To fill zones or not fill zones

When drafting traces for single-sided PCBs I have always filled zones for GND. I did this because it meant less etching (homebrew). Now I intend to have a two-sided PCB made commercially and I am rethinking this idea.

I have the idea that a two-sided PCB with a large GND filled zone on one side and lots of tracks on the other would run the risk of becoming one clumsy capacitor which would cause all sorts of problems. Is that right? Would it be best to NOT fill the GND zone regardless of the increase in etching involved?

1 Like

When you don’t need to run tracks on both sides, allocating one side to be a ground plane, usually the top for a through hole, is usually the best solution. You are eliminating ground bounce problems between the components.

Having little islands of copper, either floating or grounded at just one point is a bad idea as these islands become patch antennas at UHF frequencies. This used to be called copper flood.


This project runs two voltages, 3.3V and 5V. I kept 5V (arbitrary choice) and GND on B.Cu and (most of) the rest on F.Cu. It looks like this:

Have I made any glaring, ghastly mistake? I would really appreciate you checking it out. It is my first attempt at this sort of thing. (I have attached the project files.)

Thanks (38.2 KB)

Yes and no.
GND as big as whole PCB is very good from EMC point of view.
You must understand that currents always flow in closed circles. If signal goes from one IC to another it must come back via GND. GND plane gives the best way for coming back. Current don’t travels via GND the shortest way back (only DC travels that way). The higher signal frequency (digital signals have big frequency band) the more it likes to travel back just under the track it traveled forth. It is good as that way the area surrounded by current is smaller for higher frequencies. The smaller area means smaller unwonted emission. It works the same if we look at sensitivity of our circuit to incoming radio frequency disturbances. GND plane is the best way to give each back current the best way for him and if possible you should use it.

The higher capacity between tracks and GND generally is not a problem but advantage. You can make your digital signal have less high frequency contents by adding only the resistor at IC output - you get RC filter (where C is the track to plane).

But, as you correctly suppose, in some cases it can be a problem. I felt into that problem only once. Operational amplifier worked stable on PCB with no big GND and became unstable after adding GND plane (OpAmps don’t like capacity loads) . But I preferred to left GND plane and add one small feedback capacitor to ensure stability than to abandon GND plane.


In V4 (don’t know yet how is in V5) the default colours were red for F.Cu and green for B.Cu.
You changed the x.Cu layers colours or you don’t have most of the rest at F.Cu.

1 Like

Red and Green are “standardised” as Red F.Cu as @Piotr notes.

Make your tracks much wider for a start (eg 0.5~1mm), more robust and it moves heat around.
How hot do you expect those regulators to get? If you expect more than 1W you need to rearrange them to allow heatsinks. As they are placed, shoulder to shoulder most types would not fit.
The barrel socket uses slots, for a low cost board you are better off with circular holes. Measure the tab of a socket to see what you need.

The barrel socket has rectangular-cross-section pins, so I either go for slots or very large holes which might be tricky to solder across. I am working on having this thing manufactured so I’ll leave the slotting problem up to the maker. I guess they’ll have done it before :laughing:.

You really should calculate the regulator power dissipation first. You just need to know the load current and the input voltage range.

Many of us use those barrel jacks with round holes, you just use a big iron or wave solder. The tab is bent first for strength. Slots are a special operation which always costs more and the cheap pcb fabs won’t do at all.

I’ll just have to see what a fabricator says when I submit the files. :thinking:

I have tried this idea with the traces like this

Filling in for GND on B.Cu I get

and for F.Cu I get

This certainly has the effect of minimizing the amount of etching required. My worry is, “What havoc have I created?”

When writeing look at right half of screen to see how your message will be looking. The post I am answering is hard to see what is quote and what your text.

I work that way always.

I don’t understand what you meen. If you expect capacitor problems then haveing fiiled GND planes on both sides makes this problems bigger and not lower comparing to haveing the GND plane on one side.

If you order the PCB in factory amount of etching is not your problem :slightly_smiling_face:
There are some rules that copper density at whole PCB should be xxxx. The rules come not from amount of etching but rather from PCB like to curve itself during soldering but I’m not sure of enything in that subject so should not write about it.

The track need not be the same width at whole its length.

It can be hard to believe in it, but it can be counted. I’m serious :slight_smile:
Look in datasheet for Thermal resistance (Junction to air - means without heatsinks) - something in °C/W. Let us assume it is 100°C/W. This means that if you dissipate 1W in that element than its junction will be 100°C hotter than surrounding air. The maximum operating junction temperature also should be defined in dastasheet. But better assume working at lower junction temperatures.
I think - if you dissipate 1W in TO120 like package it will be hard to touch but still in working range. I would not disspitate more than 0,5W without heatsink but I like to have a solid margin.
Fo heatsinks you can also find their thermal resistances and then use part junction to case resistance.

Mistake - I thought TO220.

This is my thinking as a Mechanical Engineer:

Having filled planes on both sides of a PCB gives me two copper plates separated by an insulator (I believe that’s called a dielectric), i.e. a capacitor. However, having both plates as GND must surely cancel any capacitance. It would have the effect of running a short-circuit across the capacitor
putting the same charge on either plate so no charge storage. If I had a four-layer PCB and did the same thing I would get this effect

Once again there would be no stored charge.

Would that not cancel any effect on the rest of the circuit?

What you describe is only valid in direct current models. For alternating current there is no such thing as a direct connection. Everything is a mixture of resistors, capacitors and inductors. Even a via. (A via might have near to 0 ohms of resistance. But its inductance is quite high. The voltage drop across an inductor is higher with higher frequencies or faster changes in voltage.)

Currents do not follow the way of least resistance. They follow the way of least Impedance! (Impedance is the combination of the aforementioned 3.)
There is a good (but also simplified) post on the sister forum about that:

The capacitance provided by one zone connected to a power rail and the other to ground can actually be a good thing, although it is quite small. For a 100mm x 100mm two layer board with solid planes it would be about 260pf.

There’s more to impedance than just resistance, capacitance and inductance. This is illustrated by the fact that the return current follows the path of least impedance which, where possible, is directly adjacent to the source path.

1 Like

Assume you have one layer (I will name it signal layer) used for your signal tracks and second layer (GND layer) used for GND plate.
Till now I was speaking about capacitance betwean any your signal track and GND plate on GND layer.
When you fill all free space on your signal layer also with GND plate than in pararell to capacitnce betwean your signal track and GND on GND layer you will also had capacitances betwean your signal track and GND on both sides of your signal track on your signal layer. I use typical saparation betwean tracks and GND fill of 10mis. Typical PCB width is 1,5mm = 60mils. Typical PCB material increases capacitance (compared to air) 4 times. You can assume that distance betwean your track and GND on signal layer is in half filled with PCB material and in half with air. All that means that capacitnaces betwean your track and GND on signal layer are enough high to not omit them.

If the capacitnace betwean signal track and GND on GND layer can be a problem then capacitance betwean signal track and GND if also signal layer is filled with GND can be a bigger problem.

Must break my writeing. Something also I will write later.

You are right it is a capacitor. When shorted you are also right it is rather no longer a capacitor. So you can understand both filled planes as a one pice of metal but…it is no so simple.
I am not an expert in such subjects but can say same sentences to open your eyes on how complicated things can be in electronic.
You probably know that microvawes fregently travel not through wires but in wave-guides (metal pipes). When such pipe is opened at its and the wave bounces and travels backward and when on other side the pipe is also opened the way can travel forward and backward. If its wave length is according to have its arrows (don’t sure if it is right English term to describe the points with highest amplitude) at the pipe ends than you can get a standing wave and it its frequency is a resonant frequency of this pipe. The pipe lenght have to be 1/2 or 1 or 1,5 or… of wave length to get such situation. You can also consider the pipe closed at one side but when you get the numbers like 1/4, 3/4, …
The PCB with both sides covered with GND (even if at one side there are also signal tracks) can work as wave-quide with wave bouncing at PCB edges. Assume wave speed 2E8 m/s, PCB length 10cm. From that we get first resonance for wave length of 20cm=2E-1m. Such wave frquency is 2E8/2E-1 = 1E9 = 1GHz. For current electronic it is not a very high frequency - see a clock of your PC. If at that PCB there is any signal with enough high harmonic at 1GHz (for squere signals all odd harmonics (1,3,5,7,9,11,…) are important - a squere signal of 66,667MHz have 15-th harmonic at 1GHz) then it can be amplified by PCB resonance and disturb another signal in that device or emit that disturbane aout of device making if fail to pass limits od EMC regulations (in Europe it is EMC directive - elsewhere I don’t know but some regulations certainly exists).
If you have squere PCB 7x10cm then in one direction it can resonane at 1GHz, 2GHz, 3GHz and in second direction at 1,43GHz, 2,86GHz and so on.
What I wonted to say is - the PCB in current times is not a simple set of connections, and if something works at schematic level it may not work at practical PCB level.

No it`s not which is illustrated by Maxwells equations.

No what’s not? If you are referring to the return current path then, when it comes to high frequency AC currents, yes it is. And Maxwell’s equations have no problem with this.

The OP has an Arduino and a couple of sensors and instead of general advice about zones this topic is now discussing harmonic content of square waves, and wave guides.

No, there is not more to Impedance than L, R and C. The document is not contradicting my statement, it backs it up.