Some doubts with a 50A PCB Design

[D.Kruger]

Hi everyone, I'm designing a 2 layer board to measure current in solar panel arrays, on rooftops, not roadways

The 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.

[Miyuki]

It all depends just on losses you want to accept
You can pass an insane amount of current with tiny traces

Even if you pass so much current to have like +60K temperature rise on traces nothing really happens

[penfold]

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 nearby

The 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.

[richard.cs]

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.

[Berni]

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.

[Siwastaja]

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.

[Renate]

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.

[Siwastaja]

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.

[voltsandjolts]

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

[D.Kruger]

Thanks a lot for the answers, I've done this draft to explain myself better.
 

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 nearby

The 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.

The 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.

[D.Kruger]

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.

Thanks 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?

[D.Kruger]

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

Hi, unfortunately the client specified that he wants a shunt, not a hall sensor

[penfold]

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 solid
You 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 area
The 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

[nctnico]

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

Hi, unfortunately the client specified that he wants a shunt, not a hall sensor

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.

[Renate]

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.

[D.Kruger]

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 solid
You 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 area
The 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

Hi, 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

[T3sl4co1l]

What's wrong with this kind?
https://www.digikey.com/en/products/detail/murata-power-solutions-inc/3020-01096-0/1926137
Has its own board, and hardware, just mount a few to a DIN bracket.

Tim

[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

[D.Kruger]

What's wrong with this kind?
https://www.digikey.com/en/products/detail/murata-power-solutions-inc/3020-01096-0/1926137
Has its own board, and hardware, just mount a few to a DIN bracket.

Tim

That would solve a lot of my problems, but it's too expensive, the product will have between 4 to 16 shunts

[gnuarm]

The 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.

I'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.

[penfold]

The 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.

I'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.

Neither 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.

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

I'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.

[gnuarm]

The 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.

I'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.

Neither of those is something that actually measured in practice, what sort of level would you suggest the solder improved the conductivity?

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?

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.

Ok, 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.

[Siwastaja]

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?

[schratterulrich]

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.

[Renate]

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.