Split Ground plane - to do or not to do? - Page 1
Forum section: electronics / beginners

author: Saimoun
author_rank: Frequent Contributor
timestamp: January 05, 2021, 05:55:56 pm
content: HiI keep reading online opposite answers to that question. This article even says both!https://www.autodesk.com/products/eagle/blog/8-pcb-grounding-rules/(see #2 and #8)Maybe I misunderstood something.I remember seeing in particular on learnEMC that many engineers would split their plane between analog and digital but keeping the plane whole would improve EMC.My question more precisely is about a board with an analog part and a digital part. Both are on each side of the board, with each their own power source (LDO). I designed the board so that the ground return path from the LDO's to the main power source do not cross.Having this - is it a good idea to split my ground planes (2 layer board) to only have one small connection point or should I leave the ground planes full?Thank you!Simon

author: Elasia
author_rank: Frequent Contributor
timestamp: January 05, 2021, 06:29:03 pm
content: Your goal is to control the fields. By having the return / reference plane close to the traces, you contain that energy between the source and destination. With enough spacing, splitting planes is not needed.. that said it completely depends on your board layout requirements as to if you should or not. If you cant have a reference plane then you can also use triplet traces with the trace having reference traces on each side instead of a planeThe worst thing to do is have a high frequency trace on one plane and then just go off a cliff into the sunset letting the fields escape

author: Neilm
author_rank: Super Contributor
timestamp: January 05, 2021, 06:57:13 pm
content: I have been bitten by the "must split 0V plane" too often at work. Some years ago, I was given a bunch of instruments to retest and fix as the EMC regulations had changed. In all cases the instrument performace was improved by having an unsplit 0V plane. Not all passed without additional work but I was able to bring the BOM cost of one instrument down by about 1% by removing all the ferrites that had been put in to get the unit to pass.Generally, I would only advocate that only spliting the plane if it is required for safety reasons - in which case they will be completely isolated.Remember, the return currents will always take the path it wants and generally that path is directly below the signal path. Also, remember that the power supplies to a chip are a thing. I have seen several compatent engineers point at a signal coming out of a chip and saying "this signal is referenced to 0VA" when the chip generating that signal was powered by a supply on a different reference.Keeping the above in mind, properly partitioning the circuit in blocks on the PCB and keeping sensitive bits away from noisy bits will "mostly" keep the sensitive bits unaffected.Note that if you are only on a 2 layer board then you are reasonably stuffed and you will almost have to split them.

author: Saimoun
author_rank: Frequent Contributor
timestamp: January 05, 2021, 07:14:46 pm
content: Quote from: Elasia on January 05, 2021, 06:29:03 pmNot sure if that helped but it was very poeticThank you both for your answers. It's really nice to hear and confirms my ideas on the subject.Just an additional question regarding how the current will flow, and in particular the return path. If I have the following:5V source (f.x. USB plug) --> 3.3V LDO -> analog IC -> 32 ohm loadwill the return path be32 ohm load GND pin -> 5V source GND pinor will it go through the GND of the analog IC first, and then the GND of the LDO, and finally back to the 5V source?

author: Saimoun
author_rank: Frequent Contributor
timestamp: January 05, 2021, 07:25:46 pm
content: If it makes more sense visually:In this example, would the return path take the blue arrow, the green arrow, or both at the same time?PS: I know in this example I could move the USB plug closer to the LDO, but there are other factors and I would rather keep the USB plug where it is.

author: Elasia
author_rank: Frequent Contributor
timestamp: January 06, 2021, 05:08:15 am
content: This video from Robert Feranec might be of better useAs for how your fields will return it will depend on both your geometry and frequency as the impedance will change as fq changes causing the fields to flow differently around your layout

author: EEEnthusiast
author_rank: Frequent Contributor
timestamp: January 06, 2021, 06:04:43 am
content: There is no universal answer to this question. But having different ground net names in the schematics will help to group them together in the layout. In case of high current devices like relay, power transistors etc, it may be better to keep them on a separate plane in order to avoid IR drops on your sensitive grounds. For EMI cases, having a split plane can cause more issues , if there are signals crossing the splits. The return current takes a longer route and this can cause unwanted EMI or noise pickups. But careful placement of the components and laying out the traces well, will most likely cause your design to work well with a single unsplit ground.As a rule of thumb1. Precision analog + Digital + High Power : Split ground will improve noise (Not EMI, but the overall noise coupling from power electronics & digital to the precision analog section)2. RF + Digital boards : Single ground plane designs perform better to help with EMI3. Digital + High power : Splitting will be safer4. A lot of ADCs and DACs + Digital : Split ground is better as it helps to place the analog and digital components in separate areas of the PCB. Less chances of digital component being placed close to analog ones.But one thing to remember : When you split the plane, ensure that no high speed lines crosses over the split.

author: David Hess
author_rank: Super Contributor
timestamp: January 06, 2021, 03:15:10 pm
content: The return currents create differences in potential even within a ground plane which is what makes a single plane unsuitable for precision analog applications unless differential signalling is used, and even then differential signalling is ultimately lower performance. Sometimes slots can be cut in a ground plane to route return currents around sensitive areas.The part I always found fascinating is application notes for high resolution converters which recommend connecting the digital and analog ground planes at the converter. That makes complete sense however what happens when you have more than one converter?

author: Siwastaja
author_rank: Super Contributor
timestamp: January 07, 2021, 09:50:45 am
content: For a beginner who needs to ask, follow the rule of keeping things simple.Again, splitting planes may be beneficial sometimes but such cases are always complex. It also creates a possibility for doing much much worse.Using one full low-impedance plane is never a catastrophic failure, so default on that if unsure.Splits are useful for DC accuracy; DC current flows all over and can cause voltage shifts in single ended systems. But that's not what you are usually doing; when DC accuracy is needed, you tend to use differential signaling instead. (A split plane is like a poor man's reference voltage trace, just made wider than you would do in an actually differential system; treat it as such.)But EMI is all about high frequencies, and high frequency currents (over a few MHz, say) donotrun all over like DC, instead they follow the route under the trace in the plane even without the split! This makesplacementof components and traces important. Keep a bit of extra distance to "low-noise" regions. Even if the sections share the same ground plane, the high frequency return currents under a CPU, for example, don't spread far from there.And if you accidentally split the plane under such high-frequency return current, then you are creating an EMI catastrophe. Happens easily in a complex design if you try to add even more complexity with the splits.

author: perdrix
author_rank: Frequent Contributor
timestamp: January 07, 2021, 10:29:28 am
content: This isn't a simple question to answer, and it certainly won't fit into a forum post.An excellent coverage of the problem can be found in Henry Ott's book "Electromagnetic Compatability Engineering":http://www.hottconsultants.com/book.htmlwhich will give you an excellent grounding in the relevant theory and practice. I strongly recommend it (and there aren't very many books to which I give that accolade).David

author: Saimoun
author_rank: Frequent Contributor
timestamp: January 09, 2021, 02:17:18 pm
content: Thank you all very much for your replies!! Very helpful as always and very appreciatedI was busy finalizing the board and contacting some manufacturers, but I went through your answers.@Elasia: that video blew my mind actually@perdrix: will definitely read that book!!I understand it's a complicated question, but I guess the short answer would be it helps noise but does not help EMC. In my case I am more concerned about EMC and I tried to reduce noise by placing the components smartly, so I'll keep the ground plane full

author: janoc
author_rank: Super Contributor
timestamp: January 09, 2021, 02:28:59 pm
content: Here is a very good (and accessible!) video by Rick Harley on this subject. He specifically talks about the splitting (or not) of ground planes as well:TLDR; Don't do it except in a few very specific situations.

author: Saimoun
author_rank: Frequent Contributor
timestamp: January 09, 2021, 04:12:47 pm
content: Amazing janoc - Merci !

author: robertferanec
author_rank: Regular Contributor
timestamp: January 14, 2021, 12:01:54 pm
content: I do not normally split grounds. I usually use solid GND planes for the kind of boards I design (mostly processor boards)BTW: I asked Rick Hartley about ground splitting. And maybe it can help:

author: Dennis Frie
author_rank: Contributor
timestamp: January 14, 2021, 07:52:20 pm
content: I've been doing a lot of high-power + low noise designs at work. We've often had the discussion and tested cutouts in the ground plane. While it does help in specific cases, it often seems to cause way more problems than it solves, at least in my experience. I would go with a solid plane unless really needed.

author: Saimoun
author_rank: Frequent Contributor
timestamp: February 15, 2021, 04:28:48 pm
content: @robertferanec: yes I already watched it ha ha - thank you@Dennis: nice to know! Where do you work?Just FYI I went for a solid GND place, no issues at all