Circuit and PCB advice and comments please - Page 1
Forum section: electronics / beginners

author: frich
author_rank: Contributor
timestamp: August 19, 2025, 05:30:05 pm
content: being very new at electronics, i would very much like comments on the below design.it consists of a HLK-7628N router with LAN transformer, and a MP2338 buck converter.been using Kicad for the project, and i have gone for having all the components on 1 side for ease of assembly.i am very interested in what could be better, but also what was made correctly.

author: Benta
author_rank: Super Contributor
timestamp: August 19, 2025, 06:58:56 pm
content: Very good for a first-timer.Two comments:It's common practice to place power on the right side of the schematic, and inputs on the left, which would be a mirror of what you have.And don't forget to mark unused pins (the X on the right-side KiCAD menu), otherwise you'll get a bucketload of errors when running ERC.Cheers, keep it up.

author: frich
author_rank: Contributor
timestamp: August 19, 2025, 08:09:30 pm
content: okay yet another thing opposite from electrician workthere it is very common to have the power on the left sidebut good to know, and something i will try to keep in mind.haven't gotten to the ERC function yet, its all a fairly steep learning curve when you are used to 240-36.000Vone question thou, when looking at other schematics, i noticed a lot of the time there is many GND symbols. is that just to avoid having to draw the connections ? or is there a deeper meaning?one of the big things i was worried about is the traces with the ethernet signals running fairly close to the buck converter. i am mainly thinking about noise.

author: Benta
author_rank: Super Contributor
timestamp: August 19, 2025, 08:33:40 pm
content: Quote from: frich on August 19, 2025, 08:09:30 pmAbout the left-to-right thing: we're on the same page, but as an electrician you're focused on the power flow in your schematics.In electronics, thesignalflow is the main thing. The power supply is something auxiliary and usually placed on the right side to "keep it out of the way"The GND symbol thing is a matter of taste. You can get along with only one, but if readability is improved by removing GND wires and adding discrete GND symbols, go ahead.I didn't look at the PCB, so I can't comment on your last point.

author: ftg
author_rank: Frequent Contributor
timestamp: August 20, 2025, 11:39:04 am
content: The LED series resistors seem to be 15ohms, which seems very low.I'd expect LED1 to shine very brightly, if briefly.

author: frich
author_rank: Contributor
timestamp: August 20, 2025, 11:47:37 am
content: they are indeed brighter than i anticipated, but according to the specifications they have a forward voltage of 3.2V and the output voltage of the buck converter is 3.3V

author: xvr
author_rank: Frequent Contributor
timestamp: August 20, 2025, 12:11:05 pm
content: QuoteIn datasheet stated:Operating voltage: 2.0V - 4.5V (I don't know how it's possible)Operating current: max 0.2mA with 'no load' condition (do not ask me what does it means)Driving Current: typ 20mA at @VDS=1.0V (what is VDS unclear)Very strange devicehttps://mm.digikey.com/Volume0/opasdata/d220001/medias/docus/6472/5962_XL-2012UGC-DS%20%20%20%20%200805%E5%8D%95%E9%97%AA%E7%BF%A0%E7%BB%BF.pdfPS. LCSC has another datasheed. Forward Voltage is 2.6V-3.4Vhttps://www.lcsc.com/datasheet/C965815.pdf

author: PGPG
author_rank: Frequent Contributor
timestamp: August 20, 2025, 05:07:39 pm
content: At schematic your Ethernet connection looks good - is rather short, but at PCB it goes through all its length.Do you know that you should make this connection using differential pairs - total length of both wires in each pair should be the same. If you have impedance matching resistors along these lines than track length of both wires from connector to each R should also be equal. Also tracks should have their impedance controlled (to be 50Ω). If the connection is short it is not so important, but you made it as long as possible.Read articles you will find here:https://forum.kicad.info/t/decoupling-capacitor-via-placement/25132/14https://forum.kicad.info/t/decoupling-capacitor-via-placement/25132/19to became PCB design expertAs you come here from high voltages zone you probably noticed that T1 trafo was tested with 1.5kV Vrms and it is not 'by chance' that Ethernet connections are made with galvanic isolation withstanding such voltages. Look at your schematic and think what will happen when Ethernet cables will get 1kV voltage (can happen during near-by lightning strike).About GND.Don't think of GND as of a connection 'to be made' but as of reference level for everything.GND symbol used instead of wire is better telling this.Most important lesson about PCB design:Imagine at PCB ABC triangle. Signal goes from point A to point C, but because of something disturbing the track goes through point B. All currents flow in closed circuits so return current goes from C to A. Current knows better than we how to get back from C to A in the most economical way (loosing as little energy as possible). For DC and low frequency current components it means going directly from C to A, but for higher frequency components the electromagnetic field emission becomes an important part of looses. Minimizing the circuit area minimizes these looses (as well as unwanted emissions from your PCB). Fortunately only what you need to do is to not disturb the current to choose the best path (for high frequency it is just under the track so from C to B and then to A).Not disturbing in finding the return path for signals in all tracks at your PCB means ensuring continuous GND to let current go in each case as it wants.My example of 2 layer PCB with continuous GND is here:https://forum.kicad.info/t/approaching-pcb-track-routing-for-a-newbie/36302/8

author: frich
author_rank: Contributor
timestamp: August 20, 2025, 05:28:21 pm
content: Quote from: xvr on August 20, 2025, 12:11:05 pmglad that it is not just me getting confusedthey are bright, but does not seem to burn out (initial test was 8 hours for the entire board)

author: frich
author_rank: Contributor
timestamp: August 20, 2025, 05:54:34 pm
content: Quote from: PGPG on August 20, 2025, 05:07:39 pmi pretty much put everything i could dig up about ethernet connections onto that board, so no i did not know about differential pairsi do now.the initial reason for making the board, was to be able to use the HLK-7628. at the time i bought it, i was not aware that i needed a LAN transformerso a couple of weeks researching on google, and i found that i needed a transformer, and some resistors aswellQuotealot of readingthanks for the link.not sure i will be an expert when finished, but i will know moreQuotenot too concerned about lightning, since where this gets plugged in, there is surge arresters on both the ethernet and 24V supply on the other side of the connector. but i see you point.i do however want to add surge protection for the 24V input, at the moment there is only reverse polarity protection.but i haven't had the time to read up on how to do thatthe whole board gets put into a plastic shell, and is used as a way to connect to machinery, so you can use your phone or tablet to control it. instead of a big and heavy cabled controller.

author: PGPG
author_rank: Frequent Contributor
timestamp: August 20, 2025, 06:55:05 pm
content: Quote from: frich on August 20, 2025, 05:54:34 pmNow it looks that your Ethernet connection is few cm length and not 100m.If connection is short than it will work without Bob Smith termination (R5,R6,C3).As trafo is 1:1 and coils are not used to supply DC (via their center taps) and connection is (probably) very short and both connected devices (probably) have common GND than I think it will be also working when trafo would be replaced by 4 capacitors just to allow for other DC voltage components at connected device interfaces.But I have designed only 2 devices having Ethernet.

author: frich
author_rank: Contributor
timestamp: August 20, 2025, 08:28:22 pm
content: Quote from: PGPG on August 20, 2025, 06:55:05 pmi did not try with capacitors, wasnt aware it was a possibility, but i did end up reading about the bob smith termination, and a few articles about the side between the transformer and the chipset.that part was however very hard to find anything consistent. there seems to be quite a few different approaches, i tried to combine as much as possible, and with some trial and error on a breadboard, i found this setup to work.the overall board is about 80mm, so not far at all. the main concern, as mentioned before, is noise.since it is used in an inviroment with alot of noise that i cannot affect, reducing it as much as possible internally have been a goal.it is used in power generation up to around 21MW with full converter switching around 1500Khz. so there is quite some noise to interfere with signals.

author: PGPG
author_rank: Frequent Contributor
timestamp: August 20, 2025, 10:01:06 pm
content: Quote from: frich on August 20, 2025, 08:28:22 pmI have never seen such solution, but I think it is possible. It will certainly be more sensitive to interference so it is not what you want.Quote from: frich on August 20, 2025, 08:28:22 pmTrafo has some asymmetry and some capacitance between windings (trafos are very small so capacitance is not so small). Because of this even driven by pure symmetrical signal it converts part of it into common mode. So common mode chokes are added to dump it. Until you don't have DC component the CM choke probably is better to be at IC side (CM choke at cable side degrades Bob Smith termination, I think). But if you have DC (some drivers/receivers are powered through trafo center tap) then CM choke at IC side would be saturated by this DC so have to be moved to the opposite side. With driver and receiver needing, not needing DC we have 4 combinations. Adding different plug orientations, pin orders, LED or not LED, Bob Smith integrated or not you get an infinite number of different variants.And it is not the end. If someone don't want CM choke at cable side (because of Bob Smith) you can make CM with third wire to compensate DC. And a completely different story begins when you consider PoE.Quote from: frich on August 20, 2025, 08:28:22 pmquite some ... rather unimaginable level of interference.I suppose the best would be to have 4 or more layer PCB and your differential pairs routed at internal signal layer between two GND layers with rows of vias on both sides of pairs making it being like in shielded cable.

author: frich
author_rank: Contributor
timestamp: August 21, 2025, 04:53:25 am
content: Quote from: PGPG on August 20, 2025, 10:01:06 pmyeah that would create a good shielding around it.

author: frich
author_rank: Contributor
timestamp: September 26, 2025, 06:20:51 pm
content: So after testing 10 of these in the field, i have seen a failure rate of 20%not realy that niceboth cases was the buck converter blowing up (first made a short between Vin and Vout causing everything to blow upthe only thing i can think off at the moment is that the inrush must be causing it, it seems to be 100% to fail when connecting it to a specific generation of cabinet, that generation has long wires from the PSU to the cabinet connector, and that pushes me to the theory that it could be caused by increase inrush current from the inductance of these long wires.so i need to get some surge protection built in. but what would your recomendation be ?should i try with a cap or 2 ? (limited height causes problems with larger caps),a TVS ? or should i go all in and add a hot swap controller ? something like an LM5069 ?

author: Vovk_Z
author_rank: Super Contributor
timestamp: September 29, 2025, 02:24:06 am
content: A generl use type electrolytc capacitor or 0.1 R resistor inseries with a ceramic type nput capacitor may help.