For Multiple ADC circuits PCB layout grounding, why is "single point ground" important?

Question

I am reading this article from Maxim on mixed-signal circuits grounding: https://www.maximintegrated.com/en/app-notes/index.mvp/id/5450

Everything makes sense to me until I read the "Grounding Challenge of Multiple Mixed-Signal ICs". It shows the following diagram to indicate that the cut plane technique does not suit for the multiple mixed-signal ICs.

They think splitting ground plane into analog plane and digital plane is bad for multiple mixed-signal ICs. The reason they gave is: there is no single point ground any more.

Why is single point ground important in this case?

That some devices have different grounds (analog and digital, or on DC-DC converters power and signal) is mostly used to hint you into doing a better layouting job. Digital switching generates much noise. And if you let that noise feed directly into your analog ground, you may get wrong ADC measurements. How you implement that separation is mostly up to you. — jwsc, Oct 15 '15 at 07:16

Peter Smith · Accepted Answer · 2015-10-15T07:51:17.783

The reason is quite simply that we are trying to make a 'moat' with a single bridge across it. With two cuts in the plane, the analogue returns currents from each device can get mixed together, introducing noise from one set of ADC inputs to the other. In addition, we have provided a circular route for the digital returns to go around the analogue side of the ADCs.

Digital noise from ADC2 could take a path behind it, as could digital noise from ADC1. Put a little curved trace around the analogue side of ADC2 from the two cuts; this is where some digital noise could flow.

I have actually had to fix a board that did precisely this, and the faults were subtle and induced a great deal of hair pulling.

To avoid the issue, do the following (works for relatively slow analogue, fast analogue have different segregation requirements - Note 2):

Do not route digital power in the same area (on any layer) in the same area as the sensitive analogue signals. I have found that such power tends to re-radiate from other planes. Note 1.
Ensure the primary power source is on the digital side of the board. This ensures that all returns paths move away from the analogue side.
Do not take high speed tracks in the same area as the analogue circuitry (on any layer)
Arrange the ADCs / DACs or whatever such that there is a single gap in the return planes. If you have differing speed analogue signals, put the fastest ones closest to the gap.
If you are driving the analogue circuitry with a separate regulator, put the regulator such that is spans the split in the plane with the output and feedback (if used) on the analogue side. If using a ferrite (a very common practice), then the same placement rule applies.
Do separate the power either through a ferrite or regulator.

Note 1. This is primarily due to the limitations of layout tools. If I could make the tool attach a via to only specific layers, I would, but this is very difficult with most existing toolsets.

Note 2. Use a separate moated area (each with its own local ground and ferrite / regulator) for each section with high speed analogue signals. See this excellent guide for some more details.

[Update] Added note on slot antenna

The two cuts in the plane can produce a slot antenna, where a great deal of the digital noise can accumulate, depending on the frequency content and the aperture sizes and distances.

HTH

Thanks for your reply. Could you please explain why there will be circulating currents if there are two or more bridges? — richieqianle, Oct 23 '15 at 02:38
I need to be at a real keyboard for this and draw a couple of diagrams - maybe a couple of days. — Peter Smith, Oct 23 '15 at 17:47
Thanks for the answer. I had an arduino audio shield but there was a loty of noise from the digital board. So i am creating my own pcb. I read your excellent points but i have some questions. For point number 1. Can the parte be in the same layer though (Upper Copper) organized and grouped left to right so the analog and digital are separate apart? 2. What do you mean digital side of the board? Even the analog regulator goes there? Like Front copper layer? 3. You mean even in other layers, dont pass right below the analog circuits right? 4.Could you explain this please? What's return plane? — user1584421, Jan 20 '18 at 18:47
Thanks a lot! I have created a new question here: https://electronics.stackexchange.com/questions/352095/how-to-create-a-mixed-signal-pcb Could you at least explain number 4 and 5, because these two i did not understand them at all? Thanks a ton! — user1584421, Jan 25 '18 at 21:02

score 2 · Answer 2 · answered Oct 15 '15 at 18:49

This shows one possible way this can cause trouble...

Here most of the digital return current goes on the digital side, but some of it can go around through the analog side as show in the top arrow; especially at low frequencies.

If the regulators are placed such that straight line from them to the ADCs doesn't cross anything, then it likely wouldn't matter whether there is a cut in the plane or not.

score 1 · Answer 3 · answered Oct 10 '15 at 09:03

A single point ground prevents digital currents produced by an ADC chips getting onto analogue ground and creating noise that may disrupt an analogue signal chain.

If you have 2 ADCs (or more) then there is a concern that a digital current can flow thru the analogue part of the ground plane and back round to the digital plane via the other "single point connection". Some folk will use ferrite beads in series with the multiple single-point connections but, I don't think it is necessary. When you have earth planes (digital or not), return currents tend to flow in the part of the earth plane that is directly below the power plane (or track) so, providing the digital power plane (or track) doesn't extend across into the analogue section of the board then digital return currents won't even if you have multiple connections.

So, my advice is avoid power supply lines entering the analogue part of the circuit board or else make those lines clean with ferrite beads/filters to prevent digital "hot" currents flowing through any power connections that might be routed into the analogue section.

hi, thanks for your reply. Maxim app note suggest that it is bad to have two connection points in ground. And I am asking for the reasons behind that. — richieqianle, Oct 11 '15 at 05:08
The people who write app notes, sometimes don't know what they are talking about. The people that do know what they are talking about, don't always have time to write stuff. That was according to Rick Hartley, and what he says makes sense. Be careful with app notes (for the reasons above), treat them as wrong until proven right, rather than treat them right until proven wrong. — efox29, Oct 15 '15 at 03:23

score 1 · Answer 4 · answered Oct 20 '15 at 12:12

The truth is it depends on the frequencies you care about.

For low frequency systems and especially systems requiring precision DC performance "shared impedance" is the main enemy. So you want the analog and digital grounds to meet at a single point with mixed signal devices being located as close to that point as possible.

For high frequency systems on the other hand return currents will naturally follow the outgoing currents. The main enemy is anything that prevents that happening, so any signal passing (explicitly on a track or implicitly inside a chip) over a slot is bad as it will cause both magnetic emissions and difficult to predict return paths. If you don't care about precision DC then a solid ground plane is often the best bet.

If you need both then you want a single point for DC grounds but then bypass capacitors between the analog and digital ground planes to allow a direct return path for high frequency signals.

I also echo the comment from another answerer that appnotes are often full of rubbish.

For Multiple ADC circuits PCB layout grounding, why is "single point ground" important?

4 Answers4

Linked