Mixed signal ground planes - Page 1
Forum section: electronics / general

author: IanJ
author_rank: Unknown
timestamp: May 31, 2015, 08:20:03 pm
content: Hi all,I haven't laid out a helluva lot of mixed signal boards where the grounding is likely to be as crucial as it will be on this design and have been deliberating on the ground plane.There's seems to be two camps where one says just lay down one big ground plane and let the grounding for each IC do it's own thing (as long as the ground plane is comprehensive enough), and two which says to group route the grounding accordingly (star the grounding) back to a central point.I have opted for option two, and as you can see below, albeit not optimized fully, shows the digital, analogue and power supply sections all routing back to the battery terminals.I just wondered how others have experienced such issues.The analogue section consists of an 18bit DAC c/w Vref, the digital a uController, the power supply a low current buck converter. Battery is 18v and about 10mA max.NB. The main DAC digital ground does route the the main digital ground section.This is not a production design, just a hobby project.Ian.

author: nctnico
author_rank: Super Contributor
timestamp: May 31, 2015, 08:54:01 pm
content: Don't split power planes but use ferrite beads and filters (for example an extra regulator) in the power supply to keep the currents flowing where you want them to flow. If you start with a project which has sensitive analog stuff start by drawing a diagram of the power supply and translate that into how the various blocks should be placed on the PCB. Getting the power supply right can be a design task in its own.

author: c4757p
author_rank: Super Contributor
timestamp: May 31, 2015, 08:58:55 pm
content: I will occasionally make small 'incisions' in the ground plane to guide currents a bit (for instance, to create a channel for large currents to flow past a sensitive analog section, if I had no way to just move the section), but I don't really split them. That's just asking for trouble.

author: IanJ
author_rank: Unknown
timestamp: May 31, 2015, 09:27:43 pm
content: Quote from: c4757p on May 31, 2015, 08:58:55 pmI have built in some solder mask resist pads along the gaps so I can jumper across the areas thus leaving incisions. Will be interesting to compare once I get this first version up & running.Ian

author: T3sl4co1l
author_rank: Super Contributor
timestamp: May 31, 2015, 09:54:27 pm
content: The key qualifier is this:Do you ever have anything connecting between subcircuits?If the answer is no, you can split them and it will make no difference.If the answer is yes, then consider the effect of that split voltage on any signals that might cross. And on the signal current carried by that signal, inducing more voltage in the split than otherwise.The mortal sin is crossing signals over a ground split.If you can route signals down and around the split (which avoids inducing voltage across the split -- see: path of least impedance), then one might rightly question why make the split at all?If you're only making the split because you have no reason not to, you're probably missing the point.Note that "signals between" includes wires connecting to the board. Or even just radiation into space from the board itself -- conducted and radiated emissions are a big reason not to split planes.Ultimately, splitting is almost always avoidable. Best practice is always to route signals only where they must go, and keep sensitive signals away from other signals' path of least impedance. Segregate the layout into neat subcircuits is the best way to avoid crosstalk.Tim

author: John_ITIC
author_rank: Frequent Contributor
timestamp: May 31, 2015, 10:16:07 pm
content: What you should be asking is whether all power rails meet their ripple specs at all power pins of all devices. Rather than designing boards with split analog and digital power planes with the same voltage, I always try to share power (and GND) planes and instead carefully DESIGNING the power distribution network such that the ripple specs are met. Use of ferrite beads are then not needed.https://www.google.com/?gws_rd=ssl#q=PDN+designPractically, it helps tremendously to have software tools like Hyperlynx that can take your finished PCB layout and actually simulate the actual noise (ripple) you would see on all PWR and GND pins given power regulator and load pin models.http://www.mentor.com/pcb/hyperlynx/power-integrity/

author: John_ITIC
author_rank: Frequent Contributor
timestamp: May 31, 2015, 10:19:12 pm
content: Quote from: John_ITIC on May 31, 2015, 10:16:07 pmWith known currents and impedance at all locations on the board, you can effectively simulate exactly the noise you'll get at any point on the board. Noise around GND planes for a (single-ended) ADC would cause the input voltage to be noisy too (relative to the GND plane). With a known GND plane noise, you will know your maximum ADC noise. If less ADC noise is needed then do a better PDN design.

author: IanJ
author_rank: Unknown
timestamp: June 01, 2015, 07:48:35 am
content: Hi all,Found these useful practical guides:-http://www.hottconsultants.com/pdf_files/june2001pcd_mixedsignal.pdfhttp://www.ti.com/lit/an/slyt499/slyt499.pdfhttp://www.ti.com/lit/an/slyt512/slyt512.pdfFrom the first PDF:-Mixed-Signal Design Checklist:-- Partition your PCB with separate analog and digital section.- Place components properly.- Straddle the partition with the A-D converters.- Do not split the ground plane. Use one solid groundplane under both analog and digital sections of the board.- Route digital signals only in the digital section of the board. Applie to all layers.- Route analog signals only in the analog section of the board. Applie to all layers.- Separate analogue and digital power planes.- Do not route traces over the split in the power planes.- Traces that must go over the power plane split must be on layers adjacent to the solid ground plane.- Think about where and how the ground currents are actually flowing.- Use routing discipline.So, version 1 of my board will be here soon and I'll work on a version 2 and it will be good to compare directly. It's a 2-layer board and I hadn't planned of making a 4-layer, but if I do then that'll be a version 3 to compare to.Here's another article for info.https://www.sparkfun.com/datasheets/BreakoutBoards/mixed_signal_design.pdfGreat fun!Ian.

author: Feynman
author_rank: Regular Contributor
timestamp: June 04, 2015, 04:39:00 pm
content: I think it is safe to say that split ground planes do not provide any benefit. Like in your last post, it is more important to seperate analog an digital circuits by proper placing of components and tracks. Split ground planes may even cause EMI problems, because 100% separation of analog and digital is very difficult to achieve and you will always have return currents between the analog and digital part. And a split plane will then cause bigger loops in the current path. You always want to let the return current flow the direction it wants to (e.g. due to proximity effect), and not force it somewhere else.-> No to split ground planes

author: Howardlong
author_rank: Super Contributor
timestamp: June 04, 2015, 05:52:37 pm
content: And it's a "No" to split ground planes here too. If it helps, I too spent hours and hours about ten years ago trying to figure out the best layout method for mixed signal deisgns. At that time the split method seemed to have more traction and acceptance. I did do a few boards split, but it was a PITA routing those few signals that needed to cross domains over a single bridge area in the board.

author: dmills
author_rank: Super Contributor
timestamp: June 11, 2015, 09:25:10 am
content: Solid plane here too, with a few provisos.I will sometimes organise an island for something like a precision clock (and its associated ultra low noise LDO), but there you have just 3 nets in play (Power, ground and output) so routing to ensure the power and output nets are over the ground bridge is easy.The issue here is that low frequency noise (right the way down to DC) risks upsetting the PN performance of the osc, and the low frequency currents in the plane are not held as tightly to minimum loop area.That said, a solid plane is usually the best starting point, and 4 layers is not really more expensive then two these days (While being easier to lay out in all ways, buried power and ground is a good thing).I always think that placement is 2/3rds of the art, get that right and the board almost routes itself, get it wrong and the thing will never quite work right.I would reiterate the point about never crossing a split, reference planes should be continuous under signals, and to a few layer spacings either side.Regards, Dan.