Robert Feranec · Transcript · · Updated
How to Decide on Your PCB Layer Ordering, Pouring and Stackup (with Rick Hartley) – Transcript
Video by Robert Feranec · Watch the original on YouTube
Summary
AI-generated from the transcript. Verify details against the source video.
- Rick Hartley explains that a transmission line consists of both a trace and its return path, which is important for board stack-up.
- Rick Hartley states that decoupling capacitors only work up to 2 or 300 megahertz and become inductors with faster rising edges.
- Rick Hartley points out that vias have the highest inductance of anything in the board stack-up.
Use this video with Pro
Reading, copying and transcript downloads are free. Create saved AI results for this video with a signed-in Pro account ($9/month).
Transcript
Search ignores accents. All transcript text stays visible.
This video is going to be all about stack-ups. And I really hope after you finish watching this video, you will have better understanding why you would like to order layers in your PCB specific way.
So, I really hope after watching this video you will completely understand, why you would like to order signal and ground and power plane layers in your PCBs specific way. And I really hope also after you watch this video, you will know how you would like to maybe order layers in your own PCBs.
We are going to start this video with some basic theory. Nothing complicated, okay? We just would like to see, what is happening around the tracks and also what is happening between the layers and tracks between the power planes and ground planes in your PCB.
We would like to talk a little bit about these fields because then, you will better understand why we would like to order layers specific way because of these fields. But as I said it’s not going to be nothing complicated.
It is just to help you to imagine better what is happening in your PCBs. Then, we will talk also about copper pour when you would like to pour for example ground or power planes on the same layer where your signals are.
We are going to talk about changing reference planes, so when your signal travels and you have to change reference planes, what is actually happening on your PCB and why you need to be careful and then, we are going to talk also about distances between, between layers in your stack-up, how the distance is important
for power planes or how the distance between signal layers and ground plane or power plane is important in your stack-up. And then, of course, we will have a look at some examples. We will talk about 4-layer stack-ups, 6-layer, 8-layer, up to 34-layer all the kind of different stack-ups.
We will have a look at some specific examples of these stack-ups, and we will try to understand, why specific layer ordering is good or bad for these specific stack-ups.
This video is based on my call with Rick Hartley. I would like to thank you very much to Rick for finding time for this call and I really hope you will find it useful, and you will find it interesting.
So, next I’m going to play the video from my call with Rick and as I mentioned before, we are going to start with fields. So, here it is. When you launch a signal into this transmission line and keep in mind, and I know you know this as well, a transmission line doesn’t consist of a trace.
It consists of a trace and its return path. You have to have both sides, you have to have both pieces of copper to have a transmission line. And that’s very important when understanding board stacks. So, when you launch energy into this transmission line, the energy starts out as a set of electric fields that travel into the dielectric space attaching themselves to the trace and to the planes.
Those electric, the energy in the electric fields causes the movement of electrons in the copper. The movement of electrons act as charge carriers to help move that energy through and also at the same time, to generate a magnetic field where the rest of the energy resides.
So, all of the energy in this case is in the electric and magnetic fields and it moves through the dielectric and attaches itself to this copper, because the copper helps create a lower impedance path. When you have an outer layer trace like this one, then the fields aren’t quite as well contained as they are on the inner layer.
And that’s a key component which we’ll talk about in a short while relative to board stack-up. But anyway, fields are better contained in this arrangement, than they are in that arrangement. Here is an example of a 4-layer board that I see a lot. I do a lot of consulting with people who call me up or email me and say Rick, I’ve got an EMI problem, I have a signal integrity problem, I have a this, I have a that.
And the very first question I ask them is what’s your board stack-up. I’m sure you know exactly why that’s the first question I ask. Because if they don’t get the board stack-up right, the rest is moot. And when I see this board stack-up, what concerns me, the reason this is a problem, if this were a digital board for example, and with signals on one going let’s say in the X direction and signals on two going in the Y direction.
The fact is the signals are going in opposite directions, one on the X one on the Y. So, the coupling that occurs between those lines is very small. But why is there coupling at all? Because both of these, the fields from both of these reference the ground plane on layer three.
The signals on one couple all the way to three, and the signals on two couple to three to develop their fields. Now, some of the energy from the signals on one, also couples into the fields for the signals on two.
And that’s why people often have EMI problems with a board like this. I see this a lot in the automotive industry, the US automotive industry. I don’t know about Europe, but in the US this is a commonly used board. Because they’re often using microcontrollers.
They don’t need to have a power plane, they can usually route power. Because micros typically have fairly slow rise times. And power delivery is not as critical as it would be with a high-end microprocessor. So, they will usually route power route signals and they’ll have one ground plane and three layers of routing.
And the reason this creates a problem is the amount of energy that’s coupled between layer 1 and layer 2 is very small. It’s not enough to cause signal integrity problems in a digital board, but it’s more than enough to set up enough common mode current to create an EMI problem.
And therein lies the rub. It might take tens of milliamps or even hundreds of milliamps of common coupling to cause a signal integrity problem. Because of our, because we have noise margins. ICs have noise margin. But EMI can be generated through a few microamps of common mode energy.
And it takes almost nothing to generate that low level of common mode current. So, does it mean? This is one way. Go ahead, sorry. Sorry for interrupting you, but I would like to ask. So, does it mean that even if you have like more layer stack-up, then, it is still better to have like ground plane, signal layer and ground plane comparing to ground plane, plane, then signals routed in X direction,
signals routed in Y direction and ground plane? This would be still bad if the signals are going out of the board. Not necessarily. The fact that you have two ground planes with two signals in between them, that’s where dielectric thickness comes into play.
Okay, so this is specially important for if it’s routed on top layer, then. That’s, that, it’s really a problem when it’s the outer two layers. Okay. That’s where this becomes a really serious problem. Now, what I generally tell people who contact me to do with this, is to treat the top layer, layer 1, as its own circuit board.
Now, keep in mind layer 2 and layer 3 are both, both directly referencing, I’m sorry, layer 2 and 4 are directly referencing the ground plane on 3, right? So, they’re in pretty good shape. What you need to do is to keep the fields from layer one out of that dielectric space between 2 and 3.
And how can we do that? By routing ground with the signals. There are a lot of people who will tell you, that pouring copper on signal layers or routing ground on signal layers is not a good idea.
And sometimes, it isn’t a good idea. There are times when it doesn’t help. But if you have a board like this, you have to do something with layer 1. And the only way you’re gonna control that energy is to have a coplanar return path.
Now, this is a board that was designed, it was redesigned by my friend Dan Baker. He’s an app engineer for NXP semiconductor. He works in the automotive industry. One of his customers contacted him with this problem and he had them reroute the board and route the grounds between the signals.
And it got rid of the problem. In truth, as Eric Bogatin pointed out with his Altium presentation last year, his Altium live presentation, connecting these ground traces only at both ends is probably not good enough.
Now, it worked in Dan’s case, but in truth, these ground traces should be, should be grounded every tenth wavelength of the maximum harmonic frequency in the signals. That’s how often they should be grounded.