True, but the same holds for through-hole components. In general, the bigger the component, the lower the frequency at which it doesn't behave as an ideal lumped component anymore.
As I said in a previous post, would be interesting to see the difference by measuring comparable amplifier designs. 2 layer vs 4 layer (with ground plane), SMD vs through hole.
I've not seen through hole resistor designs in an EMC chamber, I have seen SMD parts. Given the larger size of through hole parts I would be interested to see if they are affected in the 2GHz+ region the same way SMD parts are. Given the abundance of that type of interference around now, it must have an impact on noise in some way. Maybe it's at such low level you would never notice it.
I've not seen through hole resistor designs in an EMC chamber, I have seen SMD parts. Given the larger size of through hole parts I would be interested to see if they are affected in the 2GHz+ region the same way SMD parts are. Given the abundance of that type of interference around now, it must have an impact on noise in some way. Maybe it's at such low level you would never notice it.
But, when looking at something like an audio application where it is an output signal you listen to, to what level and extent, and how is it affect by something simple like a ground plane and 2 layer vs 4 layer.
Unlikely to be a simple answer, and a power amplifier running off +/-50V will likely differ from something like my DSP boards with analogue stages working at <1Vrms with lots of digital signals.
If you have something like an audio power amplifier with limit bandwidth (say 100khz), then I thought the noise it picks up can "fold down" into it's working range, as it can't do anything else with it, so more output noise? Would it benefit from a 4 layer ground plane on the input sections, what is the real difference from through hole to SMD...
Unlikely to be a simple answer, and a power amplifier running off +/-50V will likely differ from something like my DSP boards with analogue stages working at <1Vrms with lots of digital signals.
If you have something like an audio power amplifier with limit bandwidth (say 100khz), then I thought the noise it picks up can "fold down" into it's working range, as it can't do anything else with it, so more output noise? Would it benefit from a 4 layer ground plane on the input sections, what is the real difference from through hole to SMD...
Yes, IMD, rectification, etc. These implementation differences are easily measurable with the proper tools.
The amplifier can have wider bandwidth but use input/output filters, which only addresses some problems.
https://www.edn.com/connect-signals-to-oscilloscopes-minimize-errors/
Last edited:
Please feel free to perform the experiment and report the results! Lay out two PCBs from the same amplifier schematic; build them out into identical chassis with identical power supplies, and then measure their performance. I'm sure that (a) you'd have a lot of fun; (b) other diyAudio members would be delighted to peruse your data.
Sure. Have a look at page 12 here: https://www.ti.com/lit/an/snoa497b/snoa497b.pdf
If those changes made less RF energy reach the inputs of the opamp, definitely.
In case of the EMI-hardened opamps from National (now TI), the benefit is from a filter on die.
Tom
True, must be other people that can do it though (if they were also interested). My turn around on hobby projects is generally 3+ years, have boards from my own project I received several years ago, and all the bits, that are still waiting to be built....
I’m currently designing a small amplifier front end PCB and this is going to have four layers. First I planned two layers, but then realized that I have way too many crossings and need four layers. The plan is to use the outer layers as ground planes and route everything on the inner layers. Stitching the the ground planes together forms a nice Faraday cage shielding the routing inside.
The only downside I see, is parasitic capacitance. In case the dielectric between the signal and ground plane is 0.2mm and the width of the routing 0.4mm, then the capacitance is 1pF per 10mm.
I simulated how parasitic inductance and capacitance affect the circuit and it seems to tolerate this. A bit of phase margin is lost. It is a VFA design. CFAs might be less tolerant.
Any ideas or experience regarding added PCB capacitance?
The only downside I see, is parasitic capacitance. In case the dielectric between the signal and ground plane is 0.2mm and the width of the routing 0.4mm, then the capacitance is 1pF per 10mm.
I simulated how parasitic inductance and capacitance affect the circuit and it seems to tolerate this. A bit of phase margin is lost. It is a VFA design. CFAs might be less tolerant.
Any ideas or experience regarding added PCB capacitance?
Its common to use internal layers as ground and supply, external layers for signal - then you have a chance of fixing any silly errors in the layout. I strongly suggest you do this, issues with buried traces are more than annoying, and any Faraday cage effect is minimal as the components themselves aren't in the cage.
In standard solid state audio amps the VAS stage and driver inputs have large voltage swing and meant to be lightly loaded - this would be compromised with lots of ground plane surrounding those nodes, I think its best to leave them away from a groundplane, or simply use the output node as the plane for them, bootstrapping away most of the capacitive loading.
In standard solid state audio amps the VAS stage and driver inputs have large voltage swing and meant to be lightly loaded - this would be compromised with lots of ground plane surrounding those nodes, I think its best to leave them away from a groundplane, or simply use the output node as the plane for them, bootstrapping away most of the capacitive loading.
I agree on the Faraday effect being almost nonexistent with the components outside.
Meanwhile I detangled the routing and reduced layer count to a standard two layer design. Much better now although some connections are a bit longer.
While adjusting the design from four to two layers I noticed one big advantage of routing on internal layers:
Unused pad removal on internal layers and much smaller pads on internal layers free up a lot of space and allow to route in between where this would not be possible on outer layers. Of course those features depend on software support. I aim to have the pads twice the diameter of the drill for nice solder fillets. And on internal layers, I set the pad to be larger than the drill by 0.6mm. In case of a 0.8mm drill, the outer layer pads may be 2mm in diameter and the inner layer pads have only 1.4mm diameter. And in case there in no connection to this pin on an internal layer, one can route even closer to the drill hole since the 1.4mm pad is now an anti-pad requiring only 0.3mm clearance between drill hole and routing.
The layer stack with ground on the outer layers was a result of actually needing three layers only as some people mentioned earlier in the discussion. I just duplicated the ground layers and facing the choice to put ground on both internal layers or both external layers, I decided for latter option.
Both solutions have the drawback of high capacitance to the routing layers. For most electronics this is fine and even desirable, but extra capacitance do no good in audio as Mark pointed out. Thanks for confirming my concerns since this made me change my mind finally.
A better four layers stack would be:
Signal
Signal
Ground
Power
Meanwhile I detangled the routing and reduced layer count to a standard two layer design. Much better now although some connections are a bit longer.
While adjusting the design from four to two layers I noticed one big advantage of routing on internal layers:
Unused pad removal on internal layers and much smaller pads on internal layers free up a lot of space and allow to route in between where this would not be possible on outer layers. Of course those features depend on software support. I aim to have the pads twice the diameter of the drill for nice solder fillets. And on internal layers, I set the pad to be larger than the drill by 0.6mm. In case of a 0.8mm drill, the outer layer pads may be 2mm in diameter and the inner layer pads have only 1.4mm diameter. And in case there in no connection to this pin on an internal layer, one can route even closer to the drill hole since the 1.4mm pad is now an anti-pad requiring only 0.3mm clearance between drill hole and routing.
The layer stack with ground on the outer layers was a result of actually needing three layers only as some people mentioned earlier in the discussion. I just duplicated the ground layers and facing the choice to put ground on both internal layers or both external layers, I decided for latter option.
Both solutions have the drawback of high capacitance to the routing layers. For most electronics this is fine and even desirable, but extra capacitance do no good in audio as Mark pointed out. Thanks for confirming my concerns since this made me change my mind finally.
A better four layers stack would be:
Signal
Signal
Ground
Power
There are cases where four layers can make a lot of sense though. For example, I’m currently designing a power output stage featuring multiple devices in parallel. I want to place them interleaved, i.e. not grouped by P and N type, but P-N-P-N and so on. This avoids nasty half wave rectified currents flowing around. This i a tip I have from Bob Cordell’s book. Now distribution of power, ground and the output signal becomes a challenge. Here, four layer boards are super useful since power and ground can be routed as a stack with the ground on outer layers and the power sandwiched in between. This results in very small loop area. Also, the output node that collects the current from all transistors, now can be routed on all four layers in parallel for super low resistance. Make sure not to create a capacitor at the output node as this destabilizes the amplifier.
Interesting - the meanwell SMPS 12V in my koi pond filter controller distinctly looked single layer!
From what I can see a top layer two shielding layers and then the bottom layer for small signal sensitive feedback etc:
Cu L1 = High dI/dt, main supply currents. Ie this is the layer with 3-400V and if you're using 24V 20A..
Prepreg 2x layers
Cu L2 = Ground return for the above. so that the EMI is minimised.
FR4
Cu L3 = Ground plane
prepreg 2x
Cu L4 = small signal and feedback.
I've deliberately steered clear of internal tracks given the current in use and resulting heating effect.
Last edited:
What is even more fun is that if doing a bridged design you can organise things such that the power AND both outputs form a stack cancelling not just the half wave stuff but also the speaker current fields.
My default board these days is usually 4 layers, it does not add the massive cost it once did, and the savings in layout time are worth it even before you get clever.
Interesting - the meanwell SMPS 12V in my koi pond filter controller distinctly looked single layer!
From what I can see a top layer two shielding layers and then the bottom layer for small signal sensitive feedback etc:
Cu L1 = High dI/dt, main supply currents. Ie this is the layer with 3-400V and if you're using 24V 20A..
Prepreg 2x layers
Cu L2 = Ground return for the above. so that the EMI is minimised.
FR4
Cu L3 = Ground plane
prepreg 2x
Cu L4 = small signal and feedback.
I've deliberately steered clear of internal tracks given the current in use and resulting heating effect.
Hartley seems to recommend, assuming a 4 layer board
Either
L1. Sig/Pwr
L2. Gnd
L3. Sig/Pwr
L4. Gnd
Or
L1. Sig//Pwr
L2. Gnd
L3. Gnd
L4. Sig/Pwr
How might these alternates be affected/preferred by the specific considerations of power audio amplifier PCB design (e.g. Self Audio Power Amplifier Design - he considers only single/double sided PCBs and not in depth).
It has always annoyed me that the super low cost PCB fabs who cater to prototyping quantity orders, will gladly quote and build boards with 2 oz copper, BUT on the outer layers only. Inner layers are 0.5 oz and there are no other possibilities.
Have a play on www dot pcbshopper dot com for some additional data.
Have a play on www dot pcbshopper dot com for some additional data.