Avoiding Oscillation - Do's and Don'ts?

[exclamationmark]

I've designed plenty of small simple PCB's for my own projects (it costs me literally $5 and about half a day to etch/drill the board - more time goes into planning the thing!), but I have a particular project in mind that requires more than a single layer, hence it is impossible for me to avoid crossing traces. I'm just wondering about the rules regarding oscillation and trace crossing... For example if we have V1 and V2 which are SINGLE triode tubes, is it safe to say the main concern to avoid oscillation is for V1's grid to be kept away from the plate and/or cathode of V2. Are there any other things I should avoid?

[soundguruman]

What should you avoid? Multi layer circuit boards.

[Jazz P Bass]

If it was mine to do, I would start the layout with the high current traces.
Do the layout to avoid having to go through a via to the other side of the board.
Then I would run the bias & signal traces.
You will have much less problems with the lower current traces, if they must be routed through a via.
I think it would be best to run the heater traces away from the B+.

[soundguruman]

Inevitably, it will arch and burn through the layers. Even 1 mil insulation is not enough with fiberglass.

[R.G.]

Oscillation requires three things: a feedback path, gain through the forward amplification path that is more than the feedback path attenuates, and a total phase through the amplifier and feedback path that adds up to one or more times 360 degrees.

The first and second are kind of the same thing: no feedback path is the same as saying the feedback path attenuation is infinite, no signal gets through it. In the real world, there are always feedback paths of some kind: stray capacitances, inductive coupling loops, and unforseen common resistances in power or ground paths. These unforseen feedback paths are what trip you up most often.

You avoid common resistance feedback issues with good decoupling and grounding practices.
You avoid inductive coupling by keeping the send and return lines for high current carrying traces as close together as possible and as far from signal lines and signal returns as possible.
You avoid capacitive coupling by minimizing the AREA of conductors which have different voltages on them, maximizing the DISTANCE between conductors with different voltages on them, and the voltage difference itself.

So: to avoid unwanted capacitive feedback, get as much distance between the traces you want to isolate as you can. For crossing conductors, make them cross at 90 degrees if they must cross at all, and never run parallel traces of outputs and inputs if you can avoid it. If you can't avoid it, run a ground trace between them. This cuts the signal-to-signal capacitance hugely (but not entirely).

You're already there with the signal routing: keep grids away from plates unless you WANT to connect them, and then connect them with as short and direct a line as possible. The more gain there is after a grid, the harder you have to work at keeping it from stray pickup.

Two layer boards are often easier to keep quiet than single layer boards because you have another two degrees of freedom in placing conductors.

[exclamationmark]

This PCB is only for a pre-amp, hence currents are somewhat low. On this particular board the heaters are wired off-board (ie, handwired), because I don't have the real-estate to route differential heater traces as I would do normally. Since I etch my own boards, my via's are somewhat... "heavy duty". Basically a lump of solid copper wire is jammed into the via, snipped, filed down, and soldered to both sides. Other things to note is that my trace width is 50 mil on 2 ounce copper, distance between high voltage traces and anything around ground potential is 300 mil+ and signal traces are generally 100 mil or more away from anything. I've followed these design parameters on a couple other builds, and have had nothing blow up... yet

Back on topic...Usually I would route power and signal on the same side, with a star ground/ground plane on the other side of the board. However, in this case there is signal and power on one side of the board, and ground and signal on the other side. Given there is signal on both sides of the board, I just want to make sure where signal wires DO intersect (albeit on different sides), there is no opportunity for oscillation.

I know in hand-wired builds, the wires of each respective half of a valve are usually twisted together, and kept away from the other half, so I know this is safe to do on PCB. Taking this a step further, the plate wire of a valve is actually at the same potential as the grid wire of the NEXT stage. So I can deduce that the grid of V2 and the plate of V1 can co-exist happily. Gotta do more thinking on other situations, though...

[Steve Conner]

When doing double sided boards for analog circuitry, I like to make the whole top side a solid groundplane, and route as much as possible on the bottom. When I get stuck, I'll start adding tracks to the top, taking care not to split the groundplane up too badly. I think this general approach would help with the oscillation problems, as capacitance would tend to be to ground, rather than feedback.

This maybe isn't such a good way to do high voltage circuitry, though: you'll have to leave a big clearance around every component lead on the groundplane side.

[J M Fahey]

Fully agree with crossing traces at 90º and finding long, close by, parallel ones far more dangerous.
Plus using common sense: when you can´t avoid crossing *some* tracks *somewhere*, be very careful with high impedance low signal level ones , route them "clean" first, and leave unavoidable "bad" choices to less sensitive ones, such as power rails, or cathode tracks, which will be more forgiving.
So far, you seem to have done it well.
Good luck.

[defaced]

Some manufacturers (Peavey for instance), include traces of their boards copper in their service manuals. Look at those for ideas on what has been done and works.

[exclamationmark]

When doing double sided boards for analog circuitry, I like to make the whole top side a solid groundplane, and route as much as possible on the bottom. When I get stuck, I'll start adding tracks to the top, taking care not to split the groundplane up too badly. I think this general approach would help with the oscillation problems, as capacitance would tend to be to ground, rather than feedback.

This maybe isn't such a good way to do high voltage circuitry, though: you'll have to leave a big clearance around every component lead on the groundplane side.

Funny you should mention this, because it's EXACTLY how I designed my last couple of projects. I'm using some surplus 12x8 inch copper clad sheets, so it's quite easy to have at least 200 mil clearance between anything at HV and ground (I actually need the huge PCB for this project, however). I've done some experiments on star grounds and ground planes, and could honestly not tell the difference. People say all sorts of bad stuff about having high impedance lines over ground planes because of the capacitance, but the reality is, the capacitance is only in the order of 17 pF per square inch using the dielectric equation. I don't know who actually runs 20 inch grid traces over ground, but at this point, I would say they probably deserve the slight capacitance! I've also heard some horror stories where poorly set up ground planes have actually coupled noise into input circuits, leading to feedback.

I will definitely look into some commercial designs, although a majority of them seem to be single sided.

[Steve Conner]

Commercial boards were typically single sided because they intended to do a large production run, and paring costs down was very important. It was worth spending extra design time and effort to achieve it.

For a DIY project, where you'll only make one or two boards, the balance is different. It is worth going with a more expensive manufacturing process to make the design stage quicker and easier.

I always argued that it's not worth spending an hour trying to get rid of a wire link in your single sided design, when it only takes 2 minutes to drill the holes for it and solder it in. But if you were making 60 of the boards, suddenly that link takes up 2 hours of your time, and it's worth trying to optimise it out.

The cost of double sided, plated through hole boards has also come down a great deal. Not many PCB houses even bother making the single sided ones any more.

[soundguruman]

Remember the lessons of mesa boogie boards:
arching from grid to plate voltage
arching from heater to plate voltage
Remember your minimum clearances, volts per mil insulation values.
I would use G10 fiberglass, at the minimum.

[J M Fahey]

arching from grid to plate voltage
arching from heater to plate voltage

What does "arching" mean?

[exclamationmark]

There's actually some pretty funny stuff going on in regards to creepage distances and high voltages. On one hand there are stringent safety regulations detailing the distance between traces or primary and secondary sides of a circuit. They specify comparatively HUGE distances, but for good reason... Arc over can easily occur where dust or moisture accumulates (I've personally seen it happen on an amp - not my own of course ). Then on the other hand you have manufacturers coming out with TO-220 package MOSFETS with specified operating voltages up to 1kV with roughly 1.2 millimetres between the leads! Luckily, coated boards tend to minimize much of the risk in regards to environmental factors (I like to go nuts with acrylic conformal coating - you can actually solder through the stuff too).

You really can't get anything less than FR4 nowadays (which is the successor to G10 - FR4 doesn't burn). And in regards to mesa... They like to run pre-amp tubes with a B+ of up to 450 volts in some of their amps, so I would expect some issues further down the line. I'm sticking with a more sane 300v B+ and have accordingly (over)designed around it. Arcing is easy to avoid. Oscillation on the other hand... I don't want to end up like Mesa and have to put plate capacitors on every 2nd gain stage .

[R.G.]

Oscillation on the other hand... I don't want to end up like Mesa and have to put plate capacitors on every 2nd gain stage .

Whether to ground plane or not depends on the signals being carried above the ground and the source/load impedances on each end of the trace.

At DC and very low frequencies (like most of audio) the best way to ground is usually to send a signal/ground pair to carry the signal current. At RF, a ground plane is better in the sense that it lets the currents flow where they want and keep them local to the signal path.

The issue of trace impedance, source, and load impedance gets into it too. Every conductor has some stray capacitance to every other conductor in the universe. This drops off by the square (or cube? I'll have to look) of the distance between the conductors, but it's always there. The stray capacitance is small for any distances more than a few millimeters, but the impedances connected to the trace form a divider with the stray capacitances. High impedances can make even very small capacitances couple unwanted stray signal levels and feedback.

There are (at least) three impedances to worry about on a trace. There is the source impedance, the load impedance, and the RLC impedance of the trace conductors themselves. The source and load impedances matter a lot at low frequencies where you don't have to consider the transmission line nature of the trace. If either the source or load impedance is much lower than the impedance of the stray coupling capacitors, it forms a large divider with the signal on the other side of the strays, and attenuates the stray coupling a lot. This means that as you'd expect from the Nyquist criterion, a lot more gain is needed to make oscillation an issue, so the gain of the circuit itself can be quite high for audio work and still not give oscillation and stability problems. So driving a trace with a low source impedance or loading it with a low load impedance cuts oscillation issues by allowing much higher gain without oscillation issues.

The matter of signal size comes up in tube circuits. Where you have a signal of hundreds of volts on the driving side of a stray capacitance, even small capacitances can couple enough signal into the input of a high gain amplifier to cause oscillation. The best way to deal with this is to make the capacitances as small as possible by placing the input conductors as far away from the high voltage signals as possible.

The trace impedance itself starts to matter either at frequencies where the signal must be considered a transmission line, or where its capacitive or inductive nature affects the signal. At audio, it is quite difficult to route a trace in a way where the trace inductance itself matters. Not impossible, but difficult. But it's easy to make the trace self-capacitance matter if the source and load impedances are high.

Running a ground plane maximizes the capacitance of every trace to ground. This matters for oscillation considerations by maximizing the possible phase shift contribution of the capacitances, so it makes gain-phase oscillation issues worse. It also shunts signals to ground from every conductor, so it reduces trace-to-trace capacitive coupling between traces, as opposed to trace-to-ground capacitances. Wide, flat traces over a ground plane can in some instances contribute enough self-capacitance to matter in audio treble loss if the source and load impedances are high, but for lower source/load impedances, do not matter much.

All this is quite aside from the voltage breakdown and arcing issues.

Ground planes are good, but they're not a panacea, and can have side effects. The trick with ground planes is just like with all grounding schemes: know the nature of the signal source and load impedances, and the voltage and currents of the signal, as well as where the current flows.