As long as there's soldermask covering it, and it meets the fab rules, it's fine.
Tim
For the high voltage traces and pads, I would go larger than 8mil spacing. Although solder mask is an insulator, the coating properties and thickness are not well controlled. I would try for 25mils.
Oh, my first reaction was "you're going to put a shield can over that?!"
Exposed metal sinks surface leakage currents, but even with poor soldering and no cleaning, you can expect to work with megohms pretty confidently. 32k crystals are around 100s kohms so it's well inside of the range to worry about.
Keep in mind some tricks to reduce routing pressure. For example that D2 can be duplicated between, say, every pair or triplet of drivers, so you don't have to route it around between all of them.
I think I'm seeing big gaps in ground support. For example under "U14" (the label), a peninsula of ground dead-ends; on the other side, U13 has some ground nearby, but I don't think it extends up far enough, and in any case I don't see a via between them. So the nearest ground, to any copper in that area, is either downwards (behind the chips) or all the way left or right, around the chips and associated routing, and on the top around the tubes as well, to that area. It's a huge open loop, which can be a problem for EMI (again, unlikely in this case -- more as an example of best practice).
Oh, may want to revise those footprints, the pin-1 indicator -- it's only a circle underneath the chip. How are you going to inspect that once it's placed? A dot beside the pin, say, below and to the left (again referring to U14 and friends), is a typical way to show that. Could also be a number (although then you have to orient it for every damn part that's turned, so it still reads right..?); or the outline drawn (currently just corners I guess) can stick out enough to be visible, and could show a semicircle on the pin-1 end, etc.
Definitely not Are those guard rings normally used in conjunction with shields?
I'm assuming you mean it's in the range I don't have to worry about, i.e. the guard ring wasn't necessary? Sorry the language was a little unclear
So ground "peninsulas" are bad for EMI?
I took care of that particular example by shoving the traces above U13 (push and shove routing is really neat) and nailing down some vias.
I also looked around the board for a little bit and got rid of some peninsulas that were unnecessary, i.e. didn't connect to the GND pad of any component.
Also redid the via stitching to spread it out a lot more, rather than only have a few points where the planes are connected. Not sure if this is an improvement.
Thankfully, since everything outside of the oscillator area and the 170V power supply module runs at a frequency of 1Hz or less (unless someone has a field day with one of the buttons ) I think I have plenty of room for error.
Oh gosh I had a mini heart attack when I read that first part, I thought I was about to have to redesign the board like when I got the nixie footprint wrong the first time around!
I just moved the circle to the outside of the chip.
Not so much that they're bad, just that they aren't doing anything for you, and generally mean there's a gap or loop nearby.
RF currents flow between a trace (signal current) and ground (image current). Ground proximity is key.
A trace running across a slot or hole in the ground plane, is no longer close to its image. The image current has to flow around the edges of the loop, taking a much longer distance, and coupling into a larger field -- potentially a radiating field, as an antenna. (These are called "slot antennas" when made intentionally. Or unintentionally, too, I suppose.)
Note that, between the pairs of chips on top and bottom, there's a big hole in the ground plane. You can train your eye to see positive space (traces and footprints) as negative space in the ground pour, and vice versa.
To the trace, the lack of ground proximity, manifests as an increase in its impedance -- or at low frequencies, as stray inductance. So it has some effect on signal quality as well.
Again, hardly an issue with CD4000 family logic, with ~100ns edges (so slow, you need 10s of meters of cable to see any wave effects), and already high impedances (pin drivers ~250 ohms at 10V, compared to trace impedances being in the 50-150 ohm ballpark), but worth thinking about with microcontrollers and 74HC and faster logic; and mandatory if you find yourself working with the good stuff (fast CMOS, ECL, LVDS..).
You are swapping layers frequently (like, horizontally, between the pairs of drivers), and without a transparent view I'm not sure if that's necessary (there is stuff on the other side), or if it's, in part, an effort to get more ground fill? But that's something that can help. Downside is it does use up more vias for the signal traces. (Which, I don't think is much of a reliability problem, and with stitching, you're using plenty of vias already, right?)
If you're not routing around components, it's fine to keep everything largely on the same layer (switching layers only where needed to cross traces, say); as long as there's ground available underneath it, you're golden. Same-side ground doesn't do nearly as much as opposite-side ground does -- the edge-wise coupling between traces, or trace and ground fill, is fairly mild.
Interestingly enough, while edge rates do matter (and, again, are hardly an issue here because they're so slow!), a repeat rate that low is probably low enough that it might get away with a lot, even with a noisy design (fast logic family, poor layout). The reason is, EMI testing is done with a certain receiver response, which averages over modest time scales; a crash of noise every second will average down to much less than a peak-detect receiver. Also, if the receiver is doing scans faster than 1 sec per band, it might simply skip over -- that is, when it was measuring a frequency, no noise happened to coincide, so it reads really low, but the next sample say catches the whole peak or something. The plot ends up spiky, but it's not because of harmonics!
Not that that's a good thing, the intermittent popping sound will still be just as irritating to affected radio channels. One of those kind of "meets the word of [the law], but not the spirit" things.
Whoa -- I had no idea about these sorts of effects!
While I understand the specific points you've brought up, overall I am in the dark in terms of RF, and how it works with PCB design. Hence me originally not having any ground plane, then putting a fence around the 32kHz oscillator Is there a place I can get started with learning the basics of RF black magic? Not that it's necessary for this particular project, but the topic just seems really interesting and it could come in handy for future projects where I need to worry about this kind of stuff. Or is this something that's too convoluted so I should just wait for college?
With the signal current and image current, and impedance stuff - is that the reason why some traces on a computer motherboard are squiggly? So the signal and image traces are the same length?
Here's an image of what I'm talking about
Yes, I did switch layers often for that very reason, to get the ground fill everywhere. I should be fine without doing this in the future?
Looking back at the board, I think if I didn't do all of that layer switching as much the final board might've turned out better. Though I don't think it's worth changing it now unless I need to go back and do other major modifications to the board.
And yes, currently I have a grand total of 314 vias I don't think JLCPCB charges any extra for excess vias until they have to drill more than 1000 holes on a single board.
There's one major concern I have about selling this project - what if it somehow emits tons of EMI and starts messing with people's devices? I've heard that could land people in big trouble. But there's absolutely no way I'm going to spend ten grand for a product I'd be surprised (pleasantly) if I sold more than five units. Maybe I pull that one trick and market it as a pre-assembled kit, or something.
But then again, with the slow repeat rate and super slow edge rates (I was completely unaware that CD4000 logic was that slow, guess that's a good thing!) it won't emit more than a bee's dick of EMI
But then again again I kinda threw on a random 170V SMPS and I think it makes a slightly audible noise in operation, so that might be spewing out stuff continuously...
Never too early to start thinking and reading about it. Developing a feel for fields and waves is a valuable skill, and it won't come overnight!
I don't have any good book recommendations unfortunately, but perhaps others can chime in.
Sort of. The fact that the board is multilayer, and the traces are routed over or between solid planes, and that they are of consistent width, and spaced adequately, is what's most important. The squiggles are to match delays, so that the waves propagating down each trace in a bus arrive at their destinations at the same time.
As for the differential pairs, you want to route their traces identically -- first of all, obviously you want to avoid routing the pair over some disturbance, like a gap between planes, or underneath a noisy power converter. If you can't avoid it, then you want the noise in each trace to match, so they get subtracted out at the receiver. The fact that the waves created by those disturbances, arrive at the receiver at the same time, means they will be ignored. At least while the disturbance is small (maybe a volt or less) -- it still has to fit within the receiver's voltage range.
Waves propagate along the traces at equal velocity (they're on the same PCB and have the same geometry), so it's just a matter of keeping the lengths matched, from the transmitter, to any noise source, to the receiver.
I try to prioritize single side placement -- that saves an additional assembly step. For a hand soldered assembly, meh, not a huge deal, but it's another buck here and there in commercial applications.
Then there's not much that obstructs the bottom side, and it can be used largely for ground.
If I am doing double sided placement, I want to ask myself some other minimization problem: how much board area do I need, to get a reasonable design (in terms of functional, thermal and EMI performance, say)? How many parts can I group in what arrangement, without running out of routing area?
But, that is me, and I have plenty of time to think about things while I'm idly poking at a design. Others, I know they just want the stupid thing done, damn the style; artwork, what's that?
Whatever level you're working at, you need to develop a toolbox of skills you are fluent with, and how to apply them. A lot of EEs don't develop a feel for fields; that can be compensated with more time spent testing or iterating. (Maybe not the least cost option, but that's for the managers to deal with... )
Yeah, that's about right for something that size. Like I said, I'd probably find a more optimal arrangement, preferably single sided, but barring something we've both missed -- you definitely have something buildable there.
Theory meets practice on law enforcement... I've heard of products produced on the 10k unit scale that went without testing, and apparently without complaint, so it's not impossible... that doesn't mean they passed accidentally, just that no one a. had a persistent problem that was b. traceable to the product.
So, the way the law on this (in the US) works is, AFAIK:
- Sometimes the FCC drives around, listening for things. With their budget and priorities these days, this doesn't happen very often.
- More often, a licensed user -- who takes legal priority, and has authority to file a complaint with the FCC, who then sends a C&D -- complains, and then most often the user simply stops using the offending thing. Assuming they figure out the culprit of course, which may not be obvious.
- If it's persistent, it can escalate to fines and so on.
- And there are clauses for tracing it back to the supplier of an offending product.
So, you need the combination of a customer, and a potential victim that is licensed, and enough complaints to bring it back to you. Or for Part 15 compliance, I honestly don't remember what the deal is, but I'm guessing?- a non-licensed user can complain of interference in relevant bands (broadcast radio for an important example; listeners are of course users of licensed bandwidth in that case), in which case the FCC may decide to investigate further, or may let it sit unless they get repeat complaints, etc. (Rules are different by band, for example the Part 15 permitted unlicensed emissions in ISM bands (13.56MHz, 2.45GHz, etc.) are higher than elsewhere, but still limited to fairly harmless levels.)
Mind, this is not a professional assessment or recommendation. It's a business decision, and like any other, incurs risk -- there's nothing life-changing about violating a law, it's just another cost of operation. (Indeed, legal defenses -- whether vs. civil or state -- are accounted as just another operating expense.)
In short, I would be very, very surprised if this ended up so bad that someone just happened to complain about it, and it ultimately came back to you as a direct liability.
The HV converter is indeed the elephant in the board, and it might be cheap insurance for example to add an LC around it, both ends. At best, jumper the L's and no-pop the C's; at worst, put in values large enough to deal with it. The module being small means it shouldn't radiate too horribly, even if made badly.
This is really interesting stuff. What kind of signals are sent through differential pairs?
This is similar to the theory behind balanced XLR cables right?, where there are two copies of the same audio signal but one is reverse polarity, and since any induced noise will be identical it can be cancelled out by switching the polarity of that audio signal back again and summing them together. I thought that was the coolest thing when I read about it.
To be honest, I have no idea how I'd start designing that LC filter. If it helps, the HV converter already has two honkin capacitors:
[image]
With a quick continuity test, the one on the left is connected between the +5V input and GND, and the one on the right is between the 170V output and GND, just what you'd expect. I don't have a device that can measure their capacitance. If I could use those as part of the filter and just throw on a couple coils it'd probably save the price of a capacitor that can handle that voltage, though I don't know if those caps would be on the wrong side of the LC filter. I've never dealt with inductors or LC filters before and I have no intuition on what values to use. Would it need testing or do you know of some values that are likely to work well and suppress potential EMI?
QuoteTo be honest, I have no idea how I'd start designing that LC filter. If it helps, the HV converter already has two honkin capacitors:
[image]
With a quick continuity test, the one on the left is connected between the +5V input and GND, and the one on the right is between the 170V output and GND, just what you'd expect. I don't have a device that can measure their capacitance. If I could use those as part of the filter and just throw on a couple coils it'd probably save the price of a capacitor that can handle that voltage, though I don't know if those caps would be on the wrong side of the LC filter. I've never dealt with inductors or LC filters before and I have no intuition on what values to use. Would it need testing or do you know of some values that are likely to work well and suppress potential EMI?
A filter needs three inputs:
Impedance (input and output)
Cutoff frequency
Sharpness (prototype and order, or some attenuation at some other frequency, etc.)
Nice thing is the cutoff doesn't have to be very precise for EMI. You can basically toss on a 1uH 1A chip inductor and say it's probably fine, for the 5V side. Maybe a 10uF electrolytic after that. So, it goes C, L, converter. Similarly, on the output, maybe it goes converter, 100uH, 10nF (maybe a 250V film cap, maybe with say 3.3 ohms in series with it).
There's a bit of algebra concerning input and output impedances, but the most important relation underlying it is Zo = sqrt(L/C). Exactly which L and C you should pick, also depends (in the middle of a filter network, you generally have to bisect individual components -- think of it as, in a CLC filter say, half the L works with the first C, and half with the other).
Frequency of course is 1 / (2 pi sqrt(L C)), and you need to pick the right L and C by the same rules, of course.
If the capacitors on that module are quite large (seems an okay assumption for now), then if we use much smaller C's outside, we can ignore the module caps by saying they're just "large". Treat it as an AC short circuit. We have L and C in series off of it, a nice simple network. No bisection we need to worry about. L is L, and C is C.
We don't want them to resonate, so we need an impedance to terminate them into. This is pretty free; we generally want a low impedance -- since this is around the impedance seen by the rest of the circuit. The nixies won't mind a few hundred ohms, of course, so we have a lot of freedom on that side; on the 5V side, we should keep it low, say less than 20% of the DC load equivalent (say if it draws 5V at 1A, that's 5 ohms, so 1 ohm would be fine).
By "impedance seen by circuit", consider a step change in voltage on the 5V rail, or 170V rail -- how much current is drawn in the instant surrounding that step change? Z = dV/dI. If you want tight supply regulation, you need a low impedance, so you want to design the filter for a low impedance in that case.
Ideally, we'd have a load resistor that serves as termination, but our load is probably higher impedance than the filter (partly due to the above suggestion), so what do we do? If we leave it alone, it can resonate, and end up with a transmission peak around the cutoff point; that's not good!
If we simply put R in series with C, we can introduce damping resistance, without consuming DC current, and without relying on the load.
If we use the entire C as an R+C, we lose some high frequency filtering -- at very high frequencies, the capacitive reactance goes towards zero, so the equivalent circuit is an L dividing into an R -- a 1st order lowpass filter, not 2nd order. (It's worse than that, for a number of factors, actually; we choose components small enough that these parasitic effects are either negligible, or expected to fall at a higher frequency than the converter creates.)
So a better option is using a smaller C in parallel with a larger C with loss, i.e., C || (R+C). I don't think this is important here, but it's nice to know. (Typically the lossy C is >= 3 times the parallel C; this gives good damping at the cutoff frequency.)
What's the significance of an electrolytic capacitor? It comes with ESR for free, that's all. A ceramic of the same value, with about 0.33 ohm wired in series, would also do.
Tim
Here's the updated power supply schematic:
C4 is electrolytic.
Is there a particular reason why C17 should be a film capacitor? Limiting to SMD parts and having a minimum purchase quantity no greater than 1, I was able to find equivalent ceramic capacitors that are 10nF and can sustain 250V for significantly less money on digikey than film capacitors.
Like you said, the nice thing about this is if it doesn't work somehow, I can just depopulate the caps (and R27) and jump the inductors.
If it matters, here are some digikey parts I found, I do not know if they have some fatal flaw I didn't notice:
- 1uH Inductor: https://www.digikey.com/product-detail/en/samsung-electro-mechanics/CIGT252010LM1R0MNE/1276-6939-1-ND/7041339
- 100uH Inductor: https://www.digikey.com/product-detail/en/tdk-corporation/MLZ2012N101LTD25/445-181376-1-ND/9740582
- 10nF 250V Film Capacitor: https://www.digikey.com/product-detail/en/kemet/LDEIB2100KA0N00/399-12880-1-ND/5731504
- 10nF 250V Ceramic Capacitor (Cheaper, but will ceramic mess things up?): https://www.digikey.com/product-detail/en/kemet/C1206C103JARACTU/399-7174-1-ND/3439312
- 10uF Electrolytic Capacitor: https://www.digikey.com/product-detail/en/panasonic-electronic-components/EEE-1CA100SR/PCE3878CT-ND/766254
- Might as well throw in the resistor: https://www.digikey.com/product-detail/en/vishay-dale/CRCW08053R30FKEA/541-3-30CCCT-ND/1962168
Since I honestly don't know very much about what I'm doing here, it feels like I'm shooting in the dark. Would there happen to be a college-student-friendly way to tell whether this is pumping out EMI? Maybe loop some copper and hook it up to my scope? Maybe turn it on and off next to a radio?? I don't know