Jensen as017 preamp Adaptation

What's real purpose of using ground planes on LF circuits except saving the etching chemicals?

squarewave said:

I think we're starting to mix up grounding issue principles (which is easy to do).

Click to expand...

I don't think I'm mixing anything. Grounding is a one and single issue.

My understanding is, and correct me if I'm wrong, that the "ground follows signal" rule has to do with EMI and magnetic coupling of noise into other parts of the circuit.

Click to expand...

Isn't it what grounding is about?

Then you have parasitic resistance / inductance which is a separate issue

Click to expand...

How is it a separate issue? We are debating about how to connect different "grounds" in such a way that noise performance is optimized.

However, I think there's a 3rd issue (although it does have to do with parasitics) which is that, because the circuit in question is high gain, any noise on the input is going to be amplified and, if the output ground is connected to the input ground,

Click to expand...

Here you are again with your notion of a dirty ground that should not be connected because its "dirt" will be amplified by the high-gain circuit. What would cause the output "ground" to be dirty vs. the input "ground"? If currents are well balanced and referenced to a single point in the output "ground", why would it be dirty?

Icegoldnixon said:

Another layout with minor updates.

Click to expand...

You should really check the pitch of the parts you are using. 

moamps said:

What's real purpose of using ground planes on LF circuits except saving the etching chemicals?

Click to expand...

A) When well designed, i.e. not allowing output currents to circulate in sensitive nodes, a ground pour has lower resistance (and inductance) than a basic ground trace.
B) It acts as an electrostatic shield that allows reducing unwanted capacitive coupling between nodes.

abbey road d enfer said:

A) When well designed, i.e. not allowing output currents to circulate in sensitive nodes, a ground pour has lower resistance (and inductance) than a basic ground trace.
B) It acts as an electrostatic shield that allows reducing unwanted capacitive coupling between nodes.

Click to expand...

All this can be done without ground planes.
B) with ground planes you have capacitive coupling to the ground, forming LF filters.

moamps said:

All this can be done without ground planes.

Click to expand...

Do you think there is no benefit in decreasing the impedance of the reference node? I do. What do you suggest? Adding copper wire?

  B) with ground planes you have capacitive coupling to the ground, forming LF filters.

Click to expand...

The capacitance of a 0.3mm trace respective to a ground plane is about 1pF/inch  (4pF/dm). Not an issue, unless dealing with extremely high impedance nodes. I wouldn't use a ground plane with the gate connection of an FET in condenser microphone, but apart from that, a few pF capacitance is not significant.

moamps said:

What's real purpose of using ground planes on LF circuits except saving the etching chemicals?

Click to expand...

In general, you can get less ground impedance if you can make the unbroken portions of ground foil larger. The sheet resistance of 1  oz. copper is 500µΩ per square. The square could be 1 mm x 1 mm, or  1 m x  1 m, and it's the same 500µΩ. So, if you can arrange for the area of unbroken copper to be larger, then the impedance in ground will go down. Generally, this helps all circuits regardless of operating frequency. I can't afford the luxury of unbroken ground planes - 4 layer boards are pricey enough. Still, aiming for large pours seems much better than relying on wide traces alone.

One other point: even though an audio circuit may have only a 100kHz passband, I find it's useful to use an LM4562, a 50MHz op amp that has enough gain bandwidth to allow a lot of feedback below 20kHz. So, despite my slow signals, I want to use an amp with a lot of gain bandwidth, and that forces me to deal with HF layout techniques. Having a lot of copper in the power planes and the ground pours helps keep the impedance down

abbey road d enfer said:

Here you are again with your notion of a dirty ground that should not be connected because its "dirt" will be amplified by the high-gain circuit. What would cause the output "ground" to be dirty vs. the input "ground"? If currents are well balanced and referenced to a single point in the output "ground", why would it be dirty?

Click to expand...

There is noise on the input. Just from Johnson noise or whatever. That is going to be amplified 100x because the circuit is high gain and then some of that noise is going to leak back into the input and be amplified again resulting in overall a slightly higher noise floor.

I never said anything was "dirty". I can only guess you are getting that from the name "DGND" that I use to mean a ground for anything that is not relatively quiet. So if there IS something "dirty" like digital or relay stuff it sound use DGND. I did not mean to say something was "dirty".

squarewave said:

There is noise on the input. Just from Johnson noise or whatever. That is going to be amplified 100x because the circuit is high gain

Click to expand...

That is true.

and then some of that noise is going to leak back into the input

Click to expand...

Why would it be so? Adequate design makes sure this does not happen.

I never said anything was "dirty". I can only guess you are getting that from the name "DGND" that I use to mean a ground for anything that is not relatively quiet.

Click to expand...

No. DGND stands for "digital ground"; calling it dirty ground is an abuse.

So if there IS something "dirty" like digital or relay stuff it sound use DGND. I did not mean to say something was "dirty".

Click to expand...

That's exactly what you say in the former sentence. You contradict yourself. Again, "digital or relay stuff" is dirty only if the currents are not properly returned and they are allowed to flow and develop a voltage that may possibly be amplified. That is the first thing that needs to be addressed.

abbey road d enfer said:

Why would it be so? Adequate design makes sure this does not happen.

Click to expand...

True. It depends on the load. But the circuit as shown could be any load. If it's a 600R load there will be amplified noise on the ground. If it's a 5K pot feeding another stage, then it would not be a problem.

squarewave said:

True. It depends on the load. But the circuit as shown could be any load. If it's a 600R load there will be amplified noise on the ground. If it's a 5K pot feeding another stage, then it would not be a problem.

Click to expand...

It does not depend on the load; it depends on how the load current is returned to ground. It this point is well chosen, whatever the current, there would be no interference with the input.

You guys advice really makes me want to have an EE check my boards before I send to fab house... >.<
0V's make me nervous.

Icegoldnixion, if it wasn't already mentioned, the shortest distance between two points is a straight line.  Where you can connect two parts with a straight line that does not get close to anything else or choke your ground plane, choose a straight line from pad to pad over making unnecessary 45 degree angles. Just a few examples: R7 to C10,  R8,9 to  pads 2&3 respectively.  Honestly little changes like those almost never make a sonic difference, but efficient routing is pleasing to look at.  Also never learn how to miter traces. Once you do, you'll want everything to be all flowy and sexy looking like the hand drawn days-of-yore at the cost of shortest signal path and your sanity/time.

abbey road d enfer said:

Do you think there is no benefit in decreasing the impedance of the reference node? I do. What do you suggest? Adding copper wire?

Click to expand...

In a lot designs I saw here, using GP wasn't resulting in decreasing  this impedance. Ground planes are not a universal cure in LF circuits where impedances are not 50 or 75 ohms. 

The capacitance of a 0.3mm trace respective to a ground plane is about 1pF/inch  (4pF/dm). Not an issue, unless dealing with extremely high impedance nodes. I wouldn't use a ground plane with the gate connection of an FET in condenser microphone, but apart from that, a few pF capacitance is not significant.

Click to expand...

This capacitance depends of the thickness of the board, but also the bigger problem are too small distances of the GP to the traces on the same layer. Why you choose 0,3mm trace for your math?

abbey road d enfer said:

It does not depend on the load; it depends on how the load current is returned to ground. It this point is well chosen, whatever the current, there would be no interference with the input.

Click to expand...

Well I would do some tests but all of my electronics stuff is tucked away right now since I'm working on work right now (or at least I'm supposed to be). But you have me wondering. I'm not an EE so I rely heavily on modelling and comparative measurements. I would swear that I have seen measurable differences using a separate ground for high gain inputs but I don't have empirical data and plots and such and I don't recall the exact the circumstances. If the circuit is just a simple stand alone mic pre with nothing else going on and the planets are aligned properly, then maybe it's not a problem (I never did say it definitely would be). At the noise levels we're talking about (-127-ish dB) it can be difficult to measure differences reliably. There have been many instances where I re-dress some wires or fiddle with a test cable and I get a slightly different result. My projects can be pretty elaborate with lots of relays, leds and digital all packed together so I decided long ago to use 3 grounds that get progressively quieter (smaller / lower freq. currents) and I would swear that if I use the quietest ground for just the mic in (what we have been referring to as "signal ground" or SGND in this discussion) I get better noise results.

moamps said:

In a lot designs I saw here, using GP wasn't resulting in decreasing  this impedance.

Click to expand...

At audio frequencies, the larger the traces, the lower the resistance (inductance is negligible).

Ground planes are not a universal cure in LF circuits where impedances are not 50 or 75 ohms. 

Click to expand...

Ground planes are not supposed to be a cure, they are part of design in RF applications. In audio, they are convenient for the reasons I exposed earlier.

This capacitance depends of the thickness of the board, but also the bigger problem are too small distances of the GP to the traces on the same layer.

Click to expand...

  Distance between signal traces and copper pour is adjustable in all PCB softwares. I also use 0.3mm clearance. If I ever found that it resulted in too high a capacitance, I would increase clearance, but it just never happened.

Why you choose 0,3mm trace for your math?

Click to expand...

0.3mm (12 thou) is a very common standard for low-level signal traces; not too long ago, if you wanted smaller traces, you had to pay extra. Now PCB fabs commonly do 0.1mm (4 thou), but I haven't changed my habits.

0.3mm (12 thou) is a very common standard for low-level signal traces; not too long ago, if you wanted smaller traces, you had to pay extra. Now PCB fabs commonly do 0.1mm (4 thou), but I haven't changed my habits.

Click to expand...

What are the pros/cons to using trace widths much larger for low level signal?  I've been using 2oz , 1.27mm  for the 70's inspired stuff.  Were larger trace widths only due to fabrication limitations of the day? Respect for point to point wiring /tubes?

boji said:

What are the pros/cons to using trace widths much larger for low level signal?

Click to expand...

Ground traces benefit of being wider since it minimizes longitudinal noise. Power traces need be sized according to the current they carry.
Low-level signal traces could be very small indeed.  Large traces increase stray capacitance, which can be an issue with x-talk and interference.

I've been using 2oz , 1.27mm  for the 70's inspired stuff.  Were larger trace widths only due to fabrication limitations of the day?

Click to expand...

Remember how PCB artwork was produced then, using transfers and adhesive tape on a transparent film. The thinnest tape was about 0.5mm (20 thou) and that ended up being the actual resolution, unless you did scale 2x, which required an additional photographic step. Actually, at the time I didn't go below 0.8mm, except for logic.

Thanks Abby, I'll certainly keep that in mind in my future projects.

Icegoldnixon said:

Wow! Thank you, pedantic is what I crave.      ...  Happy Memorial Day!

Click to expand...

Great sentiment in a new player    Good luck with your endevours 

Well I didn't mean to stir up any controversy, but I ran the ground pours for PGND and DGND together, and left some space for mounting holes. So I think these boards are ready, unless folks have other thoughts?
My other problem that I've ignored is the zobel network. Attached is the schematic for the circuit the transformer came from. I don't see an obvious network I can copy for the front of this preamp. Will just using the Jensen values result in disaster? Thanks all!