Ground Plane vs Power Plane

[Fibo]

Hello,

I'm trying to layout a little board with a WiFi module (WL1835MOD), 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 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 plane?

If not, then I guess a 6-layer stack up

- signal (top)
- gnd
- pwr
- gnd
- signal (bottom)

or is that overkill?

Much thank!

 

[Rick C]

On Saturday, June 15, 2019 at 4:45:57 PM UTC-4, Fibo wrote:

Hello,

I'm trying to layout a little board with a WiFi module (WL1835MOD), 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 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 plane?

If not, then I guess a 6-layer stack up

- signal (top)
- gnd
- pwr
- gnd
- signal (bottom)

or is that overkill?

Much thank!

If they are adequately decoupled (why do they call it decoupling when the two 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 causing local voltage variations in the power plane. Typically an ADC will have a separate power/ground plane from digital circuitry connected at just one 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

 

[John Miles, KE5FX]

On Saturday, June 15, 2019 at 1:45:57 PM UTC-7, Fibo wrote:

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 plane?

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

 

[Rick C]

On Saturday, June 15, 2019 at 8:08:03 PM UTC-4, John Miles, KE5FX wrote:

On Saturday, June 15, 2019 at 1:45:57 PM UTC-7, Fibo wrote:
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 plane?

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.

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 need to reduce. Capacitors become inductive above the resonance point and so the impedance increases. At higher frequencies they become ineffective. Power 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 high 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 they 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 cap. So the exact placement of the caps are not nearly so critical as without power and ground planes.


That said, I see a number of capacitors on the actual OSD335x-SM module. But 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

 

[John Larkin]

On Sat, 15 Jun 2019 17:07:59 -0700 (PDT), "John Miles, KE5FX"
<jmiles@gmail.com> wrote:

On Saturday, June 15, 2019 at 1:45:57 PM UTC-7, Fibo wrote:
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 plane?

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

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.

https://www.dropbox.com/s/wkiehn6iowq3emf/TDR_3Vplane.JPG?raw=1





--

John Larkin Highland Technology, Inc

lunatic fringe electronics

 

[bitrex]

On 6/15/19 4:45 PM, Fibo wrote:

Hello,

I'm trying to layout a little board with a WiFi module (WL1835MOD), 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 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 plane?

If not, then I guess a 6-layer stack up

- signal (top)
- gnd
- pwr
- gnd
- signal (bottom)

or is that overkill?

Much thank!

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

 

[bitrex]

On 6/15/19 5:01 PM, Rick C wrote:

On Saturday, June 15, 2019 at 4:45:57 PM UTC-4, Fibo wrote:
Hello,

I'm trying to layout a little board with a WiFi module (WL1835MOD), 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 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 plane?

If not, then I guess a 6-layer stack up

- signal (top)
- gnd
- pwr
- gnd
- signal (bottom)

or is that overkill?

Much thank!

If they are adequately decoupled (why do they call it decoupling when the two 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 causing local voltage variations in the power plane. Typically an ADC will have a separate power/ground plane from digital circuitry connected at just one 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

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.

 

[John Miles, KE5FX]

On Saturday, June 15, 2019 at 10:11:00 PM UTC-7, John Larkin wrote:
> Fast current spikes spread out in all directions.

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

-- john, KE5FX

 

[John Larkin]

On Sun, 16 Jun 2019 02:43:39 -0700 (PDT), "John Miles, KE5FX"
<jmiles@gmail.com> wrote:

On Saturday, June 15, 2019 at 10:11:00 PM UTC-7, John Larkin wrote:
Fast current spikes spread out in all directions.

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

 

[Fibo]

On Sunday, June 16, 2019 at 1:15:53 AM UTC-5, bitrex wrote:

On 6/15/19 4:45 PM, Fibo wrote:
Hello,

I'm trying to layout a little board with a WiFi module (WL1835MOD), 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 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 plane?

If not, then I guess a 6-layer stack up

- signal (top)
- gnd
- pwr
- gnd
- signal (bottom)

or is that overkill?

Much thank!


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

I do have an ADC on the bottom of the board, I will have split analog 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:

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 the bottom, and USB on top

 

[Rick C]

On Sunday, June 16, 2019 at 1:37:18 PM UTC-4, Fibo wrote:

On Sunday, June 16, 2019 at 1:15:53 AM UTC-5, bitrex wrote:
On 6/15/19 4:45 PM, Fibo wrote:
Hello,

I'm trying to layout a little board with a WiFi module (WL1835MOD), 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 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 plane?

If not, then I guess a 6-layer stack up

- signal (top)
- gnd
- pwr
- gnd
- signal (bottom)

or is that overkill?

Much thank!


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

I do have an ADC on the bottom of the board, I will have split analog 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:

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 the bottom, and USB on top

USB is supposed to be impedance controlled. So that might work best on either 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 ground 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

 

[John Larkin]

On Sun, 16 Jun 2019 10:37:12 -0700 (PDT), Fibo <panfilero@gmail.com>
wrote:

On Sunday, June 16, 2019 at 1:15:53 AM UTC-5, bitrex wrote:
On 6/15/19 4:45 PM, Fibo wrote:
Hello,

I'm trying to layout a little board with a WiFi module (WL1835MOD), 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 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 plane?

If not, then I guess a 6-layer stack up

- signal (top)
- gnd
- pwr
- gnd
- signal (bottom)

or is that overkill?

Much thank!


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

I do have an ADC on the bottom of the board, I will have split analog 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:

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 the bottom, and USB on top

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

 

[bitrex]

On 6/16/19 6:45 PM, bitrex wrote:

On 6/16/19 5:18 PM, John Larkin wrote:
On Sun, 16 Jun 2019 10:37:12 -0700 (PDT), Fibo <panfilero@gmail.com
wrote:

On Sunday, June 16, 2019 at 1:15:53 AM UTC-5, bitrex wrote:
On 6/15/19 4:45 PM, Fibo wrote:
Hello,

I'm trying to layout a little board with a WiFi module (WL1835MOD),
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 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 plane?

If not, then I guess a 6-layer stack up

- signal (top)
- gnd
- pwr
- gnd
- signal (bottom)

or is that overkill?

Much thank!


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

I do have an ADC on the bottom of the board, I will have split analog
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:

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 the bottom, and USB on top

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.



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.

 

[bitrex]

On 6/16/19 5:18 PM, John Larkin wrote:

On Sun, 16 Jun 2019 10:37:12 -0700 (PDT), Fibo <panfilero@gmail.com
wrote:

On Sunday, June 16, 2019 at 1:15:53 AM UTC-5, bitrex wrote:
On 6/15/19 4:45 PM, Fibo wrote:
Hello,

I'm trying to layout a little board with a WiFi module (WL1835MOD), 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 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 plane?

If not, then I guess a 6-layer stack up

- signal (top)
- gnd
- pwr
- gnd
- signal (bottom)

or is that overkill?

Much thank!


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

I do have an ADC on the bottom of the board, I will have split analog 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:

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 the bottom, and USB on top

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.

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.

 

On Sun, 16 Jun 2019 13:44:16 -0700 (PDT), Rick C
<gnuarm.deletethisbit@gmail.com> wrote:

On Sunday, June 16, 2019 at 1:37:18 PM UTC-4, Fibo wrote:
On Sunday, June 16, 2019 at 1:15:53 AM UTC-5, bitrex wrote:
On 6/15/19 4:45 PM, Fibo wrote:
Hello,

I'm trying to layout a little board with a WiFi module (WL1835MOD), 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 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 plane?

If not, then I guess a 6-layer stack up

- signal (top)
- gnd
- pwr
- gnd
- signal (bottom)

or is that overkill?

Much thank!


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

I do have an ADC on the bottom of the board, I will have split analog 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:

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

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

or

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

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.

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

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

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

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.

if you can get the impedance you want. The advantage is the power and ground 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.

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).

 

On Sat, 15 Jun 2019 22:10:55 -0700, John Larkin
<jjlarkin@highlandtechnology.com> wrote:

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.

https://www.dropbox.com/s/wkiehn6iowq3emf/TDR_3Vplane.JPG?raw=1

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.

 

[John Larkin]

On Sun, 16 Jun 2019 18:49:00 -0400, bitrex <user@example.net> wrote:

On 6/16/19 6:45 PM, bitrex wrote:
On 6/16/19 5:18 PM, John Larkin wrote:
On Sun, 16 Jun 2019 10:37:12 -0700 (PDT), Fibo <panfilero@gmail.com
wrote:

On Sunday, June 16, 2019 at 1:15:53 AM UTC-5, bitrex wrote:
On 6/15/19 4:45 PM, Fibo wrote:
Hello,

I'm trying to layout a little board with a WiFi module (WL1835MOD),
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 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 plane?

If not, then I guess a 6-layer stack up

- signal (top)
- gnd
- pwr
- gnd
- signal (bottom)

or is that overkill?

Much thank!


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

I do have an ADC on the bottom of the board, I will have split analog
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:

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 the bottom, and USB on top

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.



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.

https://www.dropbox.com/s/27rb966kjivbwr7/P5_Big_BGA.jpg?raw=1

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




--

John Larkin Highland Technology, Inc

lunatic fringe electronics

 

On Sun, 16 Jun 2019 17:52:08 -0700, John Larkin
<jjlarkin@highlandtechnology.com> wrote:

On Sun, 16 Jun 2019 18:49:00 -0400, bitrex <user@example.net> wrote:

On 6/16/19 6:45 PM, bitrex wrote:
On 6/16/19 5:18 PM, John Larkin wrote:
On Sun, 16 Jun 2019 10:37:12 -0700 (PDT), Fibo <panfilero@gmail.com
wrote:

On Sunday, June 16, 2019 at 1:15:53 AM UTC-5, bitrex wrote:
On 6/15/19 4:45 PM, Fibo wrote:
Hello,

I'm trying to layout a little board with a WiFi module (WL1835MOD),
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 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 plane?

If not, then I guess a 6-layer stack up

- signal (top)
- gnd
- pwr
- gnd
- signal (bottom)

or is that overkill?

Much thank!


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

I do have an ADC on the bottom of the board, I will have split analog
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:

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 the bottom, and USB on top

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.



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.

https://www.dropbox.com/s/27rb966kjivbwr7/P5_Big_BGA.jpg?raw=1

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

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.

 

[Rick C]

On Sunday, June 16, 2019 at 11:07:59 PM UTC-4, bitrex wrote:

The SoC in the OP's design is a somewhat more modest affair; the mfgr in
question is even kind enough to provide a reference on how to free them
all on a single layer. Luxurious of them, I know!

http://octavosystems.com/octavosystems.com/wp-content/uploads/2017/05/Single-Layer-Body.png

Do they say what design rules are required? Not needing microvias is a big plus!

--

Rick C.

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

 

[Rick C]

On Sunday, June 16, 2019 at 10:59:57 PM UTC-4, k...@notreal.com wrote:

Sure but the optimum plane assignment can't be made independent of the
interplane distances. The above discussion means nothing without
knowing (or, better, specifying) the dielectric thicknesses.

I can set those distances to whatever works for the stackup I choose. What you are you trying to say? You don't need to use the same thicknesses for each stackup. This is not a test question with arbitrary constraints.

--

Rick C.

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