PCB design practices - Page 1
Forum section: electronics / projects

author: OM222O
author_rank: Frequent Contributor
timestamp: February 07, 2019, 02:44:22 pm
content: HelloI have seen these 2 PCB design practices used extremely often!1) A ton of vias on the edge of the PCB connecting 2 ground planes2) Crosshatch ground plane instead of a solid oneyou can clearly see them in dave's latest teardown video as well:vias on the edge (and even in the antena lines!):crosshatch ground plane:I'm not sure what the purpose of these 2 practices are. I had a guess that vias protects the edges of the PCB so they won't come off easily in case of some damage or a bad cut on the PCB. (Apple products, especially macbooks use ridiculous amounts of vias on the board edges) most people say it's for better grounding but that wouldn't make a ton of sense as the edges are the furthest apart for any signal to travel to. If they wanted grounding, they would have placed a lot of vias all across the the plane, not just the edge! Also I read about the crosshatch planes and everyone seems to say they are "a thing of the past" and solid planes are better, although I haven't seen a single product from microsoft that uses a solid ground plane ... If you have any thoughts or a definite explanation as to why these methods are used, please share it down below.

author: station240
author_rank: Unknown
timestamp: February 07, 2019, 04:16:01 pm
content: The vias spread over areas is called "via stitching", very common when there are power/ground planes/traces on two sides.Serves to electrically bond the two areas.Rarer but still common is via stitching around edges/mounting holes, done for mechanical reasons. Prevents the PCB substrate (fibreglass) from being compressed.

author: Bud
author_rank: Super Contributor
timestamp: February 07, 2019, 04:19:10 pm
content: Via stiching is to improve grounding properties at RF frequencies and for shielding purposes as well as to reduce RF emissions from board edges.

author: asgard
author_rank: Regular Contributor
timestamp: February 07, 2019, 04:59:41 pm
content: One other important practice applies to RF and microwave designs, especially around the antenna assemblies. Because of VSWR it is important to reduce as much as possible the parasitic coupling of from high-speed signals. One approach is understanding that if we treat such signals traces as planar waveguides then two things must happen. The other layers on the board must not have any active signal or copper under the waveguide, while surrounding the trace with via-stitched ground planes on all the layers. It also can help if we use star-layout techniques to limit signal interference within the ground plane adjacent to the waveguide. Here is a datasheet that recommends such things for a WiFi module that I have been looking at (Cypress AN-91445):https://www.cypress.com/file/136236/download

author: OM222O
author_rank: Frequent Contributor
timestamp: February 07, 2019, 05:13:07 pm
content: I think the mechanical reasons that station240 brought up would make more sense as again, the vias are mainly on the edges, not a specific trace or area. Also a laptop such as a macbook isn't a WIFI/RF module (they have seperate wifi cards and whatnot). but I'm guessing it will help with grounding or shielding signals that are near the edge naturally which makes sense. what about the crosshatch ground planes though? any specific reason for those? They still seem to be really popular

author: ajb
author_rank: Super Contributor
timestamp: February 07, 2019, 05:42:05 pm
content: Note that it's not just radios that have to consider performance at radio frequencies!The frequencies of concern in EMI are not the fundamentals, but the harmonics, which are largely determined by edge rates. Something like a switching converter operating at 100kHz can easily radiate into the tens or hundreds of MHz, because of the edge rates involved. This is also a consideration with data lines, but switching converters are a particular concern, because the voltages and currents are higher, which means that the current and voltage rates of change (dI/dt and dV/dt) are correspondingly higher, so interactions with parasitic inductance and capacitance are more significant. Thus you see via stitching in basically anything with an MCU or a switching converter, because such things are always de facto RF boards--plus via stitching costs basically nothing, so it's cheap insurance even if it's not strictly necessary for a particular application.

author: Bud
author_rank: Super Contributor
timestamp: February 07, 2019, 05:52:57 pm
content: Dave released a video recently showing the spectrum emmited by a DIY computer board. Goes into GHz range.Hatched ground pattern perhaps can help with easier reflow during board assembly as the copper mass is smaller and heating can be reduced, just speculating. I always use solid copper fills on my RF boards as i figured out long time ago more ground copper improves the Return Loss of RF building blocks such as filters, mixers, amplifies, etc.

author: georges80
author_rank: Frequent Contributor
timestamp: February 07, 2019, 07:11:56 pm
content: Vias around the edge of the PCB are to prevent RF from being emitted from internal layers etc. This requires the edge/perimeter to be ground plane on top/bottom and connect to inner ground plane etc. You are constructing a 'jail' to prevent RF from coming out of the edges of the board. The 'jail' bar spacing (the via spacing) is chosen based on the shortest wavelength you are blocking. You need to figure your highest frequency/harmonics and fence at that spacing, anything lower in frequency (larger wavelength) can't 'fit' through the fence spacing.Similar to microwave oven door 'mesh', the mesh diameter is chosen to allow you to see in but prevents the microwave RF escaping and cooking you.Vias in other areas are to provide a DC path for high edge rate current loops that would otherwise go places you don't want (e.g. a high speed signal going through to another layer. There would be a bypass capacitor placed nearby and vias added. Vias are also placed in areas that appear strange just to remove any stub antenna artifacts that would radiate RF.Simply, any via that doesn't appear to have any benefit from a pure DC perspective is likely there for RF reasons (or the layout engineer just put the via(s) in to mess with you)cheers,george.