Hand-soldering on a 4Oz/140um PCB? - Page 1
Forum section: electronics / projects

author: chconnor
author_rank: Contributor
timestamp: September 08, 2023, 06:55:43 pm
content: I'm designing a PCB and struggling to make everything fit and keep clearances and such. It will have some 240VAC 11.1A traces on the high voltage side, going through relays and the like.I think I can make it work with 3 or 4Oz copper (140um) and thick traces. (It's a one-off project so cost isn't as much of a concern.)But I'm wondering how realistic it will be to hand solder. I only have an entry-level 40W Weller iron. No ground plane on the high voltage side. Biggest/thickest components are probably the relays and SSRs (theseandthese).Edit to add: the low voltage side does have a top and bottom copper pour (and thermal reliefs for ground pads -- whatever the kicad defaults are.)If this is "turn the heat up and take your time" territory, that's fine. If this is "you're dreaming" territory, I'd like to be clued in early so I can do a more thorough re-design to see if I can make it work some other way. :-)Thanks for any insight!

author: MarkS
author_rank: Unknown
timestamp: September 08, 2023, 07:41:54 pm
content: I asked a similar question about 6 months back as to how to hand solder a large heatsink. While I asked after I had struggled through it, and so did not use the advice given at the time, one piece of advice that stands out is to preheat the board. Basically, stick in in your oven to get it as close as possible to the solder melting temperature, but not enough to burn or delaminate the board. I don't know a recommended temp, but this would help alleviate some of the heatsink effects of the larger, thicker traces.

author: mariush
author_rank: Super Contributor
timestamp: September 08, 2023, 07:53:02 pm
content: You should really think hard if you need 4oz or not, often there's other solutions.For example, maybe you could design the traces so that you could have a reasonably solid core copper wire bent to the shape of the trace and basically solder it to the trace with lots of solder?Alternatively, you could have maybe insulated solid core wire go from point to point and thicken the base trace (for example you could have some ceramic or plastic spacers to keep the solid core insulated wire at a fixed height from the board to keep it cool, and you could double insulate the wire with some fiber glass insulation tube or an extra plastic tube.

author: T3sl4co1l
author_rank: Super Contributor
timestamp: September 08, 2023, 08:58:21 pm
content: You may also find it more economical to go to more layers -- less clearance is required on inner layers, and creepage is N/A. 4 x 2oz is a common enough proto spec.Or for a literal one-off, you may find it's effective to just go with plain ass-old perfboard. Pad-per-hole or blank, doesn't really matter, as long as you can fit the components needed, and enough wire size to do it.Also assuming it can't be made somewhat larger, i.e. as panel wiring with socketed relays and wiring between screw terminals.Saying "cost isn't as much of a concern" is peculiar here, as a reasonable 100W controlled Weller/Hakko will cost as much as custom-run PCBs here. Well, I forget offhand how much they're able to pool 3 or 4oz 2-sided boards for pooled proto service, it might not be full-custom price, but it will be somewhat above the default at least.Tim

author: chconnor
author_rank: Contributor
timestamp: September 08, 2023, 09:47:22 pm
content: Thanks for the wisdom, all -- I'll consider using on-board wires, that could be a nice way to solve it... and it's good to be reminded that I can have more than 2 layers. :-)QuoteAh, yeah, it has been a while since I bought a soldering station. They are awfully cheap, aren't they. Do you think a 100W station could handle a 4Oz board OK?

author: sparkydog
author_rank: Regular Contributor
timestamp: September 08, 2023, 10:17:31 pm
content: I have a project (simmering on the back burner) with very similar power requirements (120 VAC at 20 A). I think I calculated that it would need 10oz to safely carry that, which... isdoable, but outrageously expensive, even for a one-off.This is bus bar territory. 🙂 Although I have traces drawn in KiCad, the plan is to take those shapes and have them cut in sheet copper.I'd be curious if other folks think that's a reasonable approach.Note that, in my case, each bus connects to a minimum of seven, and maximum of 12 pins, so the bus really is more of a pour than a trace. If it was just point-to-point, using actualbar, or just 12ga solid copper wire, would probably be fine. OTOH, I'm hoping that having the pins stickingthroughthe bus will help solderability.I wonder if anyone's played with using ring-type terminals on bus wire, and if that would have any impact on how easy or hard it is to solder bus wire to pins...

author: Benta
author_rank: Super Contributor
timestamp: September 08, 2023, 10:28:35 pm
content: 40 W? No problem. 25 W might be an issue.

author: chconnor
author_rank: Contributor
timestamp: September 08, 2023, 11:45:53 pm
content: Quote from: Benta on September 08, 2023, 10:28:35 pmThat's encouraging, thanks! (The 4Oz traces would be on the order of 3-6mm in width, if that changes anything.)

author: Benta
author_rank: Super Contributor
timestamp: September 08, 2023, 11:48:16 pm
content: Quote from: chconnor on September 08, 2023, 11:45:53 pmNope. Easy-peasy. The 25 W would work as well.

author: Wolfram
author_rank: Frequent Contributor
timestamp: September 09, 2023, 12:51:18 am
content: I've been doing over 100 A on 70 µm copper, 4 or 6 layers, without any issues. Using heavier copper tends to be significantly worse in terms of cost and minimum track width and spacing. Using polygon fills rather than traces helps a lot, and also optimizing component placement to shorten the high current paths when possible. For soldering, it's surprising how little power you can get away with as long as you manage to transfer the power to where it's needed, my old Metcal 40 W station with a wide tip has no issues soldering 100 mm^2 busbar to 15 mm copper piping, so high current multilayer boards without thermal reliefs are no issue at all.

author: markietas
author_rank: Newbie
timestamp: September 09, 2023, 02:05:15 am
content: The wattage of the soldering iron is only a small part of how well it will perform for you. A 25 watt cartridge based soldering iron is going to spank the pants off of a 40 or more watt traditional style.In fact I would say that a 65 watt ts100 is considerably more effective than those 250 w chonker soldering gun things.https://youtube.com/watch?v=scvS2yeUH00&si=oZq9FpNTePbs4FnaI do a lot of work with 2 to 6 oz boards and would not ever consider using an old basic 40 weller, it would be a nightmare in most situations.That all being said you probably don't need 4 oz copper for an 11 amp trace, may find a copper fill to be better and easier to route with. Of course you're still going to have a good amount of copper there so I don't think it would be easy with your current soldering iron either way.For reference I recently did a four layer 2 oz per layer board with a bunch of relays and a few DC to DC converters, the biggest currents I'm looking at on that board are 30 to 40 amps but I did need to do fairly wide copper pores on more than one layer to really get the voltage drop and heating low.I Kind of went out of my way to have very good thermal coupling between all the layers and planes because it has to be cooled through conduction from a heat sink on the back side that doesn't contact every part of the board.That board was difficult to solder (for some through hole parts) with a $1,500 240w JCB soldering station.

author: DavidAlfa
author_rank: Super Contributor
timestamp: September 09, 2023, 03:24:12 am
content: 1oz copper, 20mm/0.8" width, 10" long (Exaggerated example) is 7mOhms, drops 70mV and dissipates 0.7W, shouldn't be a problem.Or the power rails like old school, drawing polygons, using the most area possible.Thicker copper / copper rails only needed if space is constrained, a larger board will be much cheaper than 4oz copper!

author: chconnor
author_rank: Contributor
timestamp: September 09, 2023, 04:04:22 am
content: Thanks all!Yeah, space is a major constraint, and the result is that I'm threading a lot of needles re: thermals, clearance, etc.The board is like 4.5 x 4.75" and the high voltage stuff is all on one side. There are six traces that will be carrying the 11A 240VAC, and they all route to a single multi-pin screw terminal connector.I started with 2Oz copper and mid-sized traces before I realized I shouldn't be using IPC-2221B to calculate track widths and IPC-2152 is much more conservative in that regard. So I'm trying to squeeze a lot of current through tight spaces. I like the idea of four layers because I would have tons of room for big filled traces. (I also like the idea of 4Oz 2-layer because it would be a little simpler in some ways, but the 4-layer seems like it might be the more logical route.)Regardless of which i go with, it sounds like I could give the board a go with my old Weller and if it's not working I can just suck it up and get a nice new iron.Side question: there are quite a few places where a (coated) 240VAC track routes underneath other components. I'm sure it's very component-dependent, but is this possibly a rookie mistake?

author: chconnor
author_rank: Contributor
timestamp: September 12, 2023, 04:26:49 am
content: Ok, decided to go with a 4-layer board... outer layers have 2Oz copper (35um) inner two layers have 1.5Oz (53um) (seemed to be the $ sweet spot).As usual I had everything all buttoned up when I realized there was one more option on the Saturn PCB calculator that I had overlooked, specifically the "parallel conductors?" checkbox. :-) So that took some puzzle solving, but I think I've dealt with it by tripling or quadrupling the power traces (meaning, the identical trace is running on multiple layers for extra carrying capacity.)Any reason that's a dumb idea that I might be missing? (I'm thinking I might need that new iron after all if I'm soldering a connector lug through four layers of 1.5/2 Oz copper with 5.5mm traces on each layer...)If not, I think I'm sorted!

author: PCB.Wiz
author_rank: Super Contributor
timestamp: September 12, 2023, 04:40:46 am
content: Quote from: chconnor on September 09, 2023, 04:04:22 amUsing the PCB coating as insulation is certainly marginal.Even using a resistor body as insulation only give you small creepage distances.Quote from: chconnor on September 12, 2023, 04:26:49 amYou can also preheat using a hot air gun

author: chconnor
author_rank: Contributor
timestamp: September 12, 2023, 05:01:37 am
content: Quote from: PCB.Wiz on September 12, 2023, 04:40:46 amGood to know, thanks! -- under the new routing there are only three such crossings, and they are all under components with plastic or potted enclosures (one goes underan SSR, and two go undera snubber). I saw the clearance spec (for category "B4 - External Conductors, with permanent polymer coating (any elevation)") to be 0.8mm. Given the height of the component + the plastic it seemed like I was probably safe on that score. I guess I could always put some tape or conformal coating under the component before soldering, eh?

author: jonpaul
author_rank: Super Contributor
timestamp: September 13, 2023, 03:11:33 am
content: suggest to avoid 3...4 Oz Cu PCBUse std 1 oz Solder coat power traces or add some bus wire on topBest iron for power work is my Metcal Smart heat , designed the SP-200 500 kHz resonant in 1992.J

author: chconnor
author_rank: Contributor
timestamp: September 13, 2023, 04:54:02 am
content: Quote from: jonpaul on September 13, 2023, 03:11:33 amThanks jonpaul -- what do you think of the 2Oz+1.5Oz inner layers, with duplicated traces approach?Are you recommended the coating or bus wire approach because of thermal concerns or because assembly will be a pain?

author: prosper
author_rank: Regular Contributor
timestamp: September 13, 2023, 03:20:13 pm
content: Another vote for bus wires. If it were me, I'd make sure there's no solder mask on the high power traces. Then I'd solder on a fairly thick wire along those traces - still something that would benefit from a better soldering iron, but then again, almost anything would benefit from a better iron. I mean, get some cheap Chinese T12-type iron for $30 bucks, and you'll be way ahead

author: chconnor
author_rank: Contributor
timestamp: September 13, 2023, 06:41:30 pm
content: Thanks prosper -- I am planning to go ahead and get a better iron. Seems like a solid investment.May I ask what it is about the four-layer duplicated-traces method that seems unwise? Is it the ambiguity about thermal dissipation with the power traces on internal layers? Like even though I'm meeting the IPC-2152 numbers I'm still kinda cutting it close, so why not go simpler and just have some burly bus bars or wires to make it a non-issue?Reason I ask is that I have the board all ready to go and was juuuust about to pull the trigger when these last two replies came in. If I'm being dumb I can suck it up and do yet another re-design (don't want to get lost in a sunk cost fallacy) but it seemed like I had finally gotten my head straight about the trace widths, separation, etc., so I was feeling ready to go...

author: jonpaul
author_rank: Super Contributor
timestamp: September 13, 2023, 07:02:50 pm
content: Rebonjour CHConnor:Reading the thread again a moment please.With 55 years experience in power electronics design and mfg, a few notes.0/ Project is one off DIY? Small production? Volume production? Venue USA, EU, UK?00/ Impossible for me to give detailed advise without the schematic, BOM and PCB layout. Reading all this text is a waste to comprehend exactly what you are doing.1/ 240 V mains 11 a current ~ 3 kVA. Safety, fire and transients need to be worst case design.2/ Mains transients are commonly > 1.5 kV and joules of energy (lightning, inductive load switching)All insulation, PCB, transformes must be rated for the required creep and strike gaps in the materials used.3/ At 11 A it is common practice to use very wide traces, like a grd plane flood, to augment wiring with a PCB to wire connector4/ We had directly terminated transformer flying leads eg 22..14 AWG to rectifiers and mains to avoid PCB traces altogether.5/ Soldering: Affected by the parts and PCB cross sec and plating, iron tip dimensions and plating, solder quality and type, as well as iron tip temp, watts.We use only Rosin/Kester 44 flux and 63/37 Eutectic leaded solder.Besides a conventional iron we have extensive use of Weller 100 W soldering guns and Metcal Smartheat SP-2006/ Overheat can damage PCB or delaminate traces.Poor technique, poor qualty PCB, solder, irons can cause cold joints that fail.7/ YOU CANNOT USE PCB SILKSCREEN AS AN INSULATOR ESPEIALLY AT 240V MAINS!!!Use ONLY UL/VDE/TUV/CE rated electrical insulation tapes, coating, bobbins, wires.Bon Chance,Jon

author: chconnor
author_rank: Contributor
timestamp: September 13, 2023, 08:07:41 pm
content: I appreciate the time jonpaul, thanks --Quote from: jonpaul on September 13, 2023, 07:02:50 pmOne-off DIY, USA.QuoteYeah -- it's a board to control power independently to three heating elements in a sauna stove. So it's actually 8kVa over three sets of traces that are 11.1A / 2.67kVA each. I don't want to be an idiot, so I appreciate all the cautions.QuoteAh, gotcha. I've been spacing and rating based on the 340V peak AC voltage, but I have not been accounting for mains spikes of >1.5kV... I do have 12.5 fast fuses on each of the three legs, and snubber RCs on them as well (peak pulse 1kV), but I didn't lay out the traces with 1.5kV in mind.QuoteI also use Kester 44 63/37.I know this may not be helpful because you don't have all the details, but just in case -- here are images of the high voltage side of the board as it stands:top (2Oz)inner layers (both 1.5Oz)bottom (2Oz)composite...the fat traces there are 5.5-6.5mm. Only about half of the fat paths are really carrying the 11A continuously, though -- the others are just oversized.(Also, a contactor breaks L1 and L2 to the board most of the time. Only when the stove is operating would they see any voltage.)I'm not expecting anyone to do a deep analysis of the board, here, I know that's my job, I just post that in case anyone looks at it and says "oh no, you're insane". :-)

author: sparkydog
author_rank: Regular Contributor
timestamp: September 13, 2023, 09:05:10 pm
content: Have you paid attention to your creepage requirements? If you're actually following IEC 62368-1 for 1500V, yourbest casecreepage is 5.6 mm. I don't know how much creepage your board actually has, but I can tell that yourpin pitchis less than 5 mm...That said, I question whether that's actually followed for real products, as there are very few components that are evencapableof meeting that, and for that matter, I'm almost certain your mains wiring is nowhere near ensuring that.Creepage for 250V is 0.56 mm if your board is sealed against dust and condensation, up to 4 mm if it isn't.

author: chconnor
author_rank: Contributor
timestamp: September 14, 2023, 12:03:27 am
content: Thanks sparkydog --Quote from: sparkydog on September 13, 2023, 09:05:10 pmYes, but only for 240VAC (340V peak). And I was working with IPC-2221B (only because the Saturn PCB calc didn't use 62368-1 and I didn't yet understand the difference.) Having looked into it, I think I'm good for 240VAC even with 62368-1, but I assume I'm not OK in terms of 1.5kV.It seems hard to find clear calculators for 62368-1 (presumably professionals just have the spec itself and don't need to use them). I've found a few, e.g.thisandthis(my understanding is that UL60950 and IEC 62368-1:2023 match up to 30kHz), but they aren't clear (to me) re: internal vs external layers, how to handle coated vs uncoated traces, etc.QuoteIn this context does "sealed" include internal layers and top/bottom traces under solder mask? If so, I meet both of those (well, after resetting the pad sizes on the connector to the factory size).But it seems clear that there is no way I'm going to wiggle this design to be able to sustain 1.5kV spikes without a big redesign unless there is some simple protection I can add -- e.g. could I just slap some 350V gas discharge tubes near the connector?

author: jonpaul
author_rank: Super Contributor
timestamp: September 14, 2023, 07:30:30 am
content: For 240 V heater contrils:1/ No PCB needed, as industrial relays or contactors or SSRs all have 1/4' AMP tabls or screww terminals for direct wiring.2/ If you want CPU/digital controluse the PCB ONLY for control,for the controller>>relay driver>>realy/contactor coils240V 11 A power. >>cheater use point to point wiring.Or DIN railJon

author: sparkydog
author_rank: Regular Contributor
timestamp: September 14, 2023, 07:41:51 pm
content: Quote from: chconnor on September 14, 2023, 12:03:27 amYeah, I was confused about this, too, so Iasked. IIUC, you only need to spec for kV if you're trying to design your board to actually withstand a lightning strike. Otherwise, you just need to insulate the project as a whole, so that a spike won't arc over and kill a person that happens to be near it.OTOH,clearancemay be 3 mm, and you don't get the really small creepage unless you can assert that you're Pollution Group 1.Quote from: chconnor on September 14, 2023, 12:03:27 amIthinkthe requirements are the same, at least for your usage. That said, you can at least check thedraft. (I really, really hate standards organizations that charge you an arm and a leg for a standard youhaveto follow,especiallyfor safety standards. There ought to be laws against that.)Quote from: chconnor on September 14, 2023, 12:03:27 amUnclear, but my guess would be that it doesn't matter, or rather, at best you can add the layer thickness to your actual creepage.

author: prosper
author_rank: Regular Contributor
timestamp: September 14, 2023, 08:19:05 pm
content: Quote from: chconnor on September 13, 2023, 06:41:30 pmJust personal preference. I like to avoid 4-layer designs if I can (i.e. for simple circuits). Unnecessary cost and harder to bodge / prototype on. Plus, as you noted, buried traces have more complex thermal characteristics to consider. Busbars are just simpler and cheaper.

author: chconnor
author_rank: Contributor
timestamp: September 15, 2023, 01:22:25 am
content: Thanks! Very interesting reading. I don't envy professionals that need to thoroughly understand that spec, but I do respect them. :-)I'm a little surprised that 62368 doesn't seem to distinguish at all between internal/external layers, and between coated/uncoated traces. I can believe that at 240VAC you can't trust the solder mask to be rated to isolate that voltage from direct contact, but it seems like it should be relevant to trace separation, at least a little. And surely internal traces buried in the board should have milder requirements? I'm also remembering the drastic differences that internal/coated/uncoated are granted under 2221B (0.25mm, 0.8mm, and 2.5mm, respectively. That said, I suppose 2221B is obsolete for some good reasons.)As you noted, maintaining 4mm everywhere on the board, whether internal/external/coated/uncoated or pins is going to be tough... e.g. the connector pin pad edges are 4.3mm apart, so a trace of any significant width is going to bring that under 4mm. I'm using anHCPL3700MIC which feeds what for me peaks at 170V (rectified 120VAC) out to two pins that by 62368 are supposed to be 2mm apart (bare minimum 1.4mm at the most relaxed) but those pad edges are ~1.3mm apart (before a trace is even involved.) And that IC is rated for 240VAC as well... Seems like either I'm not understanding 62368 yet or they assume you will conformally coat if using ≥120VAC?At any rate, my current plan, submitted for comment by anyone gracious enough to spare this newbie any more time:- expose areas at the ends of the power traces- solder appropriate-gauge coated wire to double those traces to act as additional current path (insulated and rated to appropriate voltage). (AKA bodge wires, but, you know, nice ones. :-) )- remove power traces from the top layer (now that they are reinforced with the wires, and already doubled or tripled on the other layers, might as well not have the HV near the components on the top)- conformally coat the bottom of the board on the high voltage side of the PCB- add some high voltage transient suppression for the L1/L2/N feeding the stove (in the hopes of preventing high voltage spikes from even reaching the PCB, and allowing me to escape needing 6, 8mm clearances, etc.) (still researching details on this; e.g. not sure ifthis kind of thingwill suffice.)

author: uer166
author_rank: Super Contributor
timestamp: September 15, 2023, 01:32:12 am
content: For traces buried in PCB, you're looking for a term called "cemented joint" in UL-world. I'm not sure about that IEC standard since I'm not familiar with it, but generally internal traces are handled very differently, and spacings can be much smaller given a few conditions are met.Maybe search for "solid insulation" as well.

author: chconnor
author_rank: Contributor
timestamp: September 15, 2023, 02:00:21 am
content: Thanks -- I did see "solid insulation" in the draft 62368, and I'll check for "cemented joint" as well.