Multilayer ground

I'm working on laying out a PCB for a small DAC with 6 layers. I have a question about the digital and analog grounds. Can/should the digital and analog grounds overlap each other on separate layers or should the two grounds occupy completely separate areas of the board? Also, is a star or full ground plane preferable for the analog ground?

Thanks,
Stu
 

jcx

Member
2003-02-17 7:38 pm
..
don't overlap, the capacitance will just couple noise from digital to analog - always keep a "moat" of a few mm free of all copper between digital and analog pwr/gnd planes (including signal traces, route all signal traces that have to go between analog and digital sections over the single "bridge" that joins the digital and analog grounds), pull back the power planes and any traces a few more mm from the edges of the associated gnd plane as well

a single ground plane layer is commonly split beteen analog and digital with a few mm gap execpt at the single common connection "bridge", usually recommended to be physically at the dac - see the data sheet reference layout

in 16 bit precision instrumentation I usually find 4 layers adequate, even with a few 100+ pin dsp and processor chips on board - this requires "splitting" a power plane to distribute bipolar power, again use all the copper area you can with good bypassing at each load point

analog ground plane is usually the best approach; if you have some unually high power/frequency "analog" (esp class B/AB) it may be worth further partitioning the analog pwr/ground planes but I think a visually recognizable "star" of skinny traces is likely to be a poor approach
 

Extreme_Boky

Member
2003-12-07 11:57 am
Hi jcx,

(including signal traces, route all signal traces that have to go between analog and digital sections over the single "bridge" that joins the digital and analog grounds), pull back the power planes and any traces a few more mm from the edges of the associated gnd plane as well

So, how would you connect Iout with ground coupling traces from a DAC to analog section (I to V converter)? How exactly would analog power supply ground be coupled to analog section in regards to these links (containing ground potential!) from DAC to analog section?

Thanks,
Extreme_Boky
 
maczrool said:
I'm working on laying out a PCB for a small DAC with 6 layers. I have a question about the digital and analog grounds. Can/should the digital and analog grounds overlap each other on separate layers or should the two grounds occupy completely separate areas of the board? Also, is a star or full ground plane preferable for the analog ground?

Thanks,
Stu


Question to all:

- Which currents run from analog to dgital ?
- Where do these currents run ?

Given the 2 answers above, why would you separate into 2 planes ?

www.tentlabs.com/Info/Articles/Supply_decoupling.pdf

bottom line: keep conrtol over your currents

best regards,
 
jcx has some good advice... here's my notes.

Use a big solid ground plane on both analog and digital sides - star configurations are good for a few things but data converter designs aren't one of them. Keep your analog/digital ground planes separate, connecting them only underneath the DAC using a single copper trace or a zero ohm resistor. *don't* overlap them - I'd suggest a relief of at least 1mm between planes.

Keep your planes solid - don't drop too many vias close together which take "chunks" out of the ground plane, and don't run any traces on the ground plane itself.

And don't run any high speed digital traces over the analog ground plane, keep these on top of the digital plane. If you have to run digital traces to the analog side for digital pots or whatnot, bridge the analog/digital gap with a pi filter made with a couple 1000pf capacitors and a 600 ohm ferrite bead, and a 220 ohm resistor on the digital driving end.

I recently finished a DAC + headphone amp project using a 4 layer PCB. It's tough to get good solid power supplies and grounds using 2 layers, but I found 4 just right and I haven't found a cheap 6 layer PCB service yet. I've attached gerbers for the copper layers.

maczrool said:
I'm working on laying out a PCB for a small DAC with 6 layers. I have a question about the digital and analog grounds. Can/should the digital and analog grounds overlap each other on separate layers or should the two grounds occupy completely separate areas of the board? Also, is a star or full ground plane preferable for the analog ground?

Thanks,
Stu
 
jcx said:
don't overlap, the capacitance will just couple noise from digital to analog - always keep a "moat" of a few mm free of all copper between digital and analog pwr/gnd planes (including signal traces, route all signal traces that have to go between analog and digital sections over the single "bridge" that joins the digital and analog grounds), pull back the power planes and any traces a few more mm from the edges of the associated gnd plane as well

One idea I have seen on the Analog Devices site (haven't used it myself since I just use 2-sided) is to via together analog ground planes on separate layers -- the board is going to look a bit like swiss cheese.) the vias were layed out on a 100 mil grid.

i do use the "moat" for my amplifiers -- started doing this when i figured out that it was quicker to leave the copper on the board than to remove it. "ring" is used for the inputs of low-noise amplifiers, choppers etc.
 
jackinnj said:


One idea I have seen on the Analog Devices site (haven't used it myself since I just use 2-sided) is to via together analog ground planes on separate layers the vias were layed out on a 100 mil grid.


Yes, an expensive and complex way towards a single plane.

I've always stated, and will repeat that: Semiconductor manufactureres are no experts on board layout.

Funny, everyone has their advises but no-one so far is able or willing to answer 2 simple questions......

regards
 

jcx

Member
2003-02-17 7:38 pm
..
Keeping impedance low by maximizing copper area is important, Guido’s solid gnd plane can be very good and perhaps better for your 1st attempts – it is easy to make matters worse with poorly understood misapplication of partitioning

High speed currents flow in tight return gnd plane image paths that minimize the impedance which is dominated by loop area inductance, the low frequency part of the current flows in the path of least resistance and therefore current and associated voltage drops diffuse throughout the gnd plane, this is where “star” gnd principles and partial separation of the gnd plane by slotting or moats can reduce/control interference from digital gnd return V drops in the analog gnd
 
Hi Guido, jcx and all other ground topology experts!

- Which currents run from analog to digital ?
- Where do these currents run ?


There is no current running from digital to analog - in case of Iout DAC’s and very high input impedance I to V IC's - it is negligible. Current to voltage conversion happens across the feedback resistor (range from around 2Kohms to around 6.8Kohms). In this case, there is no need to worry about signal currents. We should use two large ground planes and separate them purely to avoid RF influence from digital to analog ground. This way we are also controlling our currents.

Now, my question still stands for you noble and wise guys:

Power supply grounds should be dropped straight down (to their corresponding) ground planes???

Yes - no?

Regards,
Extreme_Boky
 

jcx

Member
2003-02-17 7:38 pm
..
all of the current out of the DAC has to find its way back into the DAC to complete the loop (all currents flow in zero sum, closed loops lest electrostatic forces blow your equipment to peices)

interconnected gnd is usually the preferred return

ideal power is seperate, totally isolated batteries for analog and digital, all else is compromise
 
Extreme_Boky said:
Hi Guido, jcx and all other ground topology experts!

- Which currents run from analog to digital ?
- Where do these currents run ?


There is no current running from digital to analog - in case of Iout DAC’s and very high input impedance I to V IC's - it is negligible. Current to voltage conversion happens across the feedback resistor (range from around 2Kohms to around 6.8Kohms). In this case, there is no need to worry about signal currents. We should use two large ground planes and separate them purely to avoid RF influence from digital to analog ground. This way we are also controlling our currents.

Now, my question still stands for you noble and wise guys:

Power supply grounds should be dropped straight down (to their corresponding) ground planes???

Yes - no?

Regards,
Extreme_Boky

Could you explain how to transfer the information from the digital to the analog domain without current flow ?

"Power supply grounds should be dropped straight down (to their corresponding) ground planes???"

please eleborate, I do not get what you mean here ("dropped down")

regards
 

Bricolo

Member
2002-11-11 6:52 am
Something I have read, I don't remember where, is that on a groundplane the return curents flow in order to minimise the loop, so most of the time it's a mix between "a straight line from source to destination" and "following the signal traces". And the big issue was that ground return curents of different chips or pads (IOW: every different ground flow) should not cross on the groundplane.

This would lead to serious headaches. Is the above true?
 
It is impossible to transfer signal without current flow - I agree. So, there is a current flow but is negligible. Input impedance of AD8066 is 1000 G Ohms and input bias current is 3pA. I use this chip exclusively for I to V conversion and even replace the regulation if I have to from +- 15 down to +- 12 to accommodate this chip. I can only try to imagine the amount of current running from DAC Iout pin to the noninv input of AD8066 down to the ground.

So, the question is: where and how does this Iout current find its way to the ground / return ‘back to DAC’? In case of +-2mA Iout DAC chips, is this the ACTUAL current value that flows? How can it possibly flow thru such high AD8066 input impedance?

I have red some of the info (still reading and enjoying it A LOT!) that Jaka Racman posted the links to, and things are slowly starting to make sense. I am trying to understand and separate in my head power supplies' ground return currents, signal ground return currents, where and how to rout them while paying attention to shortest returns possible, noisy RF section isolation, while EVERYTHING SHARES THE SAME GROUND PLANE...!!!

Regards,
Extreme_Boky
 
Good!

This is why I to V conversion happens across a feedback resistor:

Current to voltage conversion happens across the feedback resistor (range from around 2Kohms to around 6.8Kohms)

Now, there's still one question to answer: Where and how is this current finding its way back to DAC chip - we all agreed that there must be a way for this current to flow AND come back to DAC chip!

Regards,
Extreme_Boky
 
Extreme_Boky said:
It is impossible to transfer signal without current flow - I agree. So, there is a current flow but is negligible. Input impedance of AD8066 is 1000 G Ohms and input bias current is 3pA. I use this chip exclusively for I to V conversion So, the question is: where and how does this Iout current find its way to the ground / return ‘back to DAC’? In case of +-2mA Iout DAC chips, is this the ACTUAL current value that flows? How can it possibly flow thru such high AD8066 input impedance? Extreme_Boky

You completely miss the point: An IV converter has ZERO (0) input impedance, after all that is what you wanted.

The output impedance of most current output DACs is not that high (1k-ohm for PCM63): worse however is that they are dominated at higher frequencies (steps) by output capacitance (assumed 10pF)

At the steps currents flow......

The currents I actually point at are generated internally but close externally through the gnd pins of the IC.

All other currents (supply, reference) can be controlled by design and layout in such a way that they do not cross borders

Once that has been achieved there is not a single reason not to fully interconnect these planes. The major advantage is the lower impedance between both domains, hence MUCH lower voltage is generated between these, resulting in lower RF emissions and induced voltage (on chip) in turn reducing jitter.

And yes, there's still semi manufacturers advising to put ferrites between both grounds. Do there guys ever measure ?