Requesting advice to reduce noise in car audio PCB - Page 1
Forum section: electronics / projects

author: maakbaas
author_rank: Newbie
timestamp: June 07, 2020, 08:10:58 am
content: Hello, have been reading here for a long time, but this time I was hoping to ask for some of your expertise. This is my first ever PCB design project, so please forgive me my mistakes.You can read more about the purpose of the PCB and the projecton my blog.So basically, I have developed a PCB to add bluetooth audio to my car by faking the CD changer. I did this with an ESP32 for bluetooth and an external DAC (PCM1789) for the audio outputs. I have two versions of the PCB which are shown below. The larger PCB is version 1, the smaller PCB is version 2.Version 1In version 1 I used a LM2940 linear regulator to go from 12V to 5V, and a Recom R1SX-0505-R to create an isolated 5V for the analog part of the PCB. I used a separate ground plane under all the audio components. Audio/noise performance is maybe not perfect, but acceptable for me at least. The problem with this PCB is that while it was working perfectly on my desk, the linear regulator produces too much heat in the car (14V instead of 12V), between 1 and 2 watts which it can at least with my PCB not dissipate triggering overtemperature shutdowns on the LM2940.Just the audio and power components of the PCB:Top layer:Bottom layer:Version 2To solve this in the second version I changed the LM2940 to a LM2594 switching regulator to go from 12V to 5V. What I also did as an experiment in this design was remove the isolated DC/DC converter because I had included this as a precaution and I was curious if it was really needed or not. Again I used a separate ground plane under the audio components, this time with a small connection to the main ground. So this PCB also worked fine on my desk, but in the car the audio quality is not acceptable. There is an audible high pitched whine on the audio outputs which changes with the revs of the engine of the car. To give an indication for the level, if you play music it is not too noticeable, but I listen a lot to audiobooks, and there you have more silences between sentences so there it is more noticeable. So, it is not extreme, but annoying enough to not want to live with it.Just the audio and power components of the PCB:Top layer:Bottom layer:Next stepsI am hoping with the next iteration to create the final PCB that solves both audio and temperature issues. Therefore I would like some input from you guys.Are there any obvious mistakes or poor design choices in my PCB which could lead to additional noise?The most obvious solution for me is to combine the two approaches, use the LM2594 switching regulator in combination with the Recom R1SX-0505-R. Do you think this will fix it 100%, or will the fact that the 12V to 5V is a switching regulator instead of a linear one still create more noise, regardless of the isolated DC/DC inbetween?The second choice could be to change the PCB design of design 1 with more thermal vias and copper to try to dissipate the heat, or change to a through hole package for the LM2940 which can also dissipate more. Still you are creating a lot of heatAre there completely different configurations or solutions for this design which are more commonly used that I overlooked?I guess question 2 is the main one for me, since I lack the experience and insight to judge this. Would the performance of this layout be the same as version 1? close to version 1, or rather closer to version 2?Thanks in advance for thinking with me. I am hoping that my next design will be the final one, which is why I would like some additional input rather than just continuing with the trial and error process

author: homebrew
author_rank: Frequent Contributor
timestamp: June 07, 2020, 10:35:46 am
content: Hi MaakbassAlthough being just a hobbyist, I see several things ...1) Absolutely inadequate (i.e. not existing) DC input filtering and protection. The "12V" supply in a car tends to be noisy and can contain high spikes. There might even be situations when the polarity reverses (e.g. an idiot connecting starter leads or the battery backwards).Just google for "Automotive load dump polarity reverse" and get a ton of design guidelines ...2) I would definitively add an adequate fuse!As for the PCB-Layout ...1) The ground plane layout seems BAD! With the separate ground plane you've probably build a decent magnetic pickup, because you've created large loop areas. When you split ground planes, no other tracks should cross the gaps (at least not without further measures), because the return currents can only flow through the one connection point. This is a good example, where good intention can lead to an even worse result...2) You've got a weird flood-filling algorithm, that seems to isolate already layed out ground tracks from the flood fill.Maybe the experts here will add additional thoughts or correct me, where I'm wrong ...

author: maakbaas
author_rank: Newbie
timestamp: June 07, 2020, 04:14:12 pm
content: Quote from: homebrew on June 07, 2020, 10:35:46 amThank you for your comments.1.1 Regarding your comments on the DC side, this might be true for the second design but not for the first. The LM2940 actually has built in reverse polarity detection, and can deal with spikes up to 60V. This component is very well suited for automotive for those reasons, I used the external components as per the datasheet. The second design is indeed less protected, but at the same time, this is for in my own car, so I can live with the fact that the PCB will die if I reverse polarity on the battery, which I hopefully won't do.1.2 Fuse might be a good idea to improve the design.2.1 Do you have any reference or source where I could read and learn more on these topics? Does your comment relate to the first design or the second? In the first design I am not sure if your reasoning is correct, since there there is an AGND and DGND which are separated with the isolated DC/DC, and there is no loop from AGND to DGND so I don't immediately see how there could be a loop.2.2 Yes, in part the traces were meant to be separated from the plane to provide the correct bypass paths, but I am sure I made mistakes there, and I also saw later that the plane is connected to some pads which it should not be connected to for the way I tried to design it, which might of course have been wrong in the first place.

author: homebrew
author_rank: Frequent Contributor
timestamp: June 07, 2020, 07:35:30 pm
content: Yes, all my comments referred to your second design iteration.The first design looks even more strange to me as there seems to be absolutely no connection between the AGND and the DGND at all. You would be just relying on the internal connection of the chip (if there is any) ... But I might misinterpret you design entirely ...Anyway, Section 10.2 (Page 33) of the PCM1789 datasheet provides some advise on ground plane layout.To demonstrated what my concerns are, I've overlayed your second pcb pictures and have drawn the current paths for the analog supply of the PCM1789. As you can see, power and ground diverts in different directions and the resulting loop nearly spans half of your PCB. You could trace out also the return current for the digital lines as well, that span even wider loop areas.To my understanding, having separate ground planes does not mean that they should be galvanically isolated but rather that they should not share their return currents mutually. Thus, the analog ground plane should carry only the analog currents and the digital ground plane should carry only digital return currents. At some point a common potential must be established. However, you must control where the currents flow and keep the resulting loop area as small as possible.This link could be relevant:https://www.analog.com/en/analog-dialogue/articles/staying-well-grounded.htmlIn my opinion a very good discussion of the topic:https://electronics.stackexchange.com/questions/128637/how-should-i-connect-agnd-and-dgnd

author: maakbaas
author_rank: Newbie
timestamp: June 11, 2020, 02:42:59 pm
content: Quote from: homebrew on June 07, 2020, 07:35:30 pmThank you for your time and the sources. I am currently reading and learning.

author: SilverSolder
author_rank: Super Contributor
timestamp: June 11, 2020, 04:45:41 pm
content: Ground loops are a big issue in cars, since the chassis of the car is used not only as ground, but the negative conductor... So your DC/DC converter idea is a winner, I'd keep that in the final version.Another solution could be to use an audio transformer to break the ground loop. You could try that today on your second design, and see if it removes the noise!

author: David Hess
author_rank: Super Contributor
timestamp: June 12, 2020, 11:21:06 am
content: I have had problems with alternator whine getting into my car audio before.Alternator whine usually is the result of a ground loop however in this case it could be caused by lower line regulation with the switching converter since that is what you changed. This is one of those cases where I might consider using a capacitance multiplier which could double as input protection for the switching regulator if improving the regulator's line regulation was not an option.The analog and digital ground planes usually need to be connected at one point but this point might be through the connector.

author: maakbaas
author_rank: Newbie
timestamp: June 21, 2020, 08:46:52 am
content: Thanks for all the suggestions. I understand some things better, although I am still a beginnerI made a new version of the PCB, this is the first time I attempted a 4-layer design, and this time I made sure that no single trace crosses splits in power and ground planes.I am really grateful for the comments so far, and if anyone sees any mistakes in this new version, feel free to let me know.I chose for my second suggestion and combined the isolated DC/DC with the switching 12V to 5V regulator. I did not take care of the comments for DC side protection yet.Also I did not do any pours on the signal layers. Can anybody recommend a good source that discusses this? It is not fully clear to me yet if this would be advantageous or not.Power planes:Ground planes:

author: SilverSolder
author_rank: Super Contributor
timestamp: June 21, 2020, 11:58:49 am
content: What tool are you using to create the PCB? The artwork looks pretty cool...

author: maakbaas
author_rank: Newbie
timestamp: June 21, 2020, 12:04:17 pm
content: Its Kicad. While in 3D viewer there is a menu item to enable ray tracing which improves the render (I also only found out about this today)