Feedback on my first pcb layout

[user 37518]

Thanks, John! I hadn't ever considered this, but it seems so obvious once it is said.

In general, impedance is Z = R +jX, where R is resistance and X is the reactance. When frequency is zero (DC) the reactance becomes zero and the impedance is equal to the resistance. However, when the frequency is other than zero, impedance is not the same as resistance alone.

The reactance is produced by reactive components which means capacitors and inductors , so at AC, impedance takes into account both the opposition resistance creates and the opposition to the current that reactive components create. Since now, at AC, not only resistors oppose the current but also capacitors and inductors, we need a new term which takes into account all the factors that "impede" current flow, that factor is called impedance.

If you want a deeper understanding here is an explanation, I'll try to make it as simple as I can, for those of you who know better, bear with me if I'm not being 100% accurate, I'll make it as sweet as I can.

Resistance represents the energy losses into heat when current flows through a conductor or material. As electrons collide with the atoms of the material, energy is lost, the more collisions, the more resistance so current will find it harder to move from place to place. If the current is steady, such as DC, the magnetic and electric fields will also be steady and that is basically the end of it, so the only thing which opposes current flow is resistance. However, if the fields are changing, which is the case with AC, resistance will be present in the material and oppose the current, but as current flows through the conductor it also produces a changing magnetic field, this changing magnetic field will generate (induce) a new current in the conductor, this induced current will travel in the opposite direction of the conductor relative to the initial current (Lenz Law). You can think of it this way (and this is only a simplification for educational purposes): suppose you are looking at AC current flowing to the right of a conductor for a period of time, this current creates a changing magnetic field which in turn generates an induced current which flows to the left of the conductor, therefore, this induced current opposes and reduces the initial current flowing to the right. This opposition which is produced by the changing magnetic field, and which is different from the opposition produced by the the resistance of the material, is represented by inductive reactance.

I just mentioned the effects of a changing magnetic field, but there is also a changing electric field and capacitive reactance takes into account its effects. Something interesting is that inductive reactance has a positive sign, whilst capacitive reactance has a negative sign, meaning that they counteract each other, if inductive reactance is greater, the total circuit reactance X will be positive, if capacitive reactance is greater, the sign will be negative, if they are the same, reactance will be zero and only resistance opposes the current. Reactance also varies with frequency, as opposed to resistance which doesn't depend on frequency.

Now we have this scenario in which there are basically two things which oppose current: resistance (due to collisions) and reactance (due to changing magnetic and electric fields). So we can no longer talk about resistance alone, we need a new quantity which takes into account all those things I just mentioned, the quantity which takes them all into account is called impedance. So only when you are using DC (no changing fields) or when the inductance and capacitance of the circuit is negligible, the reactance is zero and you can say that impedance = resistance, otherwise, impedance is not equal to resistance.

I hope this makes sense

 

[Matador]

My emphasis on the ground plane or trace under the signal trace applies mostly to AC, not DC. There is a general misconception that current takes the path of least resistance or the shortest path, that is only half true, the real thing is that current takes the path of least impedance, which does not necessarily means the shortest path nor the path of least resistance.

Do you think this effect is significant in audio designs?

For example, a 12 inch, 50 mil trace, on regular 63 mil FR4 material, with 1 oz copper, over a ground plane, has 0.3uH of parasitic inductance, and 12pF of parasitic capacitance, and 0.1mOhm of parasitic resistance. This could be modeled as a 1st order LPF with a -3dB point of 83MHz. The output impedance would only rise from 0.1 mOhm to 0.37 mOhm, even at 20kHz.

 

[user 37518]

Do you think this effect is significant in audio designs?

For example, a 12 inch, 50 mil trace, on regular 63 mil FR4 material, with 1 oz copper, over a ground plane, has 0.3uH of parasitic inductance, and 12pF of parasitic capacitance, and 0.1mOhm of parasitic resistance. This could be modeled as a 1st order LPF with a -3dB point of 83MHz. The output impedance would only rise from 0.1 mOhm to 0.37 mOhm, even at 20kHz.

At 20KHz, around 80% of the return current flows directly under the signal trace. I can provide references. You are only thinking in terms of a lumped pole and frequency response and neglecting completely the bigger picture, I am thinking in terms of field distribution and where the return currents travel, regardless of whether they get filtered or not.
Do you really think these sort of issues of controlling where the return currents travel only starts to become relevant at the MHz range? can you design a console without paying close attention to ground and return currents without any consequences?
You might get away with a stomp box, a preamp, or something similar, but more complex circuits are a whole different matter.

Just to stress the importance of what I am trying to convey.

From EMC for product Designers:

"... if you are using older technology, i.e. double- or single-sided, the safest way to lay out a PCB is to start with the ground traces, manually if necessary..." and continues "Track impedance is dominated by inductance at frequencies higher than a few KHz. " not MHz (this last one is mine)

Like I said, I am not saying that ground planes are a miraculous cure, but here is another excerpt from "EMC for product designers":

"A ground plane is a useful tool to combat crosstalk, which is strictly speaking an internal EMC phenomenon... The effect of the ground plane is to significantly reduce the common ground impedance Zg, by between 40-70dB, in the case of an infinite ground plane compared to a narrow track." and continues: "Crosstalk problems or internal interference coupling, are by no means limited to digital circuits, although these tend to make the problem most visible. A common threat to the immunity of analogue circuits is crosstalk from other circuits carrying high interference currents or voltages. You should always be on the lookout to minimize crosstalk by ensuring the maximum separation between circuits, or by interposing electric field screening between them, or by implementing a ground plane"

An finally, at the end of the 6th chapter he gives some grounding rules, among which this one stands out: "create, maintain and enforce a ground map"

The point I am trying to convey with all this: do not neglect ground or the path return currents take. This has been my point all along, just routing stuff willy-nilly with "traces not crossing" being the sole determining factor to select the top or the bottom layer to route a signal is not the proper way to do things.

 

[user 37518]

Just to stress the importance of what I am trying to convey.

From EMC for product Designers:

"... if you are using older technology, i.e. double- or single-sided, the safest way to lay out a PCB is to start with the ground traces, manually if necessary..." and continues "Track impedance is dominated by inductance at frequencies higher than a few KHz. "

Like I said, I am not saying that ground planes are a miraculous cure, but here is another excerpt from "EMC for product designers":

"A ground plane is a useful tool to combat crosstalk, which is strictly speaking an internal EMC phenomenon... The effect of the ground plane is to significantly reduce the common ground impedance Zg, by between 40-70dB, in the case of an infinite ground plane compared to a narrow track." and continues: "Crosstalk problems or internal interference coupling, are by no means limited to digital circuits, although these tend to make the problem most visible. A common threat to the immunity of analogue circuits is crosstalk from other circuits carrying high interference currents or voltages. You should always be on the lookout to minimize crosstalk by ensuring the maximum separation between circuits, or by interposing electric field screening between them, or by implementing a ground plane"

An finally, at the end of the 6th chapter he gives some grounding rules, amongst which this one stands out: "create, maintain and enforce a ground map"

The point I am trying to convey with all this: do not neglect ground or the path return currents take. This has been my point all along, just routing stuff willy-nilly with "traces not crossing" being the sole determining factor to select the top or the bottom layer to route a signal is not the proper way to do things.

 

[Newmarket]

Do you think this effect is significant in audio designs?

For example, a 12 inch, 50 mil trace, on regular 63 mil FR4 material, with 1 oz copper, over a ground plane, has 0.3uH of parasitic inductance, and 12pF of parasitic capacitance, and 0.1mOhm of parasitic resistance. This could be modeled as a 1st order LPF with a -3dB point of 83MHz. The output impedance would only rise from 0.1 mOhm to 0.37 mOhm, even at 20kHz.

Apart from the discussion / maths around where/if this inductive impedance at 'audio' frequencies - a circuit implementation needs to be compatible with its environment in terms of rf / emi etc. a 'poor' layout may work fine with audio itself but large loop areas will increase susceptibility to eg rf interference that is rectified / modulated into the audio band (and besides you don't want to be putting out unwanted and inaudible signals eg into a power amp / speaker setup).

 

[JMan]

Since starting this thread, I've tried my hand at several more pcb layouts, trying to put into practice all of the (sometimes conflicting) information that has been shared.

I wonder if there is any kind (or masochistic) soul who would be willing to take a look at one or two more complicated layouts that I have since worked on and give me feedback on them. I think this would perhaps be beyond the scope of this thread, given that the designs are considerably more involved than the line amp that started this (still probably quite basic in the grand scheme, though). I'd be particularly interested in an analysis of my ground paths. If you would be up for helping, please feel free to shoot me a private message or reply here and I can get you the layout(s)/schematic(s).

 

[Matador]

trying to put into practice all of the (sometimes conflicting) information that has been shared.

Welcome to GDIY.

 

[JMan]

Welcome to GDIY.

No kidding. Truly, welcome to any area of specialized knowledge. In my own field of expertise, it's no different -- well-respected peers make emphatic, "objective" claims that run directly counter to one another. It makes for a dynamic discourse, if nothing else...just so long as we maintain the understanding that I'm right.

 

[JohnRoberts]

Conflicting advice generally comes from overly broad sweeping generalizations, rules of thumb rather than laws of physics, that don't change.

Different electronic technologies can lead to different optimizations. Mixed technology like A/D conversion can raise conflicting goals between analog side and digital side.

Life is a simultaneous equation with multiple variables. Don't let perfection be the enemy of good.

JR

 

[JMan]

Life is a simultaneous equation with multiple variables. Don't let perfection be the enemy of good.

This is good advice that is always worth repeating, John. That said, I'm still at a stage where perfection(ism) isn't really a factor -- I'm just trying to make sure *I* am not the enemy of good!

 

[user 37518]

This is good advice that is always worth repeating, John. That said, I'm still at a stage where perfection(ism) isn't really a factor -- I'm just trying to make sure *I* am not the enemy of good!

The problem is when you know barely enough to cause some damage. It is usually at this stage when one makes the worst decisions. When someone is an apprentice, common sense (hopefully) serves to navigate you through the conflicts, but when you start learning, you start making decisions not so much based on common sense but on what you think you have just learned, at which point, you start messing things up because you still haven't learned enough or you really don't comprehend what you learned.

I think that George Bernard Shaw sums it best: "Beware of false knowledge; it is more dangerous than ignorance"

 

[JMan]

Yes. That's precisely where I am, and I am acutely aware of it. The problem is that awareness alone is not enough to overcome this hurdle -- I'm sure you'd agree that that requires continued experience and ideally guidance. Mistakes are also part of the learning process, but where I can avoid them with some help from those more experienced, I'm happy to do so.

 

[Newmarket]

Yes. That's precisely where I am, and I am acutely aware of it. The problem is that awareness alone is not enough to overcome this hurdle -- I'm sure you'd agree that that requires continued experience and ideally guidance. Mistakes are also part of the learning process, but where I can avoid them with some help from those more experienced, I'm happy to do so.

I'd advise - Don't worry about it now at this stage. Lots of good advice here. But bear in mind that some will be contradictory.
Where appropriate I've implemented stuff such as "extreme" via stitching etc. But for you circuits a reasonably laid DSPTH pcb will very likely be fine.
Get connectors where you need them. Minimise loop areas. Maximise signal ground pour / fill (maybe a bit more clearance at any high impedance nodes) and get your boards made.
If you do get a problem then it can likely be resolved with track cut and a patch wire. And any undesirable copper scraped away.
Your geometries are small. Think of the comparison with a big (or even medium) size mixing desk.
And if you do get a problem then resolving it will be a great learning experience.

 

[mike]

I thought maybe this could be interesting in this thread, since we're discussing designing a modern PCB of this line amp and best practices - here's a circuit trace of the original helios layout used in the console with some very slight changes to allow for available transistors with different pinouts.

It had an optional buffer there at the top. When this PCB was used in places on the console where the buffer was not needed they literally just hack-sawed off just above "LINE AMPLIFIER 22113". There were a couple components that are on the schematic that were soldered offboard - eg. directly on the edge card connector.

I know you're already finished and I wouldn't have expected you to use this for your project (I didn't) - so this is more for learning - seeing what the original designer (**** Swettenham) did compared to the advice on this thread, which was all great advice, if not sometimes contradicting, lol

We've come a long way since the 70's with PCB design.

Edit: Oh yeah, there's a wire jumper (originally on the bottom of the board) that is hard to see, going from C21 to R21. That's just in the optional buffer, so not really part of this discussion but I figured I'd mention it. One of the places this buffer was used in the console is right after the passive hi-pass filter on the EQ.



Here you can more easily see the GND and +24v

 

[JohnRoberts]

Old school hand taped (with actual tape).

JR

 

[Matador]

And no ground plane, yet it still works!