Noise isolation of digital and analog power rails - Page 1
Forum section: electronics / projects

author: ricko_uk
author_rank: Super Contributor
timestamp: November 30, 2020, 03:34:57 pm
content: Hi,to separate digital noise from the analog section (both supplied by the same linear regulator) you can use ferrite beads, or LC filters.1) Are there others?2) Which one is most effective in removing the noise?3) does placing diodes in series between the regulator output and the two separate rails help? Do diodes prevent noise going "back" into the other rail? In principle maybe not but I am thinking about reverse leakage current...?4) Finally, in an LC filter, how do I prevent ringing or noise amplification at the resonant frequency? If there is such solution...I am designing a PCB that acquires very small signals up to 200KHz and want it to be as noise free as possible but also have a micro running at 20MHz.Thank you

author: fcb
author_rank: Super Contributor
timestamp: November 30, 2020, 03:46:41 pm
content: Don't forget RC filters too.20MHz is quite low for ferrite bead filters - use them in PI configuration with smallish capacitors, although it sounds like you need to experiment to see how bad your problem is and then you can make additions and quantatively judge the results.

author: Jan Audio
author_rank: Frequent Contributor
timestamp: November 30, 2020, 04:22:03 pm
content: Ofcourse you know this already and i just want to mention it :Best to have seperate ground lines for everything, especially seperate digital and analog.

author: exe
author_rank: Unknown
timestamp: November 30, 2020, 04:35:00 pm
content: You can use dedicated supply rails for analog and digital ICs, "LDOs are cheap" (c) me.

author: Boscoe
author_rank: Frequent Contributor
timestamp: November 30, 2020, 04:41:08 pm
content: I often use LC filters in before a good linear reg. Get the LC cutoff frequency just low enough where the regulator is effective. Use low value high Q inductors in series for high frequency rejection.

author: T3sl4co1l
author_rank: Super Contributor
timestamp: November 30, 2020, 10:22:00 pm
content: Well, a ferrite bead is itself just an RLC element. Or if by "LC filter" you mean one without significant losses, well, you're depending on surrounding circuitry to provide loss -- there has to be loss somewhere, and in the classic signals case, the source and/or load are terminated. You may not be so lucky in a power distribution network (PDN)! "RLC filter" is most general. We might include losses within the filter, to dampen the network regardless of source/load resistances. This allows performance within certain bounds, while being independent of source or load impedance.The problem with ferrite beads is more that,1. The impedance isn't very high, and we often need higher impedances at low frequencies2. They saturate easily, typically 5-20% of DC rating. (The DC rating is thermal only!)So we can get away with them for some applications, but the attenuation is pretty meager, and it's even less at high currents.As for grounding,pleaseuse a solid ground plane (or as solid as can be had), andplease don'tslice it up unless you know, very exactly, what you are doing and why. There's almost never a good reason for doing it.The priority is keeping reference voltages (opamp inputs, ADC grounds?) consistent. This can be done with differential (Kelvin) connections over contiguous ground plane, and components can be laid out and routed in a star or tree pattern, so that digital and switching currents are on opposite sides of quiet analog things.Tim

author: KT88
author_rank: Frequent Contributor
timestamp: December 01, 2020, 09:28:55 am
content: Quote...well, sort of... This could be misleading and result into having split grounds for AGND and DGND, a Zombie concept from the past that does the opposite of what it is supposed to do.that said: never split the ground potential into AGND and DGND on the PCB! The purpose of these pins is to provide dedicated, clean supply rails to the analog section of the converter by not sharing the same bond wires.What should be done though is to partition the PCB into different sections as there are analog inputs, analog outputs, digital interface between ADC and controller/FPGA (in case the ADC isn't integrated) and power supply. Especially analog and digital traces must not share the same current return path. In most cases it is not nescesary to have slots in between sections of the GND plane - even with fast 18- or 20-bit fast SAR converters. Good references for that can be found at ADI or TI if you look for high-res fast ADC's eval-boards. The supplys on these boards are a good hint how to do it as well...CheersAndreas

author: tszaboo
author_rank: Super Contributor
timestamp: December 01, 2020, 10:41:05 am
content: Placing a separate LDO is often enough. And placing LC, RC and other filters often work, but the best way to get rid of noise is PSRR. Often replacing a crappy opamp with something that has higher PSRR, can yield 20-40dB noise reduction in your signal. And dont just look at the datasheet headline, and typical characteristics. That's usually defined at 10Hz or so, and that has more to do with "offset voltage vs power supply" than real PSRR. Look for the bode plot. Hint: higher PSRR at higher frequencies usually the result of higher GBW.And please dont split the ground, just have a complete groundplane.

author: ricko_uk
author_rank: Super Contributor
timestamp: December 01, 2020, 12:24:32 pm
content: Thank you all !!Ref the ground plane, yes I kept it al solid and split only the power ones.Thank you

author: KT88
author_rank: Frequent Contributor
timestamp: December 01, 2020, 12:50:49 pm
content: Don't split the power GND as well - same story as with converters.

author: Jan Audio
author_rank: Frequent Contributor
timestamp: December 01, 2020, 04:07:51 pm
content: You lost me KT88 i dont understand, please make a drawing of what is good and not good.What did i say not right ?, or maybe i forgot to mention something.Reading the MCU manuals i see the DSPIC has to be first in chain,this is the same as seperate ground lines.By example i made a VCO, with connecting the two VCOs together on 1 ground line, the VCOs will be reset by the other in some cases,with seperate ground lines they have a nice drift without reset.

author: Ice-Tea
author_rank: Super Contributor
timestamp: December 01, 2020, 04:31:48 pm
content: Something to consider when using multiple LDO's: not all of them offer the same quality of "barrier" against noise, especially at higher frequencies. Look for "PSRR" in datasheets and select accordingly if needed.

author: KT88
author_rank: Frequent Contributor
timestamp: December 01, 2020, 04:57:04 pm
content: @Jan Audio: your statement I quoted is correct, but might be misunderstood. The possible misunderstanding woud be to create an AGND- and a seperate DGND plane that then is somehow hooked together by a ferrite bead or a resistor. These joints are usually positioned under the converter. This would be a big mistake.The other way to understand it is that one takes care of the current return paths to make sure that different signals are not superimposed with each other. This is not only true for analog vs. digital but also between analog and analog as well as digital and digital. If you mean just the latter we are in violent agreement...CheersAndreas

author: radiolistener
author_rank: Super Contributor
timestamp: December 01, 2020, 05:22:44 pm
content: Quote from: KT88 on December 01, 2020, 09:28:55 amAs I know, if your circuit is sensitive to noise, you're needs to use separate AGND and DGND. And AGND and DGND should be connected through single point, otherwise you will have ground loops which will works like antenna for noise emission and reception.

author: Ice-Tea
author_rank: Super Contributor
timestamp: December 01, 2020, 05:30:47 pm
content: You can fill pages and books (and it has been done...) with discussions about split power planes. As has been mentioned a few times: more often than not it introduces more problems than it solves. Except for a few exceptions, you're better served with a low impedance (ie continuous) ground plane together with carefull positioning of your function blocks on your PCB.

author: radiolistener
author_rank: Super Contributor
timestamp: December 01, 2020, 05:40:49 pm
content: Quote from: KT88 on December 01, 2020, 12:50:49 pmfor mixed signal processing circuits, it it is mandatory to split digital and analog grounds. This is needed to avoid noise and interferences from digital part of circuit.Here is example of recommended ground design:Also here is tutorial from Analog Devices about grounding:https://www.analog.com/media/en/training-seminars/tutorials/MT-031.pdf

author: Ice-Tea
author_rank: Super Contributor
timestamp: December 01, 2020, 05:56:17 pm
content: Here's a suggestion not to partition ground planes:https://www.autodesk.com/products/eagle/blog/everyday-app-note-successfully-design-mixed-signal-pcb-partitioning/Here's separating analog and digital grounds listed as one of the worst possible ideas:https://learnemc.com/some-of-the-worst-emc-design-guidelinesWe can slap each other with app notes and white papers all day long (as I previously mentioned: books can and have been filled with this discussion). I'm sure there's scenarios where you may actually need separated grounds but I'm pretty sure you're more likely to be bitten in the ass by doing so rather than by not doing so.

author: pwlps
author_rank: Frequent Contributor
timestamp: December 01, 2020, 07:00:54 pm
content: I think I would agree with Ice-Tea.Using separate ground planes is obvious if an optical coupling is used between analog and digital sections (e.g. via voltage-to-frequency conversion, some of my lab instruments are using this principle), otherwise it's difficult to formulate any general rules.

author: uer166
author_rank: Super Contributor
timestamp: December 01, 2020, 07:53:00 pm
content: Quote from: radiolistener on December 01, 2020, 05:40:49 pmThat is almost never the case, especially for mixed-signal circuits. Unless you have some edge cases like very high currents superimposed onto very small voltage measurements (say, current shunts, where Kelvin connections might be appropriate). The entire idea breaks down when you have, for example, multiple ADCs in a system, chopping up the ground planes into many chunks, each becoming its' own reference and many tie points. It will be worse for SI, EMI, and will suck every time.What youshoulddo, unless there is a very explicit good reason is:separate analog and digital signals that go over the same, uninterrupted ground plane. This advice of DGND and AGND is outdated and unhelpful, and usually wrong, including datasheets and some appnotes that are written by interns or whatever.

author: KT88
author_rank: Frequent Contributor
timestamp: December 01, 2020, 08:02:21 pm
content: I'm aware of the MT-031 and there is nothing wrong with it.If you still build systems like that, you would do it that way. However this kind of system engineering dates back in the 60's or 70's even 80's. Back then (regulated-) power supplies were linear (cooling requirements), large, heavy and very expensive. If you open up some HP or other gear of that period you'll find a big transformer, heat sinks and very often a (noisy) fan. From there the supply rails were distributed across the system.A few things helped to make it work:1. Proper system design like described in MT-031 --> noise (common-mode-) between supply rails was taken care of in the design thus it can be kept fairly low.2. Converters at that time were usually bi-polar with structures > 1micron and R2R architectures --> internal nodes were lower impedance, slower Ft and farther apart thus capacitive coupling between digital and analog was considerably weaker.3. 12bit, 1Msps ADCs were considered 'high-end' back then --> 1LSB of a 12Bit converter is much coarser than an LSB of a 24-Bit ADC...That said, a system like that worked back then - and still does.These days systems often times utilize some sort of point-of-load power supply concept. The PoL regulators could be both linear or switched mode ones. That way the required power rails are generated dirctly on each PCB (there are exceptions possible, of course). For noisy environments or HV applications isolated DC/DC converters are not a problem anymore.As a result of that only one supply voltage needs to be provided to a PCB. Having only one GND is now a viable (and desireble) option for most systems.In case PCBs exist on different GND potentials devices with a wide common-mode range are used (galvanically coupled or isolated depending on the system requirements).That was a brief system level consideration...On part level there are many paths for noise to enter a converter: The least critical ones are the analog inputs as they can be equipped with an AAF to keep unwanted frequency content out.All other inputs - and every pin of an ADC (or DAC) has to be considered as an input! Unfortunately no inherent bandwidth limitation is available for them...I skip the countless details on that in this post as it is quite lengthy already.Now to the reason why AGND and DGND must be one GND on the PCB:1. High-res ADCs can lose a lot of their performanc at much lower levels of noise just because they are able to resolve a lot smaller (noise-) signals. I guess most people won't be happy with a 24-Bit, 1MSPS ADC that puts out only 12 steady bits of data...2. Structures are much smaller and designd in some kind of CMOS utilizing mostly switched-cap architectures that are high impedance (some caps are as small as some aF (atto-Farads). even the faintest charge picked up from somwhere would srew up the sampling and conversion process.When it comes to seperate grounds on the PCB, noise between the analog and the digital section of a (high-res-) converter WILL inject charge into the fragile analog part.Similar hazard would happen when analog and digital section would share a single bond wire. The PSRR at high frequencies barely exists and noise currents generated in the digital part would interfere with the analog part both altering the state of charge in the CAPDAC as well as noise added to amplifiers, buffers, comparators and reference voltages...This is the reason for having different GND pins on a converter - it relates to the INTERNAL supplies - not the external circuit.To make it a bit more confusing in the end of this post: seperate bypassing of AVDD and DVDD is still a must... (exept for ADCs that are supposed to run on one supply rail).CheersAndreas

author: tszaboo
author_rank: Super Contributor
timestamp: December 02, 2020, 12:05:27 am
content: Quote from: pwlps on December 01, 2020, 07:00:54 pmEven then, you need a loop to create digital noise in the analoge circuits. If you place the digital ICs on one side of the board, the analog on the other, place an optical isolator in between, and you have two ground planes... Then what? There is no current going in between the two circuits, so why would any current go between the ground planes?OP:Noise on the ground doesnt magically manifest itself, it doesnt just radiate . You need current loops. you need high impedance sections, that share current between an analoge ad a digital part. You need traces that cross planes. When you break up your plane, you create these very issue.Quote from: radiolistener on December 01, 2020, 05:40:49 pmPlease delete this. If you read the contest, this is for a system, that has backplanes, and separate digital and analog cards. This is very bad advice.

author: T3sl4co1l
author_rank: Super Contributor
timestamp: December 02, 2020, 12:52:10 am
content: Quote from: Jan Audio on December 01, 2020, 04:07:51 pmThe reason is, your original quote oversimplifies the situation, leaving it far too vague.If you can draw a diagram of your example, showing all supply, signal and ground paths (and estimates of their impedances), then the situation is definite, and the resolution is no longer mysterious, but obvious.These things are unfortunately just a little too complex, to have much luck at explaining them in brief postings. I'm not blaming you for this -- I tend to shy away from such explanations myself for this reason.Tim

author: David Hess
author_rank: Super Contributor
timestamp: December 02, 2020, 12:56:56 am
content: Quote from: ricko_uk on November 30, 2020, 03:34:57 pmPut a low resistance in parallel with the inductance to lower the Q. This lowers suppression of the filter at low frequencies but removes the peak at the resonant frequency. In old designs it is common to see the inductor wound around the resistor.

author: David Hess
author_rank: Super Contributor
timestamp: December 02, 2020, 01:06:10 am
content: Quote from: KT88 on December 01, 2020, 08:02:21 pmWe must have different expectations of high resolution converters, and high precision circuits, because the first thing I do is get rid of the combined analog and digital ground plane because the digital return currents in the plane create too much noise in the converter. They must be diverted by cutting slots into the ground plain, and the eventual outcome is if I had started with separate planes connected to a single point ground, which is where I would start anyway.My schematics explicitly show separate grounds, single point grounds, and whatever multiple separate connections to the same node are called.

author: T3sl4co1l
author_rank: Super Contributor
timestamp: December 02, 2020, 01:11:01 am
content: Quote from: uer166 on December 01, 2020, 07:53:00 pmA better way to say this might be: take signal reference (ground) at the same point as the signal source, and treat it differentially, as a Kelvin connection, say.Now it becomes apparent that:1. You aren't using this connection for power grounding: anything that might inject AC interference into the signal (or have stability issues with the long trace inductance, e.g. opamps) is prohibited!1a. Indeed, you could bypass it to local ground, but then, that limits the bandwidth of your differential signal measurement -- and you need that as good as whatever the bandwidth of your measurement is. (And if you do filter it, filter both signal and reference, together, so as to maintain reasonable CMRR.)2. You make a differential measurement, so that your reading is referenced to whatever the source is,as the source sees it, thus getting the exact signal as desired.3. You still have ground plane under everything, shielding sources of interference, and keeping a low impedance between sections, so that it's unlikely that your extra reference trace picks up noise to begin with. And even if it does, you're doing a differential measurement, or can employ filtering at the end of the route.Such connections can be made using 0-ohm jumpers, or with no physical components at all, using net bridges (look up how to create these in your specific EDA tool). You place the bridge at the reference location (your "star ground" as it were, but we're doing something more comprehensive than that, now), and route the new signal net as any other.And you can always locally filter VCC/VEE to a section, distributing power as a ladder, or a shallow tree, etc. Again, filtering is determined by PSRR, permissible crosstalk, noise levels (especially from converters, but LDOs can be quite noisy for some applications still) and acceptable filtering (since it takes a lot of large components to get a lot of attenuation at low frequencies; or capacitance multipliers might be used, at expense to some DC voltage drop, and to some regulation).You probably wouldn't have VDD (i.e., digital supply) powering VCC (analog supply), but this might prove convenient on some systems where a 0-2.5-5V supply, or AC coupling, is acceptable (or 0-1.65-3.3, or..). In that case, same story, consider the noise level of VDD and provide adequate filtering to VCC.Tim

author: T3sl4co1l
author_rank: Super Contributor
timestamp: December 02, 2020, 01:22:14 am
content: Quote from: David Hess on December 02, 2020, 01:06:10 amFWIW, I did a design and layout with 24b ADCs -- the slow serial S-D kind with differential inputs and programmable gain, for what it's worth. It used +/-15V supplies (PoL converter, modestly filtered) for the analog section, and plane VDD for converter supply (though I think the VDDA side had a ferrite bead and ceramic caps for filtering?). Layout was with analog on one corner of the board, digital on the far end. (I had marked likely ground slot locations on the design, but the customer declined using them, which is fine.) The acquired samples weren't exceptionally clean, however they were within datasheet expectations (I think it was around 60 counts RMS), and the slight excess was easily attributable to the op-amp in front. So it seems to be a success, and no revisions were made. (I wasn't involved in EMC testing, so don't know how the readings were affected by it, if any.)If you're talking higher bandwidth (which, up to about 100kSps is achievable at 24b, beyond that you hit the Johnson-Nyquist limit, isn't it?), attention may need to be paid even just to common mode currents coming in from the external signals, even if your inputs are modestly high impedance. That is, the ground plane itself may have enough impedance to matter.Tim

author: David Hess
author_rank: Super Contributor
timestamp: December 02, 2020, 03:32:18 am
content: Quote from: T3sl4co1l on December 02, 2020, 01:22:14 amWhere it really matters is with sampling converters however delta-sigma converters can still be affected. With integrating converters, which includes delta-sigma converters, problems may manifest as higher low frequency noise or poor linearity.QuoteThat is a real problem which requires careful attention to the interfacing. These days I start out very suspicious about any high resolution application if the control signals are not isolated in some way at the high resolution converter and this gets taken to extremes in the highest resolution multimeters; it is not uncommon to find transformer isolation, optocouplers made from discrete parts, or opto-interrupters used in place of optocouplers because the later were not good enough. And common mode rejection at the analog input is important if return currents are moving the converter's common mode reference around.

author: Jan Audio
author_rank: Frequent Contributor
timestamp: December 02, 2020, 02:27:42 pm
content: For me its easy, i dont dont know what a ground-plane is, i have a idea and dont need to know too keep things simple.

author: tszaboo
author_rank: Super Contributor
timestamp: December 02, 2020, 03:52:43 pm
content: Quote from: David Hess on December 02, 2020, 03:32:18 amI'm sorry, but that is not the reason for the isolation. A DMM input is floating, you could connect it to 230V common mode voltage, while the digital part is earthed. I've made boards that had 50A current sources and sinks, high speed microcontrollers, and 24 bit converters on them. For that, you reference all the analog signals to a voltage that is not your ground, and you place the reference voltage next to the ADC, and keep the digital signals and analog signals on different sides of the board. If you have a fast rising edge signal, like SPI, all the return current stays below the trace, your analog signals dont even see that. This system worked with a few PPM accuracy.There are just simple rules, that are even highlighted in the ADCs datasheet. Dont communicate with it while it is converting. Use differential measurement if you have enough inputs. Delta-sigma is especially simple, as it typically can be driven by few KOhm sources, so you could filter out all the noise. The input is integrating, all those MHz+ noise gets integrated out.The real bastards are those high speed 100+KSPS 20+bit SAR ADCs, they have to be driven by a high GBW opamp, and noise could be picked up during the entire conversion. And look at this:https://www.analog.com/media/en/technical-documentation/data-sheets/238024fa.pdfQuoteThey even went ahead and named all the grounds GND.