I am following this thread with great interest and am looking forward to see the different layouts from marce (probably in the other thread).
I am just starting a new design for an ADC and would like to hear opinions about the best layer stackup (4 layer board). From EMC perspective i've read GND SIG Power GND may be good but i am wondering about quite a lot interrupts in the top GND layer due to component pins. So question is whats a good stackup for ADC or DAC?
I am just starting a new design for an ADC and would like to hear opinions about the best layer stackup (4 layer board). From EMC perspective i've read GND SIG Power GND may be good but i am wondering about quite a lot interrupts in the top GND layer due to component pins. So question is whats a good stackup for ADC or DAC?
You want a contiguous ground plane, so I would opt for the traditional and well tested 4 layer basic of:
Top Components and signals
2nd GND unbroken especially where digital signals run over it.
3rd Power as above
Bottom Signals
Both the top and bottom layer can have copper pours to GND, with plenty of stitching via's.
Further, depending on your manufacturer we use a 1mm spaced laminate for the central power core, with 0.3mm pre-pregs between the top (and bottom) layer and the central double sided laminate. This allows for some impedance control if you want for your routes.
This is pretty much a standard 4 layer build and looking at the recent 4 layer boards we have done this covers 99.9% of them. In fact I am just doing one now, as I am on the train commuting to sonny Harrow again.
On a recent thread there was some debate over the decoupling of a ES dac, for both this thread and to promote debate on that thread I am hoping to do a couple of layouts showing different decoupling schemes, for discussion, hopefully in the next couple of days. At the moment my time is limited as I spend my weekend travelling back and forth, Harrow - Blackburn, so if I am quite it is due to lack of internet access at the hotel or travelling!
Top Components and signals
2nd GND unbroken especially where digital signals run over it.
3rd Power as above
Bottom Signals
Both the top and bottom layer can have copper pours to GND, with plenty of stitching via's.
Further, depending on your manufacturer we use a 1mm spaced laminate for the central power core, with 0.3mm pre-pregs between the top (and bottom) layer and the central double sided laminate. This allows for some impedance control if you want for your routes.
This is pretty much a standard 4 layer build and looking at the recent 4 layer boards we have done this covers 99.9% of them. In fact I am just doing one now, as I am on the train commuting to sonny Harrow again.
On a recent thread there was some debate over the decoupling of a ES dac, for both this thread and to promote debate on that thread I am hoping to do a couple of layouts showing different decoupling schemes, for discussion, hopefully in the next couple of days. At the moment my time is limited as I spend my weekend travelling back and forth, Harrow - Blackburn, so if I am quite it is due to lack of internet access at the hotel or travelling!
You're probably right. However whats the implication? Should we stop our discussion?
@marce: thank you very much! I am looking forward to seeing and discussing the decoupling schemes
I dont know, since the normal mechanisms that might stop such crap from happening dont seem to exist anymore. it seems all you can do is either design it in such a way that its not cheap, or easy to replicate, or dont share anything at all. I just dont see that they deserve any help, given there is already a clear cost of manufacture advantage. it really makes such conversations difficult, since many openly discussed designs seem to find their way to the internet, sometimes even before the real deal.
Last edited:
Didn't know where to write about this, but seems this thread would be good.
I would like to ask your opinion on the benefits of through hole pads, versus a regular single-sided pcb, for audio applications of course.
I want to order some pcb's, and I need only one layer of copper, where all soldering will be placed. So, I only need pads on the solder side.
But I have read that making these pads through hole (which means that they get through the FR4 and reach the component side) is a more robust design.
I hope I am making this clear, so is this actually beneficial?
I would like to ask your opinion on the benefits of through hole pads, versus a regular single-sided pcb, for audio applications of course.
I want to order some pcb's, and I need only one layer of copper, where all soldering will be placed. So, I only need pads on the solder side.
But I have read that making these pads through hole (which means that they get through the FR4 and reach the component side) is a more robust design.
I hope I am making this clear, so is this actually beneficial?
Thanks for the quick answer! The pads will have 1.8-3.0mm diameter, and hole sizes from 0.65mm-1.2mm (obviously the 1.8mm will have a 0.65mm hole), so I think they should be already "big" enough.
But I plan to order them from seeed, and I can't say I know how to order a single sided pcb with silkscreen on the component side. So I will post my relevant question here, not to be off-topic.
But I plan to order them from seeed, and I can't say I know how to order a single sided pcb with silkscreen on the component side. So I will post my relevant question here, not to be off-topic.
If the 3mm holes are for mounting or putting any 3mm screw/bolt through make them at least 3.2mm or 3.5mm, use this chart as a guide for these holes.
technical data from draughtsman.co.uk
technical data from draughtsman.co.uk
Yes, with a bit of practice you'll soon get good solder joints, the solder will flow up the hole.
Some info:
http://www.dynamixtechnology.com/docs/drm-pth-d.pdf
Some info:
http://www.dynamixtechnology.com/docs/drm-pth-d.pdf
Not really much different. The PTH may take a little more heat (slightly longer contact time between the soldering iron tip, and the joint being soldered) due to the slightly larger thermal mass but the difference, if any, is just barely perceptible. It can be actually easier to consistently make good, reliable solder joints with PTH: Touch the iron to the joint on one side of the PWB, and feed the solder from the other side. When the joint has heated through to flow the solder, you know the solder will flow through the hole and adhere to the pads on both sides of the PWB.
Dale
Well I guess I am an audio PCB Pro these days as I spend far too much time in DX and Pads (Come back Altium all is forgiven!) for all that I am not in the class of say Marce, doing mostly medium speed mixed signal.
Lets assume an ADC as an example, lets see:
First set up the board outline and turn DRC (Ideally online DRC) up to stun with some fairly conservative rules set (No point in doing 0.15 T/G if you can avoid it), you can always ease it down a little later if you must.
Part 1: It all starts with component placement...
If you get the placement right the board practically routes itself (And this stays true all the way to at least 10 layers), get it wrong and you will have nothing but pain.
Now getting it right is highly context dependent but generally comes down to minimising loop areas keeping fast edges away from mV level audio and trying to arrange things such that the signal flow is sane (Also so the thermal load is reasonably spread around).
Start with the connectors, generally some of these at least are constrained by metalwork, but ideally you want all the connectors on one edge of the board (Make this your RFI hot zone) where all your RFI and transient protection can connect to a stiff common connection to chassis ground (Stiff in this context means multiple points).
Ideally there should be common mode chokes or ferrite in all circuits crossing out of this hot zone, there are some very good 1206 sized common mode parts for signal lines from the likes of Wurth.
Decide on mounting holes at this point, some in that RFI hot zone are useful as additional ways to tie it to chassis, do make sure the annular rings are sized for whatever washers and screws you use (Embarassing this one), M3 needs somewhere around a 3.2mm hole and a 6mm or so annular ring, check your mechanical tolerences and do the sums.
The corners of the board (Particularly the ones opposite the connectors) are valuable real estate as there will be nothing much in terms of agressor currents flowing in the ground planes in these areas (There shouldn't be anyway, but...), think clock generators and ADC/DAC parts here.
One of the best bits of mixed signal advice I saw went something along the lines of 'Design your board with a split groundplane between analogue and digital, have no tracks cross the split, then after you are done routing, remove the split!', solid planes really are better most of the time.
Routing
Now in my designs after the RFI and transient protection we typically come to the differential to single ended stages, decouple the power rails well (see notes on decoupling later), and consider carefully what you do with the single ended 'reference', connecting it to ground here may be reasonable, but sometimes there are smarter options.
Note that the balance in terms of both component tolerence and layout is **IMPORTANT** up to this point if you want the latest line recevers to be able to do as well as they spec, in particular T networks with low values to ground beat simple caps to ground for RFI as the low value to ground reduces the line imbalance due to the tolerence on the caps to the lines.
There can be something to be said for starting with the really critical signals either from a susceptibility or agression point of view, and in the digital bits I often do (High speed LVDS, Clocks, DDR2, Matched lengths, all that sort of pain), but for the analogue sections it is usually easy to deal with any of this stuff as it comes up.
Signal processing in the analogue domain is usually best kept single ended, and well decoupled, on that subject do not make all the decoupling too evenly spaced around the board, scatter a few parts around at irregular spacings to break up any resonances in the planes (Mainly an issue in high speed bits like around DSP parts, A small series resistor and a small tant or modern elco is good for this, I don't like tants directly across power rails), and have a good look at the ground plane at the end of the job to make sure it is basically continious, I don't do star earthing (Sacrelige, burn him!).
Remember that line recever reference I mentioned earlier? Well you might want to track it to somewhere in this region and pin it to the ground plane either here or at the ADC, that way you pick up a reference from the ground plane at one point and dont have general low frequency currents flowing in this connection (If you do this then this trace should be really butch).
Next we reach the ADC driver (A single ended to differential conversion with DC shift), this looks superficially like a simple opamp circuit set up to drive a few nF of cap, but is actually an RF circuit, and as such is worth a little discussion.
Firstly, anywhere you want to isolate HF noise from the power supply, soft ferrite beads (Wurth again) and caps (Including, but not limited to a tant or low esr elco with my usual series resistor of an ohm or so) are useful, so add such a network in the supply rails to this opamp to keep ADC switching noise out of the opamp supply to the low frequency stages.
That output cap wants to be as close as possible to the AD converter, 3 inches away on skinny traces will not do it (And SMT film walks all over some enormous film and foil horror here).
The loop between the ADC pins and this cap carries fast pulses and measures should be taken to minimise loop area (Always a good refrain in PCB layout).
A solid ground plane under this lot is very helpful, but that does not mean you have to be hard of thinking in how and where you connect to it. Sometimes for example there is an ADC_Ref pin or such that clearly needs to go to ground, but there is also a couple of reference decoupling caps that need to be returned to ADC_Ref not the local ground plane, just because they are the same net does not always make a via the right thing to do, it does not take much to introduce a 1uV error (-120dB ref 1V signal). Here a careful reading of the datasheet can pay dividends.
ADCs usually do better in slave mode (Not driving so many outputs), but any outputs they do drive should have a very local resistor (a few tens of ohms is typical) and should be buffered if being sent across the board.
These days I consider life too short for single layer designs and it does NOT take much to convince me to move to 4 layers (That buried ground plane is a great thing), this is reasonably cost effective these days even for prototype quantities.
Decoupling Part 1
Smaller parts are generally better when decoupling, 0402 trumps 0603 trumps 0805 stomps all over anything thru hole, but it only does it if you get it near the pin it needs to decouple.
Modern electrolyics are not the horror show they were in the 80s, good quality parts for Panasonic or Cornell Dubillier are in my view entirely acceptable for power decoupling and are often lower ESR then tants (as well as being less likely to spontaniously decide to go short and explode in a direct connection across the power lines, and cheaper), use 105 degree parts.
I will do some discussion of the digital side of a mixed signal board another night.
Summary:
IO along one edge.
EMC Hot zone direct to chassis.
Loop areas.
Parts placement is everything.
Don't split the ground plane (In general).
Corners equals quiet (often).
Ferrite is a good and happymaking thing.
Loop areas (Said it again).
Loops often involve the nearest decoupling cap, worth remembering.
More ferrite is sometimes just enough.
Loop Areas (And again, this matters).
Regards, Dan.
Lets assume an ADC as an example, lets see:
First set up the board outline and turn DRC (Ideally online DRC) up to stun with some fairly conservative rules set (No point in doing 0.15 T/G if you can avoid it), you can always ease it down a little later if you must.
Part 1: It all starts with component placement...
If you get the placement right the board practically routes itself (And this stays true all the way to at least 10 layers), get it wrong and you will have nothing but pain.
Now getting it right is highly context dependent but generally comes down to minimising loop areas keeping fast edges away from mV level audio and trying to arrange things such that the signal flow is sane (Also so the thermal load is reasonably spread around).
Start with the connectors, generally some of these at least are constrained by metalwork, but ideally you want all the connectors on one edge of the board (Make this your RFI hot zone) where all your RFI and transient protection can connect to a stiff common connection to chassis ground (Stiff in this context means multiple points).
Ideally there should be common mode chokes or ferrite in all circuits crossing out of this hot zone, there are some very good 1206 sized common mode parts for signal lines from the likes of Wurth.
Decide on mounting holes at this point, some in that RFI hot zone are useful as additional ways to tie it to chassis, do make sure the annular rings are sized for whatever washers and screws you use (Embarassing this one), M3 needs somewhere around a 3.2mm hole and a 6mm or so annular ring, check your mechanical tolerences and do the sums.
The corners of the board (Particularly the ones opposite the connectors) are valuable real estate as there will be nothing much in terms of agressor currents flowing in the ground planes in these areas (There shouldn't be anyway, but...), think clock generators and ADC/DAC parts here.
One of the best bits of mixed signal advice I saw went something along the lines of 'Design your board with a split groundplane between analogue and digital, have no tracks cross the split, then after you are done routing, remove the split!', solid planes really are better most of the time.
Routing
Now in my designs after the RFI and transient protection we typically come to the differential to single ended stages, decouple the power rails well (see notes on decoupling later), and consider carefully what you do with the single ended 'reference', connecting it to ground here may be reasonable, but sometimes there are smarter options.
Note that the balance in terms of both component tolerence and layout is **IMPORTANT** up to this point if you want the latest line recevers to be able to do as well as they spec, in particular T networks with low values to ground beat simple caps to ground for RFI as the low value to ground reduces the line imbalance due to the tolerence on the caps to the lines.
There can be something to be said for starting with the really critical signals either from a susceptibility or agression point of view, and in the digital bits I often do (High speed LVDS, Clocks, DDR2, Matched lengths, all that sort of pain), but for the analogue sections it is usually easy to deal with any of this stuff as it comes up.
Signal processing in the analogue domain is usually best kept single ended, and well decoupled, on that subject do not make all the decoupling too evenly spaced around the board, scatter a few parts around at irregular spacings to break up any resonances in the planes (Mainly an issue in high speed bits like around DSP parts, A small series resistor and a small tant or modern elco is good for this, I don't like tants directly across power rails), and have a good look at the ground plane at the end of the job to make sure it is basically continious, I don't do star earthing (Sacrelige, burn him!).
Remember that line recever reference I mentioned earlier? Well you might want to track it to somewhere in this region and pin it to the ground plane either here or at the ADC, that way you pick up a reference from the ground plane at one point and dont have general low frequency currents flowing in this connection (If you do this then this trace should be really butch).
Next we reach the ADC driver (A single ended to differential conversion with DC shift), this looks superficially like a simple opamp circuit set up to drive a few nF of cap, but is actually an RF circuit, and as such is worth a little discussion.
Firstly, anywhere you want to isolate HF noise from the power supply, soft ferrite beads (Wurth again) and caps (Including, but not limited to a tant or low esr elco with my usual series resistor of an ohm or so) are useful, so add such a network in the supply rails to this opamp to keep ADC switching noise out of the opamp supply to the low frequency stages.
That output cap wants to be as close as possible to the AD converter, 3 inches away on skinny traces will not do it (And SMT film walks all over some enormous film and foil horror here).
The loop between the ADC pins and this cap carries fast pulses and measures should be taken to minimise loop area (Always a good refrain in PCB layout).
A solid ground plane under this lot is very helpful, but that does not mean you have to be hard of thinking in how and where you connect to it. Sometimes for example there is an ADC_Ref pin or such that clearly needs to go to ground, but there is also a couple of reference decoupling caps that need to be returned to ADC_Ref not the local ground plane, just because they are the same net does not always make a via the right thing to do, it does not take much to introduce a 1uV error (-120dB ref 1V signal). Here a careful reading of the datasheet can pay dividends.
ADCs usually do better in slave mode (Not driving so many outputs), but any outputs they do drive should have a very local resistor (a few tens of ohms is typical) and should be buffered if being sent across the board.
These days I consider life too short for single layer designs and it does NOT take much to convince me to move to 4 layers (That buried ground plane is a great thing), this is reasonably cost effective these days even for prototype quantities.
Decoupling Part 1
Smaller parts are generally better when decoupling, 0402 trumps 0603 trumps 0805 stomps all over anything thru hole, but it only does it if you get it near the pin it needs to decouple.
Modern electrolyics are not the horror show they were in the 80s, good quality parts for Panasonic or Cornell Dubillier are in my view entirely acceptable for power decoupling and are often lower ESR then tants (as well as being less likely to spontaniously decide to go short and explode in a direct connection across the power lines, and cheaper), use 105 degree parts.
I will do some discussion of the digital side of a mixed signal board another night.
Summary:
IO along one edge.
EMC Hot zone direct to chassis.
Loop areas.
Parts placement is everything.
Don't split the ground plane (In general).
Corners equals quiet (often).
Ferrite is a good and happymaking thing.
Loop areas (Said it again).
Loops often involve the nearest decoupling cap, worth remembering.
More ferrite is sometimes just enough.
Loop Areas (And again, this matters).
Regards, Dan.
asprinv.
It's late, and I want to do this topic justice, so I'll mull over it and write a long writeup, a paper so to speak, for you and whoever else is interested.
I am qualified to speak to this matter.
I am an electrical engineer, with a graduate degree in electromagnetics (the discipline most conducive to printed circuit board technology) over two decades of experience, and the top recognized subject matter expert in printed circuit board physics at my company, which is a multinational commercial, industrial, and military electronics giant. I have published multiple technical papers on noise, have developed a novel, proprietary PCB routing technique for integrating ultra-high speed baseband controller circuits into super-sensitive RF transceiver sets, I give lectures on the subject and teach classes on this topic at my company, and hold several US patents on PCB and noise-related technologies.
I am a PCB and circuit noise expert. (also the technical director of our multi-million dollar noise lab) I get "called in" and flown out to design centers around the world to fix PCB noise issues when entire teams cannot (in industry jargon, I am a "cleaner". Think Pulp Fiction. Cleaners clean up the scene of a crime (a broken design that's late for ship), remove the body, clear evidence, and make the crime scene disappear. "It never happened".). It's my bread and butter and I can definitely talk to this.
Give me a little while and I'll write something up that hopefully all can use. You'd be surprised at the little tricks that you can employ to reduce noise and crosstalk on a PCB.
So many experienced and seasoned folks here have helped me tremendously with speaker design concepts and the physics associated with them that I'd be happy, actually enthusiastic to "give back" for a change.
This is my element.
OP never delivered