High-speed signals crossing a split-ground

Hi,

I'm working a design that has isolation between two sub-systems on one PCB (the grounds are separate). One side is a "high-speed" digital side with FPGAs and DDR doing DSP and the other side is an analog side that has high-resolution 24-bit ADCs and DACs.

I'm planning on using DC-balanced capacitive coupling to move data back and forth between the two sides. My concern is at happens when I AC-couple my signals across cross the split-grounds? Am I creating more noise due to the return/image current not having a continuous return plane? I have worked out both single-ended AC-coupling and schemes using LVDS/CML.

The capacitively coupled signals are

Reply to
ee_ether
Loading thread data ...

Sounds like you are rolling your own?

Might be smarter/easier to look at Analog Devices Digital Isolators ?

-jg

Reply to
-jg

Isolation for safety purposes should probably be done in front of the ADC. In most other cases splitting ground creates more problems than it solves. If you can show that you need roughly more than 60 dB of isolation between your circuits then you might need to resort to splitting grounds, but you need to know what you are doing very well. AC coupled or not return currents will still want to travel through the plane, so you can only split it under the chip. The best resource for discussions on this topic is the Signal Integrity mailing list. The SI-List archive can be found at

formatting link

/Mikhail

Reply to
MM

Are you sure that split ground planes would really help? Think about the layout of your board, and the way current on the ground plane would flow. DC ground currents aim to follow a direct path on the ground plane, and high frequency currents aim to minimize the current loop area (i.e., minimal impedance in both cases). If the ground currents created by the digital logic are flowing around the digital parts, there is no reason they should wander off under the analogue parts to cause noise there.

(That's my understanding of the theory - I've not worked on any high frequency, high sensitivity analogue boards in practice.)

Reply to
David Brown

The OP mentioned a 24 bit ADC, which suggests much more than

60dB is needed.

If it is differential shouldn't it be mostly balanced?

(snip)

-- glen

Reply to
glen herrmannsfeldt

I agree with jg - the AD parts are worth looking into. They're not that expensive, and they've been tested to international standards for high voltage isolation. That will help with agency certification, assuming that your product requires it.

Chris

Reply to
Chris Abele

My experiences have shown:

You can probably run data lines single-ended, with series resistors to slow the edges and limit the current. You are right about the long return current path causing radiated noise, but the random nature of the data lines will make it rather spread-spectrum, so it should be tolerable. Clocks, on the other hand, should only cross a split-plane as differential signals. You still get radiated emissions, but much less. The diff pair over split plane can be modeled as a diff pair over continuous plane plus a small loop antenna with dimensions equal to the split width and the pair spacing. So make the split small and the lvds traces close together. Henry Ott covered this in one of his books; sorry I don't remember which one.

Barry

Reply to
Barry

Glen,

I noticed this fact, but taken out of the context of application it doesn't necessarily mean anything.

Balanced doesn't mean that return current for one side actually uses another side.

/Mikhail

Reply to
MM

(snip)

(after I wrote)

I qualified with "mostly". One would have to look at the individual case. Properly terminated, it is hard to see whereelse the current would go, but signals aren't always properly terminated.

-- glen

Reply to
glen herrmannsfeldt

Please check out this article by Eric Bogatin:

formatting link

It should be available on his web site

formatting link
as well in a better format but I couldn't find it quickly...

/Mikhail

Reply to
MM

formatting link

I will look at it, though it is the OP who really needs to know.

Also, for a similar question not so long ago I was calculating the capacitance of a ground plane. (Even with no other plate nearby the capacitance is still there. Much higher with other planes nearby.)

thanks,

-- glen

Reply to
glen herrmannsfeldt

ell

That's an interesting article. I had never known that there was so little coupling in a differential pair, although I should have known that. A class I took made the point that when it comes to cross coupling between unrelated signals, you only need to consider signals running on different layers with no ground/power plane between them. The coupling between adjacent signals is so small that it can be ignored.

In fact, would that make a good differential pair, to run the traces opposite each other with a ground plane between them? The ground currents would clearly cancel in that case. I guess in practice it would be hard to do unless you were willing to use a lot of plane layers so that the two traces see the same environment.

But it wouldn't be hard to put two signal layers between two plane layers. That would be very similar to the shielded, twisted-pair mentioned in the article. I prefer to keep my power planes on adjacent layers to provide the maximum decoupling, but this could be done locally if you were using eight or more layers.

Rick

Reply to
rickman

... snip ...

The major problem solved by separated grounds is common noise by spikes on the power lines. So you want to ensure the two grounds are completely separate, and have only one common point, which does not include power supply leads that can provide common impedances.

--
 [mail]: Chuck F (cbfalconer at maineline dot net) 
 [page]: 
 Click to see the full signature
Reply to
CBFalconer

In comp.arch.fpga rickman wrote: (Someone wrote)

Bogatin:

formatting link

I didn't get a chance to read it yet. What should be important is that the impedance of the two are equal. Well, also that the lengths are equal. The lines on modern motherboards between CPU and memory often follow a zig-zag path to equalize the lengths.

More usual is to run a ground between the traces, but that should work, too. But you can't put them so close together or they will couple to other signals.

-- glen

Reply to
glen herrmannsfeldt

I don't think so. Two sides of such a pair would be subjected to different common mode (or in fact not so common) noise which wouldn't be cancelled by a receiver. It might be irrelevant for the types of the digital signals the OP is interested in, but it certainly matters for sensitive analog signals.

It's not so clear. At high frequencies the currents flow on the surface of the plane. In fact, this can and frequently is used to separate analog from digital when space is limited, i.e. you can treat a single physical GND plane as almost two separate GND planes relative to the traces above and below it.

/Mikhail

Reply to
MM

ElectronDepot website is not affiliated with any of the manufacturers or service providers discussed here. All logos and trade names are the property of their respective owners.