How ground plane acts as low impedance path.

[hioyo]

I am new to high speed design .Please don't flame me if this question is very basic

Below statement is from AD application note.

"The ground plane not only acts as a low impedance return path for decoupling high-frequency currents (caused by fast digital logic) but also minimizes EMI/RFI emissions. Because of the shielding action of the ground plane, the circuit’s susceptibility to external EMI/RFI is also reduced."

But it does not explain how this is happening.I have 2 questions.

1 ) May I know how ground plane acts as a low impedance return path.
2 ) Shelding action of GND plane.

Regards
hari

 

[KlausST]

Hi,

1)
What is a GND plane?
* It's a layer of solid copper in a PCB.
For beginners: no cuts, no other signals. Pure solid sheet of copper
Advanced designers know where the current flows, know where the current is allowed to flow and where it is not allowed to flow. Thus they are able to add "foreign signals" into the GND plane ... and may add cuts to avoid noise to travel for example.

How does signal flow?
* signals flow always in a loop.
On a PCB there is no signal from A to B, there always is a signal back (return path). If a transmitter A sends out a signal ....it does it as voltage with respect to it's GND. And the receiver B "sees" it also with respect to it's own GND. So if there is a short signal trace between A and B .... but a long winding return path ... then the receiver's input is not stable before the return path is stable. Here often the power supply bypass capacitors are part of the return path. Thus their placement and connection to the GND plane is very important.

* impedance of a signal path
Mainly depends on the inductance of a signal path. And inductance of a signal path depend on the magnetic field it causes. The longer the trace, the higher the inductance. But trace width and trace thickness have only very small impact on impedance. Thus one can not compensate a lengthy trace by making it thicker and wider. (This is only true for ohmic part of the impedance)
But this is only half of the truth ... because the other "half" is the return path. Since in the return path is the same current as in the signal path (don't focus on DC current, but the current caused by the signal edge ... usually with high dV/dt) ... and this current is in the opposite direction ... it also causes a magnetic field. Also in opposite direction. So the resulting magnetic field becomes lower. This has two major effects:
* This magnetic field "by accident" does the same as a transmitter anntenna does: it sends out signals ... in this case unwanted switching noise. (EMI). Maybe causing problems with WiFi connections ... or malfunction of your sound system
* But also the decreased magnetic field caused decreased inductivity ... and thus you get a lower overall signal impedance --> more stable signals.
A measure of the "inductance" is the enclosed area of the signal and it's return path.

Example: imagine a straight signal trace from A to B with length of 50mm on a PCB.
Then imagine the return path also as a straight trace back from B to A but side shifted by 10mm. So the enclosed area is 50mm x 10mm = 500 mm^2.
And if the return path is lengthy, then the area may easily be 1000mm^2.
Now imagine the return path to exsctly follow the signal trace but at the opposite side of the PCB. (Or in another layer) So the distance is minimized and thus the impedance is minimized.
And this exactly happens on a GND plane. The return current in the GND plane (due to the magnetic field) automatically follows the path of the signal trace.

2)
It acts as "shield" for a magnetic field. As described above ... the magnetic field becomes compensated. Only a tiny part of the already small field is abke to "pass" the GND plane ... or travel around the whole PCB
And due to it's low impedance and low ohmic there is about zero voltage, thus about zero electric field.
Since both magnetic as well as electric field is very low, you may see a GND plane as some kind of faraday's cage. Not that perfect, though.

I recommend to watch some good youtube videos about this topic.

Klaus

 

[hioyo]

Hi,

1)
What is a GND plane?
* It's a layer of solid copper in a PCB.
For beginners: no cuts, no other signals. Pure solid sheet of copper
Advanced designers know where the current flows, know where the current is allowed to flow and where it is not allowed to flow. Thus they are able to add "foreign signals" into the GND plane ... and may add cuts to avoid noise to travel for example.

How does signal flow?
* signals flow always in a loop.
On a PCB there is no signal from A to B, there always is a signal back (return path). If a transmitter A sends out a signal ....it does it as voltage with respect to it's GND. And the receiver B "sees" it also with respect to it's own GND. So if there is a short signal trace between A and B .... but a long winding return path ... then the receiver's input is not stable before the return path is stable. Here often the power supply bypass capacitors are part of the return path. Thus their placement and connection to the GND plane is very important.

* impedance of a signal path
Mainly depends on the inductance of a signal path. And inductance of a signal path depend on the magnetic field it causes. The longer the trace, the higher the inductance. But trace width and trace thickness have only very small impact on impedance. Thus one can not compensate a lengthy trace by making it thicker and wider. (This is only true for ohmic part of the impedance)
But this is only half of the truth ... because the other "half" is the return path. Since in the return path is the same current as in the signal path (don't focus on DC current, but the current caused by the signal edge ... usually with high dV/dt) ... and this current is in the opposite direction ... it also causes a magnetic field. Also in opposite direction. So the resulting magnetic field becomes lower. This has two major effects:
* This magnetic field "by accident" does the same as a transmitter anntenna does: it sends out signals ... in this case unwanted switching noise. (EMI). Maybe causing problems with WiFi connections ... or malfunction of your sound system
* But also the decreased magnetic field caused decreased inductivity ... and thus you get a lower overall signal impedance --> more stable signals.
A measure of the "inductance" is the enclosed area of the signal and it's return path.

Example: imagine a straight signal trace from A to B with length of 50mm on a PCB.
Then imagine the return path also as a straight trace back from B to A but side shifted by 10mm. So the enclosed area is 50mm x 10mm = 500 mm^2.
And if the return path is lengthy, then the area may easily be 1000mm^2.
Now imagine the return path to exsctly follow the signal trace but at the opposite side of the PCB. (Or in another layer) So the distance is minimized and thus the impedance is minimized.
And this exactly happens on a GND plane. The return current in the GND plane (due to the magnetic field) automatically follows the path of the signal trace.

2)
It acts as "shield" for a magnetic field. As described above ... the magnetic field becomes compensated. Only a tiny part of the already small field is abke to "pass" the GND plane ... or travel around the whole PCB
And due to it's low impedance and low ohmic there is about zero voltage, thus about zero electric field.
Since both magnetic as well as electric field is very low, you may see a GND plane as some kind of faraday's cage. Not that perfect, though.

I recommend to watch some good youtube videos about this topic.

Klaus

Thank you for a nice explanation .If you don't mind could you please share the youtube video links

 

[KlausST]

Hi,

Just do a search. There should be plenty of content.
(I also had to do a search)

Klaus

 

[marce]

Think of the signal propagating as a wave on water, the wave front moves between the GND plane and the signal wire through the dielectric, the signal and return travel together... It may help to think of the current for a wave rather than the voltage... A wave consists of two current spikes, turn on, turn off, this narrow spike travels down the signal path. Like a ball down a path, the ball is the wave travelling between the conductors, it is always in contact with both the positive and the return conductors...

 

[crutschow]

A fast (rise/fall) signal on a trace needs a low-impedance path for the return signal directly below the trace to minimize radiation of the trace signal and distortions of the signal.
(The propagation of the signal current along the trace is mirrored by the return signal current on the ground plane.)
This is provided by a ground plane beneath the signal, which has a low resistance and inductance, due to large area of the plane.

 

[hioyo]

A fast (rise/fall) signal on a trace needs a low-impedance path for the return signal directly below the trace to minimize radiation of the trace signal and distortions of the signal.
(The propagation of the signal current along the trace is mirrored by the return signal current on the ground plane.)
This is provided by a ground plane beneath the signal, which has a low resistance and inductance, due to large area of the plane.

Equation of inductance is given by L = μN2A/l. where A is the area. When area increases the inductance will increase.But your statement is "This is provided by a ground plane beneath the signal, which has a low resistance and inductance, due to large area of the plane".May I know where I went wrong

 

[FvM]

The "Equation of inductance" is an approximation formula for a cylinder coil. Can you explain why it has nothing to do with inductance of a PCB trace?

 

[stenzer]

A fast (rise/fall) signal on a trace needs a low-impedance path for the return signal directly below the trace to minimize radiation of the trace signal and distortions of the signal.

Have a look here [1], which provides a good (graphical) explaination.

[1] https://incompliancemag.com/article/alternative-paths-of-the-return-current/

BR

 

[hioyo]

The "Equation of inductance" is an approximation formula for a cylinder coil. Can you explain why it has nothing to do with inductance of a PCB trace?

I don't know that. If you don't mind could you please explain how large area reduces the inductance

 

[FvM]

I suggest to compare three trace configurations:
1. A trace pair with some spacing, e.g. w = 0.5 mm, d = 10 mm
2. A vertical (top/bottom) trace pair, w = 0.5, d = 1.6 mm
3. The same top trace above a wide bottom plane

How is the trace pair inductance (per length unit) ordered? You can refer to w/d inductance relation of double wire transmission line, use PCB calculation tools or 2D FEM analysis. Clearly L1 > L2 > L3.

 

[Akanimo]

1 ) May I know how ground plane acts as a low impedance return path.
2 ) Shelding action of GND plane.

2) For magnetic field shielding: See this link for the action of copper plane to magnetic fields. This is a proof that the ground plane is a good shield from external magnetic fields.
Also take a look at the shape of the magnetic fields in the diagrams in this page, this one, this one and other diagrams on the internet and you will realize that the magnetic field between the microstrip trace and the ground plane is usually compressed within the available space. This goes to say that the ground plane also serves to confine electromagnetic field from radiating beyond the plane.

For electric field shielding: