Notifications
Q&A

High Speed Design - Which grounding strategy to choose?

+5
−0

Although I have done multiple PCB designs which passed FCC and CE equivalents using the MCU's/Multiple MCU's, I have a doubt about how to approach the high speed design using FPGA SoC - main thing that bothers me is choosing the right grounding strategy.

By the high-speed design I mean >2GHz memory layout where timings, impedance matching and length matching play the huge role not whether the design would pass the compliance testing but if the design would work at all.

I used to follow the approach similar to Olin's when doing the grounding strategy - https://electronics.stackexchange.com/questions/15135/decoupling-caps-pcb-layout/15143

I am usually putting the good ceramic capacitors very near to the pins of the MCU(mostly in 0603), connect them directly to the pins, join the ground's together(usually in a plane on top or one of the internal layers) and punch the via to the "main ground plane". The use of the power plane is usually avoided since good old 60mil trace is enough for low power devices.

This approach suit me fine even with multiple USB 2.0 Hubs, radio circuitry and dc-dc converters on PCB.

However when doing the DDR4-2666MHz memory layout the return path from the "punch to the nearest GND plane" via and the signal pad will influence the return path impedance of the signal.

Furthermore, FPGA board would be made as a SoM board attached with the carrier/motherboard. SoM board would then be connected with the carrier board "in one single place" - the connector. This leaves the i/o cables connected with the carrier board, which could be made by using the same layout approach as a regular "MCU board" minimizing the patch antenna influence.

Which approach would you follow?

Why should this post be closed?

0 comments

1 answer

+4
−0

You are right in that at high speeds, like over 2 GHz, things are different than in "ordinary" circuits. The post of mine that you quoted was written in the context of such ordinary circuits.

The lumped system approximation that is valid for ordinary boards fails at high frequencies. You have to think of traces as transmission lines.

For example, the free space wavelength of 2 GHz is 150 mm. Let's figure that due to transmission line effects on a board, the propagation speed is about half the speed of light. Now we have 75 mm wavelength. We generally have to start considering transmission line effects at about 1/10 the wavelength, so any trace more than about 7.5 mm (0.3 inches) gets more complicated.

The approach I mentioned in the linked post, where local ground nets contain the local high frequency currents with single point connections to the main ground, was intended for lumped systems. The main motivation there was to keep the local high frequency currents off the ground plane to avoid it becoming a patch antenna. The considerations at high frequencies are different.

At high frequencies, the return currents in the ground plane actually follow the path of the outgoing currents in X and Y (where X and Y are the normal board edge dimensions, and the planes are stacked in Z). This is true even if the ground plane is uninterrupted. This means that there is essentially a separate return path for each outgoing signal. Chips intended to run at such frequencies usually have ground pins near high speed output pins for this reason. You have to make sure in routing that the return currents to these ground pins aren't obstructed and don't need to take a circuitous route.

But what about the ground plane patch antenna problem? It still exists for the lower frequencies, but is actually less of a problem at high frequencies. That is because the return currents flow right underneath the outgoing currents.

There are no easy answers. Every layout and route is going to be the result of compromises between competing concerns. Really high frequency circuits tend to be more expensive for other reasons anyway, so a few extra copper layers is expected.

One possibility is to explicitly route the ground return lines directly underneath (or above) the outgoing lines in an adjacent layer. Sometimes you can use a local ground plane that extends to the high frequency chips and the high speed traces connecting them. This plane should be in an adjacent layer. Since the high frequency currents signals are all contained there, this plane can have a single (and therefore lower frequency) connection to the main ground.

There are no easy answers. High frequency design takes some intuition, experience, and often experimentation. If you get into trouble, go find a guy with a pointy hat and a wand.


elaborate a bit about "At high frequencies, the return currents in the ground plane actually follow the path of the outgoing currents in X and Y"

Let's say you have a trace that zig-zags across the board, with the next layer down being a ground plane. Now you send a signal down that single trace.

At low frequencies, the return current will take the path on the ground plane inversely proportional to resistance. For a consistent uninterrupted plane, that's a direct line.

This is different at high frequencies. Even if the ground plane is an uninterrupted layer, the return currents will follow the zig-zag path of the outgoing currents. Of course this doesn't suddenly happen at some magic frequency. As the frequency gets higher, the return currents follow the outgoing path more tightly.

You can think of the return currents being a blurry zig-zag, where the blurriness is related to the wavelength. The shorter the wavelength, the less the return path is blurred from the outgoing path. This also nicely degrades to the low frequency case where the return currents are a directly line. In that case, the wavelength is large, and the blurriness region much larger than the board.

This effect is due to the outgoing trace and the ground plane directly underneath it becoming a transmission line. It is no longer a lumped system.

What this means to a PCB designer is that at high frequencies, each outgoing signal essentially has its own return path. Those return paths should have return connections nearby the outgoing connections.

Note that differential signals do this explicitly by providing a separate return signal for each outgoing signal. The ground plane is then no longer directly involved in transmitting the signal itself. The differential signals can then be routed next to each other (sideways or on an adjacent plane) to try to maintain consistent transmission line characteristics over the whole route. This is one reason we see differential pairs being used for really high speed signals.

1 comment

@Olin. Always a pleasure to read the masters. Could you elaborate a bit about "At high frequencies, the return currents in the ground plane actually follow the path of the outgoing currents in X and Y etc." it's not very clear to my mind of poor mortal. ‭coquelicot‭ 19 days ago

Sign up to answer this question »