Ground Plane vs Power Plane

glebone Black on a chip (OSD335x-SM), and a 20MHz ADC (AD9238)... they don' t all fit on one side of the board, their datasheets all want ground planes under them... if I put the ADC on the bottom of the board and have a Power Plane under it, is that close enough to having a ground plane under the pa rt? or can a ground pour under the IC take the place of a ground plane?

If they are adequately decoupled (why do they call it decoupling when the t wo planes are being coupled together?) the power plane is just as good as a ground. But that's only true if you do not have significant currents caus ing local voltage variations in the power plane. Typically an ADC will hav e a separate power/ground plane from digital circuitry connected at just on e point to prevent digitally induced currents from messing with the ADC.

Your stackup is actually 5 layers, but you have the idea. You can do S1 G1 P1 P2 G2 S2

--

  Rick C. 

  - Get 1,000 miles of free Supercharging 
  - Tesla referral code - https://ts.la/richard11209

In most designs, power is best obtained from (actual) capacitors, not from large planes. Read the guidelines on the data sheet, certainly, but bear in mind that some of those guidelines are more important than others. Some are good advice, some are bad advice, some are superstitious bullshit. In all of those cases, the guidelines are often the product of mindless cutting-and-pasting from data sheets for (much) older parts. The really important guidelines are the ones that talk about using physically small MLCCs close to the power pins. Unbroken ground planes are a vital part of that strategy, power planes not so much.

There are those who strongly advocate power planes, but unless you need a truly large amount of current in a hurry and don't have room for sufficient bypassing at the point of load, you can generally make *much* better use of a copper layer for signal routing than by dedicating the whole region to a power plane. At least that's what I've always found. YMMV, and it will depend to some extent by the number of layers you have to work with.

-- john, KE5FX

.

t.

That all depends on the noise you are trying to minimize. I don't think it is so much the current as it is the frequency content of the noise you nee d to reduce. Capacitors become inductive above the resonance point and so the impedance increases. At higher frequencies they become ineffective. P ower planes continue to reduce noise into the GHz range depending on their geometry. The resonances in power planes actually depend on the dimensions . I suppose it is a matter of standing waves.

So with internal clocks at hundreds of MHz the edge rates will have to be h igh enough to produce harmonics into the GHz range where capacitors are not as effective as power planes. The other reason for using planes is that t hey create a transmission line coupling between the cap and the chip which supplies the current to the chip while the wave front is traveling to the c ap. So the exact placement of the caps are not nearly so critical as witho ut power and ground planes.

That said, I see a number of capacitors on the actual OSD335x-SM module. B ut I'd bet they use ground and power planes.

--

  Rick C. 

  + Get 1,000 miles of free Supercharging 
  + Tesla referral code - https://ts.la/richard11209

Big power planes have a useful amount of fast capacitance. But what's really great about power planes or pours is their super low inductance, compared to a trace. A plane is a great way to connect several bypass caps to several parts. Fast current spikes spread out in all directions.

If you TDR a power plane against ground, it looks like an almost perfect capacitor. If you then add bypass caps anywhere on the plane, it looks like a bigger capacitor.

--

John Larkin         Highland Technology, Inc 

lunatic fringe electronics

If you're talking about an ADC then you're implicitly talking about a mixed-signal board. you're not mixing your analog and digital supplies, are you?

There should be independent supplies for the analog and digital sections. They should be isolated from each other on the board, too. Many ADC mfgrs kindly put all the digital pins on one side of the IC and the analog pins on the other to help accomplish this

Low-current ADC/DAC should be on a separate supply but can/should just be grounded to the analog ground both AGND and DGND pins.

Yeah, just the other day I was thinking about ways to make fast current spikes spread out in all directions.

-- john, KE5FX

Nanohenries are free!

--

John Larkin         Highland Technology, Inc 

lunatic fringe electronics

eaglebone Black on a chip (OSD335x-SM), and a 20MHz ADC (AD9238)... they do n't all fit on one side of the board, their datasheets all want ground plan es under them... if I put the ADC on the bottom of the board and have a Pow er Plane under it, is that close enough to having a ground plane under the part? or can a ground pour under the IC take the place of a ground plane?

I do have an ADC on the bottom of the board, I will have split analog and d igital power planes, but just one solid ground... I have the processor and wifi modules on top, and adc on bottom... I'm going to do six layers.... I' m debating between these two stack ups:

1 - top 2 - gnd 3 - sig 4 - pwr 5 - gnd 6 - bottom

or

1 - top 2 - gnd 3 - sig 4 - sig 5 - pwr 6 - bottom

I feel like the first stack up may be better? There's also an SD card on th e bottom, and USB on top

Beaglebone Black on a chip (OSD335x-SM), and a 20MHz ADC (AD9238)... they don't all fit on one side of the board, their datasheets all want ground pl anes under them... if I put the ADC on the bottom of the board and have a P ower Plane under it, is that close enough to having a ground plane under th e part? or can a ground pour under the IC take the place of a ground plane?

d

digital power planes, but just one solid ground... I have the processor an d wifi modules on top, and adc on bottom... I'm going to do six layers.... I'm debating between these two stack ups:

the bottom, and USB on top

USB is supposed to be impedance controlled. So that might work best on eit her of your stackups. I would prefer to use

1 - top 2 - sig 3 - gnd 4 - pwr 5 - sig 6 - bottom

if you can get the impedance you want. The advantage is the power and grou nd planes will be much better coupled. But I think any of these will work and your impedance controlled traces probably should be next to a power or ground plane.

--

  Rick C. 

  -- Get 1,000 miles of free Supercharging 
  -- Tesla referral code - https://ts.la/richard11209

Probably doesn't matter. Just avoid crosstalk on the sig-sig pair. Well, avoid crosstalk everywhere!

We generally use just one ground plane, so as to have more routing and sometimes power pour space.

L3 power close to L2 ground is probably better for *really* fast stuff. It minimizes power inductance and maximizes plane capacitance.

There are so many competing theories (and so much included nonsense) about signal integrity precisely because most of the theories work.

The Saturn PCB Toolkit is good for calculating trace impedances, especially for odd things like asymmetric microstrip, which is what you have with plane-sig-sig-plane.

--

John Larkin         Highland Technology, Inc 

lunatic fringe electronics

A six-layer board seems an awful big stack for three chips, where one is a BGA SoC. The non-SoC Beaglebone with external RAM, etc. is 6 layers it's a much more complicated board.

Shit you could probably do a budget-oriented PCIe video card in six layers nowatimes.

(I have learned to wait until you finish discussing things with yourself.)

The problem with BGAs is getting the traces out. You can get the two outer rows of balls out on layer 1, but after that each row needs another layer. Then you have ground and probably several power supplies to pour into the array.

This was intended to be an 8 layer board, but it was taking so long to route we went to 10.

That needs four layers to get ground and power into the chip.

--

John Larkin         Highland Technology, Inc 

lunatic fringe electronics

How much lumped capacitance is on the board? ...or is this all the ground plane? It would be good to see the same trace with and without a lumped capacitor at a significant distance (e.g. 5ns) from the injection point.

I've been trying to get management to buy a TDR but everyone else is arguing that a network analyzer and software is a better use of the limited cash. They won't buy eBay stuff. Go figure.

Good, though it uses an additional plane. The grounds have to be well stitched, too.

This is good if there are a large number of high-speed traces. We did this sort of stackup (a ground or power against all signals) when I was at IBM.

The issue is the distance between the planes. They're not always equidistant. I'd prefer this stackup but only if there is only prepreg between 3&4.

The big thing, not addressed here, is that the components of the switching power supplies should be on the same side with a pour between the switch, and input/output capacitors. That pour can then be staked to a plane at the appropriate point (the common point of the input and output loops, usually).

Yep. Then depending on the pitch, you may need to change the thickness of the board (via aspect ratio limitations) and/or go to blind/buried vias. $$$$

BGAs are great for some things but there are a lot of hidden costs.

a Beaglebone Black on a chip (OSD335x-SM), and a 20MHz ADC (AD9238)... they don't all fit on one side of the board, their datasheets all want ground p lanes under them... if I put the ADC on the bottom of the board and have a Power Plane under it, is that close enough to having a ground plane under t he part? or can a ground pour under the IC take the place of a ground plane ?

s,

and

and digital power planes, but just one solid ground... I have the processor and wifi modules on top, and adc on bottom... I'm going to do six layers.. .. I'm debating between these two stack ups:

on the bottom, and USB on top

If you want full power and ground planes, depending on the specific BGA, it can be hard to route all the signals on a 4 layer board.

--

  Rick C. 

  -+ Get 1,000 miles of free Supercharging 
  -+ Tesla referral code - https://ts.la/richard11209

, a Beaglebone Black on a chip (OSD335x-SM), and a 20MHz ADC (AD9238)... th ey don't all fit on one side of the board, their datasheets all want ground planes under them... if I put the ADC on the bottom of the board and have a Power Plane under it, is that close enough to having a ground plane under the part? or can a ground pour under the IC take the place of a ground pla ne?

a

es,

and

and digital power planes, but just one solid ground... I have the processor and wifi modules on top, and adc on bottom... I'm going to do six layers.. .. I'm debating between these two stack ups:

on the bottom, and USB on top

either of your stackups. I would prefer to use

What do you mean "they" are not always equidistant? If you mean the layer thicknesses that is for the designer to specify.

--

  Rick C. 

  +- Get 1,000 miles of free Supercharging 
  +- Tesla referral code - https://ts.la/richard11209