Options for increasing the current carrying capabilities of PCB traces - Page 1
Forum section: electronics / projects

author: Kryptychon
author_rank: Contributor
timestamp: January 30, 2022, 03:31:11 pm
content: 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!

author: Hawaka
author_rank: Regular Contributor
timestamp: January 30, 2022, 04:24:53 pm
content: 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.

author: Siwastaja
author_rank: Super Contributor
timestamp: January 30, 2022, 04:30:35 pm
content: 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.

author: nctnico
author_rank: Super Contributor
timestamp: January 30, 2022, 05:06:23 pm
content: Quote from: Kryptychon on January 30, 2022, 03:31:11 pmWhen 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.pdfIt 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.

author: free_electron
author_rank: Super Contributor
timestamp: January 30, 2022, 05:18:45 pm
content: - 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 solvedi've done boards that have 400 to 800 ampere feeds.

author: Kryptychon
author_rank: Contributor
timestamp: January 30, 2022, 07:51:50 pm
content: 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?

author: bob91343
author_rank: Super Contributor
timestamp: January 30, 2022, 10:37:36 pm
content: 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.

author: jbb
author_rank: Super Contributor
timestamp: January 31, 2022, 02:49:14 am
content: 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: 35uMid1: 18uMid2: 18uBottom: 35u

author: Siwastaja
author_rank: Super Contributor
timestamp: January 31, 2022, 07:30:24 am
content: 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.

author: Berni
author_rank: Super Contributor
timestamp: January 31, 2022, 08:02:41 am
content: 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 MOSFETsThat 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.

author: Kryptychon
author_rank: Contributor
timestamp: January 31, 2022, 10:08:30 am
content: 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 problemIn 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.Quote from: bob91343 on January 30, 2022, 10:37:36 pmI 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!

author: Berni
author_rank: Super Contributor
timestamp: January 31, 2022, 11:30:43 am
content: 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.

author: jonpaul
author_rank: Super Contributor
timestamp: January 31, 2022, 11:40:20 am
content: Bonjour since 1980s..1990s we designed many SMPS and ballasts to 100A1/ 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 chanceJon

author: Kryptychon
author_rank: Contributor
timestamp: January 31, 2022, 12:55:42 pm
content: 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.

author: Siwastaja
author_rank: Super Contributor
timestamp: January 31, 2022, 03:21:12 pm
content: 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.

author: tooki
author_rank: Super Contributor
timestamp: January 31, 2022, 03:56:10 pm
content: Quote from: Hawaka on January 30, 2022, 04:24:53 pmDave did an entire video on this topic, and it showed that it definitely does make a difference.

author: Siwastaja
author_rank: Super Contributor
timestamp: January 31, 2022, 04:06:36 pm
content: Quote from: tooki on January 31, 2022, 03:56:10 pmYes, 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.

author: CatalinaWOW
author_rank: Super Contributor
timestamp: January 31, 2022, 04:18:24 pm
content: 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.

author: tooki
author_rank: Super Contributor
timestamp: January 31, 2022, 08:53:12 pm
content: Commercial PCBs are not made by etching away large amounts of copper. They begin withextremelythin copper layers, etch those, and then electroplate copper onto them to buildupto 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.

author: nctnico
author_rank: Super Contributor
timestamp: February 01, 2022, 02:27:48 am
content: Quote from: tooki on January 31, 2022, 08:53:12 pmNo. 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.

author: CatalinaWOW
author_rank: Super Contributor
timestamp: February 01, 2022, 04:19:10 am
content: 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.

author: daqq
author_rank: Super Contributor
timestamp: February 01, 2022, 07:06:09 am
content: QuoteNo idea. But something like that gets done.(https://www.epectec.com/articles/heavy-copper-pcb-design.html)

author: Berni
author_rank: Super Contributor
timestamp: February 01, 2022, 07:08:55 am
content: 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.

author: tooki
author_rank: Super Contributor
timestamp: February 01, 2022, 10:07:29 am
content: Quote from: nctnico on February 01, 2022, 02:27:48 amPlease 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.

author: tooki
author_rank: Super Contributor
timestamp: February 01, 2022, 10:11:53 am
content: Quote from: CatalinaWOW on February 01, 2022, 04:19:10 amYep, for sure. The longer a step takes, the more it costs!

author: Kryptychon
author_rank: Contributor
timestamp: February 01, 2022, 02:00:46 pm
content: Quote from: Siwastaja on January 31, 2022, 03:21:12 pmYes, the high power part of this board will be all THT. I designed the current sensing circuit on a separate boards where I will use LT1999 (current sense amplifier) which is a SMD part.I thought it might be beneficial for the layout to keep the high current board all THT, so I can easily do my prototype at home and swap parts if necessary.Quote from: Siwastaja on January 31, 2022, 03:21:12 pmThat's a nice idea! I'll think about that.Quote from: Siwastaja on January 31, 2022, 03:21:12 pmThat's also a nice approach. I'm relatively new to PCB layout (I only did two project related boards: a DC/DC converter board and a logic/protection board which some TTL logic an zener clamped signal level limitation.), so I'm a little bit scared of going 4-layer right away...Quote from: Siwastaja on January 31, 2022, 03:21:12 pmYou're absolutely right. I wanted to start some layout experiments with the most difficult parts. I'll include capacitance of course!Quote from: Siwastaja on January 31, 2022, 03:21:12 pmWow, that's some very important information for me. I did almost one year of research and math before feeling confident enough to build a single ("high power") h-bridge prototype. I read a lot of controversial discussion about the necessity of free wheeling diodes in h-bridge configurations. To be honest, I'm still unsure if I need to include them or not. I'm using two IR2184 half-bridge driver ICs per h-bridge and they work indeed in synchronous mode with a fixed dead time between input signal changes. I think, using a synchronous control for the h-bridge (almost) eliminates the need for free wheeling diods as reverse currents will only occure during dead time but as I said, I'm not 100% sure about my thinking. Maybe you can teach me a lesson about that too.I would be more than happy to learn that I can get rid of these huge shottky diodes as they take a lot of valuable space on both, the heatsinks and the PCB. Additionally, they're not cheap in this size.I don't expect any problems with software or gate drive. I've designed an external logic board which provides the needed signal levels for the IR2184. In addition there will be a current sensing/temperature monitoring circuit which is a daughter board on the h-bridge PCB. The purpose if this daughter board is to provide a hardware level shutdown of the gate driver ICs in an overcurrent / over temperature situation as well as providing an analog ratiometric voltage signal for the MCU to control/limit acceleration based on bridge current. The fuses are "last resort" measures to protect the MOSFETs and PCB.Quote from: Siwastaja on January 31, 2022, 03:21:12 pmYou're right again! I used the wrong part number. It's the IRFP1405PbF (which comes in a TO-247AC package).Quote from: Siwastaja on January 31, 2022, 03:21:12 pmIf I really can get rid of the diodes, this definitely is the way to go.Thank you very much. Your input is very appreciated!I attached the unfinished schematic and images of the perfboard prototype.

author: Siwastaja
author_rank: Super Contributor
timestamp: February 01, 2022, 02:29:54 pm
content: LT1999 is a nice amplifier with way more bandwidth than necessary for a motor controller. Downsides are high cost and less than stellar offset specifications because it isn't auto-zero type (auto-zero types are not available much beyond 100-200kHz or so in bandwidth, but that is enough for motor controllers). Anyway, it's more than fine.Don't be afraid about adding layers, that makes layout work only easier. Beginners fear large number of layers because it feels like an "indication" of complexity. In reality, the complexity is what it is; more layers only makes the work easier, and results better. Fortunately, 4-layer boards from China cost less today than 2-layer boards just a decade ago.You don't need to do anything else than make it 4-layer and fill both mid-layers as full ground planes. Job done, now wherever you need GND, you can just add a via, and don't need to think about ground routing. The planes acts as heat spreaders, making the whole PCB act like a heatsink, this is because FR4 is a crappy thermal conductor in lateral direction. But the distance between the top layer and the next mid layer is very small, like 100-250µm, so heat flows well into the ground plane, which then spreads it over larger area.You understood right, the idea is to drive the bridge so that two MOSFETs conduct; for example, lower MOSFET from bridge 1, upper MOSFET from bridge 2. The diode which would conduct, is shorted by the on-state MOSFET, because this is more efficient as it's easy to select low enough Rds_on, so that voltage drop is smaller than the Vf of diode. This only leaves the very short deadtime. Diode is needed during that time, yes, but MOSFETs come with the body diodes. During that tiny time period, the loss from using the MOSFET body diode is minuscule. Sometimes synchronous buck designs add parallel schottkys, but usually not, and even more rare in motor controllers, IMHO. I'd start without. You can of course try measure if they do any good. I have done many motor controllers and never added diodes in the MOSFET designs. Now IGBTs need the diodes but OTOH you can buy co-packaged IGBT+diode modules.Fuses can't protect the MOSFETs, way too slow. MOSFET blows into short circuit in 10-100µs, then fuse takes 1-10ms to blow. But they are important because they protect against fire and tracks burning off. Buy extra MOSFETs, you will blow a few, but also buy gate drivers because they usually go at the same time. Personally I don't like to waste any more time trying my luck with just replacing the MOSFETs hoping the driver is OK, just to see the driver is weirdly damaged, misbehaves and blows the new MOSFETs - I just replace both the FETs and the driver at the same time.Current sense circuit is critical indeed, if you want to minimize number of blown MOSFETs, start from verifying your current limitation works. Before I even solder the MOSFETs in, I like to just charge a capacitor to 1V or so, and discharge it over the shunt resistor, giving a brief pulse. Using oscilloscope, measure sense amp output, and the gate driver enable signal etc., verify it goes low within some reasonable time, should be a few µs max really. Hardware solutions are better than software, although a few times I have just used analog comparator triggering highest priority interrupt and in the ISR, just turn the gate drive off as the first thing.It takes just one too long pulse to destroy the MOSFETs, this is why you need such pulse-by-pulse measurement and limitation. Now if you implement a PI feedback loop for regulating average current and torque, that can be slower.

author: Siwastaja
author_rank: Super Contributor
timestamp: February 01, 2022, 02:47:20 pm
content: Also, remove that three-different-capacitor-values bullshit from the gate driver Vcc, it's based on some urban myths which was kinda relevant with ages old combinations of electrolytic caps and smaller film/ceramic caps due to the large ESL and ESR of then-available few-µF sizes. Irrelevant with MLCCs, and only does harm - risk of parasitic oscillation. Just use the largest value MLCC (here 1u) alone, in as small package as possible, close to the IC (I'd recommend 0603, but 0805 works fine).Also remove the RCD snubbers. Start from tight layout, test and measure. Simple RC snubbers may be needed, in the end, but it takes some experimentation. You can of course add the footprints. I don't think the 1N4007 does any good, just small R+C footprints physically as close as possible over the MOSFET and nothing else. Start testing without. If the switch nodes ring excessively and you can't tame it with modest increase in Rg, then start playing with snubbers.That TVS bank of yours is nice to have, as motors can regenerate. More importantly, remember to have a way to sense the DC bus voltage (with resistor divider to MCU ADC, for example), so you can set the motor to freewheel in case of overvoltage. TVS bank becomes handy if someone rotates the motor to excessive speed so that Back-EMF exceeds the voltage ratings.Did I mention DC bus capacitance? With such low DC bus voltage, MLCC is an option. Soft terminated parts are a good idea. Up to 50V, I like to use some 2.2uF in 0805 so I can sprinkle them all over the place, but larger values in 1206 or 1210 is fine, too. Exact amount of capacitance is not important and I don't even have an idea how I would calculate that. Lowest possible ESL is critical and low ESR good, too. This means, placement, placement and placement. And basically, ESL is nothing more than package size. Smallest is best, and you can get it closer, too.What will be the actual highest DC link voltage?

author: Kryptychon
author_rank: Contributor
timestamp: February 01, 2022, 03:32:28 pm
content: You seem to be exactly the well of knowledge I was looking for so long.Quote from: Siwastaja on February 01, 2022, 02:29:54 pmPerfect! Thanks for the encouring words. I'm worried about using GND planes for everything because I fear voltage drop along the GND plane which might lead to insufficient signal levels on the logic inputs of the IR2184. I had this problem with the prototype and solved it by bypassing their GND connections with added wires to the DC input terminals. So I thought, having a star ground arragmenent for the driver ICs is a must have. On the other side, if the inner GND planes don't carry the motor currents, it will be fine I guess as it IS a star ground arrangement of some sort.Quote from: Siwastaja on February 01, 2022, 02:29:54 pmSounds reasonable. I'll definitely will get rid of the shottky diodes and rely on the body diodes. It's so valuable to hear it from someone who actually did it this way. Very encouring. Thanks!Quote from: Siwastaja on February 01, 2022, 02:29:54 pmI fully aknowledge that. Already wasted hours with debugging just to find a damaged gate driver in the end. Regarding the fuses, of course, I was wrong, they're way too slow to protect the MOSFETs, but as you said, they protect the PCB from catching fire. The battery pack itself is fused too of course.Quote from: Siwastaja on February 01, 2022, 02:29:54 pmThat's exactly why I chose two layers of protection. One very fast at hardware level and another one at software level. The hardware protection can always override the enable signal from the MCU. But you pointed me to check my current sensing circuit regarding reaction time. As I mentioned, I use a LT1999 along with an LM339 which has an open collector output which pulls the driver IC's enable pin to directly to ground if settable current threshold is reached.Quote from: Siwastaja on February 01, 2022, 02:47:20 pmShame on me indeed (I knew the "myth") and good to know. I'll go with a single 1u one per driver.Quote from: Siwastaja on February 01, 2022, 02:47:20 pmI read an application note from Toshiba regarding the need for snubber circuitery (I attached it, see Chapter 2.8.2, section "c) Discharge Supressing RCD snubber") and computed the RCD snubber for to aim for a maximum of 40V surge at 15kHz PWM. My decision using a RCD snubber was based on the energy effiency stated. For the EV project, energy effiency and recuperation is not of great importance as it will be a tracked vehicle but I plan to use this design in other EV applications as well, so energy effiecency seems important to me. Even with the "efficient" RCD I have, I'm wasting 1.2W based on the calculations I did. Might be foolish to focus on that at this power level...In the shown perfoboard prototype, I even only added a C "snubber". Before that, I suffered from severe voltage spikes and corresponding ringing of the DC bus. After adding Cs between drain and source it was almost gone. Adding bulk C on the DC bus lowered it again significantly. I know, a C only "snubber" might be prone to oscillation but it worked for me. Of course, I did extensive measurements up to 15 A on the prototype.Nevertheless, I'm happy about anything that makes the circuit and layout easier. I'll add the footprints just in case and try a RC snubber.Quote from: Siwastaja on February 01, 2022, 02:47:20 pmCan you elaborate on that please? You mean adding TVS diodes on the DC bus for simple overvoltage conditions from Back-EMF when there is now power supply connected?Does it make sense to parallel some beefy TVS? (I have a bunch of 33v/1.5kA rated ones).Quote from: Siwastaja on February 01, 2022, 02:47:20 pmI'm using a 8S LiFePO4 custom built battery pack, so the DC bus voltage will be 30V. The MOSFETs have 55V breakdown voltage, the shottky diodes only 45V. If I can get rid of them, no worries about them.I attached a picture of the whole setup. Ignore the guy in weird clothes...

author: free_electron
author_rank: Super Contributor
timestamp: February 01, 2022, 03:45:26 pm
content: Quote from: nctnico on February 01, 2022, 02:27:48 amit depends. for thick copper boards they often do selective plating. there are many different techniques to do this.start with thin foil.drill holesapply negative mask ( copper that needs to REMAIN is exposed ) at this point the entire foil is still intact so every "future trace" is still shorted as one massive planeelectroplate thicktin-flash after plating.remove masknow you have a thin solid copper plane with thick plating on top. the plating is covered in tin . the tin flash is now your 'positive mask'etch. tin is not etchable. only copper. so you etch the thin foil in the 'valleys' and the walls of the valleys.the tin is chemically deposited / stripped / reused . There is no mask alignment issue as the same imaging mask is used to create the "tin mask". you make the positive tinmask directly from the negative photomask without requiring another photo-optical step.

author: Siwastaja
author_rank: Super Contributor
timestamp: February 01, 2022, 04:23:44 pm
content: f_sw and Vsw_max should not be in the same equation, so I'm quite sure you somehow miscalculated the snubber. f_sw only relates to the power loss of the snubber.Anyway, calculation is very difficult because estimating stray inductance (Lm in the appnote) is quite approximate. You can use rules of thumb like 0.1nH per millimeter of loop, of course. In any case, 1N4007 is too slow, use a fast diode, or a schottky. Also the whole idea of the snubber is, its stray inductance must be significantly less than the stray inductance of the loop it's snubbing, otherwise it has no chance. So use small components, close to the switches. You can add placeholder footprints like in your schematic, that's fine, but start with them unpopulated, measure and see. Testing the snubbers is highly educational. I remember the first time reading appnotes how to calculate the values, and ending up with more than order of magnitude different values by testing. Obviously, testing wins.Forget star ground, that's a recipe for EMI disaster, and significantly increases voltage drops along the paths simply because of having so much less copper. If you somehow manage to arrange the star in a way avoiding resistive voltage drops, then your loops are excessively long and have a lot of ESL. Star grounding works for really low-frequency high-precision analog. In power electronics, we just use contiguous low-impedance planes because some 10mV resistive drops mean nothing. Thanks to laws of physics, the return current of fast signals automagically follow on the ground plane right below the trace in question, minimizing the loop without you doing anything. You can only make it worse by introducing cuts or routing ground with traces. Now, DC or low frequency return currents concentrate on the path of least resistance, so you can see it's different. Cuts are sometimes used for precision analog.But this is also why you have current sense amplifier with gain, the sensitive part is tiny. The rest: just route the output and the reference pin as two kinda-pseudo-differential traces to the MCU. Even better if the MCU has differential ADC.If two full 18um planes in parallel (in other words, any arbitrary square-shaped region will be 0.5mOhm, remember, it's only about the aspect ratio, a thinner 2:1 section is 1.0mOhm) is too much resistance, then you need to reinforce it by introducing more copper from one of the outer layers, or soldering in those copper sheets or whatever that was already discussed in this thread. In any case, the solid planes offer optimal AC impedance everywhere.Regarding the TVS comment, I misread the tiny schematic picture, those were just IO protection diodes. Oh well, good to have those, too, they don't hurt. Personally, I prefer simplicity and integration, so just put the MCU on the same board, close enough, and trust the protection diodes within the MCU IO cells.Whether to add TVS clamping on the DC bus is up to you to decide. If you have enough DC link capacitance (i.e., some electrolytics, too), and overvoltage detection that turns off gate drive instantly, the capacitance itself limits voltage rise enough (you can simply calculate this from inductor and capacitor energy equations, knowing motor inductance and maximum motor current, and assume all this energy is dumped into the capacitors through freewheeling after you turn off the FETs at the very cycle you detect overvoltage. How much does the voltage rise after this?)Then the question of adding a TVS bank is: "can I afford that much capacitors", and if you can, then "is somebody going to physically rotate the motor beyond the maximum speed the motor rotates at full voltage". And then the TVS bank needs to be beefy enough in case that someone keeps rotating it despite feeling increased torque. This energy is converted into heat so finally a large enough TVS bank might be excessively big or expensive. You can also make a possibly unsafe assumption that the battery never disconnects, and assume no one is living on the top of the hill and regenerating the pack into overcharge. Or maybe you add an additional disconnection relay for the motor. Or, maybe you don't need to think about all of this from day 1, but at some point, it all needs to be considered, and how this integrates with the BMS. For a start, a TVS bank dimensioned based on available board area and pocket money is better than nothing.

author: Faranight
author_rank: Unknown
timestamp: February 01, 2022, 04:34:49 pm
content: Hai Ho!I'm gonna budge in here for a bit. I'm also trying to design a PSU board for several tens of amps. Is there any benefit (other than EMI reduction) when putting a ground plane directly underneath every power trace i.e. to serve as the current return path? For example on a 4 layer board you would alternate Power/GND/Power/GND or maybe Power/GND/GND/Power? I can't help, but wonder after watching so many of the Rick Hartley's videos where he explains that theenergy is in the fields™. I take it this only applies to high frequency traces, not the DC ones?Thanks.

author: poorchava
author_rank: Super Contributor
timestamp: February 04, 2022, 07:34:48 pm
content: When I was in Automotive, Wuerth Elektronic offered something called Wire-Laid PCB, which basically amounted to them ultrasonic welding strips of thick copper to inner layers of PCB before lamination. But that's probably absurdly expensive for a one-off, if even doable.In my work, when we had to design a 200A 8ph buck, we ended up doing a 2oz PCB and just soldered 5x5mm solid copper bars on both sides of the PCB. We do all the soldering in a standard reflow oven. Works just fine. Actually one time when software went tits-up it did something like 380A and the bars didnt overheat (eventually inductors desoldered themselves from the PCB )We used the bars, because thicker copper PCBs are quite expensive and they reduce the minimum track/gap parameters. For a very heavy copper like 10oz I'd imagine u need 1...2mm wide traces and gaps or something along those lines. And even then the cross section is rather small. At 0.5mm thick copper, which is like 12oz you'd still need a 50mm wide trace to equal a piece of a 5x5 copper bar.Unfortunately not at liberty to share the exact details of the technique to solder the bars successfully. It needed some figuring stuff out, and some trial and error, but is not difficult by any measure. We even managed to get good results using standard temperature profile.MCPCB just increases current handling capability of copper by effectively heatsinking the whole traces, while at the same being a paint in the butt because of (unless super special technology is used) only one layer.

author: SiliconWizard
author_rank: Super Contributor
timestamp: February 04, 2022, 07:42:55 pm
content: Quote from: tooki on January 31, 2022, 03:56:10 pmYep. It does.As already said, thicker copper can be an option, but: it's more expensive (sometimes pretty significantly so), and it's harder to solder on indeed. So, say you have one PCB with a mix of high-current traces and then small SMD parts, these may be pretty hard to reflow properly. It's not just a matter of picking thicker copper when ordering the PCB - it requires proper design.

author: Berni
author_rank: Super Contributor
timestamp: February 04, 2022, 08:06:31 pm
content: 5x5mm sounds like a serious chunk of copper there. With soldering copper plate onto boards i found its fairly important for the board not to twist and bend during the process, but solder paste can still fill quite a bit of a gap. Yes solder is much less conductive but its conducting in the vertical dimension while the copper is handling the horizontal spreading of current.One way to also deal with huge currents is place all your power electronics on a single sided aluminium core PCB (then stick that on a heatsink). The single sided does make layout more challenging but you can offload all the control electronics onto a normal board that sandwiches onto it with connectors. These boards are commonly used for cooling LEDs and are rather cheep even for prototype runs. You can get aluminium core in 2 sided or 2 layers but those are more specialized and much more expensive as a result.

author: T3sl4co1l
author_rank: Super Contributor
timestamp: February 04, 2022, 10:07:59 pm
content: Note that there is a physical limit to power capacity. It depends on device and layout size, switching speed, and voltage and current ratings.Consider an inverter (half bridge) circuit with two transistors switching alternately (or one is a diode, as for the regular buck/boost converter; it doesn't matter). When one transistor switches on or off, load current must reroute from that path, to another (i.e., between VCC and GND). This takes time, and extracts a price, paid as peak voltage drop across the inductance between those paths. Voltage drop is given by the inductance equation: V = L dI/dt. L is given by circuit dimensions and geometry. If V is limited by device ratings (say we have a 24V converter using 40 or 60V devices, so only 16-36V headroom), then we can't endlessly increase current, while keeping the same switching speed (holding dt constant). Instead, at some point, we need to limit switching speed to avoid device destruction.And so to maintain efficiency above some limit, we might need to lower f_sw to compensate for the increase in t_r and t_f, etc. Which makes the inductor and capacitors much larger, and the whole thing gets to be a mess.If we can afford higher supply voltage, headroom will be proportionally greater as well, and we can tolerate more L dI/dt. A 50A converter at 12V might be challenging to build, but a 50A converter at 600V is standard fare (you can even buy integrated modules for that).But if you want more current, at low voltage, and still keeping high efficiency and compact size, eventually you'll hit a wall.What then?Just use more.The key is not to merely wire devices in parallel: this does reduce device inductance, but suffers from difficulty in layout (you need a lot of overlapping connections to get everything connected solidly), and poor current sharing besides (because turn-on/off times won't quite match between devices, and it takes more time for those currents to equalize: on the order of t = Ls / Rds(on)).Instead, use smaller (individual) inverters, and wire them in parallel, modularly. They can also be phase-interleaved, partially cancelling input and output ripple, saving greatly on bypass caps.The downside is additional control complexity. For common applications, these are available in chip form (especially multiphase buck: consider the 8+ phases typical on PC CPU supplies!). You may have to employ hacks or custom solutions for slightly off-beat applications though (e.g. making a full CC/CV bench supply). And, some things I'm not sure about; does anyone make multiphase-inverter motor controllers, for example? (That is, the motor is whatever, but the inverters driving each phase of the motor, are in turn multiphase converters. I think, at the power levels where that would mostly be relevant (mains inverters, motive power / EVs), you'd rather use multilevel inverters instead?)The trick for something like a DC-DC converter is, assuming you don't have a controller to do it directly -- start by making each module a constant-current stage: a power transconductance amplifier, taking some input voltage setpoint, and delivering a proportional output current. A master error amp then adjusts current setpoint to regulate output voltage, say. This is especially easy with current-mode controllers (peak or average being the most common types), and then you can do stuff like full CC/CV by simply clamping the current setpoint, or at worst adding another error amp wired-OR in parallel with the voltage amp.Quote from: Faranight on February 01, 2022, 04:34:49 pmI'll do you one better:Top: gate drive signals (including Kelvin source connection if possible)Mid 1: +VMid 2: SWBottom: GNDThis minimizes layout inductance, so that it's limited almost entirely by device strays. For TO-247s, figure about 10nH per device. So, along with a film or polymer cap out front, maybe 25 or 30nH total. Which for say 16V overhead is about 500 A/us, or 200ns t_r/t_f at 100A peak. Not great, but doable. 200kHz would probably be a bit much for that, but lower is fine.Or at less load (or with multiple phases), 100ns at 50A would be reasonable for a compact and efficient design, or even dropping to TO-220s or SMDs (PowerDFN-8 or D2PAK with thermal pads top and bottom?) for 50ns or less at 30A.Tim

author: Neepa
author_rank: Regular Contributor
timestamp: February 04, 2022, 10:30:29 pm
content: May be a stupid noob idea, but a cheap one.Instead of using copper foil strips soldered to the trace couldn't one use fine copper solder wick instead?Burn the flux coating off of it with a lighter and then use the flux braid as flat woven copper wire.Or would that be a nightmare to properly solder without creating solder stalagmites pointing everwhere?Might need Louis Rossmann amounts of flux then.

author: T3sl4co1l
author_rank: Super Contributor
timestamp: February 04, 2022, 11:03:45 pm
content: Well no, leave the flux on it, you need it solderable don't you? Displace the flux with a modest slathering of solder -- cleans up real easy.I hang on to offcuts of wick for just this reason, though I don't actually use it much so it's slowly accumulating in my box of offcuts.Tim

author: Siwastaja
author_rank: Super Contributor
timestamp: February 05, 2022, 08:33:44 am
content: I have solderedusedsolder wick on the tracks once or twice. Brand new stuff - feels like a waste! It's going to end up soaked in solder anyway when you solder it on the tracks. Doesn't matter if it's already tin-soaked.Yes, it's copper braid so pretty useful. You don't have specified number for total cross sectional are of the copper strands, though, so exact calculations are impossible. Not that it usually matters.

author: EPAIII
author_rank: Super Contributor
timestamp: February 05, 2022, 10:06:59 am
content: I suspect that in addition to the lower volume, boards with thicker copper also require more time and chemicals to etch and may have more problems with undercutting so more time and care is needed in processing them.Quote from: Kryptychon on January 30, 2022, 07:51:50 pm

author: nvmR
author_rank: Regular Contributor
timestamp: February 05, 2022, 10:31:10 am
content: I usually use SaturnPCB software to get a general idea of what my situation is in terms of resistance\current carrying capability.Also, outside wire bodges do exists in different fashions, as described above and see the eevblog video here:

author: EPAIII
author_rank: Super Contributor
timestamp: February 05, 2022, 10:57:31 am
content: Well, the energy may be in or flow in the fields, BUT the current flows in the conductors, in the wires or copper traces. And we are talking about CURRENT here. You need copper or some other conductor (silver?) to handle that current. I worked with high powered transmitters (25 - 50 KWs) which used large diameter coaxial lines to transmit the power from the final amplifiers to the antenna. Those coaxial lines ranged from 3" to 6" and even 9" diameters and used copper tube with a thickness of about 1/16" or more. And we often talked about the energy traveling in the air, dry nitrogen or more exotic gasses between the inner and outer conductors. This volume was very important as it was vital to the characteristic impedance of the line. Now, just imagine reducing the thickness of those copper tubes from 1/16" down to 1/1000", about the thickness of common, household aluminum foil, while keeping the same dimensions for that inner space between them. Same area, same shape of that area for the fields. Same conducting copper surfaces on both sides of that space. And then apply that 35KWs to 50KWs of energy from the transmitter.I don't want to be standing anywhere near that transmission line when you do. The energy may be flowing down the space between those two conductors (inner and outer) but there is REAL CURRENT flowing in the conductors themselves. We talk about it as surface currents. A routine maintenance check at these high power transmitting plants was to climb on a ladder and feel the outside of the coax for hot spots. Those hot spots occurred at points where the impedance was not as continuous as it should be and the currents in the copper were out of balance and locally excessive. That is REAL current flowing in those copper conductors at VHF and UHF frequencies. And it can be enough to actually MELT the copper line, even the full thickness copper line.In all of science, it is important to remember that our understanding of the physical world is embodied in a number of THEORIES. These are theories, NOT LAWS. Oh sure, we talk about Ohms Law or Newton's Laws, but, in the end, these are really just theories. In science, theories come and go when new observations require it. Just how that electrical energy gets from point A to point B is also explained by theories. So when we are talking about how an electric current, AC or DC, moves from point to point, it is most often convenient to talk about charges moving around inside a conductor and obeying Ohm's Law. This is a THEORY. And it is only as good as it does accurately predict what we observe.Now, when we want to talk about high frequency electrical events or the very short time interval after a switch is first thrown in a DC circuit, then it may be more convenient to think in terms of E-M fields and how they expand, travel, interact, and are distributed in the space around and between those conductors. This is the area of another THEORY. And again, it is only as good as it accurately predicts what we observe.These are two different theories and neither is more right or more wrong than the other, at least in our present world and with our present understanding of the science. We, as practicing engineers, need to be able to choose which one is most relevant to what we are doing.These guys on YouTube may know alittlebit about science, but they know almostNOTHINGabout the way that science, in general, functions. A lot of presently, well known, medical doctors also fit into that category of ignorance.Quote from: Faranight on February 01, 2022, 04:34:49 pm

author: tooki
author_rank: Super Contributor
timestamp: February 05, 2022, 12:03:21 pm
content: Quote from: EPAIII on February 05, 2022, 10:06:59 amAgain, the thickening is performed additively, so undercutting isn’t a big issue because only averythin layer of copper is etched away at all. The rest of the copper is plated on after masking off the areas that will later be free of copper. It’s a fundamentally different process from the one used for DIY PCB etching.

author: Berni
author_rank: Super Contributor
timestamp: February 05, 2022, 12:18:44 pm
content: Quote from: EPAIII on February 05, 2022, 10:57:31 amWell he did pose a perfectly reasonable question. It is about weather the return currents in the ground plane also follow the shape of the traces in the case of this H bridge. This is typically the first thing people explain when it comes to high speed PCB design.So if the return current is motivated to follow the trace shape this means that the current is getting focused down along a more narrow channel, making less effective use of the available copper cross section, leading to a higher apparent resistance and so more heat losses. It is indeed the fields that motivate the current to do this.That being said the PWM frequencies involved in a Hbridge along with the relatively small physical size mean these effects should not be significant enough to really affect the current path in any meaningful way, so we can assume steady state DC current flowing trough the tracks using all the available copper crosssection. This is indeed only significant in keeping down EMI emisions as those can go well into the MHz ranges due to the sharp edges, as those will follow the ground plane and might decide to ignore your filtering capacitors if they are in the wrong place. Only case where this might become important is if you really snake things around too much and pick bad spots to hook up the ground for mosfet gate drive. This might accidentally create a RF amplifier using the MOSFET, that then finds a positive feedback path and so turns into a RF oscillator. This can actually spew out massive amount of RF while the transistor gets really hot really fast (Trust me those huge slow power MOSFETs can actually sing at >400MHz in the right conditions).So circling back to using 4 layers. Yes there is benefit to using them since the typical 4 layer keeps layer pairs(1-2 and 3-4) close together so you get significant thermal transfer between those two layers. A large internal ground plane can act as a heatsink for a smaller track on the top, spreading out its heat and so allowing the track to handle more current before it gets too hot. But one off prototype boards with thick internal copper are going to be even more expensive.For a one off board like this i agree with the suggestion above of manually soldering extra copper wire on top of the high current tracks. This helps increase the current capacity way way way more than just putting a thick layer of solder on them.My other single sided aluminium core PCB is more of a production solution since it provides the ability for densely packed power electronics to be cooled by just bolting the whole PCB to a heatsink rather than assembling the power parts from individual transistors that need to be individually thermally bonded to a heatsink. Most smaller electric vehicle motor controllers are built this way

author: T3sl4co1l
author_rank: Super Contributor
timestamp: February 05, 2022, 08:38:40 pm
content: Quote from: Berni on February 05, 2022, 12:18:44 pmTypically, the problem is a low gate impedance, particularly reactive. So, avoid capacitance between G and S, for example. A somewhat common instance is clamping gate voltage with a zener/TVS: the junction capacitance, merely 50pF or whatever it might be, is enough to form a resonant stub with its body, trace and pin lengths, in the loop with the FET. Those lengths might total say 20nH, so the combination has a series resonance at 160MHz. It takes even less (length and C) to sing at 400!This seems crazy, or perhaps useful if you're a schemer like me. Well, it comes down to power bandwidth.The transistor is amplifying up there, just like under any other condition. The microscopic FET structures themselves, are ideal in comparison, and are limited by internal and pin impedances. Resistances act to dampen behavior and set a limiting  impedance, while the capacitances and inductances act to set a roll-off in response, or a ceiling on ultimate bandwidth, depending on how they're arranged internally. On-die, the spreading resistance and gate capacitance dominate, while packaging tends to dominate in inductance (corresponding to pin lengths).Some transistors may roll off smoothly (i.e. ~1st order), thus exhibiting a GBW, like an opamp does. This is more common these days I think, suggestive of a fractal interconnect pattern (i.e., giving similar spreading resistance to every transistor cell).In the olden days, they'd just fill the die with gate and source metallization and that's that, so the spreading resistance depends on region, and gate drive tends to diffuse out from the bond pad -- literally diffuse, as in, having a 1/sqrt(f) dependency. You can think of it as, when a step is applied, a wave spreads out from the bond pad; or at a given frequency, some radius of area around the pad is actively amplifying, while the rest is just dead weight, and only at low enough frequencies does the whole thing act together to amplify or switch.For example, the GBW of a 2N7002 seems to be about 40MHz when measured at, whatever it was, 5MHz or something (i.e., having a useful gain around 18dB). But it doesn't go to zero at 40MHz. In fact there's still a few, 8dB or so left at that point, suggesting GBW is actually 120MHz or so. And so on; it drops off gradually, not along a proportional GBW curve but shallower than that. It might still have real gain out at 200MHz -- it's just that you'll be wasting so very much power, eking out just those few decibels, that, there's no way, obviously you will go out of your way to get a proper RF transistor at this point.(Apologies for the vagueness; I once measured this for a simple amplifier test case, years ago, and not sure if/where I wrote down the data. Anyway, the exact measurements don't matter, just something representative.)Whatever the case, gain drops with rising frequency, but it doesn't suddenly go to zero or anything. If you figure you've got full power response at some MHz, for a modern switching transistor*, then that's some ~kW perhaps, and if it's dropping at 20dB/dec then that's still a few W left at some 100s MHz!*Mind, not that you'd want to, or be able to, run it this hot -- think of it as doing switching edges 100% of the time, the dissipation is insane. You could run a pulsed (tone-burst) amplifier this way, but not any kind of continuous amplifier or power supply.The thing with switching transistors is, they're intentionally made to have much greater switching capacity (Vds(max) * Id(max)) than power dissipation. RF transistors have it equal, or even the other way around, so that they can handle full continuous power in a linear amplifier. Which is likewise why you never see RF transistors in switching circuits. You can get quite high efficiency from something like that, say a 100W transistor doing >90% eff. at 10MHz or more -- but only getting like 10W for all that trouble, and that transistor cost $20!So, all that, just to introduce the idea that, power capacity and gain are related, and that not much gain is required to make a power oscillator: much less than a practical amplifier might need.And, obviously, for EMI purposes, a watt at 400MHz is not something you want your power supply doing!Anyway, the typical behavior is, given a low impedance (series resonant) gate circuit, it will light up when the FET has enough GBW: it won't oscillate in saturation (ohmic region) because there's no gm at all; at low Vds, capacitances dominate and dampen everything out; and in cutoff, gm is again nil. So it's during the middle portion of swing, where Vds and Id are modest, so the capacitances are small and gm is large -- you get a little tone burst, maybe a dozen cycles of 400MHz or something, maybe 10V tall.Because it's well into the cutoff range, there's unfortunately nothing useful about it; you can't set up an amplifier tuned to that frequency and trick it into high gain, even if the bandwidth is low. It's only enough gain to be an annoyance when it goes unstable.As for other circumstances -- it's usually pretty hard to get that kind of low impedance just from layout. Plain inductance isn't as dangerous for gate drive purposes, and you'd never have enough trace width to get the impedance that low. (I did once make a protoboard with ~2cm width transmission lines going between controller/gate driver and the power stage; this had I think ~200MHz blips. A ferrite bead on the gate pin did a fine job squelching that: the ferrite saturates under peak gate current so doesn't impact switching speed much, and its inductance (when not saturated) stores little enough energy that overshoot was insignificant. Downside, this was a test at like 2MHz and the bead got pretty toasty -- something like half a watt was flowing to that gate!)And yeah, in any case the most likely fix is to increase the minimum impedance to the gate pin: simply add a resistor. This makes it safe to use a zener diode, for instance.Tim

author: mawyatt
author_rank: Super Contributor
timestamp: February 05, 2022, 10:18:08 pm
content: Quote from: T3sl4co1l on February 05, 2022, 08:38:40 pmThis is not uncommon behavior with modern day high speed transistors and FETs, and why Fmax (unity power gain) is generally a better metric to judge these type devices. Ft is more a figure of merit that is somewhat valid as long as you are well below 1/10 Ft, whereas Fmax is something you need to pay attention to everywhere. Dr Ken O at University of Florida proved this point over 20 years ago with a 32nm NMOS device, he created an oscillator at 402GHz, and recall the device Ft wasn't even close to 100GHz!!, He published this work, and followed with another paper that answered the obvious question, "How do you know it's oscillating?". He slowly ON/OFF modulated the VDD power and cleverly illuminated the NMOS device with an attenuated laser signal, then looked at the optical sidebands of the reflected optical signal with an optical spectrometer. Two sidebands appeared around the laser signal at +-402GHz in synch with the ON/OFF modulation!! The message here is one needs to pay attention to things well beyond Ft with modern high speed devices, and Fmax is is the actual limit of performance.QuoteOne of the very interesting research topics that was just emerging when I retired a few years ago, was related to the need for very low noise RF/MW/MMW power amplifiers. Traditionally these were linear type amplifiers, but research had shown that contrary to common belief switchmode power amplifiers could challenge and even surpass linear amplifiers in noise performance!! The general idea was the active device (usually GaN) produced no active noise when saturated (no gain) and no noise when cutoff (no gain), and only produced noise in transition when the channel was active with gain. This required devices capable of extremely fast switching speeds which were becoming available. If interested I'm sure a search over at IEEE Circuits & Systems, Solid State Journal, and Microwave Techniques will turn up a number of papers today. Anyway, another good example of how new semiconductor devices are changing the way things are viewed and approached.Best,

author: Kryptychon
author_rank: Contributor
timestamp: February 06, 2022, 12:40:07 pm
content: Hello again,Quote from: Siwastaja on February 01, 2022, 04:23:44 pmI'm aware that peak voltage is idependent from switching frequency. I know, that the power dissipated depends on the amount of C, the delta of Vcc and Vpeak and the switching frequency.I did the calculations with 40V target peak voltage at 30A peak current. I assumed a stray inductance of 200nH. The MOSFETs have 55V breakdown voltage, which gives 15V headroom. That might be "okay".I don't know reasonable safety margins in industrial applications.Quote from: Siwastaja on February 01, 2022, 04:23:44 pmOkay, got that. Thanks. As you probaly already noticed, my concerns come from missing experiene in the field. I read a lot about all these things but I've not much experience. Identifying what is important in what situation is a challenge for me. It's so helpful how you break it down in simple and intelligible sentences. Now, I've a far better understanding of the relevance of the different GND routing techniques and their applications.Quote from: Siwastaja on February 01, 2022, 04:23:44 pmNice, that's exactly what I was thinking to do. Unfortunatelly, the MCU does not have a real differential ADC input. I'm also thinking about having a dedicated ADC on the current sensing board because I'm concerned of using analog signals on cables which connect the different modules (H-bridge and current sensing board with the MCU board). I guess, if I use a schielded cable at reasonable length and provide the reference protential to the MCU's ADC that might not be a problem.Quote from: Siwastaja on February 01, 2022, 04:23:44 pmI understand that and I'll do it this way. I need to reinforce the high current traces anyways, so I decided to not bother too much about the layer stackup. I'll do it like you proposed: 4 layers, two inner GND layers and Vcc on the top or bottom layer. I'll reinforce Vcc and GND (which then must be routed on top or bottem layer for these traces) where needed.Quote from: Siwastaja on February 01, 2022, 04:23:44 pmMy abitious goal is to develop modules which can be plugged together as needed. The driver IC inputs come from external sources might even be a different MCU or whatever digital input), I think putting the input protection in front of the drivers is a must have in this design.Quote from: Siwastaja on February 01, 2022, 04:23:44 pmYou're right, I think it's up to me to decide. I'll go with some additionaly DC link capacitance and add the TVS diodes. I think you nailed the most important point in any project: Defining the requirements. There are reasonable requirements which might cover 90% of the possible application area and there are extraordinary requirements. The latter ones, I want to push to the next revision of this circuit ;-)Thanks for all your help!

author: Kryptychon
author_rank: Contributor
timestamp: February 06, 2022, 12:46:10 pm
content: Quote from: Berni on January 31, 2022, 11:30:43 amThanks for this advise! I'll try to spread the heat produced by using polygon pours as Siwastaja proposed.