# How to calculate the size of ground plane we need to use in a PCB (printed circuit board) design [closed]

I searched about the ground plane and found out the ground plane is a good solution to reduce noise and get a seamless ground.

• How do I calculate the size of the ground plane for a PCB?
• When and where don't we need a ground plane? (Actually the ground plane is destructive.)
• Is it for an analog circuit, digital circuit, switching power supply, RF circuit - ??? Typically a ground plane covers the entire board on an internal layer, but of course it depends on what the board's circuits are doing. AND, what do you mean by "destructive"? – AnalogKid Nov 7 '19 at 4:54
• actually for all circuits.I wanna know where ground plane is need and how to use it ? "destructive" means "sth is not good to use AND is not correct to use in electronics. – reza ghasemi Nov 7 '19 at 5:19
• The answer is:- as big as necessary. Many circuits don't need a ground plane at all (even if they normally would have one), and putting it in the wrong place may cause more harm than good. There is no general formula for calculating the size of the ground plane in any PCB. If you want some advice for a specific design then show it to us. – Bruce Abbott Nov 7 '19 at 7:17

There are two aspects of a ground plane: its performance, and its appearance. The first is important. The second is not. Unfortunately, many people starting out concentrate on the second, to the detriment of the first.

A ground plane should be as big as it needs to be. That is, it should be present at or near* every connector, every IC, every supply decoupling capacitor, and every signal track.

A ground pour is not necessarily a ground plane. It can have the appearance of a ground plane. It's easy to do a pour as the last step laying out a board, it's difficult to check whether it does in fact connect all the points that should be connected.

There are two ways to make a good ground plane. One is to lay out a ground track as you make the board, so that you can see it that it follows all the signals, visits every IC directly, before you confuse yourself with the pour. If you couldn't route the track, then the pour will not have made the necessary connection either! 'Letting the pour take care of that connection' is asking for trouble.

The other is to dedicate a ground plane layer, and then don't cut it up. Too often we via a track onto the ground plane layer 'just for a few mm' to ease tracking problems, and then another, and another. Done once or twice, with a short track, it's OK. Done excessively, it cuts the ground plane to shreds, and it can't do its job. You can via across breaks on the other side, but it's hard work to make sure you've caught them all, best not to cut in the first place.

There are only a few instances where a ground plane should not be, and in almost all cases, it's where a component's data sheet tells you not to. Near to a chip antenna, where the data sheet gives you a detailed footprint. Under the inverting input of a fast high impedance op-amp, where excess capacitance can hurt stability. Near to pins carrying dangerous voltage, opto-couplers will often tell you what distances are required for what voltages.

*Near. For low frequency boards, 'near' can be quite big, without hurting performance. For RF boards and logic boards with fast edges, 'near' usually means directly underneath.

• Could you clarify what you mean about ground pour not being connected? If a copper pour is designated net GND and is not connected to all the other parts of GND then it will fail the design rules? Eagle for example has an "allow orphans" option for copper pour, but it's not the default – Rodney Nov 7 '19 at 13:09
• @Rodney even a pour where every part is electrically connected to each other is still not necessarily an adequate ground plane if it has cuts under transmission lines. The return current has to flow below the line, not take take a detour round the board. If the current is diverted in the ground, it will have the effect of putting an effective inductance in series with the line, and will allow different points of the 'ground' to have different transient voltages, not what you want, hence the word 'direct' in my answer. – Neil_UK Nov 7 '19 at 13:14
• OK agreed and it's a good answer it was just the it's difficult to check whether it does in fact connect all the points that should be connected that I found a bit misleading. – Rodney Nov 7 '19 at 13:26
• @Rodney it depends how big the board is I guess. Generally we can design bigger boards than we can check thoroughly. Checking always seems one of those unproductive things, like documentation, that gets left till last and not done properly. – Neil_UK Nov 7 '19 at 14:02
• @FMashiro That would be just for all but the very highest frequencies. A via through a ground puts a hole in it, a track makes a slot. Current flowing in the ground doesn't need to deviate much to miss a hole, whereas round the end of a slot is much further. You must avoid a line of closely spaced vias, where the clearances join up and form a slot in the ground. Ground on layer 2 is a very common way to go. The length of a via is minimal extra inductance, and you can use multiple vias to reduce it. – Neil_UK Nov 8 '19 at 13:58

Apart from specific cases: high voltage (where you need as big of an insulator between your signal and ground), controlled impedance (RF, high speed, the plane might help you also if done correctly) or very low noise analog circuitry. A complete and uniform ground plane bellow your signal layer should not do any harm.

There might be other scenarios where having power planes could harm your signals, please comment below, I would love to know !

Also as a matter of good practice, one should try to remove as little copper as possible. Thus on your top and bottom layers you will usually do ground pours (fill in the empty space with gnd) first to help you route the gnd (on all your decoupling caps for instance) but also to prevent massive amount of copper to be dissolved during the manufacturing process.

If your design can be routed on two layers, and you can live with the noise from a less uniform gnd/power planes. You should always challenge yourself to use as little layers as possible, just for the sake of being more cost efficient with your designs.

{Summary: this answer illustrates the method of DESIGNING a Ground Plane to achieve 60dB isolation between regions.}

Ground planes are excellent for attracting electric field flux. Instead of your signal trace having the burden of handling all the displacement-current, the Ground Plane provides the return path for most of the displacement-current.

Thus high dV/dT situations, such as electric-train speed-controllers, should use Ground planes.

And low noise situations, where the Znode * C_couple_aggressor_victim * dV/dT is larger than your trash budget (you do have a trash budget, right?), a Ground plane is the first step in improving signal_noise_ratio (ENOB).

Audio people tell you to use Star Grounds, not using Ground planes. People at diyAudio.com use Gnd planes in "NJFET RIAA preamplifier" discussion thread, with the various components of low-noise (Rnoise approximately 50 ohms, thus 0.8 nanoVolts/rtHz) RIAA over a Ground plane and the RIAA corner at 50Hz constricts the total integrated random noise to about 0.8 nanoV * sqrt(50 * PI/2) == 0.8nV * sqrt(81) = 0.8nV * 9 == 7 nanoVolts RMS noise.

And a Ground plane (inside a steel or thick aluminum case; power supply was in separate case, 1 or 2 meters away) was used in achieving that 7 nanoVolt RMS floor. For audio RIAA circuit.

Here is the floor plan of the 7 nanoVolt RIAA low-noise audio PCB GND plane. The key to audio performance is: minimize crosstalk between Input (Left) and 60dB_stronger Output (Right).

simulate this circuit – Schematic created using CircuitLab