Ground Fill and Ground Plane Dynamics Best Practice? - Page 1
Forum section: electronics / projects

author: kreyszig
author_rank: Regular Contributor
timestamp: February 22, 2023, 12:40:14 am
content: When designing a multi-layer PCB with SMD components, usually each component is not connected to the ground plane using its own separate via, and some components end up sharing ground on the first layer. Also, it is recommended to use a ground fill for the top layer. So my question is, what is the best practice when sharing ground between SMD components on the first layer:1) Interconnect components that are close together using a trace / local ground fill, and use a single via / via cluster to ground each trace / local ground fill to the ground plane. Use separate ground fills that do not carry any current and connect each ground fill to the ground plane using a single via / via cluster.2) Connect the ground for all components directly to a ground fill, and connect the ground fills to the ground plane using multiple vias that are distributed across the PCB.When I look at different examples of 4-layer PCBs, I see designs that look more like 2), but I would have expected 1) to be preferable in order to avoid ground loops and reduce noise?Thanks!

author: ataradov
author_rank: Super Contributor
timestamp: February 22, 2023, 01:02:02 am
content: For mostly digital circuits - connect to the closest point on the ground plane and connect all the ground planes at many points using via stitching. Don't do anything extra, place the ground planes in all unused space and let components connect however topology allows.You can guess all you want how the noise is distributed, but unless you are going to simulate and prove it, solid grounds planes would be the safest approach.For analog and RF - there may be separate special considerations, of course.

author: kreyszig
author_rank: Regular Contributor
timestamp: February 22, 2023, 01:08:31 am
content: Quote from: ataradov on February 22, 2023, 01:02:02 amThank you. I am not reconsidering the usefulness of having a solid ground plane though. What I am wondering for a multi-layer PCB is what should be done about ground for the top layer only. Is it better to allow ground current to flow across the whole PCB and between all components by connecting all grounds to a top layer ground fill in addition to the ground plane layer (possibly creating ground loops), or is it better to minimize the amount of current flowing on the top layer, sending this current to the ground plane layer as early as manageable (whenever there is room for a via), and use other ground fills for the top layer to reduce noise instead of to carry current?

author: ataradov
author_rank: Super Contributor
timestamp: February 22, 2023, 01:17:59 am
content: Quote from: kreyszig on February 22, 2023, 01:08:31 amThis.Quote from: kreyszig on February 22, 2023, 01:08:31 amFor a moderately complex PCB (where any of this would matter at all), you will never guess "by eye" what creates loops and what does not. Stitch all grounds and don't overthink it.

author: kreyszig
author_rank: Regular Contributor
timestamp: February 22, 2023, 02:43:58 am
content: Quote from: ataradov on February 22, 2023, 01:17:59 amLook at the top layer for this SMPS on page 29:https://www.monolithicpower.com/en/documentview/productdocument/index/version/2/document_type/Datasheet/lang/en/sku/MPQ4576GQBE-AEC1/document_id/9741/. They use a separate ground fill for C1A, C1D, C1B, C1C and the converter. What is the reason for that? Thanks!

author: ataradov
author_rank: Super Contributor
timestamp: February 22, 2023, 02:58:24 am
content: Ok, switching power supplies is one of the special cases. In that case just follow manufacturer recommendations. This is a very local use case and I bet they optimized and simulated that design.

author: Someone
author_rank: Super Contributor
timestamp: February 22, 2023, 09:14:47 am
content: Quote from: kreyszig on February 22, 2023, 02:43:58 amNot really a ground fill just some large traces. But some power distribution/delivery/converters do use whole planes to push energy around....It's engineering, it's all tradeoffs, there are no hard rules that always apply.You fill all the space that is un-needed with something that could make use of it, that might be ground or that might be some other signal.... occasionally its best off as open space!

author: HalFoster
author_rank: Frequent Contributor
timestamp: February 22, 2023, 05:06:55 pm
content: I would recommend researching PCB design before you start laying things out - often you are better offnothaving a ground plane (or any power plane) especially if you are working with AC circuits - having a signal plane can make things much worse. Dave Jones of the EEVBlog does a video if I remember right and there is a lot of good information via Google. For reference, I like "The Circuit Designer's Companion" by Tim Williams but there are many others.Hal

author: HalFoster
author_rank: Frequent Contributor
timestamp: February 22, 2023, 07:07:20 pm
content: A link to an excellent (and free) book on the subject:https://www.thehighspeeddesignbook.com/

author: peter-h
author_rank: Super Contributor
timestamp: February 22, 2023, 08:55:04 pm
content: On a 4 layer board I normally use the inner layers for VCC and GND and the outside layers for signals.Components going to GND should use a short track (say 2mm long) and a pad to GND. That enables efficient heating of that component pad during reflow, so you don't get tombstoning (parts popping up to vertical).GND plane fill on the outside doesn't do much IME.If you want to piss off counterfeiters (for a bit, not for long) use inner layers for tracks and GND/VCC on the outside. But then it is hard for you to work with it.For analog (I do a lot of that) one often uses a split GND plane because one needs the analog circuitry to have its own clean GND - even if that piece of plane is connected to the main plane somewhere (usually with just one track link).

author: SiliconWizard
author_rank: Super Contributor
timestamp: February 22, 2023, 08:56:53 pm
content: Quote from: ataradov on February 22, 2023, 01:17:59 amExactly.

author: kreyszig
author_rank: Regular Contributor
timestamp: February 23, 2023, 03:34:15 pm
content: Quote from: peter-h on February 22, 2023, 08:55:04 pmThis is what I intended to do by default, i.e. short ground tracks to nearby via, split ground plane for SMPS, split VCC plane for components that have their own decoupling capacitor (MCU, LED array, etc) when VCC traces are not optimal.

author: kreyszig
author_rank: Regular Contributor
timestamp: February 23, 2023, 03:44:46 pm
content: A slightly different, but related question, let say I need to feed 80 mA of LEDs that are driven by 1.2 kHZ PWM off a 400 mA 300 kHZ SMPS that also drives an MCU. Would it make sense to size the decoupling capacitor for the LEDs based on the SMPS frequency? E.g. for 10 mV drop at 5V:C = I / (deltaV * f) = 80 mA / (10 mV * 300 kHz) = 27 uF