Ground Plane - Page 1
Forum section: electronics / general

author: NoelGaspar
author_rank: Newbie
timestamp: August 08, 2017, 07:20:07 pm
content: Hi! i would like to know when and why i should use a ground plane in a PCB design? and when is recomended not to use it

author: Rerouter
author_rank: Super Contributor
timestamp: August 09, 2017, 09:37:58 am
content: The only time i would say to not use a solid as possible ground plane is when you have a physically large board, >15x15cm and cannot flood fill the top side.A gross difference in copper density leads to warping.That or you have your heart set on single sided.Now there are times when you dont want a plane under grouping of traces, e.g. very high impedance, or preventing noise coupling to / between planes. But these you would just mask off, not remove the whole plane.Even with a simple 2 sided board. Its best practice to make sure if you hop signals to the other side to make sure you provide a ground path for the traces on the top side your cutting under. Its generally only required for digital logic, but it helps a lot with external noise immunity.

author: T3sl4co1l
author_rank: Super Contributor
timestamp: August 09, 2017, 10:09:33 am
content: The only time you should ever make a board without ground plane is when trace clearances must be so large as to prevent a contiguous pour in the first place (which might be under very high voltage or very high impedance conditions). Then you'll have no choice but to route the ground as traces, making room for it.Almost all boards have modest impedances and analog or digital signals, and benefit from using ground fill.Tim

author: Neilm
author_rank: Super Contributor
timestamp: August 09, 2017, 05:13:27 pm
content: Quote from: Rerouter on August 09, 2017, 09:37:58 amI am assuming that you are referring to 2 layer board? I have just made a 30cm x 30cm multilayer board with no warpage issues. I did have to make sure that the layers were balenced, with a 0V and a power plane across almost the entire PCB. The only part that wasn't was the front end were there are large spacing requirements.From experiance, I would say that having one contiguous 0V plane is the easiest single thing to help pass EMC requirements, so the only time for not having one is down to safety clearances. The single plane allows a low impedance path for the currents flowing in the circuit. This reduces the loop area and loweres both stray emissions and the loop area that is susceptable to noise. I have seen a two layer board that had an LED lighting at a certain frequency. The signal for the transistor that controlled the LED went all over the board. Measuring the loop of the signaland the return pathproduced a value of the 1/4 wavelength of the signal so what was happening was the this loop picked up enough energy to turn on the transistor and power LED.What really annoys me is the lazy way datasheets just pull up ideas that were good for 2 layer boards where there was no ground plane. I am refering to spliting 0V into analogue and digital on simple circuits. While this works if the designer knows EXACTLY where all the currents flow then it will work. However it only takes one IC connected to a different supply to cause all sorts of EMC problems (and a return of the unit marked "Failed").