Some doubts with a 50A PCB Design - Page 1
Forum section: electronics / projects

author: D.Kruger
author_rank: Contributor
timestamp: February 04, 2021, 08:44:30 am
content: Hi everyone, I'm designing a 2 layer board to measure current in solar panel arrays, on rooftops, not roadwaysThe board has 4 straight tracks with a shunt resistor in the middle of each track and vias connected to the shunt's footprint to do guide the tracks on the bottom layer and do de measurement (4 Wire measurement). Each track needs to manage up to 50 amps. The distribution should look similar to this:To select the trace width and thickness I am using Saturn PCB toolkit, for 20mm conductor with and 60mm length with a 1.6mm board and a plane in the bottom side I need at least 3oz of copper with 0.5oz plating to handle 50A (50.6A is the calculus in Saturn).I have seen that the conduction capacity is reduced largely if parallel conductors are added, if I put a board cutout between the tracks, should I consider them as parallel conductors for the calculation?Finally, to get some ideas I have teardown a solar inverter that handles 50A. This board seems to be 1.6mm, 2 layer and not more than 2oz of copper. The tracks are 20mm and the cables for the solar panels are soldered into the PCB. Isn't this to close to the limit to manage the 50A reliably?Thanks in advance for your help, It's my first time designing a board for such I high current and I don't want to mess it up.

author: Miyuki
author_rank: Frequent Contributor
timestamp: February 04, 2021, 09:34:48 am
content: It all depends just on losses you want to acceptYou can pass an insane amount of current with tiny tracesEven if you pass so much current to have like +60K temperature rise on traces nothing really happens

author: penfold
author_rank: Frequent Contributor
timestamp: February 04, 2021, 10:36:01 am
content: Adding slots between the traces will prevent the heat from nearby traces contributing to the temperature rise of any single one leading Saturn to give you a more preferable answer... but will also limit the thermal mass that any trace can diffuse its heat into. Without doing the maths, I would tend to err on the side of no slots, but allow your traces to get an extra 5 or 10 kelvin hotter at full load (how often do you anticipate actually getting a full 50A per trace and have you factored in a bit of overhead allowance?)Are you intending this to be part of a commercial product or something for experimentation? Are you using a cooling fan elsewhere nearbyThe commercial board will almost without doubt not be designed to handle 50A continuously at all worst case scenarios, and those solder 'ribs' will go some why in increasing the current handling by giving the trace a little more surface area not covered by solder resist and a little more thermal mass and mechanical bulk to the copper foil so that its less likely to end to de-laminate.

author: richard.cs
author_rank: Super Contributor
timestamp: February 04, 2021, 10:59:27 am
content: Be careful, the sense resistor will also contribute to the heating of the tracks. Is that a 500 uOhm? If so that's an extra 1.25 W that will mostly go into the adjacent copper.

author: Berni
author_rank: Super Contributor
timestamp: February 04, 2021, 11:14:49 am
content: Yep 50A gets things nicely toasty on boards.Its more a question of how hot are you okay with. Even the thickest of traces have enough resistance to heat up at these currents while heat in the shunt resistors in unavoidable, so part of it is giving the heat somewhere to go.When you have thick wires coming in then you can use those wires are heatsinks to move heat away. The enclosure around the board is also important. If its a small tightly sealed plastic box things might get much hotter inside compared to just running it in open air on your bench.It is a good idea to test these things by hooking it up to a massive power supply and seeing just how hot it gets in practice. If you don't have a big enugh power supply you can improvise a high current source out of a toroidal transofmrer and some thick cable. Get some thick 50mm2 cable and give it 2 or 3 turns trough the middle of a toroidal transformer. This creates a extra secondary coil on it for outputting ~1VAC at ~100A. You can then control it by powering the transformer from a variac and monitoring the current using a current clamp meter.

author: Siwastaja
author_rank: Super Contributor
timestamp: February 04, 2021, 11:38:02 am
content: Trace width calculators assume infinitely long traces. Because power electronics PCBs are almost never designed with long traces, this is not very useful.Very short traces work better because the connectors, component leads etc. work as heatsinks.When you approach zero length, trace width is removed from the equation, and you can just use component ratings. Do note though that components are rated in isolation, if you have two sources closely coupled you need to derate both.In practical PCB design, you can't go to zero length but can often get surprisingly close, i.e., "half square" design is often possible, for example meaning connecting a 1mm wide component leg to another 1mm wide component leg with just 0.5mm of connecting track. Half a square always has the resistance of 0.25 mOhm with 1oz copper or 0.125mOhm with 2oz, meaning that at 50A and 2oz copper, only a tad over 300mW is dissipated, similar to what 0603 thick film power resistors are rated at.A 4-layer board helps a lot, and I don't mean by paralleling traces to all 4 layers, but simply because the ground place acts as a heatsink smoothing out those hotspots caused by small connecting tracks.But in general, remember to think in terms of aspect ratios, it's more powerful mindset than plugging in track widths and lengths in a calculator! With 2oz copper, 1:1 aspect ratio is 0.25mOhm. Count parallel / series squares.

author: Renate
author_rank: Super Contributor
timestamp: February 04, 2021, 11:58:50 am
content: If all you're doing is measuring, the current is 50 A and it's coming in on cables, it's much better to just use an off-board shunt designed for this.

author: Siwastaja
author_rank: Super Contributor
timestamp: February 04, 2021, 12:07:24 pm
content: Referring to the picture, mentally move the banana plugs closer to the shunt. Do not shorten the tracks. Now the dissipation is reduced, but the heatsinking capability of the tracks stays. I.e., fill the area with copper, extend the fills beyond the current-carrying part.50A is often fine without much special tricks, length minimization and copper area maximization works out. Much beyond that, you tend to need to order either super-thick copper (like 4oz or even 6oz); sometimes it's cheaper, especially for small batches, to expose solder and paste masks, cut some 0.1mm to 0.3mm copper sheet to shape (scissors will do fine), and reflow it on the top of the tracks. You can even bend the copper to L or U shape, acting as a heatsink.

author: voltsandjolts
author_rank: Unknown
timestamp: February 04, 2021, 12:51:52 pm
content: The OP might also want to consider using hall effect current sensors which provide galvanic isolation.e.g.https://www.melexis.com/en/product/MLX91220/0-50A-isolated-5V-integrated-hall-current-sensor

author: D.Kruger
author_rank: Contributor
timestamp: February 04, 2021, 04:14:02 pm
content: Thanks a lot for the answers, I've done this draft to explain myself better.Quote from: penfold on February 04, 2021, 10:36:01 amThe project is going to be part of a commercial product. This is why I'm worried about reliability.The PCB will be attached to a DIN Rail next to circuit breaker, switches, etc. The rail will be inside of a plastics case without any active ventilation.The space limitation and ease of installation on the rail is the reason why I opted for a PCB with SMD shunts over external shunts, in some installations will be 2 or 3 board next to each other in the rail. Also, the client doesn't want to use Hall effect sensors.Generally the current will be around 30A for 4 or 5 hours a day but, the client may install the board to panel arrays that could reach 50A during 4 or 5 hours in Summer so, I want to be sure that the design is ready for this conditions.

author: D.Kruger
author_rank: Contributor
timestamp: February 04, 2021, 04:27:35 pm
content: Quote from: Siwastaja on February 04, 2021, 11:38:02 amThanks a lot for the explanation, it's helped me to think the problem in a different way.One thing I have consider is using a PCB with Aluminum core to ensure enough heat dissipation, I guess this will be even better than the 4 layer board, Am I right?

author: D.Kruger
author_rank: Contributor
timestamp: February 04, 2021, 04:32:46 pm
content: Quote from: voltsandjolts on February 04, 2021, 12:51:52 pmHi, unfortunately the client specified that he wants a shunt, not a hall sensor

author: penfold
author_rank: Frequent Contributor
timestamp: February 04, 2021, 04:46:26 pm
content: From your attached PCB layer shots... a couple of things I can't help but mention (but feel free to ignore if you've just not finished yet)The holes for your terminals have thermal reliefs when it should really be solidYou could replicate the same high current traces on the bottom layer and put plenty of vias to stitch them together (maybe have them solder filled for additional thermal mass),You could expand the traces outwards a bit unless you really need that surrounding flooded areaThe sense lines could also be a little thicker (just relatively speaking, I can't quite gauge the scale of it) and using multiple vias could help with reliability (repeated thermal cycles tend to make unfilled vias crack)If you're still concerned about power dissipation, but not enough to go for metal-clad boards, then it is possible to bolt a standard FR4 board to a heatsink so long as you have an even pressure and a compliant gap pad... it shouldn't be a preferred option, but its an option none the less

author: nctnico
author_rank: Super Contributor
timestamp: February 04, 2021, 05:07:02 pm
content: Quote from: D.Kruger on February 04, 2021, 04:32:46 pmHow precise does this shunt need to be? In the past I have used current sensing across PCB traces and an NTC temperature sensor to be able to compensate for the temperature effects of conductivity of copper.

author: Renate
author_rank: Super Contributor
timestamp: February 04, 2021, 07:09:43 pm
content: I'm kinda amazed.Despite being an Ami I'm a fan of DIN rail stuff.Looking around I can not find any 4 terminal DIN rail current shunts.(Ok, somebody offers a 0.1 Ohm crappy PCB shunt.)That seems to me a natural.Maybe it's a marketing hole.At least with a shunt, you're probably surer of the direction of the current at low values than with a Hall effect.Full disclosure: This post was delivered over a DIN rail.

author: D.Kruger
author_rank: Contributor
timestamp: February 05, 2021, 07:58:08 am
content: Quote from: penfold on February 04, 2021, 04:46:26 pmHi, thanks for the tips, the PCB from the shots isn't the board itself, it was just a fast design to show the component layout distribution and dimensions.I think I may ended up with a metal clad board, seems the best option.One last question, so you know of any good book or website to learn more about high current PCB design? I've looked around and couldn't find anything

author: T3sl4co1l
author_rank: Super Contributor
timestamp: February 05, 2021, 08:15:15 am
content: What's wrong with this kind?https://www.digikey.com/en/products/detail/murata-power-solutions-inc/3020-01096-0/1926137Has its own board, and hardware, just mount a few to a DIN bracket.Tim

author: D.Kruger
author_rank: Contributor
timestamp: February 05, 2021, 08:41:53 am
content: Quote from: nctnico on February 04, 2021, 05:07:02 pmPrecision under 1% would be ideal, but not 100% sure of which precision I can reached, because, as I said, I'm quite new with high current design

author: D.Kruger
author_rank: Contributor
timestamp: February 05, 2021, 08:46:05 am
content: Quote from: T3sl4co1l on February 05, 2021, 08:15:15 amThat would solve a lot of my problems, but it's too expensive, the product will have between 4 to 16 shunts

author: gnuarm
author_rank: Super Contributor
timestamp: February 05, 2021, 09:11:02 am
content: Quote from: penfold on February 04, 2021, 10:36:01 amI'm sure the solder ribs add to the conductivity of the traces, but I saw a report once that showed solder mask does not reduce the emissivity and in fact increases it. So there are competing effects, the improved emissivity with the solder mask and the improved electrical conduction of the solder ribs.

author: penfold
author_rank: Frequent Contributor
timestamp: February 05, 2021, 12:48:05 pm
content: Quote from: gnuarm on February 05, 2021, 09:11:02 amNeither of those is something that actually measured in practice, what sort of level would you suggest the solder improved the conductivity?With regard to emissivity of the surface, especially for this sort of thermal stuff I would be heavily critical of taking advice from "reports", unless they did their measurements using an identical board and enclosure to mine. I took an assumption that there's probably a fan in the commercial unit, in which case the main heat transfer mechanism probably isn't radiative, can also be the case when a board is housed in a metal box and the IR just reflects right back at the board.Quote from: D.Kruger on February 05, 2021, 07:58:08 amI've honestly never found a good text book reference for PCB thermals specifically and I rarely can ever find any application notes about anything sufficiently similar to what I've been doing. (I'm hoping somebody jumps in with some useful reading!).In my experience, especially with "power dense" designs, there's just nothing which can substitute for a good prototype and good measurements, approximations work much better when you're only trying to control one hotspot on a board, things get far less predictable when 90% of the board area is the hotspot.

author: gnuarm
author_rank: Super Contributor
timestamp: February 05, 2021, 06:21:44 pm
content: Quote from: penfold on February 05, 2021, 12:48:05 pmOf course, the conductivity of the solder depends on the exact composition and the thickness, but clearly the solder ismuchthicker than the copper trace which is only a few (very few) thousandths of an inch while the solder is mm (plural). Are you suggesting the solder does not significantly reduce the resistance of the traces? I did some quick calculations to find about a quarter mm of solder is equal to 1 oz of copper. How many mm thick do you think the solder ribs are in the images?QuoteOk, fair enough. My intended point was that it is often discussed that the solder mask is a resistance to heat flow by virtue of it being an "insulator" while the reality is the thinness of the layer means it has virtually no resistance to heat flow. Perhaps if a heat sink was being attached you would not want the solder mask, but otherwise it's nothing worth considering. No need to strip the solder mask off to gain thermal contact to air.

author: Siwastaja
author_rank: Super Contributor
timestamp: February 05, 2021, 06:35:12 pm
content: Adding solder to trace is a proven hence widely measured solution, IIRC Dave did a video about it. It does work, but doesn't do wonders.Roughly speaking, solder has about 1/10th of conductivity of the copper, but the typical solder thickness in a reflow or wave solder is around 5 times the thickness of the copper track (35 um vs. some 100-250 um). Also you realistically can't get 100% fill rate, you need to add solder mask to section the solder so it doesn't form a massive blob somewhere due to gravity.As a result of all this, a properly done solder opening on a track reduces the 1oz track resistance by some 20-30%.If you use 2oz copper, the relative effect is already smaller.With an iron, you can manually add thicker solder layer but this is relatively lot of work. Why not solder in some copper wire while at it?

author: schratterulrich
author_rank: Regular Contributor
timestamp: February 05, 2021, 07:59:57 pm
content: Your design would be a perfect use case for my software. I have written it for personal use, but maybe it could help someone else, too.https://leiterplatte.jimdo.com/thermal-pcb-sim/Although the result will probably be some way off the measurement results of a real board, it can certainly help in deciding how best to lay out the track.-You will see that a mirrored current carrying trace on the bottom will help more than a solid ground plane.-You will see that 4 traces 50A each needs the width calculation of one trace carrying 200A. And this is a huge difference.The operation of the software is probably very cumbersome for others,... This is the drawback.I have made a quick estimation of the layout in your screenshots. It shows a temperature rise of ~160°C.Why should a metal-clad board help?In my understanding the metal helps to distribute the heat from a small package like a LED.But it cannot dissipate more heat on its own than FR-4. It can only transport the heat.

author: Renate
author_rank: Super Contributor
timestamp: February 05, 2021, 08:08:29 pm
content: What we should take away from all this?Keep any resistance to the absolute minimum that will give us (almost) enough resolution.Use inherent resistance where you can: cable runs, fuses.Consider not running huge currents on PCBs when they don't originate there.

author: penfold
author_rank: Frequent Contributor
timestamp: February 05, 2021, 08:47:21 pm
content: QuoteI'm not debating whether or not it can be an effective option, just that it can have very marginal benefits in some applications, just that from those images and what I have experience of I cannot begin to speculate as to its effectiveness in that exact application. It certainly isn't as simple as considering the bulk resistance of solder in parallel with the copper as its a 3d structure with resistance vertically also, so its more equivalent to a load of stacked ladder networks and additional height won't just linearly decrease the total resistance and that height will be determined by the relative resistivities and length/width of the trace, so genuinely asking if you were aware of the possible advantages for any of the examples in this post

author: T3sl4co1l
author_rank: Super Contributor
timestamp: February 05, 2021, 10:31:05 pm
content: BTW, there are solid metal jumpers, 0-ohm resistors, and SMT pads that can all be used for increasing thickness, without ponying up for the heavy-copper PCB. Though you'll probably find, after BOM and assembly costs, the PCB is the cheaper option anyway.And don't discount multilayer boards. More expensive than 2-layer, sure; same heatsinking area; but with stitching vias, there's much more copper to get involved.Tim

author: ajb
author_rank: Super Contributor
timestamp: February 05, 2021, 11:18:26 pm
content: If you want to play around, Fusion 360 can do thermal simulations for a fairly low price (or free for hobbyists/small enough businesses). It would be a little annoying to get a board layout any more complicated than what you've drawn modeled up (maybe they've added this capability with the Eagle integration, I haven't looked, but that also requires you to create the PCB in what is effectively Eagle, so take that for what it's worth). But it comes with the advantage of being able to simulate the whole mechanical assembly if you want. I haven't played with it much so I'm not sure how much work it takes to get accurate results out of it, but simulation like this is FAR more accessible now than it would have been even five years ago.

author: nctnico
author_rank: Super Contributor
timestamp: February 06, 2021, 01:05:54 am
content: Quote from: D.Kruger on February 05, 2021, 08:41:53 amWell, when using the PCB traces you'd need a temperature sensor and some logic (microcontroller with ADC and lookup tables) as well. Based on the images you posted I don't think your layout will be a problem IF you use a double sided 2oz (60um) board but the dissipation in the shunts and getting the current into and from the PCB wil become a problem. At 50A a 5 milli-Ohm shunt is going to dissipate 12.5W. Your SMT style shunts are not going to handle that. Even a 1 milli-Ohm shunt will dissipate 2.5W. I think hal sensors or trace sensing (with temperature compensation) are a better approaches at these currents.And then there is getting the current into and from the board. When it comes to high currents I like to use screw terminals with multiple holes to spread the current over more than 1 PCB hole. After all tin has a relatively high resistance. Wurth has these kind of terminals:https://www.we-online.de/katalog/en/WP-THRBU_BLIND_HOLEThe M4 and M5 ones are rated for 85A at 20 degrees. But don't expect these to work at 85A. A 50% derating is a good idea which makes a single one barely suitable for your project.Wurth has other high power to board solutions as well so it can be useful to browse through their website.Last but not least a thermal image from one of my designs. This shows a 4 layer PCB with 60um outer layers carrying 70A on an outer layer and inner layer in parallel:

author: Siwastaja
author_rank: Super Contributor
timestamp: February 06, 2021, 07:35:42 am
content: 50A is generally still OK-ish with an SMD shunt; 1mOhm 3W rated parts in 2512, for example; or you can go a tad below 1mOhm to get the dissipation below 2W (2W rated parts are very ubiquitous).Ground plane in a 4-layer PCB right below the SMD shunt removes the need for any extra derating.Careful layout and very low-offset sense amps become important to get accuracy out of such small voltage drop, though. Unit calibration might be necessary, but this isn't too hard to do (if you just calibrate offset/gain, no temperature compensation tables).Hall effect sensor is indeed appealing starting at 50A.If this was 100A, I would say definitely get a hall effect sensor. If 30A, definitely a simple SMD shunt + sense amp.

author: nctnico
author_rank: Super Contributor
timestamp: February 06, 2021, 11:34:22 am
content: Quote from: Siwastaja on February 06, 2021, 07:35:42 amThat is living on the edge. PCB traces will heat considerably at 50A no matter what. 2W dissipated in a single shunt may cause it to overheat because the traces connect to it don't work as a heatsink so much. The power rating is valid when mounted on a PCB which stays around 20 degrees. Also keep thermal cycling stress on the solder joints in mind. If you look at the image the OP posted from the solar inverter you'll see they used a 250 micro Ohm shunt consisting of 4 seperate resistors. I have used 3W shunts in one of my own designs but derated the power rating by 50%.

author: T3sl4co1l
author_rank: Super Contributor
timestamp: February 06, 2021, 12:05:11 pm
content: Oh yeah, another thing you can do, especially for components: clamp the thing in thermal pads and a heatsink. Just an aluminum or copper plate will help spread out the heat, but a finned heatsink also offers the obvious benefit. Give or take how much of this can fit within the DIN-rail enclosure, of course -- but if you can replace all that air space with thermally conductive goop, it's a big advantage.Tim

author: mikeselectricstuff
author_rank: Super Contributor
timestamp: February 06, 2021, 12:28:23 pm
content: Sensing very small voltages on a board that's getting hot will be problematic and likely take quite a lot of work to get right.Unless your volumes are high, I'd just go with something where the manufacturer has solved all the tricky issues, e.g. this one with 200uR resistance.https://www.digikey.co.uk/product-detail/en/allegro-microsystems/ACS781LLRTR-050B-T/620-1823-2-ND/6189096

author: Renate
author_rank: Super Contributor
timestamp: February 06, 2021, 12:47:35 pm
content: Just laminate up your own PCB stack with 1/16" copper and 1/16" FR-4 and mill the PCB design.

author: Siwastaja
author_rank: Super Contributor
timestamp: February 06, 2021, 03:11:59 pm
content: Quote from: nctnico on February 06, 2021, 11:34:22 amOh, who wouldn't like living on the edge?Depends on how much PCB real estate you have to waste. OP seemingly wants to have multiple sensing circuits, if the space is limited and they want them side-by-side, then they may be out of luck or at least require some very clever tricks to get rid of the heat.OTOH, if you have ample space around the shunt, you can play the simple trick of doing a "track" which is wider than it is long. With minimized distance, there is not much resistance for the current to flow, yet the extensions sideways pull the heat out of the shunt. An example would be a 40mm x 10 mm fill, where the current flows through that 10mm dimension.I have played the trick of adding a large bunch of thermal vias around the pads, then add fills on the bottom side, make the bottom side with no component load, add thermal pad and bolt the PCB on a heatsink. You can model this on a napkin or Excel. An example calculation:Fill area = 10*15 mm = 150mm^2Num vias on the fill = 12Rth(via d=0.4mm) = 120 K/W (taken somewhere online)Rth(12 vias) = 10 K/WThermal pad conductivity = 4 W/mKThermal pad thickness = 0.5 mmRth(thermal pad) = 1/(4W/mK)*0.0005m/(150*10^-6 m^2) = 0.83 K/WYou can lower the Rth(via) slighly, maybe by some 20%-30% again, for no extra cost by opening paste mask on the untented vias, but don't count on this, solder flowing in the vias fully can't be guaranteed.Resistor datasheets indeed assume some specific footprint for their ratings. In a 2-layer design, you easily end up having to derate as you say. OTOH, on a 4-layer design the chances are you can use the full rating because the thermal conductivity of the 0.1 to 0.2 mm of FR4 prepreg is quite low, and ground plane beneath softens the hotspot. Most importantly, regardless if you simulate it with some expensive package, or do a simple napkin calculation, build a prototype and measure. Since actually measuring the resistor element temperature might prove difficult, I also recommend doing an overload test. For example, if your expected dissipation is 2W, make the resistor dissipate 4W over a full day or two, let it cool and verify it still has correct resistance.

author: D.Kruger
author_rank: Contributor
timestamp: February 06, 2021, 04:25:56 pm
content: Thanks a lot to everyone for so many ideas and recommendations.After comparing prices and options, I'm thinking of a metal-clad board with 2 layers, each layer 3 oz and placing thermal vias at the tracks to conduct the current through the top and bottom layers. The board total thickness will be 2 mm. Probably we will place a heatsink to the shunt resistors.I will have to test the prototype to make sure is reliable.

author: D.Kruger
author_rank: Contributor
timestamp: February 06, 2021, 04:37:01 pm
content: Quote from: nctnico on February 06, 2021, 01:05:54 amThanks for the explanations, Do you know if this connector are significantly better than screwing the crimped cable directly to the board? I've checked the prices for this connectors and they are a bit pricey, I would have to put 8 of them on each board so, could be a significant increase in the board's price. My original plan was to use crimped wires and bolt them to the board with a screw and a nut.

author: gnuarm
author_rank: Super Contributor
timestamp: February 06, 2021, 08:03:08 pm
content: Quote from: Renate on February 06, 2021, 12:47:35 pmYour comment reminded me of a thermostat I saw once that was made not with a PCB, but with a stamped circuit made from a sheet of metal. I can't recall how the components were attached or many other details, but the metal was rather thick, at least as thick as a 0.062" PWB and probably about twice that thick. I seem to recall wires attached with rivets. I can't recall how it was supported. I want to say it was self supporting, but that would imply it was all one circuit which I know it wasn't. They seemed to use round punches to separate circuits as it left curved edges.I can't find an image of this on the Internet. Maybe they supported the metal by the plastic case and secured it with the wire attachment rivets. I just don't recall.I guess my point is that maybe a PWB is not the right way to go. Is there a reason to not use simple wiring? Some time back I bought current shunts that were four terminal wired. Is that not an option?

author: Renate
author_rank: Super Contributor
timestamp: February 06, 2021, 08:40:11 pm
content: Quote from: gnuarm on February 06, 2021, 08:03:08 pm+1

author: nctnico
author_rank: Super Contributor
timestamp: February 06, 2021, 09:00:14 pm
content: Quote from: gnuarm on February 06, 2021, 08:03:08 pmI agree. Given the requirements that seems to be the most sensible route to me as well. That way using 5 milli-Ohm shunts a decent amount of output signal is also possible. And since the wires are screw terminated anyway I don't see the added value of using a circuit board with all the added complication and extra points of failure (solder joints!).

author: penfold
author_rank: Frequent Contributor
timestamp: February 06, 2021, 09:46:24 pm
content: Coincidentally, I stumbled upon an old shunt product sheet from Hobut this morning, I know the Manganin 0.5% class ones can be a bit pricey, but the 1.5% ones (didn't specify which alloy) maybe more palatable - especially considering they won't get nearly as hot as the resistor/pcb combo.. so what you lose in base accuracy you gain by mitigating some of the resistance change due to temperature (and I don't imagine it would be significant enough based on your geometry but you'd also lose some of the thermoelectric offset)There's also the WSMS2908 series from Vishay (they also have a few other in a similar vein, relatively cheap) sorta semi-PCB mounted, you could support them on the PCB with standoffs or screw terminals which also allow the current carrying lugs to attach so you're only using the PCB for carrying the signal and supporting the shunt

author: T3sl4co1l
author_rank: Super Contributor
timestamp: February 06, 2021, 10:29:05 pm
content: I'm fond of this kind,https://www.digikey.com/en/products/detail/keystone-electronics/8197/316833much cheaper than the machined-block kind (less thermal mass, too).This particular one is only rated 30A, but I would dare say it's fine to run higher than that, just use adequately sized lugs and keep the thing cool.I mean, give or take if you need to pass UL as well.Tim

author: nctnico
author_rank: Super Contributor
timestamp: February 06, 2021, 11:41:12 pm
content: Quote from: T3sl4co1l on February 06, 2021, 10:29:05 pmI'm using these as well!

author: mikeselectricstuff
author_rank: Super Contributor
timestamp: February 07, 2021, 01:56:11 am
content: Quote from: D.Kruger on February 06, 2021, 04:37:01 pmYou don't want to just bolt through the PCB, as the compression can cause the PCB material to flow slightly over time, especially at high temperatures, reducing the clamping force.You definitely need a metal part of some sort that is soldered to the PCB

author: Siwastaja
author_rank: Super Contributor
timestamp: February 07, 2021, 07:27:56 am
content: Quote from: nctnico on February 06, 2021, 09:00:14 pmI would like to agree, but apparently the problem with such easy and reliable solution was the price. If there is a hard requirement for low BOM cost and a lot of "channels" are needed, a custom PCB may end up significantly cheaper, assuming the OP succeeds in the thermal design which won't be trivial. Also assuming design time is free (learning project) or amortized over tens of thousands of units (large commercial project).

author: nctnico
author_rank: Super Contributor
timestamp: February 07, 2021, 01:44:02 pm
content: Quote from: Siwastaja on February 07, 2021, 07:27:56 amIf you shop around a bit you can source panel mounted current shunts for a few dollars each from China.Nice looking Aliexpress find:https://nl.aliexpress.com/item/4000064064917.htmlManufacturer website:http://www.cnchog.com/products/10a-50a-ID137.html

author: D.Kruger
author_rank: Contributor
timestamp: February 08, 2021, 11:16:27 am
content: Quote from: Siwastaja on February 07, 2021, 07:27:56 amThis is exactly the current situation of the project. There are space and cost limitations so, the external shunts turn out to be a more expensive option than PCBs due to the production amount required. It is a project for my employer but time length is enough to let me try the PCB solution, also a excuse to learn more about high power PCB design, other PCB stackups, thermal considerations and so on.

author: D.Kruger
author_rank: Contributor
timestamp: February 08, 2021, 12:39:00 pm
content: Quote from: nctnico on February 07, 2021, 01:44:02 pmThanks, I already knew the shunts from the aliexpress link, I will probably use them in the situations when I need currents too high for the PCB.Also, thanks for the website link. I found thishttp://www.cnchog.com/products/100a-500a-ID166.htmlI think they would solve ,y problems, they are compact, can be installed over a PCB but without the dissipation problems of soldered shunts

author: nctnico
author_rank: Super Contributor
timestamp: February 08, 2021, 02:58:52 pm
content: How about this one? It is way more compact compared to the one I linked to and there are higher current ratings available in the same footprint:http://www.cnchog.com/products/50a-50mv-ID121.html

author: D.Kruger
author_rank: Contributor
timestamp: February 08, 2021, 03:47:42 pm
content: I saw that one too. I sent an email to the company explaining the needs for my project and asking for a quote for various models.