Point to point star ground returns (Routing)

[Winston OBoogie]

'

I don't think that it's really needed in audio work but I do find that some of the things I've done in RF have fixed issues in the audio world where nothing else seemed to help.

Hey Svart,
I think it's great you have the knowledge and experience that some of us don't.  There will be solutions to things that are second nature to you but would be-fuddle me for hours.

I've only done a bit of stuff over audio.  Most of the guys I've spoken with who do do RF laugh when I tell 'em I do audio.  "So you basically just play with DC?"  is one I've heard 

When I'm working with stuff that has significant dumps, I treat them differently.  Digital doesn't touch my audio scheme.  And after one little mistake of mine that made it out in a commercial product, neither does my relay and driver logic.

Power amps: well I admit to only having built a few valve units and hand full of class "A"  minimal topology brutes. 


I would probably not use a switching supply myself for audio unless I had a boss that insisted I do.  Why, all of a sudden, would I want to be all efficient 'n' **** when I've just spent ages designing a power wasting hog of an amp?   I think switchers could probably be gotten away with for 'decent enough' audio with additional filtering and linear regs after them.  Shunt regs would probably be best as they would help more in elimination of the hi frequency.  But when I'm done, it probably might as well have been a linear supply, dunno?

Cheers,

John

 

[JohnRoberts]

John,
I, for one, enjoyed your analogy  ;D
May I ask if you are in favour of a planar approach for audio in PCB layout?
To continue with your theme, an albeit diluted reservoir at the treatment plant...

I can't recall the last time I did an audio frequency only PCB, surely more than 10 years ago...

When I was working at Peavey we only had single sided capability, in house (and cheap)  so not much opportunity for extra ground planes on analog stuff. That said the boss had figured out that you get more mileage from the etchant the less copper you remove, so he encouraged the PCB designers to leave lots of copper on the PCBs, I had to encourage the PCB designers to not turn sensitive traces into antennae.

On mixed technology boards I have used the extra layers to provide some extra shielding for sensitive circuitry, but care must be taken that your shield is actually quiet and not pumping noise back into the sensitive circuitry.

I recall working on one 4 layer design with DSP, codec, switching PS, and Low Z mic preamp on one PCB. Lots going on and the only way to sanely view ground was "relative to what?".  In that design,  that I inherited between 2nd and 3rd generation I was stuck with the switching supply physically located between the codec and DSP...  at least the mic pre was off in the corner...

To answer your question hypothetically... If I were purchasing a PCB today for an audio project, i suspect there is no cost savings (for less than massive mega  quantities) for single sided boards since the PCB house stocks 2 layer or more raw material, so I would use 2 sided and surely be tempted to use some extra shielding where appropriate.

Another trick which I haven't suitably explored is running traces as send/return pairs to play games with conductor loop area wrt magnetic fields et al. One nice unintended consequence of the SMT transition was to make layouts much tighter and cleaner from a noise pick up perspective.

One observation that may appeal to this group... for very small specialty audio companies the chief (only) designer, may also be laying out the PCB. Not only do you get a layout from somebody who understands what is going on, but i have been known to change the circuit design if it makes the layout work better. In the grand scheme of things a great layout of a mediocre design is less wonderful than a mediocre layout of a great circuit. Of course better both is always better. 


JR

 

[Svart]

"So you basically just play with DC?"

Oh you'd hear that a lot around my lab..  ;D

It's all physics and it all obeys the same laws but we have lots of fun giving the lowspeed guys hell!

On a more serious note, one common thing you'll see is the old school RF guys actually perpetuating the myth that RF is somehow black magic.  A lot of them have moved up and made lots of money through the years simply by this myth alone.  Somehow this escaped ME but I was given a stern "talking to" by one of those guys because I refused to play that game.  A couple of us have a habit of speaking in layman terms and explaining what we mean instead of simply throwing out buzzwords..  Anyway, that engineer got tired of the rest of us and left thankfully. 

for very small specialty audio companies the chief (only) designer, may also be laying out the PCB

I wish.

We have a PCB guy who does our layouts.  He has a control problem.  We'll draw something up for him with instructions for layout, links to demo board layouts, etc, but he won't follow them.  He doesn't have any formal design training, not that someone needs it to be good at anything, but he also doesn't WANT to learn any design technique.  We've offered numerous times to send him for classes/training but he refuses.  In the end, the layouts are strange and ultimately unusable and it takes us a bit of time to "help" him change things to suit the design.  Notice I mentioned he was a control freak..  He gets upset that we are changing anything and then complains the whole time he's changing stuff.  You have to babysit him just to get the thing done.  Management doesn't seem willing to do anything about it either.

Times like this, I would do my own layouts if they let me.

 

[Winston OBoogie]

Nice answer, thanks John.

To answer your question hypothetically... If I were purchasing a PCB today for an audio project, i suspect there is no cost savings (for less than massive mega  quantities) for single sided boards since the PCB house stocks 2 layer or more raw material, so I would use 2 sided and surely be tempted to use some extra shielding where appropriate.

Yes.  I do that.  I'm just not a fan of pouring the ground over everything. 
Sometimes my supply rails might be on top and will run along a power return below.  I rarely do the calculations (although they're not hard - I'm just being lazy!) but, in this case, I'm looking/hoping to pick up a bit of the dialectric properties and aid in some bypassing of the rails.

I actually like the challenge of a single-sided board.  I frequently order them that way even though the cost is the same as a 2 sider.
I do it as a game and take points off if I have to resort to a jumper:  I won't stop for a cigarette break until I've re-arranged things or, I get to goof off and watch TV for an hour if I get it right! 
Of course, my holes are plated through so it's not strictly single-sided.  I also sometimes use the other side as a permanent silk-screen, so to speak.  My markings/symbols/dedications etc. are in plated copper. 

I digress...

...the chief (only) designer, may also be laying out the PCB. Not only do you get a layout from somebody who understands what is going on, but i have been known to change the circuit design if it makes the layout work better.

  I do that too.  I don't think I've ever imported the netlist from a CAD schematic, much to the dismay of some former department heads!  Besides, rats nests give me a headache and borderline seizures. 
By the time I'm laying it out, I usually know the circuit well enough that I could probably argue the finer points while undergoing a root canal.

Cheers,

John.

 

[Winston OBoogie]

"So you basically just play with DC?"

Oh you'd hear that a lot around my lab..   ;D

It's all physics and it all obeys the same laws but we have lots of fun giving the lowspeed guys hell!

;D

I daresay I'll be needing to pick your brain should I ever move up the ladder.

Cheers Svart,

John

 

[jdbakker]

[...] i have been known to change the circuit design if it makes the layout work better. [...]

+1.

Can't remember the last non-trivial design where I didn't do that. CAD packages without back-annotation are pretty much useless to me. This is especially useful when doing digital stuff, on FPGAs, CPLDs and microcontrollers where switching I/O pins around can lead to a much simpler (and quieter) layout.

On ground planes and audio: I do use them quite a bit, but not indiscriminately. Always ask myself (or the simulator) what Mr. Maxwell would say. Subsystem placement is critical, proper local regulator ground sensing helps a lot, and power ground isn't the same as signal ground. Ground-follows-signal practices keep things nice and quiet, albeit at the expense of a few extra resistors for proper ground sensing between stages.

As for the original poster: What PRR said. If you can separate signal ground from power ground it helps to do so, otherwise a big fat ground bus (and short wires!) can work well enough for DIY.

JDB.
[Svart: has anyone pointed out that your layout guy isn't exactly maximizing shareholder value?]

 

[dmills]

These days a scary amount of 'Audio' circuitry needs to be treated as at least being likely to be carrying significant RF, and appropriate measures should IMHO be taken (Even purely analogue stages tend to need some help with immunity from cell phones and other RF sources).

I am working an a ADC board at the moment, where the input RFI protection network has a ground plane bonded to the chassis (RF bypass caps connect to this), but where the rest of the circuit shares a large common plane (layer 2).

Certainly any ADC or DAC should be treated as mixed signal if not outright as an RF circuit (Note that the currents flowing between the cap at the adc inputs and the chip are most certainly RF for example).  One saving grace is that given a continuous ground plane, RF return currents will flow directly under the trace that carries them out! You do not need to force this, it just works by Magic (Physics).

For anything mixed signal, I am a fan of a single continuous ground plane, resistance is not the enemy, inductance is! Star grounding does not work when the loop currents are 24MHz square(ish) waves!  Further, there is a lot of rubbish talked about the correct way to ground ADC and DAC chips, BOTH AGND and DGND should connect to a single ground plane (The reason for the separate pins is bond lead inductance, not a desire for separate ground plains).

So, sorry but I like solid ground plains and extensively flooded power plains (the distributed capacitance to the ground plain if you put them on opposite sides of a thin prepreg is useful).
 
Now I will grant that those using vacuum fets are operating in a very different impedance regime then my fast clocks and low impedance transmission lines territory, but it might be worthwhile reading up on some of the techniques the instrumentation guys have developed to deal with high impedance low level signals..... You think a cap mic is unfriendly, try a helium 3 neutron detector (~2KV bias, Gohm impedance, 100ns events, sometimes within feet of a 100KV power line).    

 

[Winston OBoogie]

it might be worthwhile reading up on some of the techniques the instrumentation guys have developed to deal with high impedance low level signals...

Two I have read:

Grounding and Shielding Techniques - Ralph Morrison

High Speed Digital Design: A Handbook of Black Magic - Howard Johnson and Martin Graham

Are there others you recommend?

Thanks 

 

[JohnRoberts]

We have a PCB guy who does our layouts.  He has a control problem.  We'll draw something up for him with instructions for layout, links to demo board layouts, etc, but he won't follow them.  He doesn't have any formal design training, not that someone needs it to be good at anything, but he also doesn't WANT to learn any design technique.  We've offered numerous times to send him for classes/training but he refuses.  In the end, the layouts are strange and ultimately unusable and it takes us a bit of time to "help" him change things to suit the design.  Notice I mentioned he was a control freak..  He gets upset that we are changing anything and then complains the whole time he's changing stuff.  You have to babysit him just to get the thing done.  Management doesn't seem willing to do anything about it either.

Times like this, I would do my own layouts if they let me.

In my experience good layout guys will want to improve their performance and accept guidance. If not there may be some perverse incentive where he benefits from do-overs, or maybe he is just a square peg that must be hammered into the round hole.. I recall working with one designer who was convinced a layout couldn't be done. Of course this is a self fulfilling prophecy if he is the one doing it... he was finally led to a workable solution but that is the price we pay in larger organizations for delegating work. The good news is we should be able to get more accomplished and have more consistent output by specializing.

I am back to laying out my own stuff and my main complaint about me as a PCB layout guy is I spend too much time tweaking the layout.

JR

 

[PRR]

> I am in favor of over thinking

So am I; but the topic is riddled with subtle points, takes a LOT of thinking. In my slow-witted experience, decades.

> I think of grounds like a sewer pipe...

I've used that analogy. Both for grounds and for HIGH-voltage output leads dripping into input stages.

> have to remember that "RF" is never just RF.  It's really mixed signal.

Sure. But it is the >1MHz <100r stuff that kicks your butt.

 

[Svart]

has anyone pointed out that your layout guy isn't exactly maximizing shareholder value?

yep.  He's an older guy and as much grief as he gives us about layouts, he is a pretty nice guy otherwise.  It turns out that he headed a CAD department for a decade+ in the days of actual blueprints.  One of the engineers has worked with him before during that time period and has said that he just can't seem to let go of those "good ole days" when he controlled everything.

That being said, yes management knows that we could get someone else with more initiative and we've voiced complaints about his work ethic but they just don't do anything.

I think the board of directors has heard our complaints too but so far they haven't said anything either.

High Speed Digital Design: A Handbook of Black Magic - Howard Johnson and Martin Graham

That Howard Johnson book is like the Bible around my job.  One of the engineers actually worked at a place who paid to have HJ to come in and consult.  For 5K-15K$ a day..  But he solved a problem they couldn't solve in 3 months and he did it in 3 days.  He learned a lot and now he's the primary engineer for high speed digital (and he's younger than me...  ???  ).

Sure. But it is the >1MHz <100r stuff that kicks your butt.

If it's narrow band RF then not so much.  If it's wideband RF then yes yes yes yes yes, your ass will be sore from all the kicking!  It's the frequency tilt and phase noise that really hurts.  Both can really be affected by layouts and not just by being routed near something noisy.  Simply having specified impedance traces that are calculated incorrectly or simply going through a via to another layer can really hurt your signal integrity if you don't account for it.  Simply having a ground trace too long and skinny can do this on passive filters but then in something like a PLL you might actually want your digital ground trace to be long and skinny so that the added impedance helps keep the digital ground hash from getting back into the analog ground traces near it.  It's extremely tricky and unless you have an expensive 3d field solving program, you pretty much have to go with gut feelings and lab experiments.

These days a scary amount of 'Audio' circuitry needs to be treated as at least being likely to be carrying significant RF, and appropriate measures should IMHO be taken (Even purely analogue stages tend to need some help with immunity from cell phones and other RF sources).

I am working an a ADC board at the moment, where the input RFI protection network has a ground plane bonded to the chassis (RF bypass caps connect to this), but where the rest of the circuit shares a large common plane (layer 2).

Certainly any ADC or DAC should be treated as mixed signal if not outright as an RF circuit (Note that the currents flowing between the cap at the adc inputs and the chip are most certainly RF for example).  One saving grace is that given a continuous ground plane, RF return currents will flow directly under the trace that carries them out! You do not need to force this, it just works by Magic (Physics).

For anything mixed signal, I am a fan of a single continuous ground plane, resistance is not the enemy, inductance is! Star grounding does not work when the loop currents are 24MHz square(ish) waves!  Further, there is a lot of rubbish talked about the correct way to ground ADC and DAC chips, BOTH AGND and DGND should connect to a single ground plane (The reason for the separate pins is bond lead inductance, not a desire for separate ground plains).

So, sorry but I like solid ground plains and extensively flooded power plains (the distributed capacitance to the ground plain if you put them on opposite sides of a thin prepreg is useful).
 
Now I will grant that those using vacuum fets are operating in a very different impedance regime then my fast clocks and low impedance transmission lines territory, but it might be worthwhile reading up on some of the techniques the instrumentation guys have developed to deal with high impedance low level signals..... You think a cap mic is unfriendly, try a helium 3 neutron detector (~2KV bias, Gohm impedance, 100ns events, sometimes within feet of a 100KV power line).    

You got it.  Glad you are on my side..   ;D

 

[Andy Peters]

Further, there is a lot of rubbish talked about the correct way to ground ADC and DAC chips, BOTH AGND and DGND should connect to a single ground plane (The reason for the separate pins is bond lead inductance, not a desire for separate ground plains).

I am amazed that converter manufacturers have app notes and reference designs for new devices that recommend separate analog and digital grounds. The data sheets say, "join analog and digital ground at one point, underneath the converter." Inevitably, one has to ask, "So what do we do when we have more than one converter in a design?"

Anyways, put me in with the guys who do a single ground while paying attention to routing and return currents.

I suppose I should say that at the day job, we are not overly cost-constrained so that if a board needs eight layers, it gets eight layers (four routing layers, ground planes on 2 and 7, power on 4, ground on 5). So if you need four routing layers, you get better signal integrity with this stack-up rather than trying to save a buck or three by sticking with six layers (ground plane on 3, power on 4). When a signal needs to jump layers, keep it adjacent to the same ground: jump between 1 and 3, or 6 and 8, unless it is absolutely necessary to do otherwise.

-a

 

[Andy Peters]

I don't think I've ever imported the netlist from a CAD schematic, much to the dismay of some former department heads!  Besides, rats nests give me a headache and borderline seizures. 

I cannot imagine NOT importing a netlist from a proper schematic capture program! Though I suppose my world is BGA-packaged FPGAs and memory and very fast image sensor data interfaces. Lots of parts, lots of signals, not a lot of board space.

By the time I'm laying it out, I usually know the circuit well enough that I could probably argue the finer points while undergoing a root canal.

As the design engineer, I have to know the circuit well enough to communicate with my layout person how things should be routed: which buses need to have matched lengths, which nets are sensitive (fast clocks, etc) and which are static or slow, what gates can be swapped, and all of that. And with FPGAs, it can get hairy, as some pins can be swapped without problem, some cannot be swapped at all, some signals have to be on special clock pins, some pins are input-only, some pins/pin-pairs do not have internal LVDS termination, and so forth. Oh, and mind your bank I/O voltages -- don't put that 3.3V signal onto a 2.5V bank!

(You might read the marketing crap that talks about how you can "decrease time to market by doing the FPGA design in parallel with the PCB layout," but you have to be somewhat crazy to believe that. As a general rule, before we release a PCB to fab, we run the FPGA tools on the design so that we are sure that no signals are put on impossible pins. This means that you need a decent amount of your design complete before you build the board.)

-a

 

[Winston OBoogie]

I cannot imagine NOT importing a netlist from a proper schematic capture program! Though I suppose my world is BGA-packaged FPGAs and memory and very fast image sensor data interfaces. Lots of parts, lots of signals, not a lot of board space.

Hi Andy,
Yep.  I don't doubt I would have to do it that way if I had your job.  What I do might be considered child's play in comparison?

My design is usually 90% done and a prototypical is working on the bench.  I've usually made a preliminary CAD schem. but that gets printed out and is usually penciled with notes detailing loops, important nodes etc. by the time I start the layout. 
Invariably, I might come up with an idea while plonked in front of the screen.  It might be a way to simplify matters or could be something that I hadn't thought of before. 
I see the layout as a part of the design process and, psychologically, I start to feel locked in and less creative if I'm moving or changing nets around or having to make back changes to the capture program.
I like being able to make quick changes on the proto build, see what happens and, if it works, make a note on the schem and alter the layout without having switch brain sides and go into data management mode.

Thanks for the post and insights,

John.

 

[Winston OBoogie]

I suppose I should say that at the day job, we are not overly cost-constrained so that if a board needs eight layers, it gets eight layers (four routing layers, ground planes on 2 and 7, power on 4, ground on 5). So if you need four routing layers, you get better signal integrity with this stack-up rather than trying to save a buck or three by sticking with six layers (ground plane on 3, power on 4). When a signal needs to jump layers, keep it adjacent to the same ground: jump between 1 and 3, or 6 and 8, unless it is absolutely necessary to do otherwise.

Well that's a bit different.  My complaint was with the audio guys that have signal traces on both sides of a two layer board and pour copper within 20 mils of all traces as the signal and power return/ground 'planes' with a few via's here and there to link both sides up.

AD and DA converters: I've only been involved in two.  One I didn't do the layout for and the other was a DA with a hefty valve line driver. I did it two layer and the H.T., L.T. and AC returns were separate from digital.  It did work as hoped... 

 

[Winston OBoogie]

I missed this:

If your output is via a transformer, and there are no intermediate in/out taps, then there is no strong reason to have your amplifier ground bus tied to chassis. Many rack-amps have been built with all internal circuitry floating from chassis. A link allows the guts to be tied to chassis for simple systems, or floated and tied to an isolated studio ground bus for more complex systems.

To be clear to the OP, you are advocating either linking amplifier ground to chassis at the source device or taking it externally to a technical studio ground bus.  Taking it external is part of what is called "transmission grounding". 
To leave it floating is not recommended. 

 

[JohnRoberts]

Further, there is a lot of rubbish talked about the correct way to ground ADC and DAC chips, BOTH AGND and DGND should connect to a single ground plane (The reason for the separate pins is bond lead inductance, not a desire for separate ground plains).

I am amazed that converter manufacturers have app notes and reference designs for new devices that recommend separate analog and digital grounds. The data sheets say, "join analog and digital ground at one point, underneath the converter." Inevitably, one has to ask, "So what do we do when we have more than one converter in a design?"

Anyways, put me in with the guys who do a single ground while paying attention to routing and return currents.

-a

The one DSP that I had to support was laid out for a CODEC and a higher performance A/D but luckily for me I didn't have to get the A/D working during my tenure.. At least the two chips were right next to each other, but no way could both AGNDs be the same.

Yes it is logical that AGND and DGND are bonded at the CODEC. Analog ground needs to telescope out from there to the rest of the analog world. I have experienced (heard) quite a bit of difference in how that simple ground connection is made at the codec, multiple DGND pins with different amounts and kinds of sewage.

JR

 

[Svart]

We are using 125 and 250msps ADCs in our design.  The digital guys use a single plane and use trace inductance as I mentioned before to get an amount of isolation between the dgnd and agnd pins.  

I am amazed that converter manufacturers have app notes and reference designs for new devices that recommend separate analog and digital grounds. The data sheets say, "join analog and digital ground at one point, underneath the converter." Inevitably, one has to ask, "So what do we do when we have more than one converter in a design?"

A lot of these app notes/datasheets were written many years ago and the usage information tends to just be recycled since.  Otherwise, the datasheet guys are being extremely careful and telling you to use their part in a way that would cause you less grief.  In high speed sampling, that discontinuity in the ground plane will show up as a signal integrity problem, mostly caused by a change in inductance of the return path.  Our high speed guys would punch anyone who did that at our site right in the junk.

This discussion is pretty cool, we pretty much have all of the heavy weights in here.

 

[Winston OBoogie]

Further, there is a lot of rubbish talked about the correct way to ground ADC and DAC chips, BOTH AGND and DGND should connect to a single ground plane (The reason for the separate pins is bond lead inductance, not a desire for separate ground plains).

I am amazed that converter manufacturers have app notes and reference designs for new devices that recommend separate analog and digital grounds. The data sheets say, "join analog and digital ground at one point, underneath the converter." Inevitably, one has to ask, "So what do we do when we have more than one converter in a design?"

At least a few books say otherwise when dealing with AD/DA.  Although it didn't work for my tube hog DA... from "Grounding And Shielding Techniques" I referenced above:

"The best solution for interfacing analog and digital functions is to use a common unbroken ground plane. It is important to make sure that the fields associated with analog and digital functions do not share the same physical space. The following six rules apply:

1.  Analog circuit components must not be intermixed with digital circuit components.
2.  Make sure that the analog fi elds do not share the same physical space as the digital fi elds.
3.  The pin assignments in connectors should separate function so that the analog fields and digital fields are separated.
4.  The A/D converter should have an internal forward referencing amplifier.
5. Orient the A/D converter to limit field coupling.
6. The circuits should pull energy from different decoupling capacitors."


Edit: Quote typo's fixed

 

[JohnRoberts]

Further, there is a lot of rubbish talked about the correct way to ground ADC and DAC chips, BOTH AGND and DGND should connect to a single ground plane (The reason for the separate pins is bond lead inductance, not a desire for separate ground plains).

I am amazed that converter manufacturers have app notes and reference designs for new devices that recommend separate analog and digital grounds. The data sheets say, "join analog and digital ground at one point, underneath the converter." Inevitably, one has to ask, "So what do we do when we have more than one converter in a design?"

At least a few books say otherwise when dealing with AD/DA.  Although it didn't work for my tube hog DA... from "Grounding And Shielding Techniques" I referenced above:

"The best solution for interfacing analog and digital functions is to use a common unbroken ground plane. It is important to make sure that the fields associated with analog and digital functions do not share the same physical space. The following six rules apply:

1.  Analog circuit components must not be intermixed with digital circuit components.
2.  Make sure that the analog fi elds do not share the same physical space as the digital fi elds.
3.  The pin assignments in connectors should separate function so that the analog fields and digital fields are separated.
4.  The A/D converter should have an internal forward referencing amplifier.
5. Orient the A/D converter to limit field coupling.
6. The circuits should pull energy from different decoupling capacitors."


Edit: Quote typo's fixed

My limited experience agrees with Andy.

Some of those suggestions sound odd to impractical..  but if it's in a book it must be right. 

JR