Two-phase Boost Converter Layout Questions - Page 1
Forum section: electronics / general

author: tinfever
author_rank: Regular Contributor
timestamp: June 05, 2025, 05:46:53 pm
content: I’m hoping to get some big picture feedback on the layout for the next rev. of a two-phase boost converter I've faced some stubborn stability issues with (detailed here:https://www.eevblog.com/forum/projects/boost-converter-oscillation-bursts-during-load-step).This converter is designed to boost from 18-34 V input to 60 V 16 A output with only intermittent loading. It uses an LM5171 two-phase controller operating at 600 kHz.I’ve attached images of the first board revision layout that I'm starting from.The first board showed instability in the current control loop and the controller’s IMON signal that output the measured inductor current looked very strange for one of the phases.Primary question: Could the layout of the sense trace pairs (Layer 3, partially circled in blue) for the inductor current shunt cause issues?The sense traces are between two solid ground planes, but the sense traces are also near the ground vias for the switching current going through the output capacitors. Could somehow the ground switching currents be coupling into these sense traces and creating issues? Would there be a better way to route these? I see some examples routing them on adjacent layers, one on top of the other.Secondary questions:I’m planning to get rid of the split analog ground (highlighted in last photo). Does that seem reasonable?Would it be worth changing the layout by relocating the controller to the input side of the board, to the left of the inductors and FETs? This would in theory be quieter, away the discontinuous switching currents, but it would also make the input high-continuous-current path longer. It would also lengthen the gate drive traces but would shorten the current sense traces.I’ve read some recommendations to have the power input and output connectors right next to each other, rather than on opposite sides of the board. Would this offer any benefits in this case?

author: mtwieg
author_rank: Frequent Contributor
timestamp: June 07, 2025, 05:10:00 pm
content: Quote from: tinfever on June 05, 2025, 05:46:53 pmSo you still have the issue with Imon2 looking wrong?My first assumption would be something wrong with your current sense circuitry (bad solder joints, damaged components, wrong values, broken traces, etc). After that, I would assume the LM5171 itself is damaged somehow, and would try replacing it.QuoteI think the way you've routed them is fine. I highly doubt that routing could explain the IMON2 issue you've had. If you're really worried, you could route them on the bottom layer so they're even more shielded from the switching currents.QuoteI don't think broadside coupling has any real advantage over edge coupling (as you have) for this sort of application. The choice between them is mainly about what stackup you have.Quote"split GND" is always something I caution against, as it usually means someone is trying to split the board area into different partitions, and then we have to worry about via stitching and ferrite beads and it turns into a nightmare.But what the LM5171 datasheet suggests (particularly figure 7-36) is a much more reasonable approach which I usually refer to as a local star ground. Basically all of the signal conditioning components (and their bypass caps) have their own AGND which connects to PGND at one physical point. This ensures that the large switching currents on PGND will not flow on AGND (the single-point connection to PGND means there is no return path available through AGND).I do this often for PWM controllers. Though keep in mind that this is only really helpful from the perspective of the PWM controller itself. In reality, AGND will likely have common mode bounce on it, but for other circuits referenced to AGND this bounce doesn't matter. If you were to probe those circuits with a scope, they might have a lot of switching noise on them (because your scope is not referenced to AGND).QuoteAgain I don't think one way has a significant advantage over the other. Both can work fine if done smartly, or fail miserably otherwise. If one option is more attractive from the standpoint of troubleshooting and testing, go with that.QuoteI'm assuming this is regarding common mode emissions. Such decisions should be made at the system level, not a board level. For example, need to know where the input power is coming from, where the load is, along with all signal inputs/outputs, and how everything ties to safety or functional earths....Overall I would try and space things out a little bit around the LM5171. The only paths you should really keep as short as possible are the discontinuous current paths in the power circuitry, and I think you've done find there. But you don't have to cram everything so close to the LM5171 itself. Let the stuff breathe a bit.As for the gate driver routing, you can actually get away with adding quite a bit of distance so long as the return paths are done properly. But I can't tell from your screenshots what's going on there, higher resolution would help.

author: tinfever
author_rank: Regular Contributor
timestamp: June 10, 2025, 06:03:51 pm
content: Thank you very much for the feedback! That all makes a lot of sense. Getting input from someone experienced helps me tremendously in sorting out what I should and shouldn't be concerned about.QuoteCorrect. That makes that a physical problem is the most likely culprit for the IMON2 problem. I've done so many modifications to this board that it's hard for me to know what it's state is. I just decided to just do a new revision incorporating what I learned from the first one so I have a clean place to work from. I've included an image of the work-in-progress placement for this second revision.QuoteI'm trying to design this to be as compact as possible because it will hopefully, eventually, go into a very space-constrained robotics application. Once I get this working properly, I'll probably try doing a version with the controller on the back just to make it even more compact. What are the benefits of spacing things out a bit more? I guess ease of rework is one?QuoteIf I'm planning on cramming stuff as tightly together as possible, would that be more of a reason for me to keep the local star ground on the controller? Although, I don't fully understand how a local star ground helps the controller. It makes sense to me that if the controller circuitry references the same ground planes that contain the switching currents, ground for one part of the controller circuit will be at a different potential than ground at another part. My gut instinct is that the differences can't be that high across several solid copper pours stitched together, maybe 10's of mV? Can it be enough to create problems?If I keep the local star ground, then I'm concerned about having all the analog signals not routed over their associated ground plane, so now I have a lot of loops that can pick up interference. I'm not sure if this is a rational concern though. Maybe with PWM controller analog circuitry we are more concerned about "conducted" interference like ground bounce than we are about radiated interference?If I keep the local star ground, can I route that any better? (Zoomed in image attached)QuoteI've attached zoomed in images of the gate drive routing. Ithinkthis is decent.The high-side gate drive signal (pin 15) goes down to layer 3, across and then back to layer 1 for the gate resistors for each FET, back to layer 3 and across, then up to the respective FET gate pins. The return is a switch node copper pour on layer 4 connected to the FETs and run directly underneath the gate drive traces until it connects to the SW2 pin (pin 16) on the LM5171.The low-side gate drive signal (pin 17) goes down to layer 3, over to the FETs, then up to the gate resistors and into the FET gate pins. The return is the power ground place directly adjacent on layer 2 connected to pin 18 on the LM5171.

author: mtwieg
author_rank: Frequent Contributor
timestamp: June 11, 2025, 12:03:50 pm
content: Quote from: tinfever on June 10, 2025, 06:03:51 pmEase of rework is certainly one. Also trying to pack components as tightly as possible leads to routing becoming far more complicated and requiring more layer changes and vias (like in your current sense filters).Putting SMT components on the bottom side would certainly help. Specifically the current sense input filter components. I think if you just do that, then the top side layout can be cleaned up quite a bit (and the AGND can become a lot more compact).QuoteImpossible to say whether the local star ground is necessary/helpful without empirical measurements or extremely sophisticated simulations. I think of it like choosing bypass caps for MLCCs. Sure you could analyze things and determine the minimum/optimal bypass capacitor values, but 99% of the time it's a waste of time and just following the datasheet's suggestions is fine.QuoteIt's assumed that even with the local star ground, you still have at least one completely solid ground/supply plane underneath everything. That should shield out most magnetically induced emf, even for circuits that don't connect directly to that plane.QuoteI think you have the most important aspect down (overlapping the gate traces over their return paths). I might try and use the layers differently, but that depends on the details of your stackup.