, all the way to very advanced topics as well. And I've started the podcast series, basically informal conversations with experts in the industry, a chance for me to have a one-on-one conversation, learn something new and let everybody else listen in on the conversation.

And then in addition to the textbook and Signal Integrity Journal, I've done a bunch of webinars for Teledyne LeCroy, and they're all posted on the website, and they're all for free. You go to the left side of the website, you'll see the list of the different topics. If you're interested in transmission lines, then I would strongly recommend taking a look at the webinars that are posted under the TDR applications. There are about a dozen or so webinars that I've done over the last few years on this topic and they all involve properties of transmission lines. So you definitely want to check out those webinars. You can go to the link, read a little bit of what's covered, and then you'll be directed to the landing page to view the webinar and download a copy of the slides as well.

But wait, there's more, courtesy of Teledyne LeCroy, all attendees to Altium Live can receive a three month complimentary subscription to all the training that I have on the Signal Integrity Academy website. So if you go to the website, same as the beTheSignal website you'll in one of the top headings there about subscriptions. You pull that down and you'll see the subscription for three months. And if you fill out that form and use promo code ALT21, you'll get a free three month subscriptions, complete subscription access to everything. You can view all of the courses, download all the slides from it, but you only have access for three months. And then that will give you an opportunity to go through a lot of the videos and you can learn about all aspects of signal integrity, and in particular about the properties of transmission lines. So be sure to take advantage of that opportunity while it's available.

Okay, let's get into what we're going to talk about today. So I'm going to show you really quickly how to access the built-in 2D Field Solver and how easy it is to use and why I think it's so cool. We can do both analysis, that is, we'll take a structure we've already built and we'll analyze, okay, what's the characteristic impedance, or we can synthesize, if we know to the stack up and we're not sure about the line width, we can then calculate what's the line width we need for 50 ohms or whatever target impedance that we want.

And then I'm going to compare a couple of the results that we get with the built-in 2D Field Solver with what you would calculate using some of these online calculators. Really important to keep in mind that I can't think of any exception. I think it's 99% of all of the online calculators out there are really approximations. And so you don't really know how good that approximation is, they vary quite a bit. And that's the advantage of a 2D Field Solver that UUs tool and many of the other 2D Field Solvers out there are accurate to better than 1% absolute accuracy. I've done some analysis, others have done analysis, and their accuracy generally is very good typically. And we'll see that sometimes some of the online calculators can be pretty good as well, but when you're off from their sweet spot, typically around 50 ohms, it's hard to know how accurate they are.

If you're given the chance, you always want to use a 2D Field Solver in order to do the estimates of the design for a target impedance. And then once we've got an idea of how to use it, we'll use it to explore design space a little bit. We'll look at what I think are the first order factors, the most important geometry material properties that influence the characteristic impedance. And then using the Field Solver gives us the opportunity to look at some of the second order factors. And that's really the value of using the Field Solver.

And sometimes knowing that a feature is not important and does not affect the characteristic impedance very much, is just as important as knowing that it does and how it does. That tells us we can maybe ignore this feature. And that's the kind of information we can get from the 2D Field Solver.

So let's get started, and I'm going to show you from the very basic beginning, how to access the 2D Field Solver. I'm going to open up my copy of Altium Designer. Here it is. And let's go full scale here. Now I'm opening this up to an absolute blank screen. There's no project here. And instead what we have is the whole home page, and I'll just do a blatant plug for the homepage. I love coming here because there's oftentimes so much valuable information. You'll be able to do any updates, but more importantly there's information from experts, additional content that Altium is pushing out there.

Here's an example of... Hey, here's a blog that my buddy Jason has put together just in the last week or so. And you can browse through here. There are a lot of other blogs or videos or webinars that are here.

So this is always a good place to go right at the beginning, just to check and see if you've got some time, explore a little bit of additional information. Okay. Once you've had a chance to look over some of the interesting content that Altium has provided, now we're going to begin using the 2D field solve, and to do that. We have to have a PCB page or layout open so we can access the menu specific items for that page. So I'm going to come over here to the project. I'm going to create a new project, so add new project. And I'm going to just use absolute basic default, nothing fancy. And now in order to access the 2D Field Solver built-in, we need a PCB page. And to do that, I'm going to add new to project. Let's see, I want PCB. And so, here's my PCB.

Now normally, okay, you'd add a schematic you'd type or work on the schematic, you get the schematic page, it's all done, and then you're ready to push it to the layout page. And on the layout page, you're going to define the outline of your board, and then you're going to select the layer count. So I'm not even going to grab an outline of a board or move any of the parts over. I'm going to go straight to the, define the stack up of the board. And so we do that over on design, and there's a pull down item that says, "layer stack manager," and when I select that, it comes up with my default stack up, which in this case is just a two layer board. Now, if I have a two layer board, I really can only do surface traces. So I can do microstrip. I could do microstrip coplanar. But to get a stripline, I need at least four layers.

And so I'm going to, instead of using the two layer default, just so I can show you all the features, I'm going to use a four layer. And to do that, we come over here to tools and now presets, and I'm going to just grab the four layer preset. You can manipulate it and adjust it any way you want. The most important thing is that there are four metal layers. And you can see the color coding here. Nicely, the oranges are the copper layers. You got the top layer. This is layer one, this is defined as internal power bottom layer. Now just on the side personally, I would not use a ground and power layer. I'd make them both ground layers, but that's a different talk. But however, the important thing is that I got four layers. And on each of these layers, I can define they can be signal or they can be planes.

And so just for the heck of it, let's see, can I make this a signal layer? And can I make this a signal layer as well? There we go. Everybody's a signal layer. The important thing is we can only calculate the characteristic impedance of a signal line, and then we have to define where the return planes are or the term used in our team designers, the reference planes. So I can use any of these layers, now that they define as signals as the signal layer for which I'm going to calculate the characteristic impedance, and I can define whichever layer is going to have the plane, the return plane on it. So that's the first step, I got my stack up. And we'll adjust the dimensions of the prepreg layers or the core layers. We got different thicknesses. We got different thickness for the copper.

So here is one ohm copper. We can change that. Of course, we can do half ounce copper, and there's the new thickness. We'll keep that as half ounce, we'll do one ounce. So usually there, they were around. Let's do that. Let's make this half ounce in the middle, and let's go back to one ounce up above. And there are the dimensions, we have the dielectric thicknesses. So we got the prepregs over here and their dielectric constants as well. And this is what we get from the data sheets, for example. We're not going to do anything with the dissipation factors for now. We're just going to deal with the dielectric constants. And so you would adjust this based on the stack that you think you're going to use or what the vendor's going to provide for you.

The next step is, we're going to come down here to the bottom set of tabs, and we're going to push the middle one impedance. Now, there are a lot of other cool features in the stack up manager I'm not going to go through, you can play around and click the buttons and take a look at some of the other features. We're just going to go to impedance. And when we do impedance, now we're going to have the opportunity to calculate the characteristic impedance of lines on any of the layers defined as signal layers. And to do that, we need to click this button that says add impedance profile. And you can see that each of the signal layers now has a line that is pulled out here and we can define for each signal layer, where is the top reference or the bottom reference. Really, when you hear reference, think return plane, because this is a top signal layer, a surface trace. There is no top reference plane, there's only a bottom one. And we can select layer two.

So here is layer two. And I could use any of the layers depending on where that nearest plane is located. We're going to keep it on layer two. And likewise, if we've got one of these signal layers on layer two here, signal layer, then we could define where is his return plane. It could be on the top layer. So that's top layer and its bottom return could be layer three. And so we define that. And now that defines, here's layer three, this is the dimension, the distance away. That's the only information that we're going to need is, what are the thicknesses? What are the dielectric constants for the distances between the signaler that we're on here and where the top and the bottom return planes are? Okay. So that's setting up the features and the geometry, and now we want to access the Field Solver.

And the way we do that is, we have to come over here, and if we don't have the properties identified, then of course you go down to the panels and you find... Where's properties? Here's properties. And so you make sure that that is highlighted. And here it is up here. Now, turn it on. And that's where the Field Solver is located. Now, if I click off, it disappears that I'm going to close this. And so for our demo, I want to pin that down, I want to keep it from closing. And so I'm going to come up here, I'm going to click that little pin it in place. And so now we have the stack up where we can change the dimensions. We have the impedance layer, which identifies where the returns are located for each of the signal layers. And as we highlight each of the signal layers, all that information is automatically ported over to the user interface to the 2D Field Solver.

So we're on layer one, and that's microstrip. And so here's that geometry. And I can select what type of topology I have for that transmission line. So right now I could make it single-ended, that's what I've got now. I could make it differential. I got two traces. I could make it single coplanar. Now single coplanar means that I've got the signal and I have ground on either side. And in this case, I also have a ground plane underneath. I would actually call all this coplanar microstrip because I have ground above and microstrip down below. If you want to just straight up coplanar, you use this geometry, we would just have to make the dielectric thickness really thick. So this plane is far away. And then we would have just coplanar. And we could also do differential coplanar as well.

So those are the options. We're going to stick with single microstrip, really simple. And you can see the features that we have available to us. Now in the Field Solver, we have the opportunity to adjust which additional features we want. Like, for example, here I have the soldermask layer, and here I'm defining the soldermask. It's the thickness over here and dielectric constant. I can turn it off so that we're not including it in the calculation. I have the etch back. That is the difference in width between the top and the bottom. I've set that to be zero, we could turn that on and have a little bit of difference in the line width from the top and the bottom. And we can select the width on the top and width and the bottom. The fact that etch back is zero means they're going to be the same.

And then here is, if I used soldermask, I turned it on, here I could type in, "what's the thickness in the region where we have nice wide surfaces and what's the thickness covering a trace over here?" So that's the C2 over here and the C1 over here, if I was using soldermask. So we can type in all those values and then we can get the characteristic impedance. So this how we access it. And before we move on from here, I'll show you, if we have a inner layer like this one here, this is layer two, we have the opportunity of a plane above and a plane below. And so here, I'm defining the top reference layer is on layer one and the bottom is on layer three and Altium is taking the stack up information and automatically porting it over to the 2D Field Solver.

And here you see the picture, Hey, look, I've got two prepreg layers over here. I define the dielectric constant here, and I have one core over here. And there it is. So I've matched that geometry. Same thing, I can change where the layer is located and which layer the metal is located depending on the deals of the stack up. So that's how we select and set them up. And again, this is a strip line geometry, because I have planes above and below. Again, I can do the same thing. I can make it differential, I can make it coplanar. In other words, this would be a kind of a coplanar strip line geometry. I have ground on either side here, plus the grounds above and below. And likewise, I can do it as a differential. Here's my differential pair. And I have grounds on the same layer in addition to the planes that I've got.

So we're going to take a quick look at microstrip transmission line, and then we'll go to a strip line transmission line. So let's go back to our microstrip, and here's what we're going to do. We know how to access it. We know how to set it up. Let's do a simple estimate as analysis. In other words, we're going to put the geometry information in, we're going to calculate what's the characteristic impedance. Now, if you're not familiar with that term, characteristic means what it means. I didn't want to spend any time today going through that, but you check out some of the videos that I mentioned at the beginning, you check out the two textbooks I mentioned, and you'll find a lot of really valuable information about how to think about in a simple way, this concept of characteristic impedance, but you should all know it's an important design term, it's an important figure of merit.

So let's take a look at the characteristic impedance of a signal line that's on this layer. And so here it goes on layer one, and we're going to turn off soldermask initially, and we're going to turn off the surface finish so we can add, this is a different metal layer, a coating, hassle coating, for example, or plating on the top layer and with a different thickness. We're going to turn that off as well, but we have the option of including that. And so it's just bare metal. The return plane is the layer two over here. And so there are two prepreg layers, and I'm going to make each of them, and this is information we would get from the data sheet, but I'm going to make them each five mills in thickness. And I'm going to use a dielectric constant of 4.5 for each of them.

And again, this is information that you would get from the fab vendor, from the data sheet for the particular stack up you're going to use. What is the thickness of each of layers? What is the dielectric constant of each layers? And I'm using one ounce as the copper thickness for that layer. And so we got all that information that is now poured directly over to the built-in Field Solver interface to Simbeor tool. It's a single transmission line. If I wanted to synthesize the geometry for 50 ohms, then I'd put the target impedance here, but I just want to analyze, I want to put in the geometry that I can think of and then ask, what's the characteristic impedance? And so I'm going to use a width. So let's see. So we have a dielectric thickness of 10 mills between the signal and the return plane. We got 10 mils here, so I'm going to guess, I'll make that 20 mil wide line.

So I make it 20 mils wide, and I'm going to ask the question, okay, what is going to be the characteristic impedance for a 20 mil wide line? And so I type the numbers in and, look, as soon as I type it in, in fact, let me do it again. I'm going to change it. I make this 10 mils, look what happens down here. As soon as I typed in the values, the impedance was automatically calculated. That's how fast the tool is. So it takes all across section information, calculates the characteristic impedance. So I go back to my 20 mils wide. It's going to populate the 20 mils for the top and the bottom of the trace because I set the etch to be zero, and it automatically calculated the characteristic, 47.03 ohms. And it's off from, if I had my target at 50 ohms, it's off by about 6%, and you get a little bit of other additional information.

That's as simple as it is to use this tool as an analyzer to calculate the characteristic impedance. Let's just do a quick comparison between the value we calculate with the 2D Field Solver and what you would get if you used an online tool like the... One of my favorite tools is the Saturn PCB calculator, here it is. And I've got it set up for conductor impedance, a little bit misleading here, but let's set this up to be exactly the same geometry as this. So let's see. So the base copper is one ounce, I think, let's verify that. Yep. I got one ounce copper on layer one, I'm not going to have any plating on top. It's going to be bare copper, it's microstrip. Let's see, my dielectric constant is 4.5, and my thickness, this is the conductor width is, what is that? 20 mils. So I make this 20 mils. The conductor height, a little bit misleading, it's not the conductor height it's the dielectric height. It's this dimension here, which is 10 mils.

And now, what's the characteristic impedance that's calculated? So these cross sections are pretty darn similar. This is 47.47, and this is 47.03. So you can see that they are in agreement within about 1%. That's the level of accuracy you can expect when you're close to 50 ohms. This says, boy, the approximation in the Saturn tool is a pretty darn good approximation. Now, while we're here, let's do the same thing, but let's do it for a differential pair. So we come over here and say on this layer, let's make a differential pair. And I'm going to have, okay, I'll make the width 20 mils, but I want the spacing here, I want that gap to be 20 mils as well.

I know it's going to be a pretty low impedance because it's a 20 mil wide line 20 mil space and 10 mil thick dielectric. And sure enough, here it is 87.7 ohms as the differential impedance. Let's see what we get using the Saturn tool. So I'm going to go to... here we go, differential pair, conductor width is 20 and 20. The spacing is 20, conductor height again is 10. What else? The base copper is one ounce, no plating. The differential layer is... I think that's the right stack up. Yep. So there's the same cross section as what we have. I've turned off soldermask here. So there's no soldermask. Everything else looks the same. I think we're there. Just to make sure we push the solve button. So let's see, the differential impedance that the Saturn tool gives is 82.1 ohms. The differential imp heeds that Simbeor gives is 87.7.

So there's a difference of about 5 ohms. So it's like around 6% difference between these two. This is one of the reasons why you want to be careful using a approximation. That depending on what the nature of the approximation is on the inside may not be a very accurate value. And before you knew about this built-in tool, the only opportunity you might have had to calculate the characteristic impedance might have been using the Saturn or one of the similar kind of online calculators. But now that you know, you get this hidden gem built into Altium Designer, you never have to use an online calculator. You can calculate what the characteristic impedance is of your layers directly using the Simbeor 2D Field Solver.

Now, what I've demonstrated here is how you do analysis. You set up the geometry and then you calculate, okay, here's what there is resulting characteristic impedance is. The other way of using this tool is by synthesis. If you have the stack up from your fab vendor. So here's the stack up from our fab vendor, and we are going to ask, okay, given these dimensions, then what is, and given the spacing between the two lines, what is the line width we need for a target impedance of 100 ohms. So we put 100 ohms up here for target impedance, and we come over here and we say, let's keep the dimensions here, but we want to keep the gap fixed, and we want to ask what's the line width? As we come over here to this little button here, this calculate trace width automatically. And we know right now that we're at 87 ohms. And so I always recommend following rule number nine, which is, before you do that simulation, you do a quick estimate of what you expect to see.

So we're here at 20 mils wide line, 20 mils spacing between them, and that's 87 ohms. I want 100 ohms, I want a higher impedance. And if I keep the spacing fix, that means I have to make the line width narrower. So I'm going to expect to see a narrower line width for W2, the top dimension. Let's see what we get. We push that, oh, 15.76 mils is the appropriate line with. Because when I use that line width, I've got 99.96 ohms as the differential impedance, pretty darn close to my 100 ohms.

Now, if I said, "Well, I want 15 mils, but I don't want 100 ohms. I want 85 ohms." So I come over here, maybe I'm doing a piece. I express gen three for an Intel board. And so here is 85 ohms as the target impedance, I'm going to stick with 15 mil wide trace, and I don't want an etch back. So that's going to be zero. I want this to be 15. Here we go. So I got that zero. I got 15. Now I want to know, if I just keep that spacing of 20 mils, it's at a 100. I want 85 ohms, what spacing do I want between the traces in order to give me my 85 ohm target an impedance? Well, we push that button and, six mils.

So if I use my 15 mil wide trace and two of them, 15 mil wide, and I have that same dielectric thickness based on the fab vendor stack up, I have to bring the traces to within six mils to get me that 85 ohm target impedance. Sure enough, 85.01 ohms. So that's how we find the tool. That's how we set it up. That's how we use it. And so the next time you want to evaluate what is the characteristic impedance of my trace, or what line width do I need to give me 50 ohms for single ended or 100 ohm differential, this is the tool to use. Now while we have it here, let's do a little bit of exploration here. What I love about the 2D Field Solvers. It includes not just the first order factors, such as, let's go back to single-ended here, and we're going to do a target impedance of 50 ohms.

And we're going to look at, which terms influence the characteristic impedance the most? And what you'll find is that the first order term is the line width. And you should learn that intuition about, if we increase the line width, what is that going to do to the characteristic impedance of the line? So make the line wider and that's going to give us a more capacitance per length. That means that the signal propagate has to drive more current to leave that one volt in its wake, has to charge up the line a little bit. And so make it wider, lower capacitance per length. That means more current goes in for the same voltage, more current for the same lower impedance. So I'm going to expect the, if I make the line wider, I'm going to expect the characteristic impedance to go down.

So here we are at about 18 mils and we're at 50 ohms. Now let's make it 20 mils. Should be a lower impedance. Let's see. Sure enough, there it is, 47 ohms. I make it 30 mils wide, and there it is, even a lower impedance. So that's consistent. If I, let's go back to the 18 mils. So there's close to 50 ohms. Now, if I make the dielectric thickness sticker, I pull the trace and the return farther away, what's going to happen to the characteristic impedance? Well, I should find, if I pull the return farther away, I decrease the capacitance per length, and that's going to, if the capacitance has decreased the impedance is going to go up, so let's make it thicker. I go from five, make it 10 mils, everything else stays the same. I should see a higher impedance. And sure enough, I made it 10 mils, higher impedance, very consistent.

And then dielectric constant. So we'll go back to five mils over here. And now, if I use a higher dielectric constant, the impedance should go down. So let's use five for one of these layers and let's see the impact on the characteristic impedance. It should go down. And it did, not by whole lot, little bit, didn't make much of a change. And it was only in one of these layers. And so using mixed dielectrics is easy with the 2D Field Solver.

But in addition, we can also evaluate some of the second order factors. So let's go back to 4.5 and 18 mil. So we got a 50 ohm line. Now let's turn on the soldermask. What's that going to do? Well, the first order, it shouldn't have any impact at all because it's so thin. But the second order, we're going to add a little bit of higher dielectric constant in this region up above, we have some of these fringe fill lines that are going between the signal and the return. Most of the field lines are going this way, but some of them are going this way. And so where we had air before, we're going to add a higher dielectric constant, we're going to increase the capacitance a little bit. That's going to pull the impedance down.

So let's see when I use a one mill thick soldermask, and I'm going to use a dielectric constant of, they're closer to 3.2 typically, I'm going to use 3.2 as the dielectric constant, and now I'm going to turn on the soldermask. And when I turn on the soldermask, I'm going to assume that I have the same thickness covering in the general regions as on the material. And look, I went from basically 50 ohms to 48.3 ohms. So that's like 1.6 ohm difference. So that's like a 3% impact. And it went down as I expected it would. And so if that's the case and I want 50 ohm, here's my target impedance, I can ask what line width do I have to go to with the soldermask to give me 50 ohms?

Well, that's easy. I know I have to use a narrower line because I want to increase the impedance, and I'll let Simbeor calculate it for me directly. What's the line with? Oh, 17 mils gives me a 50 ohm target impedance. So that's the game that we play in exploring design space as either analysis change the stack up geometry or the material properties and put in the line with, and we'll calculate what the characteristic impedance is. Or in synthesis, we fix those things that we are sure of their value and we just use the 2D Field Solver to tell us what line width we need to use in order to achieve that target impedance.

So with that, let's go back to the slides. And now I'm going to... We just summarize what we've talked about here. You can go back and you can do these experiments yourself with your version of the Altium Designer now that you know how to access the features.

And now let's just summarize what we've done here. I wanted to introduce you to the 2D Field Solver that's built in the Altium Designer. Now you have access to it and you see how easy it is to use. You can use it for analysis or synthesis. It's better than any online calculator you're going to find, because you can do the analysis of the second order factor, mixed dielectrics, the impact of the soldermask, the impact of the etch back, in the stack up you get in multiple dielectric layers with prepreg and core each with dielectric constants. And of course you get that information from your fab vendor based on what stack up they're going to use. And we saw that it's really easy to use.

Now, finally I just want to leave you with the idea that if you would like to understand better about transmission lines and in particular, what this idea of characteristic impedance means. I recommend these two sources. One of the books I did with Artech is all about transmission line properties, understanding transmission lines, and in particular about designing the stack up and using TDR to analyze the transmission lines. And then the second reference is my textbook on Signal and Power Integrity-Simplified. There's a chapter seven in there that's all about how you're building up your engineering intuition about how the cross section information influences characteristic impedance. How we think about characteristic impedance, how we think about the signal return paths in a signal propagating down transmission line and what that idea of characteristic impedance means.

And then finally, I'm going to leave you with a blatant plug here for other references to check out. Check out my textbooks, check out my podcasts, check out the webinars that are completely free on the beTheSignal website, the ones in particular about TDR applications.

And then finally, as a courtesy from Teledyne LeCroy to all Altium live attendees, feel free to grab your complimentary three month subscription to all of the video training that we have on the signal integrity academy website. And you'll fill in the little form for the three month subscription and use ALT21 as the promo code. And with that, thank you all very much for joining us. And I'll entertain some questions here in the Q&A period. Again, thanks so much and hope to see you live in person the next time we do this.

Über den Autor / über die Autorin

Über den Autor / über die Autorin

Eric Bogatin is currently the Dean of the Teledyne LeCroy Signal Integrity Academy, at Additionally, he is an Adjunct Professor at the University of Colorado - Boulder in the ECEE dept. Bogatin received his BS in physics from MIT and MS and PhD in physics from the University of Arizona in Tucson. He has held senior engineering and management positions at Bell Labs, Raychem, Sun Microsystems, Ansoft and Interconnect Devices. He has written six technical books in the field and presented classes and lectures on signal integrity worldwide. In 2011, his company, Bogatin Enterprises, which he founded with his wife, Susan in 1990, was acquired by Teledyne LeCroy. After concluding his live public classes in 2013, he devoted his efforts into creating the Signal Integrity Academy, a web portal to provide all of his classes and training content online, for individuals and for companies.

neueste Artikel

Zur Startseite