Ground Loops in PCB design

[FIX]

It's a lot simpler than everyone says... If you are doing a whole system, like a console, then their are a lot of things to consider. If you are doing a small board or 500 module, it's pretty straight forward. Some simple rules:

If you do a ground plane, and cut out a space for a transformer, never leave the area around it connected in 360 degrees. You will pick up hum from power supplies, etc. (Eddy currents) Always cut an area out so it doesn't complete a loop.

Input grounds should go directly to the first amp, and the ground should go their too. Then connect that to the main ground.

Power should be the first thing you lay out, then all lower current things can jump over it. I usually put my power traces on the solder side.

Try to stick to the rule of one side of the board for north south and one side for east west.

Keep all balanced lines close and the same length. Unbalanced things, put a ground trace on either side.

Trace impedances are not a problem in the audio bands, as long as you keep them thick... I usually have main power 50-100 mil wide, jump offs to ships, 25 mil, and general low current traces 10 mil. Outputs to and from output transformers, 25 mil.

When selecting a board, see if they will do 2 ounce copper for the same price. The thicker the better. When you order boards, get the higher temperature ones. TG135 is for normal lead solder, TG170 is for surface mount, I always order TG180. The TG stands for Glass Transition Temperature, and is measured in degrees C, and it's when the glass becomes unstable and can start to delaminate.

Breadboard first, then I, many times, make a larger board, with things grouped, so I can prototype it and have room for mods.

Keep all AC things .150" MIN away from everything, ground plane back-off from traces is usually 10 to 12 mil.

Mix, repeat, enjoy.

 

[JohnRoberts]

One thing I missed going from a small one man company to a larger place with dedicated pcb layout artists, was no longer doing my own PCB layouts. Almost every single trace or component placement has consequences that the design engineer understands while the layout engineer does not. I even recall back in the 70s where I would sometimes make minor circuit design changes to optimize a layout.
===
pAs are probably pico amps, common vias are probably "shared" vias where two different signal currents flow through the same via junction. or not..

JR

 

[Tubetec]

I'd like to pick up on what Fix said about transformer grounding , so bolting an input transformer to the deck ie chassis ground is unlikely to be satisfactory ? I can see why exactly now you have pointed it out , it wants its own discrete path ,not a series of loops to ground . Likewise in the well designed tube gear a smoothing cap has negative terminal and case up from chassis and its own dedicated ground link to precisely where it belongs in the circuit chain .

“Logic is the Beginning of wisdom, not the end of it.” Dr Spock

 

[Audio1Man]

Hi Bo
1. Shared via to ground plain or other connections are bad as it has 2 different currents and one shared path.
2. pa = pico amps, any small current can add noise into the path.
3. Watch for steel hardware near signal loops use alum or plastic.
4. Nothing is 100%, choose your best option.

 

[FIX]

Cutting the ground plane to break the loop caused by the transformer hole. This was a problem when I designed the original API 3124, I had hum in the 4th pre. Moving the transformers did nothing. Cutting that copper created a spark that actually made one of the other people their come into the room to see what the SNAP was. If you look at how a Weller solder gun works, it's the same. Lots of windings around a single loop. Creates enough current to heat up a thick copper tip.

 

[ruffrecords]

You should really do as FIX suggests even if you do not have a transformer cut out. Attached is a scan of the bottom side of my twin line amp PCB most of which is analogue 0V plane. On the far left is the 32 way connector that routes power and signals to and from the board. The bottom two pins of this connector are the system 0V. Above this are the output pins with their 0V connection closely tied to where 0V enters the board. To the right of the outputs are the two output tubes and to their right is the input tube with the two optional input transformers above. Notice the vertical cut in the 0V plane directly above the top output tube. To the left of this cut the 0V plane goes to the outputs. To the right of the cut it goes to the input transformers and then to the input tube and finaly to the output tubes. This more or less mimics the old RCA point to point 0V technique of using a single fat copper wire running the length of the chassis. I ideally the system 0V should be closer to the outputs and in later versions of this board the pin out has been changed to achieve this.

Cheers

Ian

 

[moamps]

...This more or less mimics the old RCA point to point 0V technique of using a single fat copper wire running the length of the chassis....

I think you should improve your PCB in the next revision . Three major errors are indicated here, and there are more places where the tracks could be better placed.

 

[TheJames]

Hey Moamps...Just curious...Do you think the heater EMI would be an issue with DC heaters?

 

[Script]

never leave the area around it connected in 360 degrees. You will pick up hum from power supplies, etc. (Eddy currents) Always cut an area out so it doesn't complete a loop.

Have a question -- related, maybe not (Have no experience with PCB design). Is not having ground plane 'connect in 360 degrees' not also good practise in any solid state design ?

Said differently : is it not better to have traces and planes branch out and go around components and ultimately around entire board but never let them form a full loop, not even around entire board ?

 

[ruffrecords]

I think you should improve your PCB in the next revision . Three major errors are indicated here, and there are more places where the tracks could be better placed.

There is a loop but not where you think it is. The two left hand tubes have 6V heaters and are connected in series. Also the heaters are dc which helps a lot. But you are right, it is not ideal and there are lots of areas where the the copper pour is not connected (which is a limitation of the CAD program I am using) and areas where the plane is not wide enough (but they are all in low signal level areas).

Cheers

Ian

View attachment 91467

 

[JohnRoberts]

Don't lose too much sleep over thinking this. I recall designs where it really mattered, like inside huge power amps with large magnetic fields generated by the power transformer. Another situation is inside low noise mic preamps.

JR

 

[moamps]

Do you think the heater EMI would be an issue with DC heaters?

Such loops should always be avoided, as in reality there is no pure DC source (it’s not even a battery). If I'm not mistaken, SMPS is used here to power the heater, and it's never perfect DC. In addition, such loops can represent an unexpected load (short turn) for the AC signals flowing through the loop.

 

[Matador]

There's a common saying in software engineering (paraphrasing): "Premature optimization is the root of all evil." I think there's a corollary with PCB layouts as well. Do the best you can, then test the performance and fix it if it isn't working. I've found at least 85% success rates with simple, fully-poured ground planes, in a variety of audio projects from mike preamps all the way to tube guitar power amps, powered from simple linear regulators or SMPS's.

However I've moved away from this as a practice to doing fully differential ground layouts, not because I've found them "better" from a noise point of view, but in that they allow for far less routing congestion because it's easier to use both sides of the board fully (with a system that has top traces running left to right/horizontally, and bottom traces running top to bottom/vertically).

 

[TheJames]

However I've moved away from this as a practice to doing fully differential ground layouts

Uhhhh.....Wut?

Got a link for more info or an example of what you mean? I totally understand east/west on one layer and north/south on the other, but "fully differential ground" is throwing me.

 

[PureBasic]

I would add this as this is a common EMI mistake:

 

[PureBasic]

It's wrong when one doesn't understand why to do it.

Yes ! The guideline is to avoid them unless strictly necessary, and not to preemptively put some.

There's a common saying in software engineering (paraphrasing): "Premature optimization is the root of all evil." I think there's a corollary with PCB layouts as well. Do the best you can, then test the performance and fix it if it isn't working. [...]

Well, software costs close to nothing to revise. I mean, you can modify, recompile, flash in a matter of minutes. There is a bit more skin in the game for a board. You can go up thousands for a simple revision.

85% success rates with simple, fully-poured ground planes

Yes ! Protect your signal and offer a golden return path.

The most important thing for signal integrity and EMI performance is the return path. Think about impedance instead of resistance. Your return path will follow the least impedance always.
At 50Hz (which is almost DC), the return current will flow along the least resistance path: straight across your ground.
In AC regime (1Mhz) it's not the same story. The current will flow along the least impedance path, meaning it will follow the signal trace.

So, in audio, if your trace is a U shape, the high frequency components of your signal will flow in a U shape in the ground plane while the basses are going straight across. Weird huh?

Okay, so, the effect is not that drastic at 20kHz compared to 1MHz, but if your board is not offering a return path close to the signal trace, you've made yourself an antenna and you will catch HF noise in your circuit. And an unexpected current flow in another part of the board could generate crosstalks, nonlinearities etc...

So, always keep in mind your return path and ask yourself where the current will flow.
That would be my best advice.

fully differential ground layouts.

Would love to see a layout or a layout snippet. Curious

 

[Bo Deadly]

Okay, so, the effect is not that drastic at 20kHz compared to 1MHz, but still, that's how you get crosstalk, nonlinearities, noise susceptibility... etc...

My understanding is that the effect you're describing occurs at relatively low frequencies like 1kHz. Fortunately the confluence of circumstances required to see a real issue with small signal audio designs is not common.

 

[PureBasic]

Lots of things can be improved here:

 

[PureBasic]

My understanding is that the effect you're describing occurs at relatively low frequencies like 1kHz. Fortunately the confluence of circumstances required to see a real issue with small signal audio designs is not common.

Exactly !
It's much more complicated with digital high speed signal. You can have GHz components for a signal that change state once a day because the state changes of modern semiconductor are so fast, you can go from 3.3V to 0V at the pin in a matter of pico-seconds. Got a loop in there? Well you just rebooted the computer next door, you know the one with RGB and a plexiglass panel.

On 4+ layer boards, when a signal goes from one layer to another we even put a ground via close to the signal via to offer an uninterrupted path.
Shield to ground connection for example. You have a 4 cm long trace to do this. Measured is 0.00001ohms. But at 20MHz it might be 40 ohms. 20MHz is your I2S bus bitrate? You're screwed! Won't pass EMI.

In the end it's mostly physics. The ohm law is really not enough to design good boards. You need to have some understanding of the EM fields. A lot comes from experience too, from which comes guidelines (because not everyone has the time to dig into this).

 

[PureBasic]

*triggered* x_x

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").

No, you need field theory too.

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.

We decouple locally to compensate for power trace impedance and to power digital state changes. Some components won't even start without close decoupling. Do you think digital board designers are stupid? We don't do that for nothing!

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.

We do that too when necessary. Resistors, self, chokes... We actually calculate our filters depending on what parasitic signal we expect to cross-feed from one part of the circuit to the other. It's tweaked on the first prototypes... We just don't put things on a board automatically because it apparently works. It takes a lot of attention to a **** ton of details to do a Gbps board that passes the EMC test.

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."

Yes, because teachers are scholar. They don't design ****, they just wire arduinos and make leds blink. You learn board design in books and on the field.

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.

One true thing I've seen in this post.

Just wanted to put the discussion in perspective ...

Thanks