Purpose of dedicated Power planes in PCB stackup

[matrixofdynamism]

For high speed board design, having dedicated GND planes that are all linked together using stitching vias (to reduce impedance for return path) is essential. However, it is not clear why one would need a whole dedicated power plane in the PCB stack up.

Power can be delivered in the same layer as the signals, by using PCB tracks that are wide enough to carry the required current. Using decoupling capacitors is actually important to smooth the ripples on the supply that can form due to switching activity in the digital ICs. As long as one ensures that the PCB tracks are wide enough to carry the required sustained peak current (I believe), we can use it to deliver power.

PCB stackup has a large impact on PCB manufacture cost. If a whole plane is dedicated to power, it must not have any breaks/cuts in it. We want to use as few layers as possible to design a PCB. Since PCB tracks are good enough, why would one ever need a whole dedicated PCB layer for power?

 

[BigBoss]

If you have lot of VCC or VDD and GNDA, GNDD or similar common rails, you have to use Power Planes to reach to wanted pins. Otherwise you will have to tie those nets one by one and it will so create confusion, complexity and grounding/returning problems.

 

[matrixofdynamism]

So what if the number of rails is small, lets say 3, and the current draw requirement is not some large value like 50A?

 

[dick_freebird]

It's less about the "DC" current draw, than the dynamic impedance
to a pin. Long skinny routes make the feed inductive, resulting in
more ringing (that L and the C-to-ground at both ends, forming a
tank).

Not that you can ignore R on a FPGA with 160A peak current, either....

 

[BigBoss]

So what if the number of rails is small, lets say 3, and the current draw requirement is not some large value like 50A?

Depends...
If you have few Vcc, you don't have to use a GND/VCC Plane. Maybe you do..
Nobody say something without seeing your schematic. If rail currents are clean (analog) maybe not but if the rail currents are dirty coming from digital circuitry maybe yes..
The circuitries have to be carefully examined and decided to use GND/VCC plane OR not..

 

[matrixofdynamism]

I am trying to learn about high speed PCB design. My dream hobby project is to design an FPGA board conneced to DDR3 RAM. This is where the question come from.

The part of tracks having higher impedance than planes is quite important one. Anyway, if you know of any PCB designs that are done professionally and I can view to learn these concepts, that would be great and helpful.

 

[KlausST]

Hi,

My dream hobby project is to design an FPGA board conneced to DDR3 RAM. This is where the question come from.

Sounds if you did not design any other PCB before.
My recommendation: learn to go before you run for an olympics sprint record.

if you know of any PCB designs that are done professionally and I can view to learn these concepts, that would be great and helpful.

Aren't thousands or even millions in the internet enough?
There are thousands tutorials, documents, examples. From universities, PCB software manufacturers, FPGA manufacturers and many professional designers. As documents, as videos. Everything is available.

Klaus

 

[crutschow]

Power can be delivered in the same layer as the signals, by using PCB tracks that are wide enough to carry the required current.

In theory.
But having to run wide power traces to all the ICs and thread them through all the signal traces may end up requiring an extra conductive layer anyway, to deal with all the trace crossovers.
In that case it's easier just to make that extra layer a plane, with the bonus of a reduction in any noise on the power rail.

 

[matrixofdynamism]

I have designed 2 layer boards in Eagle PCB in the past some years ago. Last year I designed another simple PCB with two layers in Altium Designer. In both cases the design did not use anything except through hole package ICs and some SMD resistors and capacitors.

I want to move to the next level now and do some high speed design stuff. I already understand the basic concept of tracks, vias, layer stack, dielectric, prepreg, copper weight, characteristic impedance, length tuning to reduce skew, silk screen, solder mask e.t.c. Suffice to say, I do understand the basic principles behind basic PCB design. It is time to upgrade now.

--- Updated Apr 27, 2023 ---

Also, there might be several thousands of tutorials and documents, but if they repeat what I already know, it is of no benefit. I am looking for answer to specific questions. I am already a qualified electronic engineer working with FPGA - Intel, Xilinx, Microsemi tools as my day job.

 

[KlausST]

Hi,

2 layer PCBs may work. But as soon as you have high speed digital signals it´s hard to make them "reliably" working and make them according EMI/EMC standards.

Just guessing, so pleas don´t be upset if its not your reality:
There may be situations you just are not aware of regarding high speed design.
One situation may be that an FPGA works properly ... but then you change the code a tiny bit which causes to switch more cells than before on the same clock edge. This increases the pulsed power supply current. Every tiny stray inductance on the VCC or GND lines may now lead to increased ringing .. and maybe even the function to fail.
So besides correct HF signal treatment you need rock hard power supplies at the point of load.
In this case it makes a big difference if the power is routed as several traces or as true plane.

Often made mistake:
* A trace of some length has some ohmic resistance. You may improve (lower) the resitance by using a wider trace.
* but: A trace of some length has some inductance. And you can not improve inductance (in the same way) by using wider traces.
***

As far as I see your questions are properly answered.

Maybe you don´t accept these answers..
Then I agree - repeating the information won´t help.

What answer(s) do you expect?
How to go on?

Klaus

 

[matrixofdynamism]

Yes the questions have been answered. There are certain things that I know which I am not sure if they are correct or not which goes through correction with new information. At this time, I am not looking into the subject of PDN in detail although I have realized that it is essential to have a good PDN to get high speed circuits to work. This is because, the components already use low voltage and can accept only a very small ripple or drop in this supply voltage before failing. PDN analysis is of course a whole topic. I am trying to figure out the signal PCB track and PCB via subject right now.

If we use PCB tracks and then use lot of decoupling capacitors, doesn't that in theory also lead to less impedance? I can see that when we use planes, the large area of a plane means more area for EM field coupling and this less impedance.

My previous post was a reply to KS to the statement "Aren't thousands or even millions in the internet enough? There are thousands tutorials, documents, examples. From universities, PCB software manufacturers, FPGA manufacturers and many professional designers. As documents, as videos. Everything is available.". Basically everything required is not covered everywhere. One has to eventually ask questions to someone to make sense of the subject and connect the disparate pieces of information.

 

[FvM]

Agreed, you need continuous ground planes for high speed designs but not necessarily power planes. Nevertheless you find global digital supplies, e.g. +3V3 often implemented as continuous power plane, may be others too. If bypassed at many points over the board, these power planes can act as reference for transmission lines like ground planes.

Board design typically starts with a topographical component plan, estimating number of signal layers and reference planes, room for power distribution.

For products with medium volume, there's often a trade-off between PCB production costs and design effort towards using more layers, reducing design time and avoiding possible redesigns required by marginal signal quality.

 

[KlausST]

Hi,

If we use PCB tracks and then use lot of decoupling capacitors, doesn't that in theory also lead to less impedance?

I agree. It´s low impedance at the capacitor.
But not necessarily low resistance form power supply to capacitor ..
and not necessarily low impedance form capacitor to IC.

It all depends. What do you call high frequency, high current, low impedance, low voltage drop, dV/dt, dI/dt ...?

In your posts are only a few numbers. So we need to guess them.
So for an audio engineer 1MHz may be considered high frequency, for another engineer maybe high frequency starts above 1GHz.

***

Some examples from my experience.
I worked for one company doing current measurments down to 10pA. For the other company I did current measurements up to 3000A RMS. both in the same range of frequency.

When you think about a sheet of steel... what thicknes do you imagine? I was at a company they showed me their stock of steel sheets. I didn´t recognize it, I just saw huge blocks of steel. Then they explaind these 300mm thick blocks _are_ the sheets.

What I want to say: The more vague the question, the more vague the answer.
Some days ago we had a discussion where a member asked about a power supply for a microcontroller. One of our first questions was about the expectable output current. No information. So we talked about solutions for up to several 10mA.
The member tested it and reported destroyed parts. It maybe took about 40 posts until he informed us about 500mA. How could we know?
What´s your idea to avoid this waste of effort and time? I mean .. you are not that satisfied with our answers and we don´t get satisfaction in seeing you happy.

Klaus

 

[marce]

I don't know where to begin...
Power planes are a must for high speed designs...
Planar capacitance, instantaneous current requirement of high speed switching devices, the list goes on...
DDR3 power requirements...

https://www.micron.com/-/media/client/global/documents/products/technical-note/dram/tn41_01ddr3_power.pdf

Using traces for digital supply voltages worked in the 1980's but not today...
Like all PCB design, there is a lot more engineering goes into a design than people initially think, especially for the power delivery system, look at power integrity software, it will give you more information on the complexity of power deliver design...

 

[kingcrediepcba]

For high speed board design, having dedicated GND planes that are all linked together using stitching vias (to reduce impedance for return path) is essential. However, it is not clear why one would need a whole dedicated power plane in the PCB stack up.

Power can be delivered in the same layer as the signals, by using PCB tracks that are wide enough to carry the required current. Using decoupling capacitors is actually important to smooth the ripples on the supply that can form due to switching activity in the digital ICs. As long as one ensures that the PCB tracks are wide enough to carry the required sustained peak current (I believe), we can use it to deliver power.

PCB stackup has a large impact on PCB manufacture cost. If a whole plane is dedicated to power, it must not have any breaks/cuts in it. We want to use as few layers as possible to design a PCB. Since PCB tracks are good enough, why would one ever need a whole dedicated PCB layer for power?

Hello,

The power layer is an inner layer in the PCB board, which is specially used to connect the power cord and the power plane. The copper foil layer of the power layer is generally thicker，it is to reduce the impedance of the current and the noise of the power supply. The design and layout of the power plane have an important influence on the stability and interference suppression of the power supply.

Linda