PCB ground planes

[beatnik]

I am designing a few PCBs for tube preamps and would like to clarify some doubts regarding grounding and particularly the use of ground planes.
Other commercial and diy products I have seen use various solutions : star grounding, solid ground planes and even hatched ground planes.

I am keen to use a solid ground plane because it simplifies routing, but I have read that solid ground planes can be problematic for tube circuits, because of the high impedances at which tubes operate.
I am not sure this should be taken as a general rule of thumb since I am seeing many commercial products using a solid ground plane approach I guess it can be done with the right measures ?
Are there any specific considerations to keep in mind, for example isolation spacing between ground plane and signal traces, or sectioning the ground plane at specific points ?

I have designed the power supply section on a separate board, it's meant to be kind of an universal board that can power various tube circuits. It features HT output with simple crc filtering, unregulated DC for filaments and a section based on LM317 with a voltage doubler/tripler to get 48V for phantom power and a 12V/24V for relays and leds.
All the power supplies based on LM317 I have seen use a solid ground plane, whereas most tube power supply sections I found are without a ground plane, just using a star grounding approach.
Are there any reasons to avoid a ground plane in a tube power supply section ?

 

[rock soderstrom]

Interesting questions, many of which I have asked myself. I am curious what answers will come.

I use so far for tube circuits no continuous ground plane.

I like fat ground buses that follow the signal and that has worked very well for me so far. Overall, I notice that many designers use too small solder pads. Components for tube circuits are often larger and heavier than the usual low voltage components. This should be taken into account, in this way the components can be fixed more securely and also soldered better.

 

[JohnRoberts]

Did you do a search of "ground planes".

I've seen plenty of discussions about them over the years.

JR

 

[rock soderstrom]

Did you do a search of "ground planes".

I've seen plenty of discussions about them over the years.

JR

relax

 

[abbey road d enfer]

The only issue with ground planes in tube equipment is the increased capacitance of tracks, which may (or may not) result in treble loss.
In solid-state equipment, ground planes can be problematic if they provide unwanted direct path between stages that could affect each other, in particular power supply grounds should be connected in a single point to the ground plane and separated from the low level stages ground.

 

[beatnik]

Overall, I notice that many designers use too small solder pads. Components for tube circuits are often larger and heavier than the usual low voltage components. This should be taken into account, in this way the components can be fixed more securely and also soldered better.

Totally, I am using an old version of Eagle and I am finding I always have to modify the stock library footprints increasing pad sizes. This goes for the smaller through hole components as well.

The only issue with ground planes in tube equipment is the increased capacitance of tracks, which may (or may not) result in treble loss.
In solid-state equipment, ground planes can be problematic if they provide unwanted direct path between stages that could affect each other, in particular power supply grounds should be connected in a single point to the ground plane and separated from the low level stages ground.

I am keeping the psu on a separate board, so that should avoid psu ground currents affecting audio grounds.

I have read about the treble loss problem, yet I am seeing many commercial and diy products using ground planes. From the research I have done I couldn't find clear answers about this subject.

 

[ruffrecords]

Are there any reasons to avoid a ground plane in a tube power supply section ?

In a simple CRCRC HT supply the most important ground route is to/from the reservoir capacitor to/from the (bridge) rectifier. This is the dirtiest ,peakiest current in the whole supply so needs to be kept from flowing in audio grounds. Fortunately this is simple to arrange by placing the rectifier and reservoir close together and routing them to each other with big fat tracks Smaller currents flow in each successive smoothing capacitor so the audio ground should be considered the negative terminal of the last one. So basically there is no real need for a ground plane in a tube HT power supply.

Cheers

Ian

 

[abbey road d enfer]

Totally, I am using an old version of Eagle and I am finding I always have to modify the stock library footprints increasing pad sizes. This goes for the smaller through hole components as well.

I almost never use the standard library in Eagle (also an older version, 5.00).

I have read about the treble loss problem, yet I am seeing many commercial and diy products using ground planes. From the research I have done I couldn't find clear answers about this subject.

Treble loss is simply due to the low-pass effect of a node's impedance being loaded with the parasitic capacitance of a track.
High-Z nodes should be carried on thin short tracks, which should ideally be laid out at some distance from other tracks. A ground plane makes everything close to ground. In the case of VHZ nodes, it may be necessary to create a desert in the ground plane, or even to lift the components from the PCB, like it's done in many condenser mic head amps.

 

[volker]

Totally, I am using an old version of Eagle and I am finding I always have to modify the stock library footprints increasing pad sizes. This goes for the smaller through hole components as well.


I am keeping the psu on a separate board, so that should avoid psu ground currents affecting audio grounds.

I have read about the treble loss problem, yet I am seeing many commercial and diy products using ground planes. From the research I have done I couldn't find clear answers about this subject.

You don't need to manually edit all packages, you can control the size of the pads via the Restring tab in the DRC dialog. See here:
https://www.autodesk.com/products/fusion-360/blog/what-you-didnt-know-about-eagle-restring/

 

[abbey road d enfer]

Restring is a global setting. My understanding is that it would modify all pads, even those that are good.
Restring ensures adequate connectivity, but does not take into account the needs for mechanical robustness.
The underlying philosophy is that optimization is foremost concerned with useing as little tin as possible, and mechanical elements that are subject to forces are supposed to be fastened. Tell that to a console manufacturer!
Anyway, resizing pads in Eagle is so easy there is no reason not to do it.

 

[JohnRoberts]

With double sided PCBs using plated through holes pad size is mainly a solder joint quality issue.

Pads under mechanical stress (like pots or rear panel connectors ) generally rely upon secondary mechanical attachments.

Caveat I am not the tube guy around here....

JR

 

[abbey road d enfer]

Pads under mechanical stress (like pots or rear panel connectors ) generally rely upon secondary mechanical attachments.

That's the gospel, but there are many heathens.

 

[Matador]

That's the gospel, but there are many heathens.

Indeed. I wish someone would please tell that to Marshall, Carvin, Fender, Gallen Kruger, and many other device OEM's that rely on the PCB pins to hold the PCB in place with the pot's screwed to the front panel (hey, we saved a 0.00001c standoff and a screw, after all).

And god forbid you use a short wire bundle to go between the pot and the PCB which provides real mechanical separation. . (not that that doesn't have it's own problems).

So basically there is no real need for a ground plane in a tube HT power supply.

You described almost exactly how I do it - I usually make a pour under the rectifier's and the first filter cap, then run the supply rails / 0V hierarchically out to the edge of the PCB where it needs to connect elsewhere.

 

[JohnRoberts]

Indeed. I wish someone would please tell that to Marshall, Carvin, Fender, Gallen Kruger, and many other device OEM's that rely on the PCB pins to hold the PCB in place with the pot's screwed to the front panel (hey, we saved a 0.00001c standoff and a screw, after all).

when I was managing Mixer engineering for Peavey I would meet with the service department repair techs once a month and they would tell me emphatically what they were seeing on their repair benches.

JR

 

[Newmarket]

when I was managing Mixer engineering for Peavey I would meet with the service department repair techs once a month and they would tell me emphatically what they were seeing on their repair benches.

JR

I think we need the details there

 

[Mr. Moscode]

I've had good results running low impedance audio circuits with guard (shield) traces between them on the same layer. Low z traces can be covered with ground planes if necessary but you are still introducing parasitic capacitance to ground. Hi z lines are, for most cases, a no-no under a ground plane but guard traces are ok as there is only the capacitance from the edges of the traces which would be much lower than a GP.

Sometimes you need shielding to squash oscillations or cross talk but that should show up in the prototyping stage. It is better to re-route the traces that are talking to each other than to cover with a GP. Or if you're only making one unit then your choice is to find a fix with a wire or redo the board.

Miller effect capacitance would produce more severe HF rolloff in hi z ckts so keep the grid circuit away from the plate circuit. That's good idea in any case. Separate the ins and outs.

Another case is where you may need a GP is to isolate components on one side of the board from circuit traces on the other. Caps have a lot of foil. Like the output cap straddling a an input line. But you may only need just enough shield to do the job. Or reroute the trace.

BTW, the capacitors created by crossed traces or a GP have the circuit board as the dielectric which may be a concern.

The current the trace carries will create a magnetic field around it so you may want to shield AC filament traces with a GP

As for grounding in a hi current PS I used the input filter cap ground pin as the star point. In audio circuits I use the input star ground as the reference for regulators as well as decoupling caps.

This assumes my memory is functioning well. . .

That's my 2¢.

 

[JohnRoberts]

I think we need the details there

yet another Peavey anecdote requested.

First the Peavey customer service department repair technicians are remarkable, but since they spend all day getting beat up by customers they are quick to pass that (not) love downstream to us. They understand that their job is to insulate us (engineers) from needy customer calls, and they did a pretty good job of that, as long as they think we respect their input and advice. I was responsible for a few difficult products (like the $20k AMR split recording console) that were not trivial for the typical service technicians to support. When they run out of answers they forward the customer calls to me. This was OK if it didn't happen too often.

As I already mentioned I would meet with the repair techs once a month and invite them to school me on repair issues that they think might be design flaws in need of attention. This did not result in many (any?) design changes but just asking the question won me a lot of good will with the service guys.

During my stint over all product management (every product category), we decided to evaluate extending our warranty from something like 3 years to 5 years to be more competitive. To review this I evaluated all in-warranty repair claims and then out of warranty repairs where we had records. The good news is we didn't find many failures after the brief early "infant failure" period.

Curiously from this review I recall identifying one outlier SKU that had a disproportionate high number of failures. It was a modest slow selling SKU (small power amp) so the failures were handled quietly by the service departments without management noticing. Only after I reviewed the failure rate compared to the total sales did I see how out of line the failure rate was. I brought this to the attention of the director of analog engineering (Jack Sondermeyer) and he quickly identified a component in the amp design that was not rated adequately for the application. After that the failure rate for that SKU dropped even lower.

Now for the TMI part of this anecdote... Back when I was still working at Peavey, it was OK for them to refer difficult customer service calls regarding the big recording consoles to me, even thought I was no longer working in engineering.... BUT after I quit, and walked away from that job, I would still get occasional calls about console issues. At first I did not think much about it because I do not exactly hide my identity, and a motivated customer could probably find me around the internets. BUT after one too many customer calls at the house, I asked the customer where he got my number... He said "Aubrey" (the console service tech) gave him my number. I would occasionally take calls from service techs (like Aubrey) at the house to help him help customers, but I would absolutely not tolerate them just forwarding service calls to me. I was no longer a Peavey employee. I called the manager of the service dept, an old friend and told him in no uncertain terms "no more sharing my phone number with customers". He agreed and stopped it PDQ.

JR

 

[beatnik]

I've had good results running low impedance audio circuits with guard (shield) traces between them on the same layer. Low z traces can be covered with ground planes if necessary but you are still introducing parasitic capacitance to ground. Hi z lines are, for most cases, a no-no under a ground plane but guard traces are ok as there is only the capacitance from the edges of the traces which would be much lower than a GP.

Thank you for your very informative reply.
Sounds like star grounding is preferable with tube circuits which confirm my previous findings when researching this subject.

I have seen some manufacturers using hatched ground planes, I guess this is to reduce the parasitic capacitance ?
A hatched plane still makes routing simpler, but I imagine the shielding effect of a solid plane would be lost.

The current the trace carries will create a magnetic field around it so you may want to shield AC filament traces with a GP

Does that apply to DC filaments as well ?

Most often I am seeing AC filaments wired off board with the classic twisted pair , but usually DC filaments are on the top board layer.

I have attached a layout for a super simple dual triode preamp based on the RCA BA-2, I would be very interested in any opinions.

Miller effect capacitance would produce more severe HF rolloff in hi z ckts so keep the grid circuit away from the plate circuit. That's good idea in any case. Separate the ins and outs.

In this particular case that's very easy to achieve since the 1620 / 6J7 tube has the grid connection on the top of the tube.

 

[abbey road d enfer]

Sounds like star grounding is preferable with tube circuits

Star groun is a notion based on safety. It is definitely not the best solution for low-noise electronics, compared to hierarchical ground.
However, most tube circuits are low-current, even a 100W tube power amp operates with less than 500mA, except heaters. However heaters are a separate circuit, which is easy to make sure their current does not pollute the other parts. With such low currents, a rather flimsy ground circuit would still offer good performance, but nothing justifies makinf star ground a preferred choice.

which confirm my previous findings when researching this subject.

I believe the name "star ground" elicits grandeur, and allows its heralds to stand up, but really they should know it's good for safety, and poor for noise and other aspects of performance. Does one really want all their connections to ground going back and forth through lengths of wire?

I have seen some manufacturers using hatched ground planes, I guess this is to reduce the parasitic capacitance ?

I believe it's a manufacturing decision, that avoids creating large blobs of solder after wave soldering.

A hatched plane still makes routing simpler,

Maybe I misunderstand you. Does hatch mean "allowed to be crossed by other tracks"? In that case, that would be a wise decision, it it allows separating grounds that are not supposed to be mixed.

but I imagine the shielding effect of a solid plane would be lost.

Don't overestimate the value of shielding. Indeed sensitive nodes need to be protected, but remember that the most important shielding is the one done by the case/chassis.
Not too long ago (1970's), ground planes were almost unknown in audio equipment. Many brilliant pieces of equipment had single-sided PCB's. Perhaps the most significant reason for adopting ground planes in audio circuits is because it reduces chemical waste.
Actually the Brits were conscious of that and adopted a style of layout that left most of the copper intact.

Does that apply to DC filaments as well ?

DC heaters do not radiate AC, so tehy can be routed almost any old way.

Most often I am seeing AC filaments wired off board with the classic twisted pair

Yes because twisted pairs reduce magnetic radiation.

 

[Newmarket]

I believe it's a manufacturing decision, that avoids creating large blobs of solder after wave soldering.

ime it's more about avoiding an unbalanced (in weight terms !) pcb that can lead to warping (depending on the size of the pcb) during manufacture / processing. But yeah - the solder blob thing makes sense.