Separate ground planes on one PCB

[josechow]

So, I am laying out a pcb with both noisy PWM switchers to drive LEDs and a instrument pickup amplifier on the same PCB. Attached I have an image of what I have in mind to separate the ground planes. I have read a little about ensuring that the two ground connection points to the common ground point should be separate until termination out of the pcb. Also VIA stitching at the boundary points on the ground plane to help noise coupling away from the sensitive audio portion.  Obviously I will have some noise no matter what, but am I on the right track before I start routing lines?

In addition to the ground plane, I understand I want to minimize the connections of the audio outputs overlaying any of the digital PWM side of things to minimize coupling as well.

Bonus: There is sufficient power supply filtering on the audio power supply feeding the audio amplifier; Should the power supply components sit on the PWM side or on the Audio side? Or does it matter?

[radar_macgyver]

It would help to indicate on your sketch where the power supply goes. It's more important to ensure that the voltage induced across the inductance of the power and ground paths feeding the noisy parts of your board doesn't enter into the quiet part. This is partially achieved by splitting the ground planes, but is not necessary if you pay close attention to how the current flows to the noisy parts.

[Neilm]

The idea that a PCB needs separate 0Vs dates back to 2 layer PCBs where chip speeds were so slow it did not particularly matter. From my experience I would not have separate 0V planes unless I need galvanic isolation. A better technique is to try to ensure that the circuit is partitioned into separate zones (as shown in your picture). The noise in the digital and switcher circuits will naturally confine itself to the areas near the switching components - the return current flows under the trace carrying the signal.

[josechow]

It would help to indicate on your sketch where the power supply goes. It's more important to ensure that the voltage induced across the inductance of the power and ground paths feeding the noisy parts of your board doesn't enter into the quiet part. This is partially achieved by splitting the ground planes, but is not necessary if you pay close attention to how the current flows to the noisy parts.

This is my intention, that I attached below. I am still reading up on my brand new "Trilogy of Magnetics" book from Wurth Electronics just haven't gotten to that section yet.

My guess is that the RLC filters on the 12 volt linear supply feeding the audio stuff should connect somewhere else on ground? 

[josechow]

The idea that a PCB needs separate 0Vs dates back to 2 layer PCBs where chip speeds were so slow it did not particularly matter. From my experience I would not have separate 0V planes unless I need galvanic isolation. A better technique is to try to ensure that the circuit is partitioned into separate zones (as shown in your picture). The noise in the digital and switcher circuits will naturally confine itself to the areas near the switching components - the return current flows under the trace carrying the signal.

That was my thought as well, as I have done the voltage field experiment in College Physics lab with multiple shapes and drawing the traces for where the current seeks a pretty interesting path to get from one point to another. But... I've read that the ADC ground point, for which the audio stuff is connected to on the uC needs to be separated from Digital ground, so I thought this had to apply for everything else in terms of separating high power/digital/analog grounds.

[T3sl4co1l]

Control the loop currents in the local areas. That is, pack the inductors and switches and diodes and stuff closely, and keep those some distance from the other things.

Don't break ground, and DEFINITELY don't break ground and span traces over the cut in the ground!

Tim

[josechow]

Control the loop currents in the local areas. That is, pack the inductors and switches and diodes and stuff closely, and keep those some distance from the other things.

Don't break ground, and DEFINITELY don't break ground and span traces over the cut in the ground!

Tim

Roger roger.

[Neilm]

But... I've read that the ADC ground point, for which the audio stuff is connected to on the uC needs to be separated from Digital ground, so I thought this had to apply for everything else in terms of separating high power/digital/analog grounds.

There are a large number of app notes and datasheets that just re-hash the same old ideas as the company has not bothered to investigate updating their advice. They will "prove" it still works with a demo layout or two that works in the application they are doing

[cdwijs]

Hi,
I've had the same question, and this document gave me some answers:
http://www.elmac.co.uk/pdfs/Lord_of_the_board.pdf

Cheers,
Cedric

[cdwijs]

Hi All,
I have the following things in mind while routing a board:

-The return current of a track is under the track, therefore I always have a ground plane under everything.
-Loop antenna's are formed when the current can't flow under the track, so don't interrupt your ground plane.
-Dipole antenna's, or patch antenna's are formed when there are 2 separate ground planes. Always have one big ground plane, just to destroy the antenna. The return currents from noisy circuits will not propagate through, because they want to be local (under the forward track).
-When drawing noisy switching power supply's take 3 color pens, and draw out the current loops in your schematic. Then, on your board minimize the area those current loops make. This will prevent the current from flowing in a loop antenna.
-Place a ground plane under micro controllers, and interrupt it as little as possible. The closer the ground plane is to the chip, the more the fast currents in the chip are able to have a return path.
-via's are free, use them generously to stitch 2 ground planes together. If you have a track in the ground plane, make sure you have a ground plane at the top as well, and place via's so the return currents have a short path to keep following the forward currents in the tracks.
-Also use a lot of ground via's on an etched board, just drill holes, and then solder a wire on both ground planes. Not every via has to be made on the prototype, but they need to be present in the final product that's made by a board house.

-but most importantly: Think in currents, and antenna's.

Cheers,
Cedric