Copper pour as shield

[sneakers563]

Hi all,
I'm in the midst of designing my first pcb-based tube amp. I'm not going with a ground plane, rather I'm simply adapting my usual multi-star / bus approach to a pcb.

However, I have read that a grounded copper pour can provide some shielding and help prevent crosstalk in nearby traces. Is there any benefit, or perhaps more importantly, any drawback to adding a ground pour on one or both layers of the pcb, but connecting it to the chassis?

In other words, although I'm using a traditional scheme with separate ground traces, I'm considering adding a ground pour to the pcb to serve simply as shielding. This pour would NOT be a ground plane as it would carry no signals and not be connected to the circuit. It would simply serve as an extension of the chassis, connected through the plated screw holes of the pcb.

Any reason not to do this? Is there any potential benefit or drawbacks?

[toddgw]

I've found the additional shielding well worth the effort. I pour both top and bottom layers and connect the two with a grid of plate throughs, to lower the impedance between them. Just a note; In case you're not already aware, potentials above 100V require much greater attention to trace separation. The early, high wattage Marshal DSL amps, suffered horribly for failures in this area. IPC-2221B is the standard I 'base' my trace thickness and spacing on.

[tristanc]

In other words, although I'm using a traditional scheme with separate ground traces, I'm considering adding a ground pour to the pcb to serve simply as shielding. This pour would NOT be a ground plane as it would carry no signals and not be connected to the circuit. It would simply serve as an extension of the chassis, connected through the plated screw holes of the pcb.

That’s exactly what I’ve done. If I do a v2 of my boards I’d have more stitching vias throughout. Although EEs may point out they’d make hardly any difference at low frequencies, they can do no harm.

[sneakers563]

Just a note; In case you're not already aware, potentials above 100V require much greater attention to trace separation. The early, high wattage Marshal DSL amps, suffered horribly for failures in this area. IPC-2221B is the standard I 'base' my trace thickness and spacing on.

Thanks - I think I'm ok with regard to that. I've used a minimum of 1/8" between traces and components, with most traces about 1/4" apart. I tried not to go too small with this one - basically just follow what I would do with turretboard, just with a little more freedom with component placement. I haven't looked at IPC-2221B, but I will take a look before I submit the board for fabrication on Monday.

I'll go ahead with the copper pour. I was a little worried that it might capacitively couple with the traces and propagate the signals unexpectedly into other places in the circuit, but it sounds like I don't need to worry so much about that. What do you typically use for clearances around the pour?

[strelok]

One practical note when adding a copper pour when using through hole components. If you're using Kicad or some similar circuit board design program that uses a netlist and DRC, you'll want to add a 0 ohm resistor / jumper between the circuit ground and the actual ground and copper fill. Otherwise the DRC will see any component that's referenced to the GND net and automatically connect the copper fill to that pad, sending whatever star/buss grounding scheme you happen to be using right out the window. Alternately when you go to do the fill you could tell it to fill as an unused net and provide a jumper between the two.

I just saw that you're planning on connecting it right to the chassis in which case the aforementioned won't be a problem, though my inclination is that it should be connected right to the circuit ground it *probably* won't make a difference for something like this. Its easy enough to change though once you get the boards if you want to experiment and see which way has lower noise.

Also I would not worry about the capacitive coupling between the fill and traces. Its going to likely be so small that it won't be of any concern at audio frequencies.

[tristanc]

One practical note when adding a copper pour when using through hole components. If you're using Kicad or some similar circuit board design program that uses a netlist and DRC, you'll want to add a 0 ohm resistor / jumper between the circuit ground and the actual ground and copper fill. Otherwise the DRC will see any component that's referenced to the GND net and automatically connect the copper fill to that pad, sending whatever star/buss grounding scheme you happen to be using right out the window. Alternately when you go to do the fill you could tell it to fill as an unused net and provide a jumper between the two.

Yes, this got me initially. But KiCad has a few built in 'definitions' for ground / earth. I used GND to signify the chassis and AGND for audio ground. This keeps the two completely separate except with the jumper as you say. And I believe you can go further and have multiple pours per side - so an area of the PCB with GND (say, near the input connection) and then switching to AGND for the rest of the side.

I've seen a PCB for the FireFly amp which did something similar to prevent oscillations.

[sneakers563]

Yes, this got me initially. But KiCad has a few built in 'definitions' for ground / earth. I used GND to signify the chassis and AGND for audio ground.

That's a smart way to do it. I ended up just creating 4 1pin connectors in their own little net, not connected to anything else. Because the holes are plated, they will be connected to the chassis through the standoffs and screws. Your way is a lot better though, as it's apparent what the purpose is.

[sneakers563]

One practical note when adding a copper pour when using through hole components. If you're using Kicad or some similar circuit board design program that uses a netlist and DRC, you'll want to add a 0 ohm resistor / jumper between the circuit ground and the actual ground and copper fill. Otherwise the DRC will see any component that's referenced to the GND net and automatically connect the copper fill to that pad, sending whatever star/buss grounding scheme you happen to be using right out the window. Alternately when you go to do the fill you could tell it to fill as an unused net and provide a jumper between the two.

I just saw that you're planning on connecting it right to the chassis in which case the aforementioned won't be a problem, though my inclination is that it should be connected right to the circuit ground it *probably* won't make a difference for something like this. Its easy enough to change though once you get the boards if you want to experiment and see which way has lower noise.

Also I would not worry about the capacitive coupling between the fill and traces. Its going to likely be so small that it won't be of any concern at audio frequencies.

The jumper is a good idea. Unfortunately, I didn't see it before submitting the design. I'll have to try that on the next go-around.

[azatplayer]

I like to (successfully) separate my board grounds as im so locked in to my old ptp style.
If my circuit has 4 grounds thru the preamp, aimed at each nodes filter, then that how i build pcb's.
I tend yo use the standoff as teh ground nodes drop in, and pour a plane over that part of the circuit, using the plane as the localised ground.

The last board ive done for an entire build bar the output tubes (preamp tubes board mounted) ive followed that ideal, but also rather than drop the heaters on top away from the bottom signal layer, i kept the heater runs on the bottom layer and covered them with a top layer pour. Mounted on the top, ive ran my caps and resisters across at 90 degrees to the AC runs, using the plane as the shield.
I also add a 2mm trace on the bottom plane either side of the heater AC run as a sideways shield. So on the plane its shielded, and above its components are shielded.

I admit i spent about 200 hours obsessing over this board, and still made a mistake..

[chief mushroom cloud]

I agree w/ all the above, but w/ regards to oscillation prevention.....no amount copper between adjacent traces that are of the same phase will stop them from oscillating (given that one is amplified from the other). One thing I always do is crosscheck between sch and pcb, all nets that are same phase and keep them separated by DISTANCE, irregardless of what I'm doing w/ Cu plane pours.

[toddgw]

What do you typically use for clearances around the pour?

Sorry for the delay in my response... I rarely have more than 300 volts on a PCB and for that I use 55-60 mils of clearance between it and 0V or a copper pour tied to chassis.

[azatplayer]

I agree w/ all the above, but w/ regards to oscillation prevention.....no amount copper between adjacent traces that are of the same phase will stop them from oscillating (given that one is amplified from the other). One thing I always do is crosscheck between sch and pcb, all nets that are same phase and keep them separated by DISTANCE, irregardless of what I'm doing w/ Cu plane pours.

Same phase? Did you mean opposing phase?
Itend to overkill use muting circuits for multi channel, even for same phase, tho ive only seen oscillation on opposing phase circuits close to each other.