Mixed-signal board design

[xng14]

Hi everyone!

I'm currently working on a project which involves doing digital signal processing(DSP) on an analog signal. The basic flowchart looks like that:

Input buffer => ADC => DSP => DAC => Output buffer

The circuit itself is pretty much sorted out and the next step would be to lay out the board. But now I'm confused about what to do with the digital and analog grounds. I've done my own research online but there seems to be no general consensus on what would be the best approach. Some suggest using one solid ground plane and partitioning the pcb in analog and digital sections. Others(namely the adc and dac datasheets) suggest using separate digital and analog grounds and joining them at the device. Problem is that if I connect both grounds at the adc and the dac I've just created a ground loop!

And what with the supplies? The analog section needs +-12v (for the opamps) and 5v for the analog section of the adc and dac. The digital section needs 5v. Should I use separate voltage regulators and filter caps for all of these? And what should I do with the grounds in the power supply?

So my question is : What would be the best supply and grounding scheme for such a circuit?

I'm trying to design this thing on a double-sided board in order to keep the cost down so the use of separate ground and power planes isn't really an option.(altough could be used if that is really the only option)
Also the noise performance is quite important. The last thing I want is to have digital noise summed with the analog signal.

So, what do you think?
Thanks!

[Short Circuit]

Generally speaking, split groundplanes are difficult to implement in real life circuits, as you noticed already.
Additionally, they are much more difficult to pass EMC testing. Both functional and for EMC, the slightest mistake
may give you more bad than good.

I certainly recommend to move to 4-layer and take the additional cost. It's much safer and saves a lot of design time too.
Also, the board can probably get smaller too because you don't need space to route power or ground signals, as wel as the
occasional leftover traces that are hard to route (use the power layer for that and keep GND as solid as possible).

[ejeffrey]

Definitely don't follow the ADC notes and join the analog and digital ground planes at the ADC.  That works OK for demo boards where the ADC is the only important chip on the PCB, but not for most realistic circuits.

Basically, you should treat an ADC as an analog part.  Both the AGND and DGND pins should be connected together and to the (analog) ground plane right at the ADC.

In the ideal situation, you would not use split ground planes.  As short circuit said, ot is easier to get wrong that right, and when you get it right the advantage is normally small compared to the same layout without the split ground plane.  The best general purpose solution is to use a single ground plane but keep the analog and digital signals separated, relying on the natural tendency of current to follow the path of least inductance to keep the ground currents from interfering.  This is much easier with multi layer boards both because you have more freedom in routing and because the signal layers are much closer to the ground/power planes, so the currents are much better confined.

If you do split ground planes the AGND and DGND plane should usually be joined near the power supply -- not the ADC.  ADCs and DACs should be located in the analog section.  The digital signals from the mixed signal devices need special care.  You want to keep them from crossing a break in the ground plane.  The ideal situation it to run the back towards the power supply where the ground planes are connected.

[xng14]

So the best solution would be to use a single nice solid ground plane on the bottom of the board(and perhaps a few links), all the signals routes on top and physically separating the analog parts/signals from the digital ones ?

[jahonen]

I think it is easiest to just partition the components correctly (digital on one side of the board and analog at other side, and ADC/DAC in between) and use single solid ground plane. That produces less surprises than trying to split anything. Beware the noise coupling via power rails, though. See the following article by Henry Ott:

http://www.hottconsultants.com/pdf_files/june2001pcd_mixedsignal.pdf

You might want to use at least 4 layer board, it simplifies the layout considerably (no temptation to put traces in ground plane layer).

Regards,
Janne

[slateraptor]

I think it is easiest to just partition the components correctly (digital on one side of the board and analog at other side, and ADC/DAC in between) and use single solid ground plane. That produces less surprises than trying to split anything. Beware the noise coupling via power rails, though. See the following article by Henry Ott:

http://www.hottconsultants.com/pdf_files/june2001pcd_mixedsignal.pdf

You might want to use at least 4 layer board, it simplifies the layout considerably (no temptation to put traces in ground plane layer).

Regards,
Janne

Great stuff. Thanks, jahonen!


EDIT: Just realized that ejeffrey's advice is practically identical to Ott's.

Definitely don't follow the ADC notes and join the analog and digital ground planes at the ADC.  That works OK for demo boards where the ADC is the only important chip on the PCB, but not for most realistic circuits.

Basically, you should treat an ADC as an analog part.  Both the AGND and DGND pins should be connected together and to the (analog) ground plane right at the ADC.

Both highlighted comments appear to be what was done in Figure 8 from the above linked article, that is to say
1) a "bridge" was used to electrically connect AGND and DGND planes maintaining a single ground plane, and
2) both AGND and DGND pins are connected to the ground plane at the ADC.

So if I understood the paper correctly, this ensures that any current return path crossing that occurs between AGND and DGND is contained at the bridge, preventing digital noise from spreading into the rest of the AGND. Yeah?

[jahonen]

I have actually done some measurements in the past, the details are in this topic. The result was that the ground split advantage was not very great (about 2-5 dB at best), and was even negative for some frequencies due to some resonance effect.

Regards,
Janne

[slateraptor]

I have actually done some measurements in the past, the details are in this topic. The result was that the ground split advantage was not very great (about 2-5 dB at best), and was even negative for some frequencies due to some resonance effect.

Regards,
Janne

Oh, looks like a wealth of knowledge in that thread. Thanks again!

[ejeffrey]

EDIT: Just realized that ejeffrey's advice is practically identical to Ott's.

This is not an accident

If you want an whole book on the subject check out Ott's book "Electromagnetic Compatibility Engineering" or the older version "Noise Reduction Techniques in Electronic Systems."  He covers everything from building level design (how to wire the grounds of your equipment cabinets together) to signal interconnect cables down to PCB layout with concern both for functional performance and EMC.

[slateraptor]

I definitely intend to add a few books by Ott to my personal library...when I'm not a poor college student anymore. Until then, I'm "borrowing" a few PDFs from the interwebs.

In a few short months and with a bit of luck on my side, I'll be a gainfully employed full-time EE...and part-time graduate student sitting in Clayton Paul's lecture room.

www.amazon.com/dp/0471755001

[Alex]

If you want an whole book on the subject check out Ott's book "Electromagnetic Compatibility Engineering" or the older version "Noise Reduction Techniques in Electronic Systems."  He covers everything from building level design (how to wire the grounds of your equipment cabinets together) to signal interconnect cables down to PCB layout with concern both for functional performance and EMC.

...and another one the Ott followers should be aware of, thinner but also packed with great information and a bit more practical is Keith Armostrong's EMC for Printed Circuit Boards - Basic and advanced layout techniques. I think it is being reprinted at the moment.

The Paul Clayton book linked by slateraptor gives more details in the physics and maths behind EMC. Not the kind of stuff you have time for when designing a PCB, but great to develop an intuition for or solve a novel problem. I only have the Henry's and Keith's books; they are worth every penny.

[Neilm]

...and another one the Ott followers should be aware of, thinner but also packed with great information and a bit more practical is Keith Armostrong's EMC for Printed Circuit Boards - Basic and advanced layout techniques. I think it is being reprinted at the moment.

Definitely seconded. I was given the task of having to update the products of the company I worked for a few years ago when the required EMC standards changed. Most of the products were two layered units that did not perform to the new requirements. In having to understand more about EMC I found Keith Armstrong's book, and a website he regularly contributes to - http://www.compliance-club.com I found the book and website to be invaluable in what I did.

For information - the most common thing for a solution I found was to make the two layer boards four layer with a common 0V plane for both analogue and digital signals. In all cases, the EMC performance of the units was improved. On several products, the performance improved so much that we were able to remove some additional work (ferrites / shielding etc) that more than paid for going to the four layers.

Neil

[Rudolfo]

Maybe this advice from the ADC people is worst to look at: http://www.analog.com/library/analogdialogue/archives/43-09/EDch%2012%20pc%20issues.pdf