The 20H and Ground Plane Extension rules: benefits and limitations of applying them
576 2
andyfierman 8 months ago
It is important to inset the signal traces and power planes from the edges of the ground plane by as great a distance as possible. A commonly used rule of thumb is that the ground plane should extend twenty times the height (H) of the signal traces or power plane over the ground plane. In other words, the traces and power planes are inset by 20H from the edges of the ground plane. This is called the 20H rule. Also, where possible, the ground plane should be uninterrupted and should extend to the edges of the PCB. We can call this the Ground Plane Extension rule. It is important that the reasons for applying the 20H and the Ground Plane Extension rules - and the practical limitations of doing so - are clearly understood. Currents flowing through - and voltages across - signal traces and power planes and their associated return paths generate electromagnetic (EM) fields. In a PCB with a well designed, extensive, uninterrupted ground plane most of the EM field is shorted out into the ground plane. At the edges of a PCB however, the gap between signal traces and power planes and their associated return paths acts like an antenna radiating electromagnetic energy out from the edges of the PCB. ![image.png](//image.easyeda.com/pullimage/VTuTwOJZEIJIN7GycfZE1zaf6m6PQCbrmiMkfE9W.png) The higher the frequency content of the signal (including the harmonics), the more efficient this antenna effect becomes. Extending the ground plane right to the edges of the PCB and mounting the PCB close (capacitively coupled) to or even butted up against (directly coupled to) the insides of a metal enclosure can further reduce the effects of these fringing fields by shorting them out into the metal of the enclosure. * The trouble is that the reason for these rules is not well understood or even known about by many people. This lack of knowledge can result in power planes and signal tracks _as well as_ the ground plane being placed right up to the PCB where they can be exposed and so connect to - or short together through - the enclosure. On badly cut edges the exposed copper can smear and short out the bare PCB. When butted up against an enclosure, it may be that the signal traces or the power plane and not the ground plane may short to the enclosure which causes even greater EMC problems and could cause an electric shock hazard. It should also be noted that for a 1.6mm thick 2 layer PCB the 20H rule would require that signal traces and power planes where inset by 32mm from the edge of the ground plane. Even with a 4 layer PCB where the two inner layers are the ground and power planes, the gap between them may still be in the region of 1mm so the required inset is unlikely to be achievable. For small multilayer PCBs where the plane spacings are fractions of a mm the inset can often be difficult to achieve because it represents a large fraction of the available routing area. For example a 0.1mm layer spacing requires a 2mm inset. When this is applied all the way round the edges of a PCB this can represent a huge reduction of routing area. Further reading: [https://incompliancemag.com/article/avoid-critical-signals-in-edges-of-the-pcb/](https://incompliancemag.com/article/avoid-critical-signals-in-edges-of-the-pcb/) [https://www\.researchgate\.net/publication/4098429\_Analysis\_on\_the\_effectiveness\_of\_printed\_circuit\_board\_edge\_termination\_using\_discrete\_components\_instead\_of\_implementing\_the\_20\-H\_rule](https://www.researchgate.net/publication/4098429_Analysis_on_the_effectiveness_of_printed_circuit_board_edge_termination_using_discrete_components_instead_of_implementing_the_20-H_rule) [http://www.piers.org/piersonline/pdf/Vol3No7Page1097to1101.pdf](http://www.piers.org/piersonline/pdf/Vol3No7Page1097to1101.pdf)
Comments
UserSupport 8 months ago
Thanks Andy
Reply
MikeDB 8 months ago
Agreed for signal traces, but if your VCC plane is radiating anything then you don't have enough smoothing on it in the first place.  Hence the 5mm I suggested in another comment was purely for safety spacing reasons as mentioned in your para 8, and is mainly because most metal PCB guides are 3mm deep.    There should always be a ground or power plane as the outermost track on all layers to reduce the EMC effects you cover in the other paragraphs. Anyway hopefully EasyEDA will change their software now so that GND copper fills do extend to the edge whilst all others don't.  In the meantime the easiest solution is probably to begin a design by placing a GND track around the edges of the whole PCB, preferably on all layers, and just cut it away when necessary.
Reply
Login or Register to add a comment
goToTop
你现在访问的是EasyEDA海外版,使用建立访问速度更快的国内版 https://lceda.cn(需要重新注册)
如果需要转移工程请在个人中心 - 工程 - 工程高级设置 - 下载工程,下载后在https://lceda.cn/editor 打开保存即可。
有问题联系QQ 3001956291 不再提醒
svg-battery svg-battery-wifi svg-books svg-more svg-paste svg-pencil svg-plant svg-ruler svg-share svg-user svg-logo-cn svg-double-arrow
We use cookies to offer you a better experience. Detailed information on the use of cookies on this website is provided in our Privacy Policy. By using this site, you consent to the use of our cookies.