Options for increasing the current carrying capabilities of PCB traces

[Kryptychon]

Hi,

I'm layouting a double H-bridge for a DIY tracked EV project and I'm struggeling with the actual layout of the high current traces. "High" in this context means 60-80A of current on the h-bridges input terminals and 30-40A on the motor terminals.

I know I could easily buy motor controllers which satisfy this requirements with ease but I want to learn how to properly design and eventually manufacture power electronics, so I decided to go the way from zero to a "finished product".

I already have a well working prototype of a single H-bridge on perf board. Now I'm wondering how to handle high currents on a professionally manufactured PCB. Out of curiosity, I had a look into various power electronics (Li-battery BMS, BLDC driver and a SMPS). They all use different approaches to handle the high currents. The BMS for example uses aluminum(?) enforced PCB material to carry the high currents. The BLDC driver gets away with wide (and probably thick) and short traces. The SMPS (a Meanwell 12V ~10A SMPS) seems to use "regular" tracks which have been enforced with solder in a grid pattern (maybe to prevent stress due to different thermal expansion rates?).

I'm looking for pros and cons of the mentioned options as well as for further options. I'm also curious how this challenge is solved in a industrial product. Yesterday I had a look for solderable screw terminals and I found some () terminals from Würth Elektronik (Redcube) which state to be suited for 200A and more. How are these currents handled on a PCB? Maybe someone can also point me to literature regarding power electronics design from a manufacturing perspective.

Thanks for any light shed!

[Hawaka]

Hi,

From my experience adding soldering on the trace is not a good idea and doesn't really increase the ampacity. The only option there is is to increase the copper you have on the board.

Usually changing from 35u to 70u or 105u doesn't really cost more for external track. So that's a cheap way to do it.

When I usually design a board, first I make the trace as large as possible. More surface equals more thermal dissipation. Remember that the FR-4 is not good at all thermally. Then increase the copper thickness, then increase the number of layer.

A colleague of mine did an 8-layer 105u on all of them, for about 200A I think.

Also the price aspect is something to take into consideration. Sometimes 4-layer 35u is cheaper than 2-layer 70u.  I think as long as you have the same amount of copper, thermally it will be independent of the stack-up.

Solderability is another issue when you increase the copper, a 2-layer 105u is already significantly harder to solder by hand than a 2-layer 35u. Post some point you cannot hand-solder and wave soldering is your only solution.

Some supplier like PCBWAY propose up to 455u on external trace, which is kind of crazy. And that's before you start talking very specific PCB.

[Siwastaja]

Minimize distance of components, minimizing track lengths. Problem solved.

In other words, say you have a 2mm wide component leg or pad. Somehow it magically can deliver 50A without self-destructing. Now you fan the track out similar to the pad width, say still 2mm. Still OK. Then, as soon as you have space, you start to make the track or fill wider and wider to support the current. Until you have spent the whole area available. But if the next component (another semiconductor, or connector, or soldered wire) is right there, you are done.

It all boils down to the aspect ratio - see "ohms per square", which is 0.25 mOhms per square for 2oz foil. 1mm wide track and 100mm wide tracks have exact same resistances, if their lengths are in the same proportion, too!

I^2R loss is therefore only defined by the aspect ratio of tracks. That is what you should be calculating and optimizing, not width.

So avoid generating the loss to begin with. PCB width calculators assume infinitely long tracks. Shorter tracks spread heat better as the "ends" participate, any component leg or wire participates in cooling.

Finally, if you absolutely need to carry those large currents around the board and don't want to pay premium for very thick copper, for small batches and prototyping just buy some 0.3mm copper sheet, this is still easy to cut in shape with normal scissors. This copper can be reflow soldered on top of the tracks. For even better, bend the copper sheet in L or U shape before soldering, getting even more area due to 3D construction, also acting as heat sink.

[nctnico]

I'm looking for pros and cons of the mentioned options as well as for further options. I'm also curious how this challenge is solved in a industrial product. Yesterday I had a look for solderable screw terminals and I found some () terminals from Würth Elektronik (Redcube) which state to be suited for 200A and more. How are these currents handled on a PCB? Maybe someone can also point me to literature regarding power electronics design from a manufacturing perspective.

When dealing with connectors and high currents be aware that the maximum currents are specified at room temperature (20 degrees or so). So in a real circuit you have to derate the maximum current depending on the temperature. See this DIN connector datasheet for an example: https://www.distrelec.nl/Web/Downloads/40/63/DIN%2041612_eng_BRO.pdf

It is more likely those Redcube connectors can handle 100A (or even less) in a real circuit.

To increase current handling in a PCB you can also opt to use multiple layers in parallel. Now inner layers don't cool so well but with 2 similar sized conductors in parallel, you reduce the amount of power dissipated by a factor of 4.

Another option is to use through hole or surface mounted busbars to get a lot of current through a PCB.

[free_electron]

- use thick copper ( 2 or 4 oz ). you may need to restrict 4oz to inner layer to allow for fine pitch on outer layers (doing 0.5mm pitch tqfp or qfn is not possible on 4oz copper
- use via farms to link layers vertically. lots of smll vias is better than large ones. it is tunnel surface that is important.
- 4 to 8 layer boards.
- remember that current handling on inner layers is less than on outer layers due to heat spread
- if you really need power : use busbars or placeable SMD shunts in a checkerboard pattern ( overlapping )
- be careful constructing the landpatterns for your power components. make sure you have even solder distribution and prevent wicking into via holes. use a windowpane soldermask/pastemask to trap the solder in pockets, away from the vias. tent or encroach the vias on one side.
- be aware of CAF issues. drilling too close will shatter the glass strands in the prepreg. there is a risk of dendrite formation that will give spectacular failures. 10 to 12 volts is enough for dendrite growth in board.
- surface contamination is a problem. make sure the boards are cleaned well and apply copious lashings of conformal coating to keep moisture out.
- balance copper and avoid large empty spaces to prevent warping of the board during reflow. checkerboard between layers to planarize the board. use an additional buttercoat if needed.
- use pressfit terminals. they have higher current handling than soldering, are gas tight and there is no risk of solder joint cracking with resulting arcing. wurth has bolt-on pressfit terminals ( redcube series). bonus : the solderability problem of thick copper is solved

i've done boards that have 400 to 800 ampere feeds.

[Kryptychon]

Thanks for the answers!

So the main aspect is temperature and power dissipation. I get the point, that the copper thickness and the track's length is key. I'll optimize my layout according to that.

Thanks again!

Btw. I just checked JLCPCB and PCBWay and 1oz of copper and 4 oz of copper make a big difference in price. I guess it's not the difference in the amount of copper which makes a greater price but the lower volume of 4oz boards they produce, right?

[bob91343]

I don't see mention of how to get the current in and out.  The termination often is the limiting factor, making for very high current density and uneven distribution.

I would think a good way would be to solder a heavy copper bus bar on the board and also put bolts through to make it substantial.  Then external connections via screw terminals.  Finally, measure current distribution to determine tightness of the various bolts.

[jbb]

If you’re doing small quantities, non-standard boards (eg copper > 35um) really hits you in the pocket.

Have you considered upping the layer count? You can then parallel the layers.
Note that final copper thicknesses are often like Top: 35u
Mid1: 18u
Mid2: 18u
Bottom: 35u

[Siwastaja]

2oz (70um) outer layers is not much more expensive.

After that, adding two 18u internal layers in parallel isn't helping much. Thicker internal layers tend to cost more than thicker outer layers.

Having the internal layers as ground planes to spread heat probably is at least equally helpful, even if they don't contribute to the current sharing.

Adding solder on the traces gives maybe ~20-30% current rating increase. Not much but sometimes still usable if you are "almost there".

If track lengths can't be minimized to nearly nothing, the real solutions are either paying premium for really thick copper (4oz or even more), or buy those reflow solderable reinforcements, or do your own from copper sheet or even a few copper wires in parallel, soldered to tracks.

Very thick copper isn't usually a good solution because in the standard process, it limits min track width / clearance rules, and often you have small control ICs and passives etc. on the same board. 2oz still allows those 0.5mm pitch parts on the same board.

Finally, prototype and measure. All this is hard to calculate or simulate.

[Berni]

Thick copper is the way to go.

Yes thick copper is much more expensive for prototypes because they can no longer fit you in on the cheep prototype optimized production line, but once you go for larger production quantities the price difference becomes more reasonable.

Putting solder on tracks only helps a tiny bit. The trick to really increase current capability is to go to a laser cutting vendor and have them cut out some copper sheet in the shape of your trace. This can then be soldered down onto your track like any other SMD component. (They might be able to throw it into a nickel plating bath to make it easier to solder too). This gives you effectively like 100oz copper on that track, excellent for not only carrying massive currents but also for sinking heat away from large SMD components such as MOSFETs

That being said you can actually take normal copper to pretty large currents as long as you can cool it. One good way is to get some of those soft silicone thermal pads and sandwich that between the PCB and the metal case. This helps in bringing the heat outside and allows your PCB to produce 2 to 5 times more heat without getting too hot. Components on the board still produce heat, so even if you had superconducting PCB tracks the device might still overheat because transistors still need cooling when running at very high currents. But the copper is still important here in spreading out the heat over a large area, since the silicone thermal pads are not really that great heat conductors, so they need a decently large surface area to transfer a good amount of heat.

[Kryptychon]

Thanks for the answers.

Okay, so if I understood correctly, in my case it boils down to:

- make tracks as short as possible
- if possible add as much copper as needed
- if temperature is ok, there is no problem

In my design, I'm using MOSFET and free wheeling diods in TO 247 packages. Each half-bridge (4 in total, forming 2 h-bridges) sits on a heatsink. Additionally, I've two shunt resistors and two fuse holders on the PCB. Keepings tracks "short" and keeping the layout neat at the same time is very tricky but I guess, that's what layouting is all about. Feels like doing art.

Do you have and rule of thumb what "short" means at a given current? I assume it's "just" a matter of temparature.

I don't see mention of how to get the current in and out.  The termination often is the limiting factor, making for very high current density and uneven distribution.

I use these in my design:

- https://eu.mouser.com/ProductDetail/710-74651174R (rated 50A, used for the motor terminals)
- https://eu.mouser.com/ProductDetail/710-74651194R (rated 85A, used for the battery connection)

They seem very solid and provide multiple thick legs which might result in a good current distribution.

I attached my clumsy first try out of this board layout. I'm at the very beginning. If it's not asked to much, I would like to hear what you think about the general approach as well as what you think about separating the half bridges like I did.

Thank you very much!

[Berni]

It is more a matter of thermal design than electrical design at this point.

You can calculate the amount of heat in watts for a given length of trace. You can calculate the resistance of the trace, then just plug in the good ol P=I^2*R and you have the heat. Shorter the trace less miliohms it has so less watts it produces.

Watch out for fuse sockets too, they can become pretty hot at large currents because the fuse itself has to burn some of the power as heat in order to get the heat to blow the fuse, so when running close to the fuse rating it is making a lot of heat that is just barely not enough to melt the wire inside.

If this is a small volume product and you are using all troughhole transistors you can still just manually wire the transistors with wire. Otherwise modern power electronics are typically designed to be built on an aluminium plate that then gets mounted to a large heatsink. This is either as semiconductor "bricks" that contain raw silicon die directly bonded to ceramic on said aluminium plate, or at a lower level of integration in the form of large SMD package transistors soldered to a aluminium core PCB that gets bolted down to the heatsink.

[jonpaul]

Bonjour since 1980s..1990s  we designed many  SMPS and ballasts  to 100A

1/ Thick PCB 2 oz/4oz is costly, long lead and very hard to solder to especially if multilayer or PTH. Chinese made PCBs may not be the actual copper touted.

2/The high current path is very simple, this traces are reinforced with soldering bus wore on top (no silkscreen)

3/ Direct wiring off the PCB from transformer leads to rectifier  was also simple.

4/ High current PCB connectors are readily available from connector manufacturers, we used AMP and Berg.

Take apart a 1000W ATX PC PSU to see typical production preactice.

Bon chance

Jon

[Kryptychon]

Okay, thank you all for the valuable input.

In fact, it'll be a very small volume PCB as it is destined to be be part of an electric caterpillar I build for me...I mean my daughter ;-)

Nevertheless, I'm willing to do it the "proper" way as I want to learn how to design such a piece of power electronics.
With all the advice I got here, I think I'll be able to finish the layout.

I'll come back to this thread when I got the first board working.

Again, thank you all very much for your input. It is a great help.

[Siwastaja]

Oh, it's not SMT design, I guess it won't be wave soldered either, so manual work anyway. Easy to solder more copper while at it.

You can even bend the excess part of the component legs of your TO247 packages to go along with the track, then solder them down. Free copper you would otherwise cut away and waste!

Use polygon pours for nets other than GND, too. PCB EDA automation saves work, you can get maximized amount of copper without all the manual work of avoiding the surrounding other nets. This specifically applies to the nets going to the connectors. As they are now, way too long or thin. Remember, it's about aspect ratio. If the connector needs to be that far, you need wider copper as well. Automated polygon pour is the easiest way to get there.

DC link positive can be a full plane, or at least complete pour on top (or bottom) layer.

4-layer is good for EMC and stray inductance minimization. Even if you simply make the two mid layers full ground planes (DC link -), they contribute to the current handling (DC- return currents), and at the same time, work as heatsink for every top/bottom trace even if there is no electrical connection, because the typical 100-250µm FR4 prepreg thickness enables decent thermal conduction from any track to the ground plane.

I'm not seeing DC link capacitance anywhere! This is absolutely fundamental to operation. It needs to sit near the diode-MOSFET half bridges.

Also, consider making it synchronous, i.e., two MOSFETs instead of MOSFET + diode. Diode loss is HUGE at such high power levels. Needing a half-bridge gate driver is smaller expense than all the heatsinking needed for the diodes. Sorry, I misunderstood the circuit, it seems you have a full bridge per motor and just schottkys in parallel with MOSFET body diode. Are you sure you need these Schottkys? They could slightly help during the deadtime, avoiding turn-on of MOSFET body diode, but I have rarely seen them in practice and never used in motor controllers myself. In any case, they shouldn't need heatsinking except if you are anticipating problems with software / gate drive.

Datasheet for IRF1405 says it's in TO220. Are you sure about the part number / package?

In any case, add those DC link caps. Adding them allows you to see that your path from + to - through the two transistors is quite long. If you remove the diodes and rotate one of the MOSFETs 180deg and replace the diode with it, now suddenly your + and - are right next to each other, nice spot for the cap; also minimizing track length.

[tooki]

From my experience adding soldering on the trace is not a good idea and doesn't really increase the ampacity. The only option there is is to increase the copper you have on the board.

Dave did an entire video on this topic, and it showed that it definitely does make a difference.

[Siwastaja]

From my experience adding soldering on the trace is not a good idea and doesn't really increase the ampacity. The only option there is is to increase the copper you have on the board.

Dave did an entire video on this topic, and it showed that it definitely does make a difference.

Yes, and many many commercial products do that.

The reason is simple: the increased cost of solder is almost negligible, but extra production steps cost much more. Adding the necessary solder mask / paste mask openings works well in both wave and reflow soldering processes and cost nothing to do (maybe some fractions of cents if your volumes are so large that CM is billing you for solder used).

Solder is almost ten times worse conductor than copper, but the layer thickness from wave or reflow solder is easily some 5 times thicker than 1oz copper. You can't get 100% fill rate on the track, though. Practical result is some 20-30% increase in current capability, IIRC Dave measured something close to this, too (I did watch the video years ago).

If you can afford 2oz copper, then the relative effect is smaller, though. For manual soldering, instead of the hassle of adding just solder, add copper wire, and solder that down.

[CatalinaWOW]

I think cost of thicker copper is not the material cost, which is relatively small, but material removal cost.  1 oz to 4 oz means roughly four times the etch time plus added problems with undercutting etc.  The longer etch time is an opportunity cost, you could produce four thinner boards in the same machine in that time.

[tooki]

Commercial PCBs are not made by etching away large amounts of copper. They begin with extremely thin copper layers, etch those, and then electroplate copper onto them to build up to the required thickness while plating the through-holes at the same time.

I assume that aside from the copper (which is a material whose cost has skyrocketed in recent times), the longer plating times are the main cost driver on thicker copper layers.

[nctnico]

Commercial PCBs are not made by etching away large amounts of copper. They begin with extremely thin copper layers, etch those, and then electroplate copper onto them to build up to the required thickness while plating the through-holes at the same time.

No. How can you electroplate an isolated track? It is the other way around, first all the plated holes are drilled and then the PCB get electroplated including the holes. After that the board gets etched.

[CatalinaWOW]

Took, you are probably right about the process, I haven't kept up with modern processing.  But I think the same principal applies.  Long time playing, plus hookup time to contact tracers being plated.


Copper has gone up by factors, but there is still only a dollar or two of copper on a modest size board.

[daqq]

No. How can you electroplate an isolated track? It is the other way around, first all the plated holes are drilled and then the PCB get electroplated including the holes. After that the board gets etched.

No idea. But something like that gets done.

( https://www.epectec.com/articles/heavy-copper-pcb-design.html )

[Berni]

The extra copper and machine time do cost a little bit, but what you are mostly paying for is stepping out of the economy of scale on the prototype optimized production line.

PCBWay and similar have automated parallelization tech in place that fits lots of these prototype boards onto giant PCB panels that then get fed trough machines made for that panel size, at the very end the panels are sliced up by a CNC machine into boards. This is why they silkscreen a order code onto the PCB to not mix them up and why wanting anything special drives up the cost quickly. If you have a large weird shaped board they can't panelize it with others that well so more expensive. Less common thickness or color or something means grouping into a panel with less demand so they might not fill a panel or can't pack it together as well. When you get into the really unusual stuff like thick copper, weird stackups..etc then they have to make a panel just for you. If its too weird it doesn't even work on the regular production line as it might hold up the flow due to a process taking longer, so it may be passed onto a different slower line or outsourced to another manufacturer.

EDIT: Also they probably make zero profit on the cheep special deal 2$ boards, so they count on that as being marketing for selling the more expensive boards that actually make the good profit.

[tooki]

Commercial PCBs are not made by etching away large amounts of copper. They begin with extremely thin copper layers, etch those, and then electroplate copper onto them to build up to the required thickness while plating the through-holes at the same time.

No. How can you electroplate an isolated track? It is the other way around, first all the plated holes are drilled and then the PCB get electroplated including the holes. After that the board gets etched.
[video]

Please see this and the subsequent few steps (from the same source you’re using to claim I’m wrong):
https://www.eurocircuits.com/electroless-copper-deposition/

I was slightly incorrect in my description, in that they don’t etch away the unwanted parts yet, but rather mask the unwanted parts to stop them from being plated up to full thickness. So it’s been imaged, but not yet etched.

But the point was that commercial PCBs are not made by etching away large amounts of copper, but by etching away small amounts and plating up the traces to full thickness.

[tooki]

Took, you are probably right about the process, I haven't kept up with modern processing.  But I think the same principal applies.  Long time playing, plus hookup time to contact tracers being plated.


Copper has gone up by factors, but there is still only a dollar or two of copper on a modest size board.

Yep, for sure. The longer a step takes, the more it costs!