Messed up PCB layout in commercial products

[fubar.gr]

This is the PCB of the new Sonoff POW wifi enabled relay with power metering capability.



The board as a whole looks rather well laid out, but look closely at the area near the HLW8012 chip!



The first thing that caught my eye was the trace between pin 2 and 3, and I thought, what the heck? Are they using guard traces? But then I realized this part of the board is most likely autorouted and the "guard traces" are probably the result of a careless polygon pour.

There's also a small isolated island at the top left and a tiny isolated trace below the capacitor at the right.

[mariush]

.. and they use that ams1117 with ceramic capacitors .. wouldn't surprise me if it's gonna be unstable.
.. and it's ugly layout to the left of that regulator, those 4 traces forming a sort of X there
.. and those two traces from the current sense so close to the cutout .. they could have moved the resistors further and place them horizontally.

can't say that i'm a fan of 90 degree traces as well

[tszaboo]

I also think they are badly routed guard traces. Look, there is one below that capacitor for some magical reason. Note that guard traces with soldermask on them will not do anything in the first place.

[John_ITIC]

Guard traces? Oh my...
https://www.google.com/?gws_rd=ssl#q=guard+traces+pcb&spf=1498027088514

[VK3DRB]

Looks odd with that trace, but those two pins are the differential current sense inputs on the mains line side. So electrically there is little consequence with this trace in between, depending upon where else it goes. It is pretty lousy though. It is clearly an artefact of a polygon pour.

More importantly, there is no component designators. Worse still they use the old round pin 1 markers. A much better practice is to use triangles (Altium: Place -> Solid Region) as pin 1 markers. Moreover they have given simple diodes pin 1 markers. Probably to signify the cathode.

No test points either, meaning no ICT.

One good thing is the pads are a good size.

[Cyberdragon]

What is the purpose of that 0 ohm resistor? Couldn't they have just continued the trace?

[hans]

I think the 1117 will almost definitely oscillate with ceramics. Grounding on the big ceramic also seems quite horrid.
Decoupling caps for SPI flash seem to be lost in wilderness. Or in general, because it seems like no priority near the ESP  QFN chip as well.

Not sure if no silkscreen is a miss.. it's cheaper and in non-repairable products a don't care anyway.
Anyone that needs to find a certain part on the board can work from an assembly drawing. This board isn't that complex to work with.
Moreover, finding space to put the silkscreen stuff can be a waste of time at some point.
(I wouldn't skip over it on larger boards though)

I'm not surprised if the designer dropped the components in layout tool, routed the board in 1 go and sent it off for production. Someone with some experience can do a reasonably job, but when in a rush tidying up and other OCD things will be left undone.
Board will probably still function..

[hans]

Yes, the cap must have a high enough ESR to form an overdamped LCR circuit so any ringing will die off quickly.
A few designs I've seen that had their tantalums 'accidentally' replaced with ceramics near the 1117, in all designs it resulted in a hiss sound and HF pitches. None of these boards were anything special in particular.. Just a micro and some sensors.

But the boards still worked. We only noticed years after. As long as the oscillation amplitude is limited to a few 10mV's, a bad DC/DC design can have comparable effects.  It's not nice, good practice or anything to be proud off - but it can work and not explode.

Just don't attempt any EMC measurements I suppose...

[fubar.gr]

What is the purpose of that 0 ohm resistor? Couldn't they have just continued the trace?

Jumper?

I wondered about that zero ohm resistor myself.

Normally these are used as jumpers, for other traces to pass underneath them, but here as far as I can tell, there's no crossing trace! It's weird.

[brabus]

Am I the only one concerned about creepage distance?
That shunt resistor traces and related component make those PCB cuts useless.

[tszaboo]

Am I the only one concerned about creepage distance?
That shunt resistor traces and related component make those PCB cuts useless.

I'm not. It comes from china. Anyone buying mains powered stuff directly from china, without UL or Tüv approval, deserves this. It's like natural selection.
They started doing: Hey look, it has a brand, so it is not broken by design like any other chinese stuff. Yes it is. I'm sorry, but you are buying electronics from a country, where they sell fake milkpowder, that kills babies, for profit. I like chinese people, I have friends among them, but when you put a billion in a country, all the western business practices will go down the toilet. Quick profit, screw over the customer for a cent, even if you dont have to.

[bktemp]

What is wrong with the creepage distance?
Since it senses mains current, the whole pcb is connected to mains, so no reinforced insulation is necessary between mains input and the wifi section.
Therefore the slots are useless. Even without the slots all creepage distances look large enough.

[Neilm]

I don't know that chip, but I have seen guard traces like that stub used to equalise stray capacitance around a device