How to resolve EMI/EMC issues in a product during design phase - Page 1
Forum section: electronics / projects

author: Sai teja
author_rank: Regular Contributor
timestamp: April 03, 2020, 07:44:41 am
content: Hello,Currently we are developing the product for an application. During the design phase, we are facing trouble in ensuring the product will comply EMI/EMC guidelines as per the market. Before going for Pre-Compliance Testing, are there any methods or techniques to resolve the EMI/EMC issues during the design phase?Please guide me in this regard.

author: David Hess
author_rank: Super Contributor
timestamp: April 06, 2020, 03:00:24 am
content: I start by using circuits and layouts which minimize problems with EMI/EMC. This includes minimizing all loop areas, which usually means a ground plane these days, filtering and decoupling between assemblies, filtering at all chassis feed-through points, etc.

author: Siwastaja
author_rank: Super Contributor
timestamp: April 06, 2020, 10:07:56 am
content: Component miniatyrization driven by the mobile tech really helps here. I tend to choose smallest components I can deal with in prototyping (so if I need to choose between a 0.3mm, 0.5mm, 0.8mm, 1.27mm or 2.54mm pitch part, the choice is usually 0.5mm, and the passive size is 0402), then design the functional sub-parts of the PCB as tightly as possible. This has two purposes, it enables me to easier squeeze the design in any form factor later (I may even have a lot of empty space on the prototype PCB due to this!), but it also makes the EMC better by* Minimizing loop areas, but also* Making shielding easier (a small thing is easy to surround with a small shield)* Making filtering easier (now we have saved space, and can afford the area of a filter!)

author: tggzzz
author_rank: Super Contributor
timestamp: April 06, 2020, 10:22:21 am
content: You have to understand the basic physics. You have to think in terms of electromagnetic fields, not discrete circuit components.Then you design based on your understanding of the physics. You may be able to use some rules of thumb to guide you. You make design tradeoffs based on project cost/time/volume/timescales and the consequences of failures/respins.Then you test, and see what you missed.

author: Vovk_Z
author_rank: Super Contributor
timestamp: April 06, 2020, 06:34:16 pm
content: Look for "eevblog EMC" at youtube.There are some good books on noise and EMC, for example from Henry Ott (I can't find exact list).

author: Niklas
author_rank: Frequent Contributor
timestamp: April 06, 2020, 09:12:23 pm
content: You have to look at the complete setup, including housing, wires and connectors. There are a lot of things that you can do with the PCB layout to minimize the generated noise and/or to increase immunity, but often the connector placement, pinouts and wiring are not given as much attention.

author: nctnico
author_rank: Super Contributor
timestamp: April 06, 2020, 11:06:43 pm
content: In general if your board has a solid ground plane (this can be achieved on a 2 layer board as well) then the most likely cause of EMC problems are wires coming from the board. Make sure to filter all signals but even then you can get caught. A good principle is to have room for extra filtering components which aren't placed on the prototype. When the prototype is finished take it to an EMC lab for a pre-compliance test. With some luck the board doesn't need a respin.

author: T3sl4co1l
author_rank: Super Contributor
timestamp: April 07, 2020, 12:34:08 am
content: Divide the layout into sections, subcircuits, just as you would on the schematic. (I mean, assuming you're drawing things in an understandable fashion and not just net-naming everything...)This groups local currents together. Switching regulator has switching currents under itself, no where else. MCU has signal currents under itself, and nowhere else. Etc.The exception is for signals entering and leaving the section. Follow a transmission line scheme. Signals can be bused together at modest separation distance, but mind that there will be some coupling between them. Which is most likely acceptable for digital signals, but you may want some isolation for high speed analog signals. Signals always flow over ground plane, preferably surrounded by it, with stitching vias as needed.Higher level structure: try to arrange sections in a starred linear shape. Avoid making loops between sections, which will tend to pick up ground loop currents from between sections.Ground slots, if applicable: a starred linear structure is the only way (or, well, one of the few reasonably general ways) to make use of ground slots. DO NOT cross slots with traces. So, all those buses have solid ground under/around them. Only the ground between buses can be removed, mostly without ill effect.Example: if you imagine a layout in the shape of the letter 'E', there's a central node with three buses, one of which is a leaf node; the two corner nodes have one more bus each, connecting to a leaf node. The negative space between legs of the 'E' can be cut out, with no impact to signal quality.If you need to connect signals from one leaf to another, you should route them back along the common bus, through unrelated nodes. Routing them directly would cause a loop.This description implies a lot of distance between sections, but full length transmission lines are of course not necessary. As long as you can draw a conceptual divider between regions, the buses can be any length, including ~zero.Note that a leaf node cannot have any common mode (ground loop voltage) through it -- because there is no loop there. Putting switching regulators on leaf nodes, with input and output filtering at the bus entry, is a very good idea.The final caveat to this kind of structure is, there can be resonant modes between the physical branches of the circuit. These can still be somewhat excited by signal currents in the buses, leading to emissions and susceptibility; a good reason to have the buses well shielded in the first place. Slots between conductors exhibit monopole (slot to edge) or dipole (enclosed slot) resonant modes; these can be dampened by putting impedance across the slot in a useful area.You don't have to worry about slot modes with a solid ground plane, another fine reason to use it. Solid ground plane also helps to short out common mode voltages, so that if you do make loops, they are less likely to be offensive. It's still a good plan to avoid making loops, following the star routing scheme described above.Tim

author: Gibson486
author_rank: Frequent Contributor
timestamp: April 07, 2020, 01:54:46 pm
content: That is kind of a loaded question....the issue is that everyone's situation is unique, so there is no cookie cutter solution. There are suggestions that work 80% of the time (some are mentioned here), but nothing will cover 100% of the situations. I mean, there are BOOKS, not just chapters, on the very subject.