55A PCB - To many stiching vias? - Page 1
Forum section: electronics / general

author: lou6366
author_rank: Newbie
timestamp: September 13, 2025, 11:23:00 am
content: I'm designing a pcb (4oz copper) that will carry 55A at 12v across it. Power (+12V_PSU) comes in from a through hole connector (Top Layer) well rated for that amount and then it connects to a solid power plane at the bottom (hand solder). I ran the Altium Keysight power analyzer and it was flagging the through vias for the connector pins as having to much current. So I added a bunch of stitching vias from the top layer to the bottom layer to make it happy, but is this to many stitching vias? and is the Keysight power analyzer not taking into account the current capacity of the pins of the connector to the bottom layer?Thank you

author: nctnico
author_rank: Super Contributor
timestamp: September 13, 2025, 12:23:27 pm
content: I'd add thermal reliefs to the pads. Otherwise you can't get it soldered with a soldering iron. However, having only 3 holes for 55A of current seems a bit low. And what do you mean by 'well rated for 55A'? From what I've seen derating by 50% to 60% is a good idea for real world applications of connectors. Current handling capacity is specified at 25 degrees with only1pin of the connector carrying the specified current.

author: wraper
author_rank: Unknown
timestamp: September 13, 2025, 12:26:10 pm
content: QuoteSounds like it calculates as if it was a normal via transferring current from one side to another, not a connector with pins going thorough the holes. As of vias placed like this, I would not place them in lines with a short distance between the vias as it weakens the board and possibly creates a precursor to a crack formation, and would rather distribute vias evenly. In chess board order if I deeded them dense.

author: lou6366
author_rank: Newbie
timestamp: September 13, 2025, 12:46:16 pm
content: The connector (Phoenix contact P/N: 1333823 ), but quick question is it safe to take into account that the through hole pin will carry most of the current and not the vias that its in?

author: Psi
author_rank: Super Contributor
timestamp: September 13, 2025, 12:51:32 pm
content: What size are those stitching vias?I would avoid 0.2mm. Use 0.3 - 0.5mm if the goal is current flow.I'd probably go with 0.5mm on a 4oz board personally.Also keep in mind that thicker copper means you can't have thin tracks/spacing.Some components/ICs with fine pitch pins/pads are not possible on 4oz copper.For 4oz keep any gap/track more than 14mil or 0.3556mm, so ICs with 0.6mm pitch pads/pins are out.I cant see the rest of your PCB so you may not have anything that would be a problem, but just FYI

author: Psi
author_rank: Super Contributor
timestamp: September 13, 2025, 01:11:13 pm
content: Quote from: lou6366 on September 13, 2025, 12:46:16 pmAs long as it gets soldered correctly and is DC yes, the solder will link the two pieces of copper together (the pin shaft and the via) and they will share the current.More current will go through whatever has the lowest resistance (thicker copper). So the pin in this case will take a much larger percentage because it's much thicker than the plating thickness inside the via.But if the connector pin is not soldered correctly, ie. all the solder is on one side and doesnt wick through, then the via may take all the current for a short distance which can be an issue. Bad soldering is more likely to happen when your PCB has lots of thick copper because it becomes hard to get the via up to solder temp all the way through. Especially when hand soldering. This is why having thermal relief via's on the connector pins is important.

author: PGPG
author_rank: Frequent Contributor
timestamp: September 13, 2025, 01:42:53 pm
content: Quote from: nctnico on September 13, 2025, 12:23:27 pmI have no experience with high currents (in my designs 1A is 'huge' current) but using reliefs seems for me not the best idea if you consider 55A.Quote from: nctnico on September 13, 2025, 12:23:27 pmI suppose I would have no problem with soldering it.I am using (have bought it in 1980) 100W trafo (gun) soldering iron. Using it I can solder two 4mm2 wires together and I also use it (with second soldering iron) when desoldering 0603.

author: Psi
author_rank: Super Contributor
timestamp: September 13, 2025, 01:55:28 pm
content: It's mostly about the heat that will be generated which comes from the voltage drop. Normally with thermal relief the distance that has to carry the full current is tiny and spread across 4 entry points, and there's plenty of copper each side to pull any heat away.So the thermal relief can handle more amps than you think, but yes in some cases you have no choice but to leave off any thermal relief.If you're the one who will solder it, and you will make sure the solder goes all the way through, then that's fine.But if you expect someone else to make the boards for you then you might have issues unless you specify that they must solder from both sides of the PCB.But in general thick copper boards can really be a pain to solder even with a high powered iron unless you use a preheater.

author: nctnico
author_rank: Super Contributor
timestamp: September 13, 2025, 05:13:42 pm
content: Quote from: PGPG on September 13, 2025, 01:42:53 pmYou are severely underestimating the ability of large copper areas to take heat away from a solder joint. Try replacing capacitors on an old PC motherboard and you'll quickly notice that your soldering iron won't be up to the task.

author: tooki
author_rank: Super Contributor
timestamp: September 13, 2025, 09:26:59 pm
content: Quote from: PGPG on September 13, 2025, 01:42:53 pmI concur that you may be underestimating the power needed to solder this. Especially if any of the pins are connected to a top-layer plane and not to the bottom, which means a massive heatsink on the “far side” of the board. If this is the case, your pads are WAY too small IMHO, especially for hand-soldering.I would use generous preheating and some extra flux. (Ideally, you’d heat the board up to, say, 100-150C in an oven for several minutes to get it really nice and hot all the way through.)

author: PGPG
author_rank: Frequent Contributor
timestamp: September 13, 2025, 11:34:06 pm
content: Quote from: nctnico on September 13, 2025, 05:13:42 pmQuote from: tooki on September 13, 2025, 09:26:59 pmI'm inclined to think you're both right, as the PCB mentioned here is 4oz and I have never had such in my hands.My experience is that trafo (gun) soldering iron heats up its tip so fast that in normal use you should never switch it on for longer then 3s because, due to too high a temperature, the tin immediately oxidizes.The problem with capacitors in PC motherboards is to heat its both ends at once, because if you heat first and then try to heat second the first gets cold in a split second.During years I have done several specialized tips (wire in specified shape) to my iron. I have for example a tip that heats all SO8 pads. I have also 'U' shape tips allowing to heat everything along its flat bottom of 'U' part. One can be used to heat both electrolytic capacitor pins at once, other I used to cut the backpack strap without leaving any frayed fibers.

author: Smokey
author_rank: Super Contributor
timestamp: September 14, 2025, 06:04:31 am
content: To bring together two ideas here that have already been stated...If you don't add thermal relief (spokes) to those through hole pads they will not only be impossible to solder, but because the solder won't wick all the way through the hole and flow from the bottom to the top layer, so you will only be conducting through the hole plating, not the pin. All those stitching vias will help bring the current from the bottom to the top through.With the general rule of thumb of 2A/via, you would only need about 28 vias to bring 55A from the bottom to the top, even if you didn't have any conduction through the pin.

author: tooki
author_rank: Super Contributor
timestamp: September 14, 2025, 05:07:50 pm
content: My concern with thermal relief spokes is this: wouldn’t they significantly reduce the current capability that is the whole point of this exercise?

author: nctnico
author_rank: Super Contributor
timestamp: September 14, 2025, 07:05:43 pm
content: Those spokes are so short they don't add significant resistance. I have not looked into it but there are probably formulas to be found for calculating thermal reliefs versus current handling. What I do know is that having no thermal reliefs makes the board harder to produce and to repair.

author: Smokey
author_rank: Super Contributor
timestamp: September 14, 2025, 09:06:53 pm
content: The soldering iron is a huge thermal impulse. If you had that big of a thermal impulse from actual current it would have already vaporized some other part of the system.Thermal time constants of normal operation are really really long. The heat typically has plenty of time to get through the spokes and spread over the rest of the plane (assuming your plane is sufficient).

author: Psi
author_rank: Super Contributor
timestamp: September 15, 2025, 12:16:39 am
content: Quote from: tooki on September 14, 2025, 05:07:50 pmThere's no such thing as reducing current capability. The same current will flow through it, you just lose voltage across it which becomes heat.It might be so hot that it's almost on fire and dropping 3 volts across the reduced width thermal relief copper area but the same 55A will be flowing through it.For thermal relief the heat is less of an issue because there's a huge copper plane on one side and a pin on the other. So the heat can get away easily.There's also not much heat because the length is short. So the main thing to worry about is voltage drop.Do you care if you have 12V on one side of the thermal via and 11.98V on the other? (you'll have to do the math to see what that Vdrop actually is based on the total width and thickness of your copper, I just made up those numbers.)If it's via stitching for current flow, yeah no need for thermal relief.If it's for a through-hole wire/part, think very carefully before choosing not to do thermal relief.Are you trying to put 55A into a single connector pin? or multiple, or is it a huge pin?

author: thm_w
author_rank: Super Contributor
timestamp: September 15, 2025, 08:54:37 pm
content: https://www.eevblog.com/forum/beginners/how-much-current-can-thermal-reliefs-handle/Be cautious with reliefs at these high currents IF you expect high inrush and are pushing things to their limits (see nvidia). In this case the connector is reasonably well specced it seems:https://www.phoenixcontact.com/en-us/products/pcb-terminal-block-lpta-16-6-100-zb-1333823?type=pdfI would make the annular ring on the solder pad way larger though, I'm not sure why you've made it that tiny.Quote from: Psi on September 13, 2025, 01:11:13 pmIf OP is soldering it then yeah can say that, if its manufactured then they'd need to go based off of IPC.Class 2 is only 75% fill, so you'd need to explicitly call it out or go for some higher spec:https://www.nextpcb.com/blog/ipc-class-2-vs-3-the-differences-in-pcb-ipc-standards

author: tszaboo
author_rank: Super Contributor
timestamp: September 15, 2025, 11:29:10 pm
content: Quote from: nctnico on September 14, 2025, 07:05:43 pmThe heat carrying capacity of metals is equivalent to their current carrying capacity. It's quite remarkable.So if something doesn't carry the heat away, it will not carry the current.The solution is Metcal soldering irons.

author: tooki
author_rank: Super Contributor
timestamp: September 16, 2025, 07:12:05 am
content: Quote from: Psi on September 15, 2025, 12:16:39 amWhen we talk about the current capability of a conductor, unless otherwise specified we implicitly mean “while maintaining normal design requirements”, such as not self-destructing or causing malfunction.If that weren’t true we would not need PCB trace calculators, ampacity charts, etc.

author: Psi
author_rank: Super Contributor
timestamp: September 16, 2025, 10:56:14 am
content: Quote from: tooki on September 16, 2025, 07:12:05 amSorry, i misread that post. Thought it was a post from OP.

author: temperance
author_rank: Super Contributor
timestamp: September 16, 2025, 11:47:00 am
content: QuoteThe thermal conductivity of metals is inversely proportional to it's ohmic resistance and a property of materials where the carriers of heat and electric current are free electrons.

author: Psi
author_rank: Super Contributor
timestamp: September 16, 2025, 11:55:37 am
content: It would actually make a cool video to get a typical 1 or 2oz pcb made up with a selection of sizes of thermal relief through-holes.Then use a thermal camera and pump current through them one at a time to see just how hot they get.Could test, a component like a TH resistor, vs a large wire to board connection which has more heatsinking through and down the wire.Its easy to calculate how many watts they will burn off an the Vdrop, but pretty hard to know how hot they will get.

author: temperance
author_rank: Super Contributor
timestamp: September 16, 2025, 12:03:47 pm
content: Back to the original question:What is the plating thickness on the sharp edges where a plane and a plated hole connect? I always suspected the plating thickness to be less on those sharp edges.Some googling around:https://www.electronics.org/system/files/technical_resource/E9%26S33_02.pdf"Copper dissolution and erosion at the PTH knee can be a serious reliability issue if there is not enough copper left after wavesolder and mini-pot rework. This issue is exacerbated for thick boards with many copper planes, such as server boards. Previousstudies [2-4] have shown when the copper at the PTH knee goes below 0.5 mils (12.7 μm) cracks will form after temperaturecycling and possibly result in electrical opens at the solder joint."For high power connections, I like to place vias for two reasons:-The plating thickness on the knees varies.-You don't know if a proper solder fillet is being formed at the top side of the board. This is difficult to inspect and there are too many variables at play. When soldering by hand without preheating the board, the solder fillet on the top side will be very poor or non existent.For the placement of the vias you can create pads incorporating the vias into the pad.

author: Psi
author_rank: Super Contributor
timestamp: September 16, 2025, 12:09:14 pm
content: Yes, when it comes to high currents, more vias is always better. Well... until your PCB house complains and charges you more, or your PCB becomes one huge criss cross of break-away lines and it snaps in half when you flex itThe weak-ness thing is usually why you often seeX X XX XX X Xinstead ofX X XX X XX X X

author: temperance
author_rank: Super Contributor
timestamp: September 16, 2025, 12:40:12 pm
content: QuoteOr the plane resistance goes up because of too many stitching vias.