Ground Loops in PCB design

[audiomaticmastering]

I'm new to PCB design, so this is probably a noob question. I'm laying out a PCB using circuitmaker, this is not a design I'll ever have manufactured, its just practice. I making the design a two layer board, top and bottom copper, all of the components are through hole. When I use the auto router then pour my ground plane the router wants to connect all of the grounds with traces then connect the pads to the ground plane. Like I said, I'm new to PCB layout but I've done enough audio repair work to know that seems like the kind of thing that would cause a ground loop of some kind. It would be easy enough to delete the traces and leave the pads connected to the ground plane. I double checked and in this case this isn't an island, the big plane is definitely the GND net. And as an aside is there a convention for the right way to connect the top and bottom copper GND planes in an audio application? That is to say, should I add vias just to make the connection or are the through hole components doing the work? Looking for input from people with more experience doing audio PCB layout. I did a search, but didn't find any threads on the subject with this issue. Thanks.

 

[JohnRoberts]

There are many variables to consider, and more than one good solution.

JR

 

[ruffrecords]

There is obviously a problem with your CAD package. Assuming you defined you copper pour to be connected to the ground net then it should track them and then pour. I suspect this is just finger trouble with your CAD package. What it should do is just connect ground pads to the copper pour with thermal reliefs.

That aside it flooding the ground is in general a good idea because it reduces ground impedances. Having siad that, it is still good practice to try to arrange your placemenet of components so that output stages are nearest where the power enters and low level stages are furthest away. This prevents/reduces the chance of high output currents flowing in sensitive input ground copper.

Cheers

Ian

 

[Bo Deadly]

Auto-routing is does not work. At least I've never heard of one that did and I don't see how it could unless it somehow knew which nets were sending and returning currents and knew the impedances of nets and intelligence that only the designer could know. Generally PCB layout software only knows the footprints of parts and not what the parts actually do.

So it's either a problem with the auto-router or maybe some kind of mistake caused by how nets are named. In Eagle you have to give nets and planes the same name or they won't be conjoined. In your case I can see the thermals connecting the pads to the ground plane so I don't know what the problem is.

I would "rip-up" all layouts and try to "pour" the ground plane with the traces as just air wires and not layed out. Then it will probably assimilate them properly.

You have to layout things manually because there are all sorts of rules that require considering where currents are flowing and high impedance traces need to be short and signals that are amplified a lot need to be isolated and so on. The biggie is that you have to minimize the area between traces that send current and then return that current. Those traces need to be very close together (sort of like how heater wires in a tube amp must be twisted together) so that the magnetic fields generated by current running through them will cancel. If the fields are not canceled, nearby circuitry can pick that up and possibly amplify it as noise. It's all about were the electric and magnetic fields running are and how to minimize their interactions with each other.

 

[ruffrecords]

I agree - do not use the auto router. They are rather stupid in my experience (certainly for audio circuits).

Cheers

Ian

 

[audiomaticmastering]

ruffrecords and bo deadly were right, it's a bug in the software. You need to pour your ground planes before running the autorouter. If you do things in that order it grounds everything to the planes then makes the traces from there. I'm also starting to understand the no autorouter sentiment, now that I have it working right it is doing some insane stuff. Thanks for the help

 

[MidnightArrakis]

I'm new to PCB design, so this is probably a noob question. I'm laying out a PCB using circuitmaker, this is not a design I'll ever have manufactured, its just practice. I making the design a two layer board, top and bottom copper, all of the components are through hole. When I use the auto router then pour my ground plane the router wants to connect all of the grounds with traces then connect the pads to the ground plane. Like I said, I'm new to PCB layout but I've done enough audio repair work to know that seems like the kind of thing that would cause a ground loop of some kind. It would be easy enough to delete the traces and leave the pads connected to the ground plane. I double checked and in this case this isn't an island, the big plane is definitely the GND net. And as an aside is there a convention for the right way to connect the top and bottom copper GND planes in an audio application? That is to say, should I add vias just to make the connection or are the through hole components doing the work? Looking for input from people with more experience doing audio PCB layout. I did a search, but didn't find any threads on the subject with this issue. Thanks.

View attachment 91330

I am new to PCB design also and here is my 2-cents worth --- On the various types of PCB's that I have had to design for a variety of aerospace/avionics companies, defense contractors, medical electronics firms, NASA, R&D laboratories and telecommunications and video electronics corporations.....they all have a general rule about using a Copper Pour as a Ground Plane and it is: THE MORE "STITCHING" VIAS BETWEEN THE LAYERS, THE BETTER!!! (NOTE: "Stitching Vias" is a term used for vias that are connected to the GROUND net and placed within a Copper Pour). On many of the PCB's I have designed that required "stitching vias", the numbers of those stitching vias ran up into the hundreds. Prior to the COVID-19 lock-down I was working at a defense contractor that was developing a new series of avionics electronics for a new breed of U.S. fighter jets and two of the larger PCB's had over -- literally!!! -- > ONE MILLION "STITCHING" VIAS!!! < If I remember correctly, all of those vias used a 6-mil or even smaller drill hole. I think those two PCB's were being laser-drilled and were also using some manner of new Thru-Hole plating process in order to get the copper-plating into such a small area of space. But, I digress......

As has been mentioned by others, auto-routers do not work very well on audio circuits. The above-mentioned PCB's were auto-routed, but they were strictly digital layouts and even then, it took several hours to configure and setup the auto-routing routines so the end result made any sense on a 30-layer PCB!!! In short, one easy thing to remember is.....simply remove the GROUND net from the auto-routing routine and take care of it manually. You'll be fine then.

[I'm laying out a PCB using circuitmaker] -- I believe your best bet would be to download the -- FREE -- PCB Design software by KiCAD and learn how to use it. It will serve you well for all of your home-based PCB layouts. In fact, I have noticed several times this year (2022) that various commercial electronics companies have even now adopted using KiCAD as their main PCB layout tool. And, if you wish, you can even spend the "whopping" amount of $35 for their KiCAD Training Course and even download 8.5GB worth of training videos!!! All of the videos are presented in small 3-to-15 minute chunks that makes the digestion and understanding of what is being presented and taught very easy to deal with. I highly recommend it!!!

Meanwhile.....create a folder on your hard-drive and maybe call it -- PCB Design Reference Material -- and download and place the attached PDF files into it. Then, you will have the beginnings of your own "Technical Library" of material that you can read to learn more about not only PCB design, but also any other technical areas that interest you. HERE YA GO!!!.....

/

FREE KiCAD PCB Design Software Download Link

https://www.kicad.org/download/
/

 

[abbey road d enfer]

Auto-routing is does not work. At least I've never heard of one that did and I don't see how it could unless it somehow knew which nets were sending and returning currents and knew the impedances of nets and intelligence that only the designer could know.

I agree - do not use the auto router. They are rather stupid in my experience (certainly for audio circuits).

I don't fully agree with that.
Placement is key. If placement is correct, ground circulation is also more or less correct and need just a little tweaking. What's "stupid" is a copper pour that covers the whole area of a PCB.
The copper pour must be done with polygons that isolate parts of the circuit that shouldn't connect in a non-hierarchical manner.
Of course, no autorouter works right at first go, but they're great time savers.

 

[PureBasic]

For OP: Make your ground pour, and use the autorouter on the remaining nets only once your critical signals have been routed.
Autorouters may be fine once the placement is logical and critical nets have already been routed. They work if you restrict them to a small group of nets. I never use them tho... The result is just ugly and stupid...

The copper pour must be done with polygons that isolate parts of the circuit that shouldn't connect in a non-hierarchical manner.

That's actually not true. Every parts of a PCB are connected to each other in some way, and coupled to the environment the PCB is sitting in. Your reference plane MUST be sturdy and signal traces must be able to reference to it anytime to ensure proper propagation. Splitting planes are indeed what is recommended in a lot of datasheets and application notes, but it's wrong a lot of the time (even at Analog Devices). You won't see experienced mixed signals PCB designers split a plane unless it is strictly necessary*.

*pre-amped A/D conversion for example, where you might even make a split board.

 

[PureBasic]

I recommend looking at Rick Hartley talks and interviews on youtube. It mostly concerns high speed signals routing but the principles are really important to understand if you want to take routing seriously. You can't go wrong with those advices.

 

[MisterCMRR]

The ONLY fool-proof way to avoid nasty "ground loop" (actually common-impedance coupling on a circuit board design is to include the resistance of every trace that connects a component to ground. Now, if you're a real engineer and understand circuit theory (Ohms law mostly), it will become obvious which parts should not share a path to "mecca" (the star ground point on the board - most often where power-supply common meets signal path returns ("grounds"). Connecting everything as directly as possible to a big beefy and uninterrupted ground plane can help - but realize that it's a "shotgun" approach and I've seen many boards that still have noise problems and instability issues because there's a trace somewhere in a high-gain location that also has a component from the output section tied to it. It helps to put all these extra "trace resistors" in the circuit simulator - then you can see the effects. And don't even get me started about the "standard" practice (they get away with it on all-digital boards) of putting power-rail bypass caps everywhere. Remember that any noise on the power rail is coupled into the local ground system via these capacitors. At the very least, include a de-coupling impedance (resistor or inductor) in the power feeds to each "stage" in the signal chain. It takes real attention to detail to achieve 120 dB + dynamic range on an analog signal processing board. I've yet to see any kind of instruction, in college or otherwise, about this subject.

I was invited to speak to a group of 300 EE students and professors at MIT in 2009. The EE professor who invited me told me after the presentation "We don't teach any of this stuff here ... ground = ground = ground." But, if you do the math, even though the currents may be only mA or uA and the resistance only milli-ohms, micro-volts of noise and coupling easily occur unless the sequence of connections is correct. And a few micro-volts of noise can destroy a -100 dBu noise floor.

Just wanted to put the discussion in perspective ...

 

[abbey road d enfer]

Autorouters may be fine once the placement is logical and critical nets have already been routed.

I agree.

That's actually not true. Every parts of a PCB are connected to each other in some way, and coupled to the environment the PCB is sitting in.

Quite a bold statement.
Isolation must be taken in the sense of preventing current to mingle where they shouldn't. Isolation is not insulation. Of course, copper pours are eventually galvanically connected.

Splitting planes are indeed what is recommended in a lot of datasheets and application notes, but it's wrong a lot of the time (even at Analog Devices).

Maybe, but it's always worked for me. It's wrong when one doesn't understand why to do it.

You won't see experienced mixed signals PCB designers split a plane unless it is strictly necessary*.

So you agree that sometimes it's the right thing to do...

 

[Newmarket]

I am new to PCB design also and here is my 2-cents worth --- On the various types of PCB's that I have had to design for a variety of aerospace/avionics companies, defense contractors, medical electronics firms, NASA, R&D...

On many of the PCB's I have designed that required "stitching vias",

Does not compute !

 

[Matt Syson]

Of course the conundrum that needs to be 'solved' is that every conductor is an 'aerial' either 'transmitting' or 'receiving' interference from everything else. so depending on the frequencies you are interested in working with the only way to prevent 'noise' (picked up electrostatically or magnetically) is for your finished circuit to be infinitely small. A 4 inch (approx 100mm) conductor is a good aerial at microwave frequencies so one end can be an 'open circuit' node at it's resonant frequency so if it is intended as an 'earth' trace, it simply isn't.Of course this is an extreme example but nonetheless important to consider. Hence the strange claims that a 'recording studio (my area of activity) built on a second or third (or more ) floor of a building with a thick 'ground' wire is not necessarily grounded at all at some RF frequencies. Electrical safety ground yes but not necessarily even a good 'audio frequency' ground.

 

[ruffrecords]

Does not compute !

The emboldened text was a quote from the OP not from Midnight Arrakis - he should have quoted it properly.

Cheers

Ian

 

[Audio1Man]

The layout of a PCB is never an easy task. I personally know only a few people who will do a great job for ANALOG PCB layout. Many have the basic knowledge but lack the practical experience to follow through. I started out in AUDIO as a hobby, then into Microwave, Coaxial switches, Waveguides, Antennas, and RF design then later back into Audio/Analog design. When I was @ Audio Precision every little bit was used to put the PRECISION where it counts, like no common via connections (even the pa’s and less are problems >-140dB). Looking at the coupling between traces and steel hardware cause linearly problems.

Don’t ask me about Auto Routers, as you should know my answer (-60/-80dB vs -120dB or better). Bill and Abbey know this.

Duke

 

[Newmarket]

The emboldened text was a quote from the OP not from Midnight Arrakis - he should have quoted it properly.

Cheers

Ian

Thanks Ian. Makes sense now. Although the post remains a bit errr..."Intense".
To put it context - I'm well versed in the use of "via stitching" - but it's not the whole answer here.
Particularly with a 2 layer design - as the OP has in mind - not running signal over breaks in the plane (= larger loop area) is key.
Henry Ott (RIP) stuff is good on this and also the articles by Keith Armstrong (Cherryclough Consultants) even if I disagree slightly about some of his examples wrt audio.

 

[Newmarket]

Of course the conundrum that needs to be 'solved' is that every conductor is an 'aerial' either 'transmitting' or 'receiving' interference from everything else. so depending on the frequencies you are interested in working with the only way to prevent 'noise' (picked up electrostatically or magnetically) is for your finished circuit to be infinitely small. A 4 inch (approx 100mm) conductor is a good aerial at microwave frequencies so one end can be an 'open circuit' node at it's resonant frequency so if it is intended as an 'earth' trace, it simply isn't.Of course this is an extreme example but nonetheless important to consider. Hence the strange claims that a 'recording studio (my area of activity) built on a second or third (or more ) floor of a building with a thick 'ground' wire is not necessarily grounded at all at some RF frequencies. Electrical safety ground yes but not necessarily even a good 'audio frequency' ground.

All very dependent on the power distribution detail.
Connection to the actual planet Earth is not the issue for 'noise' although it is clearly often practically necessary for safety considerations and this can complicate things.
The impedance to the reference voltage is the important factor.

 

[Bo Deadly]

When I was @ Audio Precision every little bit was used to put the PRECISION where it counts, like no common via connections

What do you mean by this? Are you saying vias are not used to connect the ground plane to the other side? Why? Because currents make complex paths which equates to disturbances in fields that can now be coupled to nearby circuitry?

(even the pa’s and less are problems >-140dB).

What are "pa's"? Precision analyzers?

Looking at the coupling between traces and steel hardware cause linearly problems.

So how do you mitigate? Plastic hardware or distance?

 

[warpie]

interesting thread!