Page 1 of 1

PCB design and ground layout considerations

Posted: Tue 2010-12-21 15:17
by Panu
Ground layout is one of the trickiest parts of analog design. There's some discussion about the subject at the Simple DSP Board Application Note, at ... le_dsp.pdf, chapter 1.4, "PCB Layout".

The easiest way to good analog performance often comes with separate analog and digital grounds, while the most robust, reliable and ESD-tolerant design comes with using a single ground plane. These two goals can be achieved at the same time. Read forward to find out how.

Differences on the potentials of different GND pins can cause large ground currents in the chip, which are harmful. So if you want to use different grounds for analog and digital, you need to make all the ground tracks large enough, so that the ground is very strong at all points.

The most important thing to consider for ground layout is that all signals should flow directly over a ground plane, and that they should not cross any gaps in the ground plane. See the following picture, which is an example of bad design, try not to do this:
groundplane2.png (25.8 KiB) Viewed 15673 times
The return current of the signal is forced to go around the gap in the plane, so they don't flow directly over each other. This causes the effective ground plane to be much smaller than what it seems. Also the return paths of different frequency components in the signal are different; high frequency return currents tend to flow close to the signal trace (minimum inductance path) and low frequency components take the shortest (minimum resistance) path. The more different the forward and return paths of the current are, the more different are their impedances. The impedance difference causes signal quality problems. The "Area of Problems" is not the source of the problem, but minimizing the area minimizes the problem. Then consider that you have other signals that also cross the gap in the ground plane. It becomes highly difficult to analyze the behaviour of the return currents and how they affect each other.

All VS10xx devices in LQFP package have their analog pins along the top edge of the IC. If you want to keep analog and digital grounds different, below is one suggestion on how to split the ground plane. This is a good design example, always try to do this:
groundplane3.png (32.87 KiB) Viewed 15673 times
The plane is not split under the IC, but you should not route any signals over the dashed line, along with the planes combine under the IC (marked "No routing zone" in the picture). This way the plane is uniform under all pins of the IC, but there's minimal coupling between analog and digital signals.

Of course, as a direct consequence of the "don't cross the gap" rule, it's absolutely forbidden to route any digital signals over the analog ground area.

Also a couple of small hints for PCB layout design:
1) The RCAP capacitor should be the first component that you place and route beside the VS10xx chip. You should have no vias between RCAP and the VS10xx.
2) Try to route the analog outputs (LEFT, RIGHT, and especially GBUF) to the connector without using vias.

Comments welcome!


Re: PCB design and ground layout considerations

Posted: Fri 2015-04-17 14:15
by Panu
Design Links:

Tips and Guidelines for Designing VS1005 Boards: viewtopic.php?f=13&t=1500

Soldering and stencil design guide: download/file.php?id=1484
soldering.png (137.86 KiB) Viewed 6886 times

Please add more.

Re: PCB design and ground layout considerations

Posted: Sun 2018-03-18 22:08
by fwachsmuth
Hey Panu,

this is excellent advise and helped me with routing my board (still waiting for delivery, so can't judge yet how it sounds).
I managed to route all the Audio portions on the top layer and keep the bottom layer for GNDA.

One question though: Is it a good idea to fill the top layer with GNDA zones too and connect them with some vias to GNDA on the bottom? Or should the GNDA be on one layer only?

See below. green is bottom, red is top -- I used GNDD to fill both layers for the digital part, but for the analog part, I only used a GND zone on the bottom.

(Note that I intend to connect the two Grounds later via a solder jumper, KiCad got badly confused when I suddenly connected both GNDs after fillzones had been in place already)
GNDA.png (176.39 KiB) Viewed 5876 times

Re: PCB design and ground layout considerations

Posted: Tue 2018-04-03 20:45
by fwachsmuth
Any hint regarding the ground plane? Seems I need to get a "Rev B" of my PCB made soon anyway...

Re: PCB design and ground layout considerations

Posted: Wed 2018-04-04 13:28
by sami

The analog ground seems good.
The power routing should be low impedance too. You may consider filling analog part of top layer with AVDD.
The DGND should have lots of vias between top and bottom layers so that the impedance is kept at minimum.
The 1V8 net should be routed with thick wires for low impedance.

Re: PCB design and ground layout considerations

Posted: Wed 2018-04-04 16:30
by fwachsmuth
Thanks, that helps big time for the next PCB revision.

Re: PCB design and ground layout considerations

Posted: Thu 2018-04-05 8:38
by Panu
Any hint regarding the ground plane? Seems I need to get a "Rev B" of my PCB made soon anyway...

While your ground layout seems better than most we've seen, it seems that you still have traces going across the gap between the analog ground and digital ground. From the picture it's difficult to see if they are something else than ground traces or not. If you want maximum performance, redesign your analog ground so that there are no traces going across the gap, e.g. you could drill through the gap and nothing would be broken.

Then fill the gap so that the analog and digital grounds are not separate.

If you follow the "could drill through the gap" rule and then connect the grounds together, the analog performance is the same (in our tests, it's been even a little bit better than with the gap) but error resilience is a LOT better, e.g. no burned chips when something puts a large transient or DC bias to the analog ground (via an external connector).

Flowing current through analog ground pins to digital ground pins causes bad things to happen inside the IC.


Declicking circuit for Line Out

Posted: Wed 2019-05-01 20:24
by Panu
For a proper De-Clicking Circuit for Line Out, please see viewtopic.php?f=9&t=1107&p=12714#p12714 :!: