Multilayer ground

[maczrool]

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]

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]

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

[Guido Tent]

Originally posted by maczrool
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 ?

http://www.tentlabs.com/Info/Article...decoupling.pdf

bottom line: keep conrtol over your currents

best regards,

[gmarsh]

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.

Originally posted by maczrool
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

[jackinnj]

Originally posted by jcx
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.

[Guido Tent]

Originally posted by jackinnj


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]

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

[maczrool]

Thanks everyone! Very helpful.

Stu

[Extreme_Boky]

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