Kindly requesting help with debugging a TSP61220 (PCB) voltage boost converter - Page 1
Forum section: electronics / beginners

author: MichielvanBeers
author_rank: Contributor
timestamp: September 19, 2025, 01:58:53 pm
content: Part Number: TPS61220Datasheet:https://www.ti.com/lit/ds/symlink/tps61220.pdfFirst of all, thank you for thanking the time to read through my challenge and help me debug what might be going on. I've been bumping my head against this issue for a while bit unsure how to continue from here, so any help/thought/feedback/input is greatly appreciated!ProblemI'm seeing unexpected voltage output and fluctuating current input on the TPS61220 that I've soldered on my custom PCB (details can be found below). I would kindly request help to debug what might be going wrong in my setup.ContextI'm planning to incorporate a TPS61220 voltage boost converter in my project. To learn how to design the final PCB, I've designed a small PCB to test out just the boost converter. I've modeled the design to the TPS61220EVM-319 evaluation model. Here is the product page & data sheet for reference:https://www.ti.com/tool/TPS61220EVM-319Notes- I'm a hobbyist/enthusiast without any electrical engineering background, so could well be that I made some silly mistake, any help is appreciated- I don't have access to an Oscilloscope, but if there is something <$100 that would help with debugging, I'm okay with buying additional tooling.Notes on the data below- R1 and R2 are swapped around compared to the TPS61220 datasheet.- I've used 180k instead of 178k resistor for R1 (in my datasheet)- Therefore, I expect: VOUT = VFB × (R2 + R1)/R1 = 0.5 x (1000+180)/180 ~ 3.28VSchematic and PCBFigure 1: SchematicFigure 2: Front Layers PCBFigure 3: Back Layers PCBFigure 4: Photo of assembled PCBMeasurementsNote: I don't have an Oscilloscope so the data collected below is from my Power Profile Kit II providing input voltage and current and a Multimeter measuring the output voltage.Input voltageOutput voltageStablePower Consumption Screenshot1.00v1.56vYes1v.png1.50v1.57vYes1.5v.png2.00v1.57v - 1.59vNo2v - with load.png | 2v - without load.png2.50v1.92vYes2.5v.png3.00v2.30 - 3.00vNo3v.pngFigure 5: 1v.pngFigure 6: 1.5v.pngFigure 7: 2v - with load.pngFigure 8: 2v - without load.pngFigure 9: 3v.png

author: ahsrabrifat
author_rank: Regular Contributor
timestamp: September 20, 2025, 11:02:13 am
content: There are inexpensive hobby DSC kits/USB scopes in the <$100 range (DSO138, DSO Nano variants, low-cost USB scopes) that are capable of capturing switching waveforms for debugging.

author: MariuszD
author_rank: Regular Contributor
timestamp: September 20, 2025, 11:41:40 am
content: Quote from: ahsrabrifat on September 20, 2025, 11:02:13 amDSO138 has a 200kHz bandwidth and a 1MSPS sampling rate. It is useless for examining a converter operating up to 1MHz. Scope should be at least 10 times faster.

author: Psi
author_rank: Super Contributor
timestamp: September 20, 2025, 11:53:18 am
content: What type of inductor is it?The core material i mean

author: Slh
author_rank: Regular Contributor
timestamp: September 20, 2025, 12:11:50 pm
content: Layout isn't great. Have a look at section 13.2 of the datasheet for the TI example. There's a lot more copper and a continuous ground from input to output.The evaluation module user guidehttps://www.ti.com/lit/ug/slvu253/slvu253.pdf?ts=1758370102438&ref_url=https%253A%252F%252Fwww.ti.com%252Ftool%252FTPS61220EVM-319warns about stability issues in section 5.1 if the layout isn't good enough.

author: tooki
author_rank: Super Contributor
timestamp: September 20, 2025, 02:04:20 pm
content: Quote from: MichielvanBeers on September 19, 2025, 01:58:53 pmOK. I checked your values in WEBENCH, but the simulations show no problems.What is your load, when testing under load?Quote from: MichielvanBeers on September 19, 2025, 01:58:53 pmWeeeellll... you didn't actually model it on that, at least not the parts that matter!In a DC-DC converter, the critical layout paths are the main current loops:(Image from:https://www.powerelectronicsnews.com/the-dc-dc-boost-converter-part-3-power-supply-design-tutorial-section-5-3/)In your case, both the MOSFET and diode are integrated in your IC.The key thing is that these loops should be as short and fat as possible. Unfortunately, in your layout, the larger blue loop on the left isn't short and fat, but instead goes through the ground plane, via two vias. These increase inductance and resistance. (Think of them as very thin.) You prioritized the layout of the feedback resistors R1, R2 at the expense of the ground connection, but the ground is much more important.In the eval board, you can see that the input and output grounds are connected directly, right on the top layer.The TPS61220 web page has many documents linked, and one of them isFive Steps to a Good PBC Layout of a Boost Converter. It might be a bit advanced for you (and the example is based on a different chip), but the order of layout is important, because it's the relative importance in the layout:1. output capacitor2. inductor3. input capacitor4. small signal components (e.g. feedback resistors)5. signal groundIf anything, this document doesn't put quite enough emphasis on thepower ground, mentioning it almost in passing in step 3:QuoteThe key is that these are meant to be on the same layer, as compact and direct as possible. This is the thing you missed.Look back at the eval board layout: the input ground connects directly to the output ground as one uninterrupted fat trace. That's what you need. The feedback resistors work around that without interrupting it.Also, in your layout, all of the input current through the circuit (the large blue loop) flows past R1 en route to the ground plane. This means the voltage at R1's ground pin is actually bouncing around a tiny bit depending on input current flow, and that in turn means the feedback voltage will bounce a bit, too. Since the feedback current is very, very low, this is a somewhat noise-sensitive signal. The feedback resistor should be referenced to the output ground. In step 5, the TI guide says: "Make sure no large power current is flowing through the Signal-Ground. Otherwise, noise coupling into the control circuit could causes bad output voltage regulation, inaccurate current limit, or other abnormal behaviors." -- and that seems to be exactly your situation. (The R1 ground is your only signal ground.)One thing you could try with your board is to solder a short (!!) wire directly from the ground of C1 to the ground of C2, and maybe even also cutting the trace between C1 and R1 so that no input current is flowing through the ground plane, causing R1 to essentially be connected directly (and only) to the output ground.

author: MichielvanBeers
author_rank: Contributor
timestamp: September 21, 2025, 12:55:29 pm
content: First of all, thank you all for taking the time to read through and answer my questions (especially @tooki for theveryelaborate answer)!Quote from: MariuszD on September 20, 2025, 11:41:40 amThank you for the tips! Could you explain why I would need a scope that is at least 10 times faster? I often see second-hand 50MHz or 100MHz scopessuch as this Hameg HM504-2 50MHz Oscilloscope. Would it be worthwhile investing in one of those?Quote from: Psi on September 20, 2025, 11:53:18 amI'm using ceramic capacitors.These ones, to be precise. My understanding was that I needed ceramic capacitors due to their low ESR and ESL. Is this correct?Quote from: tooki on September 20, 2025, 02:04:20 pmThanks! This information is super informative and helped me get a better understanding of what is actually going on 🙏🏻Quote from: tooki on September 20, 2025, 02:04:20 pmJust the load of the multimeter I'm using. I'm not sure how much this is or how I could figure that out.Quote from: tooki on September 20, 2025, 02:04:20 pmReviewing my previous design after your feedback made me see all the things that were wrong with my initial design, haha! So I think I'll just go straight to ordering a new PCB.Based on your feedback and the documents provided, I've updated the PCB design, which you can find below. While updating the design and reading through the documentation you provided, some new questions came up. Could you help me answer those?QuestionsI'm trying to understand the difference between Signal-Ground and Power-Ground. Is my understanding correct that:Signal-Ground is the trace going from GND -> R2 (in my new design)?Power-Ground is the large ground plane on the front-layer?Connecting the trace from GND -> R2 instead of the large ground plane is sufficient to separate the interference?I have moved the large connecting ground plane to go through the middle of the TPS61220, as shown inFigure 1 and 2 of the TPS61120EVM-319 User's Guide(e.g. the plane going through the U1 silkscreen). This plane doesn't 'feel' very thick though. How do I know if this is thick enough (except for comparing it with the EVM design)?The VIN input is now connected through a via and the back layer to VIN Pin 1 of the TPS61220, which I think is the same way the EVM documentation shows it. My understanding is that there might be relatively a lot of current flowing through those vias and trace. Could that be problematic?I have added a large ground plane on the back layer with two vias, as shown in the EVM documentation. Is this for heat dissipation?After reading theFive Steps to a Good PCB Layout PDF, it made me wonder if the SW pin of the TPS61236 is similar to the L pin on the TPS61220. However, when comparing the layout in the five steps (see Figure 3 at the bottom), I see the inductor of the TPS61236 connected to both VOUT and VIN, which is different from the design inthe Power Electronics Tutorial that you shared. Maybe this is too in-depth, but I was curious about that difference.Changelog PCBSwapped the labels of R1 and R2 to match datasheet.Updated the value of R2 from 178k to 180k to match actual implementation.Moved the input and output pins down so L1 could move to the left and closer to the L pin of U1.Decreased length and increased thickness of Net-U1-L, using a plane instead of a trace.Connected the GND of Power In, Power Out, the capacitors, and U1 GND directly with a broad ground plane.Decreased clearance for paddings of U1 to 0.1mm to allow for broader GND connections.Decreased clearance of Net-J1-VIN to 0.2mm to allow for a broader GND plane.Figure 1: Front-layersFigure 2: Back-layersFigure 3: Comparison of TPS61236 and TPS61220

author: MichielvanBeers
author_rank: Contributor
timestamp: September 27, 2025, 05:12:52 am
content: Hi there,Thank you for all the help so far! I was wondering/hoping if someone could do a short peer-review of my updated PCB designs in the previous post. I think I've incorporated all the feedback of @tooki, but would be great if another pair of eyes could look at it, before I send it of for production. Thanks in advance 🙏🏻

author: mdijkens
author_rank: Regular Contributor
timestamp: September 27, 2025, 07:53:15 am
content: If needed you can borrow my Oscilloscope (Amsterdam)

author: Psi
author_rank: Super Contributor
timestamp: September 27, 2025, 09:42:30 am
content: Quote from: MichielvanBeers on September 21, 2025, 12:55:29 pm

author: tooki
author_rank: Super Contributor
timestamp: September 27, 2025, 11:22:42 am
content: Quote from: MichielvanBeers on September 21, 2025, 12:55:29 pmWhat he means is that thesampling rateof a digital oscilloscope needs to be at least 10x theanalog bandwidth.For example, if your DC-DC converter runs at 1MHz, then you need a scope with an analog bandwidth of at least 1MHz, and for a digital scope, the sampling rate needs to be at least 10MSa/s (10 million samples per second).With any "real" oscilloscope this is no problem. Modern entry-level digital scopes (like the ~$400 models from Rigol or Siglent) have an analog bandwidth of 50-100MHz and a 1GSa/s sampling rate.Theory:TheNyquist-Shannon sampling theorem, which forms the foundation of digital signal acquisition, stipulates that to perfectly capture a signal, you must sample at greater than twice the frequency of the highest-frequency content of the signal. Because any content above that frequency ("Nyquist frequency") causes errors called aliasing, it is critical that the input signal be strictly bandwidth-limited. But because it's actually really hard to make a super-steep low-pass filter like that, what we do instead is use easier, gentler filters and a higher sampling rate. For example, human hearing has a very best-case bandwidth of 20Hz-20kHz. Because it's basically impossible to make a filter that cuts off sharply at 20kHz, which would be needed for a 40kSa/s sampling rate, we instead use a simple filter and sample at 44.1kSa/s instead -- the simple filter easily cuts of fully by 22.05kHz.Now the part that's even less obvious: a signal with a frequency ofnHz can containcontentwell aboven. In fact, the only signal thatdoesn'tis a pure sine wave. Every other waveform can be constructed out of a sum of sine waves. Frequency content is actually a function of therise timeof a signal. A theoretical square wave with zero rise time (that is, one that transitions from high to low instantly, with no slope at all) hasinfinite frequency content. What this means in practice is that, for example, a 100MHz oscilloscope cannot actually give a realistic depiction of a 100MHz square wave. (See:https://en.wikipedia.org/wiki/Gibbs_phenomenon)Having a higher sampling rate in an oscilloscope means the scope can display the signal with a bit more accuracy, taking advantage of the fact that a scope's analog bandwidth doesn't cut off harshly, either. (Many cheap 100MHz scopes, for example, can actually "see" signals up to 300MHz or more, such signals are just severely reduced in amplitude. So you still need the sampling rate to prevent those frequencies from causing aliasing.) It also means the scope can use different approaches to signal reconstruction.FYI, the very best intro to digital sampling theory is thisvideo(transcript)As far as what scope to buy: I would recommend buying a modern entry-level scope from Rigol or Siglent for around $400-600. It's a far, far more useful tool than an old Hameg, nice as those are.Quote from: MichielvanBeers on September 21, 2025, 12:55:29 pmRead his question carefully. He didn't ask what kind of capacitors you used.(Though for the future, I would suggest not buying components from Aliexpress, Amazon, etc. whenever possible. You don't know what you're going to get, especially for "simple" parts like caps and resistors. To the extent possible, buy parts from reputable distributors like Digikey, Mouser, Farnell, Conrad, Reichelt, Distrelec, RS, TME, etc.)Quote from: MichielvanBeers on September 21, 2025, 12:55:29 pmIt's stated in the specifications of your meter as the input resistance or input impedance. It's commonly 1Mohm for very cheap meters, 1-11Mohm for handheld multimeters, and bench multimeters often go up to the Gohms. Analog multimeters are much lower.With that said, that basically means you didn't really test under load, insofar as a multimeter represents a very, very tiny load.Quote from: MichielvanBeers on September 21, 2025, 12:55:29 pmIreallythink you should test my suggested modifications before ordering a new PCB. I am just making educated guesses as to the problem, and making the modifications will help determine whether that is correct, or if the problem is actually something else. (For example, an unsuited inductor, which is why Psi asked you.)It'd be stupid to not try a simple modification to help isolate the cause.Quote from: MichielvanBeers on September 21, 2025, 12:55:29 pmAnswers:1.1. Correct1.2. Correct1.3. Yes.2. Given the small output of this converter, it should be fine. But I will say that intuitively (and contrary to the EVM), I would have just made a straight, fat top-layer connection from the grounds of C1 to C2, with the IC's GND pin touching directly through as fat a fill as you can fit. Then I would connect R1 and R2 using thin traces on the bottom layer, popping up under the chip with vias. However, I would follow the EVM layout, as they will have done it that way for a reason.3. No. Look at the block diagram of the chip: the actual switching path that the high current flows through is from "L" (pin 5) to "Vout" (pin 4). The Vin and EN pins use very little current.4. Probably for heat and EMI shielding.5.Yes, L is the same as SW.

author: MichielvanBeers
author_rank: Contributor
timestamp: September 28, 2025, 08:26:03 am
content: Thank you all once again for the detailed and helpful responses!Quote from: Psi on September 27, 2025, 09:42:30 amMy apologies, apparently got the two mixed up in my head. The inductors I'm using arethese ones(again from AliExpress, I'll make sure to order these from more reputable distributors in the future). On the product page I couldn't directly find the core material, but on Mouser.com I did findthis documentwhich looks to have the same type/number (CDRH74). Based on that datasheet I see it saysFerrite drum core construction. So, I would assume that the core material is ferrite?Quote from: mdijkens on September 27, 2025, 07:53:15 amThis would be awesome @mdijkens! I'll reach out to you in a DM.Quote from: tooki on September 27, 2025, 11:22:42 amThank you for very detailed information once again! I see I have some learning to do haha. I'll make sure to review your content and videos in depth, so I get a solid understanding of these first.Quote from: tooki on September 20, 2025, 02:04:20 pmNoted, thank you. I'll make sure to add some actual load in my load tests.Quote from: tooki on September 20, 2025, 02:04:20 pmClear as well, thank you. I'll be taking your advice to heart. Based on your input, I'll take the following steps first, before ordering a new PCB (feedback is of course welcome):Reach out to @mdijkens to borrow the oscilloscopeReview content regarding Digital Sampling Theory and oscilloscope usage.Solder the wire from GND C1 to GND C2Do the same measurements with the Power Profiler KitDo additional measurements using the oscilloscopeReport back and/or update PCBLet me wrap up by saying that I'm truly moved by the help I'm getting here! The fact that you are all willing to help some stranger fix all his silly mistakes and help me learn some new skills, really means a lot to me, thank you for that 🙏🏻

author: MichielvanBeers
author_rank: Contributor
timestamp: September 29, 2025, 01:10:45 pm
content: So, herewith a brief update:@mdijkens has been so kind to let me borrow his oscilloscope, which I will pick up next Monday (October 6th).In the meantime, I've followed up on the advice of @tooki.What I did- Soldered a wire from GND C1 and C2- Repeated the previous measurements with the Power Profile Kit ii (PPK) (see below)- Cut the trace between R1 and C1- Repeated the measurementsThese are the findings (including the previous measurements for reference):Note: I've left out the full size images to improve readability and added them as attachments below.Input voltageOutput voltageStableWire C1-C2 GNDCut Trace R1 - C1Power Consumption Screenshot1.00V1.56VYesNoNo1v.png1.50V1.57VYesNoNo1.5v.png2.00V1.57V - 1.59VNoNoNo2v - with load.png | 2v - without load.png2.50V1.92VYesNoNo2.5v.png3.00V2.30V - 3.00VNoNoNo3v.png1.00V1.55VYesYesNo1v - with wire.png1.50V1.56VNoYesNo1.5v - with wire.png2.00V1.57VYesYesNo2v - with wire.png2.50V1.87VYesYesNo2.5v - with wire.png3.00V2.33VYesYesNo3v - with wire.png1.00V1.54VYesYesYes1v - with wire - cut trace.png1.50V1.53VYesYesYes1.5v - with wire - cut trace.png2.00V1.67V - 1.72V (rising)NoYesYes2v - with wire - cut trace.png2.50V1.91VYesYesYes2.5v - with wire - cut trace.png3.00V2.35VYesYesYes3v - with wire - cut trace.pngThough the power consumption did have some different fluctuations, I don't see much difference in the voltage output. The voltage output might seem a bit more stable, though it's difficult to really tell with just the multimeter.Question: Would it make sense to include a small load/resistor in future measurements or is that not needed to validate if the TPS is working correctly?Next stepsSolder a new PCB with fresh components to rule out any broken componentsMeasure each voltage level with the oscilloscope when I have itRepeat the steps of soldering the wire and cutting the traceRepeat the same measurementsReport back hereLet me know if anyone feels I should take different next steps. If not, I'll report back in ~1.5 weeks.

author: Psi
author_rank: Super Contributor
timestamp: September 30, 2025, 12:47:49 am
content: Are you sure your input power is able to handle peak current draw.buck and boost converters behave strange if they cannot draw peak currents from the input supply.Make sure you don't have a current limit set on your input supply.

author: MichielvanBeers
author_rank: Contributor
timestamp: September 30, 2025, 09:18:14 am
content: Quote from: Psi on September 30, 2025, 12:47:49 amThe device I'm using is thePower Profiler Kit II(Technical documentation). This is rated to have a maximum output of 1A, but seems to limit to 600mA when using USB only. I tried to find some information in theTPS61220 Datasheeton the expected peak current draw, but was unsure which section to review. So, I'm unable to answer your question with confidence. Do you know how I can calculate the expected peak current draw?As I don't have a dedicated power source that outputs <3.28V (e.g., the expected output of VOUT), I did try connecting a CR2032 to VIN and GND (measured output: 3.11V). The output voltage of VOUT measures around 2.6V. However, my understanding is that these batteries also don't handle peak current very well?I do have someLM2596 Step-Down Buck Converterslaying around. Would it make sense to set those to <3V and connect them to VIN and GND? As I believe they have a maximum rating of 3A.

author: MichielvanBeers
author_rank: Contributor
timestamp: October 08, 2025, 05:48:26 pm
content: Alright, so I've borrowed the oscilloscope of @mdijkens (thanks again!). I've resoldered a new PCB to rule out a broken PCB/TPS and then did the measurements while providing a 220 Ohm load. Note that I haven't made the modifications of @tooki yet, as I wanted to allow for any additional measurement suggestions, before making more lasting modifications.These are the measurements with the oscilloscope:Figure 1: VIN PinFigure 2: VOUT PinFigure 3: L PinFigure 4: FB PinFigure 5: Power consumptionInterpretationsWhat I take from the following results:VIN is showing around 1.48V, which is expected as the Power Profile Kit is configured to 1500mVVOUT is 1.6V which I don't understandFB is at 1.04V which is way higher than the 0.5V it should beL doesn't look to have weird spikes (I think?)The power consumption seems to be relatively stable (at least at the beginning)So, I'm a bit lost on the next steps here. So far, I don't see any significant different results from the multimeter tests, but that might also be my lack of knowing how to use the oscilloscope or interpreting the results, of course. Any suggestions/tips/tricks/thoughts are welcome! Happy to do any additional measurements needed.

author: xvr
author_rank: Frequent Contributor
timestamp: October 08, 2025, 06:33:57 pm
content: Check the capacitors you used. Your Ali link lists 0.1 µF capacitors, not the 10 µF ones you should use.Also, check the 1 MOhm resistor: it looks like flux residue may have reduced the resistance.

author: MathWizard
author_rank: Super Contributor
timestamp: October 09, 2025, 06:20:49 am
content: So why does the datasheet use such large R1,R2 values, overall won't that make for much bigger time constants. I'm not very familiar with switching IC's, and I've just never seen such huge sensing resistor's, especially not for low voltage as-well.

author: tooki
author_rank: Super Contributor
timestamp: October 09, 2025, 07:24:45 am
content: Quote from: MathWizard on October 09, 2025, 06:20:49 amThe only resistors are for setting the voltage via the feedback pin, so they don’t have anything to do with an RC time constant.Anyway, here’s what the datasheet says in the design procedure:QuoteI can only assume this is to keep quiescent current low.

author: MichielvanBeers
author_rank: Contributor
timestamp: October 10, 2025, 09:06:10 am
content: Quote from: xvr on October 08, 2025, 06:33:57 pmThanks! I don't own a multimeter that can measure capacitance, but I have ordered one to validate the capacitors. The packaging that I received did show 10uF, though, so I expect/hope they are the correct ones.Quote from: xvr on October 08, 2025, 06:33:57 pmIs it possible to validate this by measuring the resistance while the resistor is still on the PCB? Or would the measurement be influenced by the other component/traces on the PCB?

author: tooki
author_rank: Super Contributor
timestamp: October 10, 2025, 09:31:30 am
content: Try putting a 10uF electrolytic in parallel with each of the 10uF ceramic caps, just in case they are actually the wrong value (why, oh why don’t they make SMD ceramic caps with the value printed on them??).Remember also that ceramic caps “lose” capacitance with voltage. A 10uF cap might only be 50, 40, or even 20uF by the time you’ve applied your working voltage to it. (The effect gets stronger the smaller the physical size of the cap.) Now, I don’t actually think this is a big factor with your low voltages and 1206 size, but just worth mentioning. This is known as the “DC bias characteristics” of a ceramic cap, should you want to read up on it.As for measuring the resistor in-circuit: no, you can’t really do that, since you will also measure anything in parallel with it. If you have a spare unpopulated board, you could try populating just the resistors, using the same methods and materials used for the others. Then you could measure the resistances alone.

author: MichielvanBeers
author_rank: Contributor
timestamp: October 10, 2025, 11:16:34 am
content: Quote from: tooki on October 10, 2025, 09:31:30 amI've added two electrolytic capacitors that I had laying around, but it didn't change much/anything in the output voltage unfortunately.Quote from: tooki on October 10, 2025, 09:31:30 amThank you! Another term to do some reading into this weekendQuote from: tooki on October 10, 2025, 09:31:30 amGotcha! Unfortunately, all the PCBs I have here have some components soldered on them now. I'm leaning more and more towards ordering the PCB with the updated design to rule out at least a couple of known design issues. What are your thoughts on that?

author: tooki
author_rank: Super Contributor
timestamp: October 10, 2025, 03:05:46 pm
content: If you’re going to order a new board, I would also select and purchase name-brand components from a reputable distributor. And the ones I’d select would be either a) the exact ones used in the eval board, or b) the exact ones used in a successful WEBENCH simulation. (WEBENCH selects some parts right from the start, but if those are unavailable, you can actually choose alternates within it, from a list of parts it knows of and can simulate with.) Resistors are an exception, in that there’s less variation in behavior among them. (I’d still use name brand and not some random aliexpress ones.)

author: MichielvanBeers
author_rank: Contributor
timestamp: October 10, 2025, 03:33:30 pm
content: Quote from: tooki on October 10, 2025, 03:05:46 pmGotcha, will do!Do you think it is safe to replace the size of certain components to make soldering easier? For example: replacethis Murata Electronics 10uF 0603/1608 capacitorthat is in theEVM BOMwiththis Samsung Electro-Mechanics 10uF 1206/3216 capacitor? And what about replacing theCoilcraft 4.7uH 3mm Inductorwith aSumida 4.7uH 7mm inductor?If this doesn't sound like a good idea, I think it will just be time to upgrade my soldering skills

author: MichielvanBeers
author_rank: Contributor
timestamp: October 11, 2025, 09:43:17 am
content: So, I've decided on remaining as close as possible to the design the Evaluation Board and thus updated the PCB to include the new footprints:Figure 1: Updated PCB with updated footprints for Inductor and CapacitorsChangelogChanged Inductor footprint from 7mm to 3mm to accommodate theCoilcraft EPL3015-472MLC InductorsChanged Capacitor footprint from 1206/3216 to 0603/1608 to fit theMurata GRM188R60J106ME47J CapacitorsBOMI've included the items I'm planning to order on Mouser this weekend. I'm replacing my AliExpress TPS61220 with the official TI ones from Mouser. I'll also order the Coilcraft inductor and Murata Capacitors to match the BOM of the EVM.Note that I'm using the GRM188R60J106ME47Jinstead of the GRM188R60J106ME47Das the D-variant was no longer in stock and inthis comparisonit looked like the only difference was the standard packaging quantity.As always, any feedback is welcome. Otherwise, I'll report back in a couple of days when the new PCB and components are in!

author: tooki
author_rank: Super Contributor
timestamp: October 11, 2025, 11:29:44 am
content: Quote from: MichielvanBeers on October 10, 2025, 03:33:30 pmWith the caps I don’t see any problem — physically larger ones will have more effective capacitance, but that’s not a bad thing per se. With the inductors… I’ll be honest, magnetics are probably the components I have the poorest understanding of, so I don’t really know what the selection criteria are here. However, you could use WEBENCH to see what TI thinks will work.How are you soldering these? If by hand, you can just make the pads bigger to give you space to reach them with the iron. (Even on the IC, you can just extend them so they stick out farther.)Quote from: MichielvanBeers on October 11, 2025, 09:43:17 amI would move the IC and inductor down, so that the capacitors align with the chip such that their ground pads align with the center of the chip, so that you can make the ground trace that runs under the chip as wide as possible. (Look at the eval board layout, but even there C1 could be a bit higher, like C2.)Also, double-check that your copper-to-copper clearances are whatever the minimum is that your PCB manufacturer can make, so you can make that ground as wide as possible. (Ideally, do a check of all the clearances/constraints, of course.)I think I missed that even your ICs were from AliExpress. Who knows if they’re any good. In general, I avoid buying components on AliExpress, except for certain things that aren’t actually available from mainstream distributors (LED filaments, COB LED modules, certain types of cables and wires, some pushbuttons, etc). It’s just not worth the hassle and risk of dealing with parts of unknown quality or functionality, as well as the lack of datasheets for most things.

author: MichielvanBeers
author_rank: Contributor
timestamp: October 11, 2025, 01:35:27 pm
content: Quote from: tooki on October 11, 2025, 11:29:44 amIndeed by hand. I've used some footprints that already have a bit larger pads, so I'll think to just give them a go. Otherwise, it might be a good excuse to buy a hot plate and some solderpaste 😏Quote from: tooki on October 11, 2025, 11:29:44 amDone! The GND trace is much thicker now, indeed. I see what they did with C2 in the EVM, but I don't think moving C2 up in the design would improve that by much anymore.Quote from: tooki on October 11, 2025, 11:29:44 amCheck. I'm ordering from PCBWay. I believe they can go down to even 0.0762 mm, but I ended up at 0.1mm to make the measurements a bit more straightforward when designing. Overall, it looks like the GND trace now has a similar thickness to the EVM (I think).Quote from: tooki on October 11, 2025, 11:29:44 amNoted. The main reason I ended up there was due to the significantly lower shipping fees, but I now learned that I pay double in the time spent debuggin afterwardsThis is the end result I'm planning on ordering:

author: tooki
author_rank: Super Contributor
timestamp: October 11, 2025, 02:02:13 pm
content: Quote from: MichielvanBeers on October 11, 2025, 01:35:27 pmLooks good, but I would eliminate the big “wedge” connecting the inductor directly to the input — the added copper will make that side harder to solder. Just do it like the EVM does.Quote from: MichielvanBeers on October 11, 2025, 01:35:27 pmDigikey and Mouser both offer free shipping on orders above €50, Farnell above €75, Distrelec above €100, Conrad above €60.50.Just keep a list of things you want (but don’t need) and things you need, but not urgently, to use as “filler” to pad orders to reach the minimum for free shipping. Or, when possible, you can use Conrad, Reichelt, and Distrelec for small orders, as their shipping costs are low. (I say “when possible” because TI no longer distributes through any of them, having restricted distribution to the largest distributors — Digikey, Mouser, and Arrow (which really isn’t for hobbyists).)

author: MichielvanBeers
author_rank: Contributor
timestamp: October 12, 2025, 02:29:13 pm
content: Quote from: tooki on October 11, 2025, 02:02:13 pmDone, added the final design below.Question on the soldering part: I'm trying to understand why the added copper would make it harder to solder. Would that be due to heat dissipation?Quote from: tooki on October 11, 2025, 02:02:13 pmNoted! Might make it more challenging for rapid prototyping, but there is always a new project waiting around the corner where I could source some parts forBoth the PCB and the components are ordered, so hopefully I can report back with some news in about a week or so 🤞🏻

author: tooki
author_rank: Super Contributor
timestamp: October 12, 2025, 06:23:27 pm
content: Quote from: MichielvanBeers on October 12, 2025, 02:29:13 pmYep. SMD inductors are already among the harder components to hand-solder because they suck away so much heat, so no need to unnecessarily add even more heatsinking. (Granted, your new inductor isn’t very big.)