PCB trace "style" between AC (mains) and DC circuits - Page 1
Forum section: electronics / beginners

author: iroc86
author_rank: Regular Contributor
timestamp: December 15, 2019, 01:16:45 pm
content: Circuits designed for AC operation at mains voltages often have a different "style" of PCB trace compared to low-voltage DC circuits. See the photos below. I see this appearance in chargers, power supplies, inverters, etc. The traces are usually chunky and cover a lot of board area, almost like a fill. I've encountered this style enough times to presume that it's not just engineers' preference.I doubt the reason is for current handling, as many of these supplies operate at relatively low output (<1 A). I figure it might have something to do with minimizing temperature rise across the tracks. Or, perhaps the intent is to keep as much copper on the board as possible for etching and mass production, since there isn't a DC ground plane to fill in the voids. Any ideas?

author: SeanB
author_rank: Super Contributor
timestamp: December 15, 2019, 05:31:53 pm
content: Probably there to both minimise etching time, and to ensure that, even with a very poor process control ( likely if the PCB is being made by a lot of labour, and not in an automated controlled bath) they will have enough trace left to both solder to, and also a wide enough trace so that shipping vibration will not peel them off the board. All 3 look like they are made with SRBP, and thus made cheaply, so likely in a building without any temperature control, other than a fan for the workers in hot weather, and a coat in winter. Massive variation in etch time, and they probably etch till the outer board is fully clear, then give it a few minutes more in the tank with the bubbler on, to get the inner ones, thus overetching the outer ones. Then wash, clean with some scouring agent ( could be a pad, river sand or even silty mud, you never know), rinse, dry and screen on the solder mask, and then either they have an old NC drill to do the holes, or there is a drill press, a stack of boards, and a mask, and somebody doing it by eye, so you want a good amount of pad around the traces in case the drill is a little skew.

author: Gyro
author_rank: Super Contributor
timestamp: December 15, 2019, 05:45:59 pm
content: The primary side is all about maximising track spacing (creepage and clearance), while the secondary side is about providing as much copper as possible to minimise the loop area between secondary windings, rectifiers and capacitors. Large copper area also assist with heat dissipation for the secondary side rectifiers (and capacitors, as they tend to be more stressed in SMPSs).I mentioned loop area, it is critical that the current loop around the transformer primary, switching device, reservoir capacitor and snubber is kept as small as possible (consistent with maintaining track spacing) to minimise EMC emissions.

author: Zero999
author_rank: Super Contributor
timestamp: December 15, 2019, 06:37:48 pm
content: Talking of creepage, the first photograph doesn't have sufficient creepage distances. This isn't a problem if the DC side is treated with the same precautions, at the mains, otherwise it's a no no and shouldn't be used.

author: Gyro
author_rank: Super Contributor
timestamp: December 15, 2019, 06:55:59 pm
content: Agreed, that first one is awful, no consideration of safety clearances whatsoever, typical 'no clue' cheapo design. I can't even identify the primary-secondary demarcation. Bin it!

author: iroc86
author_rank: Regular Contributor
timestamp: December 15, 2019, 07:41:10 pm
content: Quote from: SeanB on December 15, 2019, 05:31:53 pmThat makes sense. Most of the time I see the really dense/chunky traces on cheap single-sided boards. When building to a price point, I suppose anything that improves manufacturing yield is fair game.Quote from: Zero999 on December 15, 2019, 06:37:48 pmHa yeah, it's pretty terrible! I snagged those pictures from various sellers on AliExpress because I knew I had seen that construction on the cheap modules and whatnot.Quote from: Gyro on December 15, 2019, 05:45:59 pmThat's pretty interesting. Here's another board I found on eBay that seems to demonstrate that logic--would you agree? It's TDK-Lambda, so most likely built for quality before price. I guess the variability in the trace shapes is probably due to hand routing/taping?--What you all said about the trace shapes for manufacturing and AC/DC performance makes sense. I want to explore this a bit further though. I've attached two pictures below from another TDK-Lambda component. The chunky traces are mostly on the primary side, but there are some fairly large fills on the secondary, as well. Using the trace I highlighted, from a design standpoint, what would be the workflow for determining the ideal shape for these polygonal traces? Would something like this have been autorouted using creepage and clearance thresholds, or did a person actually sit down and draw the trace that way?

author: Nusa
author_rank: Super Contributor
timestamp: December 15, 2019, 09:26:16 pm
content: Unless you want your traces to BE the fuses, design for the worst case scenario, such as dead-short load. The traces have to last long enough for your fuse or safety device to shut it down.Also remember that nominal mains voltages are going to see huge transient spikes from time to time.

author: T3sl4co1l
author_rank: Super Contributor
timestamp: December 16, 2019, 12:03:07 am
content: I've always wondered what tools are used, because this isn't anything new, they've been doing it for decades. It's not confined to power supplies -- though you see single-layer phenolic builds there most often, for whatever reason -- you see it on VCRs and TVs, too. I assume the smoothly curved examples are hand made (mostly ending in the 70s) and the rectilinear ones (mostly starting in the 80s) are EDA.What's the most popular Japanese EDA tools?...Ed: here's a Sony example, two layer board from a Trinitron monitor.https://www.seventransistorlabs.com/Monitor/Images/Defl5_a.jpgTim

author: iroc86
author_rank: Regular Contributor
timestamp: December 17, 2019, 11:18:39 pm
content: Quote from: Nusa on December 15, 2019, 09:26:16 pmThat's insightful. I admit that in my hobby circuit designs, I don't really account for fuse timing relative to the current handling capability of the traces. Perhaps I should!Quote from: T3sl4co1l on December 16, 2019, 12:03:07 amGood call; TVs and VCRs are another place I've seen this trace styling, too. Judging by the geometry of the traces, they do look like fill zones that someone explicitly designed that way instead of letting EDA autorouting do its thing.--Here's some more food for thought. I found the following reference design from TI for an AC-to-DC power supply:http://www.ti.com/tool/TIDA-00701. They have the full schematics and PCB files available to download. On much of the AC input side, TI is using those chunky geometric traces. You can see where they neck down near some of the pads, presumably as a thermal relief, but there's a lot of copper there. The secondary side is more "conventional" with 45-degree traces and ground fills. Looking at the schematic format, as well as the drawing title block, this was designed in Altium, which I presume would favor linear traces.I've attached the artwork below with the component outlines overlaid.I also really wonder about the "flourishes" that appear on some of the chunky traces. See below--do these little angled featuresreallyhave a measurable effect on current loading, electrical performance, EMI, etc.? I just don't know why someone would add them in.

author: temperance
author_rank: Super Contributor
timestamp: December 18, 2019, 07:32:41 pm
content: -Those low cost power supply boards are produced with phenolic paper. The wider traces make for extra stability.-I've seen only one cad package able to this: PAD's. PAD's supports different routing modes.Other tools able to do this must be available because commercial products with phenolic paper based PCB's in them are all "routed" like the boards you've shown. Those Pioneer DJM CD players are mostly made with phenolic paper PCB's and ten billion wire bridges with different lengths. They even wave solder very large TQFP's onto the bottom of such boards. Those bridges seem to be a cost effective solution compared to double sides epoxy PCB's. The same goes for flat screens. The interface boards are just phenolic paper when possible with a lot of wire bridges and big fat traces to keep traces from peeling of the board. Especially around connectors. The weirdest thing I've seen is a double sided phenolic paper PCB in a commercial product with wire bridges soldered with a wave soldering process for the bottom side and the top solder joints must have been a hand soldering job. Even on some trough hole components, they hand soldered some pins onto connections on the top layer.

author: niconiconi
author_rank: Frequent Contributor
timestamp: December 19, 2019, 06:01:23 pm
content: Quote from: T3sl4co1l on December 16, 2019, 12:03:07 amA lot of cheap boards from China also heavily use this routing technique. Nowadays, low-cost power supplies are the few remaining applications that are still using a single/double-layer phenolic board, so you are most likely to find them on power boards. But I see a large number of the cheapest board they sell online (e.g. "soldering practice 101" NE555 boards) use this routing style as well.I, too, wonder what CAD packages they are using to create them. It seems the software can automatically "floodfill" every trace on the board.

author: SeanB
author_rank: Super Contributor
timestamp: December 19, 2019, 08:06:19 pm
content: Quote from: temperance on December 18, 2019, 07:32:41 pmJust took apart a dead Sharp calculator, made around 2005. Toshiba main chip, SRBP board and with a whole 2 SMD transistors under the board, the rest being through hole parts, and around 30 jumper wires, in a set of 3 different sizes for the board. Matching keyboard SRBP board, single sided, wide and narrow traces, with carbon printed contacts, along with the jumpers being carbon printed over the soldermask , with a further soldermask layer screen printed over for protection.With the thinner mass produced SRBP boards they do not actually drill the holes, but instead use a punch and die set, to make them all in a single pass with a press, saving time. There you want a wide pad and trace, as your alignment might be a little off, but so long as it still is mostly in place it will solder, and work, plus the die and punch has a much longer life over a speeding drill bit, which has a limited number of holes it can drill before it blunts and needs to be redressed.A wide trace is also much less likely to fracture all the way through if the board is cracked during processing or shipping, so lessening the chances of the device failing during the short warranty period, though the crack may eventually go all the way to open later.

author: iroc86
author_rank: Regular Contributor
timestamp: December 31, 2019, 09:37:54 pm
content: Thanks for the additional feedback, guys. It's sounding like this trace design is more due to mechanical reasons than anything, at least on the cheap phenolic boards.Just for kicks, I reached out to Texas Instruments directly to inquire about the traces in the last set of attachments I posted, the ones for theTIDA-00701power supply. This is a reference design that'd presumably be manufactured with regular FR4, which is the method TI chose based on the pictures in the preceding link.They referred me to their "E2E" (engineer-to-engineer) forum, so I posted the question there. You can read the full threadhere. I don't really feel that the TI engineer answered my question to the level of detail I wanted, but I wasn't going to push it further. They just reiterated the obvious, that traces need to be sized for current capacity and clearance/creepage. No real mention of the specific geometry aside from designer preference and the bit below about filtering performance:Quote