Some doubts with a 50A PCB Design

[penfold]

Of course, the conductivity of the solder depends on the exact composition and the thickness, but clearly the solder is much thicker 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?

I'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

[T3sl4co1l]

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

[ajb]

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.

[nctnico]

How 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.

Precision 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

Well, 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_HOLE
The 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:

[Siwastaja]

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.

[nctnico]

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).

That 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%.

[T3sl4co1l]

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

[mikeselectricstuff]

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

[Renate]

Just laminate up your own PCB stack with 1/16" copper and 1/16" FR-4 and mill the PCB design.

[Siwastaja]

That 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.

Oh, 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^2
Num vias on the fill = 12
Rth(via d=0.4mm) = 120 K/W (taken somewhere online)
Rth(12 vias) = 10 K/W
Thermal pad conductivity = 4 W/mK
Thermal pad thickness = 0.5 mm
Rth(thermal pad) = 1/(4W/mK)*0.0005m/(150*10^-6 m^2) = 0.83 K/W

You 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.

[D.Kruger]

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.

[D.Kruger]

How 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.

Precision 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

Well, 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_HOLE
The 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:

Thanks 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.

[gnuarm]

Just laminate up your own PCB stack with 1/16" copper and 1/16" FR-4 and mill the PCB design.

Your 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?

[Renate]

I guess my point is that maybe a PWB is not the right way to go.

+1

[nctnico]

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?

I 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!).

[penfold]

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

[T3sl4co1l]

I'm fond of this kind,
https://www.digikey.com/en/products/detail/keystone-electronics/8197/316833
much 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

[nctnico]

I'm fond of this kind,
https://www.digikey.com/en/products/detail/keystone-electronics/8197/316833
much cheaper than the machined-block kind (less thermal mass, too).

I'm using these as well!

[mikeselectricstuff]

My original plan was to use crimped wires and  bolt them to the board with a screw and a nut.

You 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

[Siwastaja]

I 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!).

I 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).

[nctnico]

I 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!).

I 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).

If 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.html

Manufacturer website: http://www.cnchog.com/products/10a-50a-ID137.html

[D.Kruger]

I 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!).

I 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).

This 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.

[D.Kruger]

I 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!).

I 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).

If 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.html

Manufacturer website: http://www.cnchog.com/products/10a-50a-ID137.html

Thanks, 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 this http://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

[nctnico]

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

[D.Kruger]

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.