My PSU design ripple and noise with picture measurements - Page 1
Forum section: electronics / projects

author: VEGETA
author_rank: Super Contributor
timestamp: August 22, 2021, 06:55:55 pm
content: HelloI designed a PSU as a replacement PSU for Dreamcast using TPS62913 which promises total final noise and ripple of 1 mV p-p but I got around 80-100mV p-p despite following the datasheet and design layout recommendation. Other third-party PSU delivered near identical results despite having inferior parts and basic design. I added LC filters and ferrites plus bulk filtering caps 1000uF with 22uF ceramics for the input 12v rail but still I got this result.Input 12v is supposed to come from cheap 12v PSUs, mine has 250mV p-p ripple and noise as shown in below pictures...so:1- does this mean that even good buck regulator design just cannot eliminate input ripple\noise? I mean it will get reduced but still will pass through?2- what solution to achieve such low figure of 1mV or near it?3- is adding huge inductor Pi filter will solve it? I only had 4.7uH for 12v filtering plus 1000UF elec cap and many ceramics.pictures are labelled so you can recognize it.for your kind help.regards,

author: ezalys
author_rank: Frequent Contributor
timestamp: August 22, 2021, 07:04:27 pm
content: we’d need to see your schematic and layout. Also what’s the signal on the scope look like if you do the exact same measurement but with the power supply turned off?

author: ezalys
author_rank: Frequent Contributor
timestamp: August 22, 2021, 07:08:39 pm
content: additionally, I think it’s bad engineering to just throw LC filters at the thing. I’d like to know what the cutoffs are of the filters, the parasitics of them, the layout, all these things will contribute. It’s also true that no regulator will eliminate all noise, they just suppress it with a particular amount of suppression per frequency. LC filters, bulk caps, ferrites, and regulators themselves are tools in your toolbox to be applied deliberately to reduce noise.

author: floobydust
author_rank: Super Contributor
timestamp: August 22, 2021, 07:14:08 pm
content: Who promised 1mV p-p ripple out of a buck converter? Oh TI didTPS6291x 3-V to 17-V, 2-A/3-A Low Noise and Low Ripple Buck Converter with Integrated Ferrite Bead Filter Compensationusing 8A ferrite bead BLE18PS080SN1.I think your expectations are high and a Dreamcast doesn't require such low ripple.Your PCB layout, scope grounding, choice of capacitors, ferrite bead- are all critical. You've got a 50mV noise floor so you cannot measure below that anyhow.

author: VEGETA
author_rank: Super Contributor
timestamp: August 23, 2021, 09:06:33 am
content: Quote from: ezalys on August 22, 2021, 07:08:39 pmI didn't do calculations for LC filters but rather kept it straightforward and simple. I knew 12v will be very noisy, so I put them. I will put schematic once I return from work, even though it is not open source and should be commercial product... but it is ok.QuoteYes, this is the IC. I have used different passives (from LCSC) than those of TI, but I think the ferrite is the same. why the results differ so much?QuoteI kinda went with their data and demonstration, or else what extra benefit to get from this IC over a regular one?Dreamcast is an old console which uses analog video signals which are sensitive to noise. analog video is 1v only, so 100mV ripple and noise will have an effect. Generally, less noise and ripple the better. Making a cheap PSU which has low noise\ripple is good too.QuoteScope is not mine, it is in a fablab which is far away from me. Not accessible easily due to far distance and so on. It is gw instek gds-1152a-u 150 MHz 2 channels. I used normal probe with putting the probe ground to psu ground and then get the signal. I wonder why I got such a huge noise floor.If I got 60-90mV noise for it, does that mean its real noise\ripple is just 10-40 mV p-p since the extra 50mV is just noise floor?what solutions do you suggest to achieve this low values or near them?

author: VEGETA
author_rank: Super Contributor
timestamp: August 23, 2021, 07:26:56 pm
content: Here is the schematic and layout.

author: T3sl4co1l
author_rank: Super Contributor
timestamp: August 23, 2021, 08:02:56 pm
content: Why isn't ground poured under everything? Most especially the regulators themselves, but also contiguously under the board? Likely the ripple measurement is largely common mode (due to the high ground impedance between connectors)..?C6-C8, C10 and C12 do absolutely nothing; I don't know where such tiny values came from. The ferrite beads largely do nothing as well, they saturate under bias (typically >50mA, depends on value and size -- they may still be seen to help out at light loads).Bleeder/load resistors should not be necessary. If you are finding instability, check component values, or select a regulator with external compensation so it can be better tuned.Note that such large ceramics (22uF, in, what are these, 0805s?) run out of capacitance quickly under DC bias, not so much at 3.3V, a bit at 5V, definitely at 12V. This is probably still fine because of the parallel quantities, but keep this in mind when going from design calculations to component selection.Since you're using electrolytics (well, polarized something anyway, maybe they're polymer I don't know), I don't get the large quantities of 22uF chips; a couple electrolytics would do as good a job, plus one or two ceramics to "take the edge off". Otherwise, if you're not squeamish about the cost of so many caps, why not just go all in, who needs electrolytic? (Except maybe at the input, if there's a need for bulk capacitance say for mains filtering or hold-up time.)The 3.3 and 5V outputs seem reasonably well filtered near the connector, but V12 is not at all. But the input is heavily filtered (but only differential mode).Tim

author: GigaJoe
author_rank: Frequent Contributor
timestamp: August 23, 2021, 10:00:51 pm
content: chip operated at 1-2Mhz, radio frequency , extremely short connections, filled ground, dual side for ground, shielding, etcpdf define a spec even for caps, due to freq. and resistance.proper scope measurement, your scope tail catch everything , something like thathttps://www.cui.com/blog/how-to-measure-ripple-and-transient-in-power-supplieshuge caps or L doesn't help much due to freq. find caps - freq. dependence graph.

author: VEGETA
author_rank: Super Contributor
timestamp: August 24, 2021, 09:36:28 am
content: QuoteI followed datasheet layout recommendation for ground pour. I also thought it would be a good idea to make noisy 12v ground far from clean regulated output ground due to what many people are assuming about separating ground for return current path and not mixing bad noisy signals with clean ones. On a side note, I am changing my idea towards making one unified ground pour for everything these days as some credible people are saying this nowadays.QuoteI added them as an extra caps to deal with high frequency stuff. I also put Pi filters as you see but they don't seem to have done much. I didn't do any calculations though.QuoteAdding minimal load like this is always best and doesn't cost a thing. no harm too.Quote0805 is the largest I can tolerate since it is 50x50mm board. Putting many in parallel is also helpful as you said.Quoteregulator IC doesn't require elec. caps and actually does not require a lot of capacitance at the output. In fact, there is a limit to how much I should put. recommendation suggests these 22uF caps at the output but I also added 47uF elec. caps to have extra bulk capacitance since it is well within the upper limit.Quotekindly explain differential mode filtering you mentioned.12v input is itself the 12v rail. it is heavily filtered but unfortunately doesn't seem to have done what I hoped. the third party PSU has 33uH inductors with 100uF elec.caps output filters after regulators... it gets nearly the same result.do you mean I must put big caps near the 12v output connector pin itself? but the signal is very well filtered before and the trace is thick and not too long to cause all this.Do you find it applicable to remove all that 200-260mV p-p ripple and noise from the 12v input? especially for 3.3v and 5v rails (and 12v one as well).Should I go for 33uH or similar very big inductance with elec. caps to filter the 12v? since my inductors are very small.I say this assuming that if the buck regulators are fed with very clean 12v signal, they won't add ripple and noise to it as they claim since we concluded that the input ripple and noise will be suppressed but still get in if not filtered.___QuoteI did make connections short, could be shorter too. You mean I have to make top and bottom layers as ground fills?Quotepassives are all cheap from LCSC, didn't get low ESR or so but rather suitable footprint and voltage.QuoteInput frequency is not high, so I assume big caps cap be good right? what about putting higher amount of inductors like 220~470uH as LC input filters, multistages?how can I get the low noise\ripple factor that I require?

author: VEGETA
author_rank: Super Contributor
timestamp: August 25, 2021, 10:23:13 pm
content: If anyone interested or can properly measure the ripple and noise of my small board, I can send it to him. Please advise.

author: VEGETA
author_rank: Super Contributor
timestamp: August 26, 2021, 01:00:07 pm
content: Quote from: T3sl4co1l on August 23, 2021, 08:02:56 pmI thought of your words and guessed that maybe be a simpler approach is better.Using this 100uH inductor:https://www.digikey.com/en/products/detail/pulse-electronics-power/PA4309-104NLT/5361574(or cheaper from LCSC).preceded and followed by 1000uF caps parallel to ground, which acts as 3rd order LC filter.This would be the only filtration for 12v input rail, then I feed this into the switchers and remove the useless small value ceramic caps and only keep the 22uF ones in both input and output. While also keeping 47uF elec. caps for outputs and add one elec. 47uF + 22uF ceramic + Ferrite bead just before the 12v connector itself.What do you think?I could add another stage of 100uH inductor which will take more space and require more 1000uF caps... if it is necessary, but this way I will need to use cheap LCSC inductors instead of that expensive Pulse-electronics one.I wonder about those designs where people put various ceramic caps values in parallel, especially at output. like 22u, 1u, 100n, 1n... does this really enhance HF noise suppression?Using this scope at the fablab would be problematic due to the horrible noise floor (tested by shorting the probe to GND pins) of 50mV. Should I use CH1 to get power (3.3v, 5v, 12v) and CH2 for probing GND, then do subtraction in scope software? shouldn't this eliminate the noise floor?I think I cannot go to market with this design if it is just slightly better than the best one available, I wanted it to be a lot better.

author: T3sl4co1l
author_rank: Super Contributor
timestamp: August 26, 2021, 02:01:34 pm
content: Do you know how much filtering you actually need?100uH is pretty large. Certainly large enough you need to account for its impedance, so as not to make the supplies "bouncy". Too high of an impedance into a switching regulator, at a low frequency, and you get an oscillator -- the regulator input is negative resistance (it doesn't need to draw as much current, at higher voltage, since it conserves power).Note that a supply isn't just, you stick a filter on it and it's done. Filtering is with respect to a given connection. If the input isn't noisy, you might simply wire the 12V input to the output connector and that's that. The regulators are a pretty obvious source of noise, so it makes sense to add a filter between regulator input, and power inputor output. This is why I noted the 12V output is unfiltered: it carries full regulator ripple to the output.Quote from: VEGETA on August 26, 2021, 01:00:07 pmYes, that sounds fine, or at least more reasonable; exact values still matter so it depends, but that should be in the right ballpark.Again, ferrite beads amount to nothing; it's strange that they're even shown in the regulator datasheet at all, but it's also amusing that they label it as "10nH", i.e., as good as an equivalent length of wire (well, a cm or so).If you know you need some actual output filtering, more like 0.1 to 2.2uH is probably reasonable, plus enough capacitance to get Zo low enough for required load step response, and well damped so it doesn't oscillate.Zo = sqrt(L/C) is the characteristic impedance of an LC circuit. When Zo ~ R, the network is well damped. (Whether it's greater or lesser by a modest factor (say 1-2x), depends on how it's arranged.) Zo gives the step response, as a load step change of say 1A is expected to develop Zo*1A peak voltage change. If your output is say 3.3V 1A, and regulation must be within 5% including transients, then peak voltage must be under 0.165V for a full load step or 1A change, so Zo < 0.165Ω.For 1uH and Zo < 0.165Ω, C > 36.7uF. This can be, for example, a 22uF ceramic in parallel with 47-100uF electrolytic, selected for ESR ~ 0.15Ω. Or the equivalent constructed from parallel ceramics and an explicit resistor.Or if using just ceramics, since ESR ~ 10mΩ on those, you need Zo similarly low, say L around... 10nH? Well, I suppose that explains where that number came from. Note that 10nH and 22uF has a cutoff of 340kHz so will not attenuate much more than the sheer bulk capacitance is already doing. Which makes sense, the caps themselves have 2-3nH ESL so a 10nH in series between a few of them doesn't really mean anything, it's a pretty weak impedance divider, hardly a filter at all.QuoteAt best, it's an outdated practice.The ESL of a chip capacitor is essentially its package size. Period. It hardly depends on value, it doesn't depend on voltage, it depends a bit on height, and most of all it depends on the length and aspect ratio. (Which is why wide-body components are recommended for critical applications.)The frequency of minimum impedance (series resonance) does depend on value, but the asymptote extending above there, is the same impedance -- the same ESL -- regardless of value.So you get as good performance, beyond say 10MHz, with 0.33uF as with 33uF or anything inbetween.Putting smaller caps in parallel, is likely to make things worse, due to the resonant loop formed between the smaller cap, its capacitance, and the larger cap. Such loops are on the order of 6nH, so for say a 10nF, you get Zo = 0.77Ω and Fo = 20MHz. The 10nF might have 100mΩ ESR, giving a Q of 7, or an impedance peak (parallel resonant equivalent, Zpeak = Zo * Q) of 5.4 ohms -- massively worse than the impedance of the bulk cap's inductance alone (which if it's 3nH, is only 0.377Ω at 20MHz).And for switching regulators, it's not likely to do much of anything at all, anyway: the impedance is so much lower than for an individual logic IC for example. Say the peak voltage and current are 12V 2A, then the impedance needs to be much less than their ratio, or 6Ω. A small cap like 10nF just disappears, it does nothing, the input ESL dominates. Much better to put the bulk cap there, or at least a big enough bypass (typically 1uF) to dominate over the ESL to the next bigger cap (while again being chosen for ESR to dampen that loop!).So a 1uF at each regulator, and one or a few 22uF nearby, is likely fine for your purposes. Plus whatever input filtering is needed, again dimensioned so that Zo is low enough, and with ESR provided to dampen it.QuoteWhat? You mean the scope, probe disconnected, has a noise floor that high? It sounds defective.If you mean with the probe tip grounded to its clip,and this point connected to circuit ground,then that is probably typical of your circuit's common mode noise, and this is dropped across the narrow, lengthy ground return path around the regulators. And will likewise be emitted from the power cable, failing EMC.They don't show the bottom layer in the datasheet layout example, but one should assume it's ground pour. They do show vias for this purpose. Strangely, they also show vias for VIN and VOUT, which have no business running on the bottom layer. It's not clear what they mean by that. Examples must always be taken as just that, examples; sometimes they're reasonable, sometimes they're cooked up by some random intern, who knows.Another tip: avoid VIN and VOUT on opposite sides of the board -- this guarantees that, the full voltage drop across circuit ground, appears between connectors. Instead, place them adjacent where possible, and route the connections over to the regulators, off to the other side. This confines ground-loop currents to the regulator area. Routing VIN and VOUT away from that critical area, they can be filtered with respect to a more stable GND, with less voltage drop between their respective GND connections (namely, the filter cap GNDs).Tim

author: VEGETA
author_rank: Super Contributor
timestamp: August 26, 2021, 07:05:53 pm
content: QuoteI don't know exactly but I know it needs good amount of it, switching regulator wall PSUs used are noisy.QuoteI know but it seems enough to eliminate all that. most of these PSU used and to be used are in the low frequency range, certainly less than 1 MHz. Please refer to previously shown images to see input and output waveforms on the scope.Quotetheir idea is that ferrite bead is integrated within the feedback loop itself, which is their new solution to achieve very low noise figure as shown in their datasheet and videos. it is not just an output filter.QuoteAssuming 100uH + 1000uF, Zo = 0.316 according to equation and this site:http://circuitcalculator.com/lcfilter.htm... this is without 1000uF before the inductor, only after it. So it is 1 inductor and 1 capacitor solution.3.3v will be 2.8~3A full load while 5v is only 0.5A (could go a bit more). 12v is not really used for anything but GD drive motor if it is still installed, so very little current.I didn't quite understand load step requirement you posted, kindly inform me.The system is 22 Watts, I assume 25W PSU. 12v will be 2~2.5A, 3A at beyond max. so 12/2 = 6 Ohms or 12/3 = 4 Ohms. Z = 100uH/1000uF = 0.32 Ohms. This is for 12v input only, which is both input to the 2 regulator rails and an output of 12v for the system.the regulators, say the 3.3v one is said to be 3 amps. 3A * 5% = 0.15v , now 0.15V/3A = 0.05R. Is this what you meant back then? Now this has nothing to do with 12v heavy filtering I talked about... please notice that the switching regulators circuit will not change by much if any... I was talking about 100uH 1000uF for the 12v input filtering only.I already pointed out that TI specified a number of total output capacitance limit, and I adhere to it. putting 3x22uF ceramics + 1 47uF elec. seems good enough. having 3x22uF ceramics as input filtering for the regulators (fed from the heavy filtered 12v) is also suitable to datasheet.Our whole point here is that the input noise and ripple is passing through to the output 3.3v and 5v despite using great quality switcher. therefore, the conclusion was that the switcher needs clean input to be able to provide its clean output... therefore, we will clean the 12v using heavy filtering.QuoteOk, so using 22uF 0805 seems good enough.QuoteYes, probe is connected to ground and shows 50mV p-p. It is not just my own circuit but the third-party PSU as well. this PSU uses 33uH + 100UF filtering for both rails output but of course using a traditional cheap and available generic switcher.

author: ezalys
author_rank: Frequent Contributor
timestamp: August 29, 2021, 11:23:53 pm
content: "The ferrite beads largely do nothing as well, they saturate under bias (typically >50mA, depends on value and size -- they may still be seen to help out at light loads).""Again, ferrite beads amount to nothing; it's strange that they're even shown in the regulator datasheet at all, but it's also amusing that they label it as "10nH", i.e., as good as an equivalent length of wire (well, a cm or so)."I don't get this statement at all. The wurth 74279221100 mentioned in the datasheet takes a LOT of current to saturate.https://www.mouser.com/datasheet/2/445/74279221100-1720641.pdfStill 10 ohms at 100 MHz at 5 amps.

author: T3sl4co1l
author_rank: Super Contributor
timestamp: August 30, 2021, 01:15:15 am
content: No, I didn't look at the exact part.Indeed that one handles quite a lot of current; and they actually provide curves -- a welcome sight!In fact they show closer to 14nH, an absolutebountyin there!OP didn't write down a part number or provide BOM so it's not clear if they're using same.Tim

author: VEGETA
author_rank: Super Contributor
timestamp: August 30, 2021, 08:45:44 am
content: Quote from: T3sl4co1l on August 30, 2021, 01:15:15 amI have used this one:https://www.murata.com/en-global/products/productdetail?partno=BLE18PS080SN1%23which is recommended in the datasheet of TI.Key BOM items:4.7uH inductors:https://lcsc.com/product-detail/Inductors-SMD_PSA-Prosperity-Dielectrics-MCS0630-4R7MN2_C385253.html...although in my previously made units I used PA4340.472NLT which was similar to recommended ones (XGL4030-472). I assumed that getting a cheap one will work and it did, but not sure its effect on noise performance. I plan to test my previously made units on the scope this time. Their only issue was a slightly more increased voltage on 5v, around 5.2v which made me change the values then I took the chance to add more filters..etc22uF ceramic caps:https://lcsc.com/product-detail/Multilayer-Ceramic-Capacitors-MLCC-SMD-SMT_SAMSUNG_CL21A226MAQNNNE_22uF-226-20-25V_C45783.html1uH inductor:https://lcsc.com/product-detail/New-Quadratic-Unclassified-Data_GLE-GCDA252012P-1R0MC_C439318.html1000uF elec. cap:https://lcsc.com/product-detail/Aluminum-Electrolytic-Capacitors-SMD_Lelon-VE-102M1CTR-1010_C249474.html____What can be done to enhance the performance?Anyone can kindly volunteer to test the 2 units (new and old)? I can send it via mail since I don't have a scope now and it will be very hard to do measurements.My current thought is to have a 2-stage LC filter of say 100uH+1000uF in each stage... or 47uH+1000\2200uF or similar... for the 12v input, then for 12v output connector itself I can put another 1000uF cap.I am not fond of the idea to replace the 22uF ceramics by elec. caps. datasheet wants ceramics especially for output which I added a 47uF elec. cap as an added filtration.___TPS62913 stated > 65 dB PSRR for <100 Khz which I didn't take into account. So assuming 200mV p-p actual noise and ripple (after taking off 50mV noise floor), I got 10-40mV final output (after taking off 50mV noise floor)... is that what this 65 db PSRR suggests?

author: T3sl4co1l
author_rank: Super Contributor
timestamp: August 30, 2021, 05:23:53 pm
content: Those components seem fine.The ferrite bead does not provide DC bias characteristic (Murata doesn't record it for any ferrite beads at all, I'm pretty sure) but given the other part above, it's probably fine around an ampere or so. And, again given the value, it's doing very little in any case.The 22u caps don't have a char sheet, at least that I saw from a glance. Huh, they're also listed as obsolete at other suppliers, I wonder where LCSC is getting them......Note that both (cored) inductors, and type 2 ceramic caps, lose value under bias (current and voltage respectively). You get a 22uF cap at 0V; at 12V it's probably like 3uF or so. Still enough to be useful, but keep this in mind when designing filters, and prefer parts with actual characteristics.X5R is also a bit on the low side, but it shouldn't be too much worse in terms of voltage dependency or tempco compared to X7R or better, as long as you aren't operating at high temperatures (the 5 means 85°C max, 7 is 125). Note that temp rise (power dissipated in ESR) can be relevant for caps handling high ripple currents -- probably not here, but can be important for bigger converters (100s watts?).PSRR is Power Supply Rejection Ratio. That is, how much does the output voltage change, for a given change in input voltage. For example, suppose a buck converter operates at a fixed PWM: Vo = Vin * D (D = duty cycle). In this case, PSRR = -20 * log(D), because say 1V changes at the input, and D is 0.5, then the output changes by 0.5V and the PSRR is 6dB. And this will be true for frequencies from DC up to the cutoff frequency of the input and output filters, where filter attenuation dominates (and thus PSRR goes up: PSRR = filter attenuation - converter gain). It's improved still further by the control circuit, varying D to maintain Vo. This gives high PSRR at DC, up to the error amp's cutoff frequency more or less; at which point the filters should take over. And with >65dB PSRR overall, it sounds like this is the case for their design. Put another way, the output is disturbed by less than one-thousandth the input change (20 log(1000) ~= 60dB), a generally excellent figure.Tim

author: VEGETA
author_rank: Super Contributor
timestamp: August 30, 2021, 06:29:03 pm
content: So why I am not getting the performance I expected? I mean, the input to the switchers should already be very clean in order for them to make a clean output right? therefore we need to heavily filter the 12v rail.any suggestions besides those of my previous reply?I picked cheap and suitable parts from LCSC without much hassle about characteristics. I cared about ceramic caps to be of high voltage, bigger package (for bias stuff), and a 22uF value. ferrite beads after the switchers are essential since they are part of the control loop itself and necessary to give very low output noise and ripple. FB on inputs and 12v is my own doing.I am open to your suggestions.

author: T3sl4co1l
author_rank: Super Contributor
timestamp: August 30, 2021, 09:03:33 pm
content: The problem is not so much the filter topology, it's the ground topology. Consider what you would measure in a circuit such as this:L2 might be quite small, say 10nH, but it is not at all irrelevant.Consider further the equivalent circuit of your scope probes making connection to this circuit. The ground clips have some inductance (fraction of a uH) up to the probe body not coupled with the probe tip, and the cables have some inductance between them (~1uH), looping through scope ground (and mains as applicable). Thus the probes have an inductance divider equivalent circuit, where the ground clip draws current corresponding to the inductance between probes, and the voltage dropped by the clip is not sensed by the probe tip (but the rest of the cable is reasonably shielded, i.e. the signal and shield are well coupled).This voltage is most apparent when probing with the tip attached to the ground clip, the combination being poked against various (mostly / hopefully "ground") points in the circuit; a null result shows no common mode noise with respect to the oscilloscope (presumably, whatever power supply / ground return path is shared by the power supply and scope), a non-null result shows there is voltage being dropped across this or other loops.And this common-mode voltagecannotbe filtered by taking on more LC stages, which accomplish only differential filtering. There is another mode!The best remedy is to put the connectors to one edge, solid ground pour (top and bottom, with adequate via stitching), over all, and regulators to the other (far) edge. This shorts the connector grounds together, while putting distance between the critical switching loop(s), and minimizing the value of L2 (it can be a few nH in a good layout), and its size (some mm across), thus its fields drop off rapidly with distance. And the connectors (and their respective filters) are placed at a distance from the regulator, keeping them well clear of that noise.Tim

author: ezalys
author_rank: Frequent Contributor
timestamp: August 31, 2021, 02:22:50 am
content: Even if it is a small inductor, doesn't the real impedance help with de-Qing your filter? I mean, I might just ask in what situations you see ferrites being useful.

author: Vovk_Z
author_rank: Super Contributor
timestamp: August 31, 2021, 02:58:57 am
content: I would try smaller capacitance (4.7 uF, 10 uF) but larger case X7R caps (1206, 1210) instead of 22 uF 0805 caps, possibly several in parallel.And the topology of an input cap on the PCB has a very large influence on the overall noise too. It must be very close to the noisy part. The PCB topology means much more than the C value (when we are talking about low-noise design)

author: VEGETA
author_rank: Super Contributor
timestamp: August 31, 2021, 07:57:58 am
content: Quote from: ezalys on August 31, 2021, 02:22:50 amthe ferrites are part of tps62913 circuit feedback loop. they are necessary to reach that very low noise and ripple figure. However, ferrites at input side of 12v is my own idea which I am not sure if it helps or not.You talked about real impedance of L, I don't know the exact value but if damping is required then I can put a resistor in series with a 22uF capacitor but this value I read it should be very low, meaning like 0.3 ohms or a bit more... this is not hard. I could also put elec. caps to help damping it with their higher ESR.My concern is killing the 12v noise and ripple first. This is why I got the idea of having big inductor like 100uH with 2 1000/2200/4700uF caps at the 12v source. then the inputs to the switchers are very easily done via ceramics. what about this idea? what could go wrong with these huge L and C values in terms of stability and effectiveness?Quoteswitchers require 22uF caps, but I think I can fit a slightly bigger cap size of 1206 if I try harder.Are you talking about the 12v rail or the switchers? shouldn't a big 47uH/100uH inductor with 2x of say 2200uF caps (before and after or just after) be able to filter out the ripple and noise? the cut-off frequency will be small and will attenuate a lot of the 250mV p-p of the input.I figured that the switchers need clean input in order to give the clean output. they have > 65 dB PSRR for frequencies < 100 KHz which is good but still not good enough to eliminate 200mv p-p noise and ripple, therefore I would need to make it a lot less.QuoteSo I could just make bottom layer all one ground, but top layer has to have power pours for each switcher as seen in datasheet... but every other place can be GND pour with many vias to stitch it.You mean I should re-arrange the board to have 12v input in top with its LC filter followed by the switchers circuit which is tight and compact. no distance needed between the 12v and switchers? then just send the 3.3v and 5v regulated rails to output connectors? this would mean long distance for them.Or maybe put the switcher circuit close to the connector with its filter caps very close to output connectors while all this is far from 12v circuit?QuoteDo you mind if I sent the board to you? to do some scope measurements the proper way and so on. this will really help me.

author: T3sl4co1l
author_rank: Super Contributor
timestamp: August 31, 2021, 03:40:11 pm
content: Quote from: ezalys on August 31, 2021, 02:22:50 amMind these aren't simply miniature ferrite beads like you're used to; the impedance is largely imaginary up to, what was it, 300, 500MHz? The peak impedance is in the GHz. They're actually pretty good inductors at those lower frequencies.As I demonstrated earlier, the advantage is building a filter against the very low ESR of the ceramic caps. The disadvantage is the Fc is very high, doing an okay job of filtering harmonics and a poor job of fundamental (Fsw) ripple.Quote from: VEGETA on August 31, 2021, 07:57:58 amYou've repeated this several times, but you're simply quoting from the datasheet, no? Do you understand in what way they are necessary, and to what extent they function?Without any understanding of the regulator's internal characteristics, I am confident to say that, if I merely sat down with an eval board and a handful of assorted filter components, I would be able to improve the input and output noise characteristics by a hundredfold. (Or by perhaps 1k to 10k times, in case of your original example -- I would need some additional materials then, to build a shield around the PCB, to avoid the ground-loop issue.)You can give this a spin, yourself, I think, on TI's WEBENCH simulator. They should have a full-enough model of this part, and enough flexibility to implement a variety of filter types. It may even design them for you, and simulate the likely ripple -- again, assuming ground-loop voltage is avoided.The biggest key is likely using a bulk cap (capacitance several times the surrounding (low-ESR) capacitance (C), with ESR = sqrt(L/C), L being the filter inductor(s)). This "de-Qs" the filter, as ezalys hinted at. Other terms: damping, snubbing, terminating.A filter is an impedance network, and just like a transmission line, it must operate into a terminated load resistance; it just happens that its characteristic impedance is low (for typical power supply applications), and so will be the resistance needed for it. And, since we want to pass DC without shorting it, we put a coupling capacitor in series with the resistance, and as a coupling capacitor, it simply needs enough capacitance so that it's largely resistive at the frequencies relevant to the filter (namely the transition band of the filter, Fc = 1 / (2 pi sqrt(LC)) give or take say a factor of 2).QuoteSo, exactly this; but not just one, it will be dominated by the others in parallel; the balance must be more like 1 alone versus 2 or 3 with ESR. So it's kind of inefficient to do this with ceramic caps plus external resistor, and electrolytic or tantalum are often preferred.QuoteMore likely 0.1 to 4.7uH is more than sufficient, and such large values aren't necessary. You have very little to gain, I think, from going to any larger value.QuoteExcuse me, do you understand what 65dB represents?The observed noise isn't at <100kHz anyway, I'm willing to bet. All the more reason why filtering is needed, but also why common mode filtering is critical.QuoteYes!The power pours can be smaller; they don't need to be much bigger than the chip, really, and that's all they show in the datasheet anyway. Around them, can be filled with GND.QuoteConnectors, plural. All of them. If you can't physically move the 12V input down to the bottom edge, then route it down along its side, over by the outputs, and place its filter there. Slot the ground pour beside this route, so that any ground loop currents by the regulators, do not bypass the filter and jump into the 12V connector directly.DO NOT ROUTE TRACES OR POWER POURS OVER A GROUND SLOT.QuoteHonestly I don't think it will make much difference. And the grounding problem is not an easy one to solve by hand, even with heroic effort (cutting and patching pours!).Also, you have some lingering questions about the quality of your source power supplies, I think. You should evaluate those as well.What I think would be much more valuable, is simply iterating the layout. Layouts are cheap. If it took you a long time to build the first one, I can understand your hesitance, but appreciate that it will go faster each and every time after, as you gain familiarity with the tools, and begin to understand the current flow paths. We've spent far, far more time in this thread, than it would take an experienced designer to re-lay the entire circuit. And proto PCBs are cheap to order, unless you're strapped for cash of course, in which case all the more reason to get it right the first time.Tim

author: Vovk_Z
author_rank: Super Contributor
timestamp: August 31, 2021, 03:54:55 pm
content: Quote from: VEGETA on August 31, 2021, 07:57:58 amYes, I'm talking about an input (12VDC side) cap. The main thing is rather not to filter, but to make low-impedance low-area input loop. 2200 uF or even 22 0000000 uF caps won't help, but 1 uF well-placed may do the job.Your DC-DC has some PSRR so it doesn't need very "clean input". The purpose of input filter is not to filter an input voltage, but rather to isolate your DC-DC from other circuit. It filters spreading a generated noise into other area through input.

author: VEGETA
author_rank: Super Contributor
timestamp: August 31, 2021, 05:22:21 pm
content: QuoteI didn't dig into this much tbh, but they keep repeating it as their way to achieve that very low noise\ripple figure. Also, as you mentioned, the FBs won't do anything bad if by any chance they didn't do good. I don't think they are the problem here, do you?QuoteI will try that sometime soon I hope. But maybe it is not accurate since it may not include the type of noise from source.Quoteyou mean the 12v input side LC filter? it does have 1000uF elec. cap at the end but not directly after the main 4.7uH inductor.Or you mean the input to each switcher? there I can put 2 47uF elec. caps in parallel plus say 2 22uF ceramics and one 2.2nF to be closest to the IC pin as requested in datasheet. How about that? putting 1000uF instead of the 2 47uF ones or instead of one of them is doable too but needs a lot of rearrangement.QuoteI already have 4.7uH since I used it in the switchers circuit. as you see, it is followed by other 1uF ones in series plus the caps..etc.However, is putting a larger (47uH) inductor will make it bad? notice that the 12v input sources are assumed to be bad in terms of ripple and noise... one source could have little noise\ripple and another one is large ripple..etc. this design is done assuming the people get any reasonably-good 12v 3amps wall-adapter and it should work fine.QuoteYou don't need to bet, I posted pictures with this reply to show 12v input, 3.3v output, and 5v output for both MYPSU and OTHERPSU as label suggests. Looks like frequency of the ripple is a lot less than expected which should be attenuated better IMO. I think with pictures you can judge better.Notice that ground probing sometimes shows 100Hz and sometimes > 800Hz... I posted the picture of 800Hz but from waveform you can judge better.QuoteI am afraid 12v input and its switch connector have to be on top.Can't I put it in top along with its filters then put close vias to GND for each cap?also, will the switchers and their circuit be near the 12v connector and filters?if so, then your idea is to make the output connector very far from the actual switching loop... with bulk caps near the output connector itself rather than the switchers?QuoteHmmm so you agree with T3sl4co1l on the ground pour, and with me on putting short and close ground vias to caps of input filter and switcher circuit?still, big LC values are better than small ones for 12v rail... due to different quality of input sources. So, isolating the DC-DC switchers from input 12v is done via good routing and making very short loops... plus, making output connector with its caps far from switcher loop itself. correct?Do you honestly think we can match the < 1mV p-p output capability of the switcher by doing this?thanks all for your help, I am willing to enhance the design as much as I can._________as for making another board.. it is not cheap since it needs machine setup and so on. I even got a good discount from allpcb this time.I can however, use JLC PCB very cheap service which has everything from inductors and caps but it doesn't have that particular ferrite bead and of course the TPS62913 chip which is extremely small.. I don't have much confident I could desolder it from the current boards then re-solder it on the cheap jlcpcb produced board.

author: Vovk_Z
author_rank: Super Contributor
timestamp: August 31, 2021, 07:38:40 pm
content: I can't say anything about ground pour. It's a subject which is better to investigate with a real PCB on hands. I'm not as experienced to give all the answers via the internet, unfortunately. There may be Application notes covering this topic for other similar ICs.

author: iMo
author_rank: Super Contributor
timestamp: August 31, 2021, 09:00:13 pm
content: I would highly recommend you to start with LTSpice simulator, for example (it is free and you may get help here).You should put all your parasitics (ie. the trace inductance L2 in Tim's schematics above, as an example), inlcusive RLC of your capacitors and inductors, resistance/inductance of your pcb tracks, etc.I've done similar exercise recently - where on the o'scope I saw 3Vpp ringing instead of a clean signal. I did a simulation with my real 20mm long wires (20nH parasitic inductance) and I got exactly the same picture in the LTSpice.Thus instead of excessive soldering and elaborating do spend more time with simulation, it works.Also - a filter made of 100uH and 1000uF would work perfectly on a paper, in reality not so - see below your low pass (the values are examples only)..

author: T3sl4co1l
author_rank: Super Contributor
timestamp: August 31, 2021, 09:01:07 pm
content: You know what the fuzzy waveforms mean, right?Zoom in until you see smooth curves. There's high frequency noise that's merely riding on, or modulated by, those low frequencies.Tim

author: thm_w
author_rank: Super Contributor
timestamp: September 01, 2021, 12:15:26 am
content: gofundme for OP to get a decent starter oscilloscope?

author: VEGETA
author_rank: Super Contributor
timestamp: September 01, 2021, 10:09:24 am
content: Quote from: T3sl4co1l on August 31, 2021, 09:01:07 pmWhat is your opinion on the actual waveforms I posted in my latest reply? they show everything... I hope we can understand the problem from them. what shocked me is that the frequency is very little < 100 Hz, what is going on?Right now, the to-do solution is better routing and grounding, plus to see which values of CLC circuit to put + input filters to switchers.I am interested on your analysis of waveforms of scope.

author: xavier60
author_rank: Super Contributor
timestamp: September 01, 2021, 11:53:46 am
content: Quote from: VEGETA on September 01, 2021, 10:09:24 amThe 100Hz modulation is likely caused by the bridge rectifier at the mains input of a SMPS. Because the diodes conduct only at the mains waveform's peaks, they act as switches that conduct switching noise.

author: Vovk_Z
author_rank: Super Contributor
timestamp: September 01, 2021, 12:14:35 pm
content: Quote from: VEGETA on September 01, 2021, 10:09:24 amLow frequency oscillation is a feedback instability. It happens in some voltage-current modes. There can be application note how to get rid of them (may not).I've seen such a thing in one of my DC-DC modules with XL4016, there was found a decision on the internet, to use C or RC-circuit in parallel to IC feedback resistor. I played with it and finally used 10 nF cap in parallel to feedback resistor.

author: Vovk_Z
author_rank: Super Contributor
timestamp: September 01, 2021, 12:26:48 pm
content: Quote from: VEGETA on August 31, 2021, 05:22:21 pmExperience I have: I have low-noise DC-DC (with XL4016) with less then 1 mV RMS noise and I didn't use large ground pour. Design was made with wide printed wires which go somewhere near each other, more or less close to each other.

author: Vovk_Z
author_rank: Super Contributor
timestamp: September 01, 2021, 12:35:24 pm
content: Quote from: VEGETA on August 31, 2021, 05:22:21 pmBig L values everywhere except main switcher L may worsen stability but not help. That's one of the reasons you are told not to use large L values.For example, it you decide to add post-filter after switcher with large L - it will provoke instability. And similar things may happen with unlucky L before the switcher. A typical 'safe' post-filter L value may be no more than 10-20% of a main switcher L.

author: VEGETA
author_rank: Super Contributor
timestamp: September 01, 2021, 12:39:32 pm
content: Quotethere are no AC on board, I use 12v laptop-style SMPS. It works perfectly fine in terms of continuous operation without issues, I played Dreamcast using it for hours and hours.Quotethat is called bootstrap capacitor if I am correct, and I have one for each switcher feedback as mentioned in datasheet. Mine is 1uF which is the best value which includes maximum performance (stability, noise cancellation) while being not near the upper limit.However, if this analysis is correct, it may be coming from the 12v input wall charger itself.Don't you think some extra input filter elec. caps can help here since it is low frequency?QuoteI am interested in this solution if you can explain more or post circuit or methods.QuoteRight now I didn't add any but maybe a 1uH is good? assuming the main switcher L is 4.7uH.That is for post-filter, but why also pre-filter?____from my previous waveforms... how much is the actual ripple and noise figure is? how can we know it for sure without the oscillation?

author: Terry Bites
author_rank: Super Contributor
timestamp: September 01, 2021, 12:40:20 pm
content: TI publish a usefulk guide on ouput filtering.https://www.google.co.uk/url?sa=i&url=https%3A%2F%2Fwww.ti.com%2Flit%2Fpdf%2Fsnva871&psig=AOvVaw3GzlT0oUMPBwz4b9SZrIwX&ust=1630586197218000&source=images&cd=vfe&ved=0CAcQjhxqFwoTCPjAlaDl3fICFQAAAAAdAAAAABAD

author: Vovk_Z
author_rank: Super Contributor
timestamp: September 01, 2021, 01:04:46 pm
content: Quote from: VEGETA on September 01, 2021, 12:39:32 pmNo, I am definitely not talking about bootstrap cap. I'm talking about additional feedback elements (not shown in the datasheet).

author: xavier60
author_rank: Super Contributor
timestamp: September 01, 2021, 01:05:02 pm
content: A mains powered SMPS with PFC stage could also possibly produce 100Hz modulated interference.

author: Vovk_Z
author_rank: Super Contributor
timestamp: September 01, 2021, 01:15:16 pm
content: Quote from: VEGETA on September 01, 2021, 12:39:32 pmThere is nothing interesting to show because the PCB exists in only 'first breed' generation (zero version), but real device have some small changes and improvements made to achieve low noise (<1 mV RMS), made with a knife and wires. So there isn't much sense to show it.In the attachment I show an additional cap I'm talking about which calmed my switcher.

author: VEGETA
author_rank: Super Contributor
timestamp: September 01, 2021, 01:58:00 pm
content: Quote from: Vovk_Z on September 01, 2021, 01:15:16 pmPlease check my schematichere.I understood what it is but failed to remember the name, it is called "feed-forward capacitor" and it is not specific for TPS62913 but rather for all DC-DC converters. I choose 1uF, I wonder if low values such as 2.2nF or your 10nF is better. they claim their low noise performance is done without it.TPS62913 has also the NR/SS cap which affects soft-start and noise reduction, that too is 1uF.

author: Vovk_Z
author_rank: Super Contributor
timestamp: September 01, 2021, 03:27:22 pm
content: Quote from: VEGETA on September 01, 2021, 01:58:00 pmC22, C23 - 1 uF, really? Why so large value?

author: T3sl4co1l
author_rank: Super Contributor
timestamp: September 01, 2021, 03:36:15 pm
content: Quote from: VEGETA on September 01, 2021, 10:09:24 amThey show very little, the scale is 25ms and the waveforms are solid blocks of pixels indicating multiple cycles per pixel. More like 10µs/div would be more interesting.Tim

author: Vovk_Z
author_rank: Super Contributor
timestamp: September 01, 2021, 03:37:45 pm
content: Quote from: VEGETA on September 01, 2021, 12:39:32 pmI guess you confused it (C22, C23) with Cnr/ss. This is possibly a root of your low-freq oscillation.

author: Vovk_Z
author_rank: Super Contributor
timestamp: September 01, 2021, 03:40:19 pm
content: Quote from: VEGETA on September 01, 2021, 01:58:00 pmSo you haven't tried yet another value for C22, C23 and ask us for a solution?

author: VEGETA
author_rank: Super Contributor
timestamp: September 01, 2021, 05:45:18 pm
content: Quote from: Vovk_Z on September 01, 2021, 03:40:19 pmI didn't find a value recommended for these so I put the same as SS\NR one. but why is this the reason for the issue? I mean, the switcher regulates very precisely without issues.Quotebut doesn't it show the ripple period and its magnitude?

author: T3sl4co1l
author_rank: Super Contributor
timestamp: September 01, 2021, 06:18:44 pm
content: There are many periods and magnitudes of interest here...

author: Vovk_Z
author_rank: Super Contributor
timestamp: September 01, 2021, 07:49:47 pm
content: Quote from: VEGETA"NP" near that cap means "do not place".

author: VEGETA
author_rank: Super Contributor
timestamp: September 07, 2021, 05:12:02 pm
content: I am now re-making the board, I have attached the current schematic. I have added one common-mode choke to help attenuate the common-mode ripple if it exist. all 22uF caps are 1206 package instead of 0805.I have started doing the PCB, right now I put full ground pour (solid, no thermal reliefs) and also top all solid ground plain except of course the traces. Each GND pad (filter caps, etc..) has a very close via to ground plane.

author: VEGETA
author_rank: Super Contributor
timestamp: September 09, 2021, 06:44:37 pm
content: I removed 1 22uF from each switchers to allow maximum of 200uF total capacitance.Should I add 1uF before and after the common-mode choke?right now this is the CMC I choose:https://www.lcsc.com/product-detail/Common-Mode-Filters_Murata-Electronics-DLW5BTM501SQ2L_C91597.htmlrelatively cheap murata from LCSC. I could go for cheaper stuff as well if they won't make a difference.

author: VEGETA
author_rank: Super Contributor
timestamp: September 09, 2021, 07:45:57 pm
content: I have done the new layout based on last schematic. Please see it in attachments.I put bottom layer full ground pour + top layer full ground pour except for the traces and vias. Also in top plane there is a small +12v pour near top right as you can see.Nearly every cap GND pin has a ground via nearby very very close to it.Please rate the design and give me your awesome feedback. I am willing to learn.

author: T3sl4co1l
author_rank: Super Contributor
timestamp: September 09, 2021, 09:45:36 pm
content: Can you show top copper with pours enabled?You'll have a heck of a time soldering FL1, best check those pads.Tim

author: VEGETA
author_rank: Super Contributor
timestamp: September 10, 2021, 10:33:05 am
content: Quote from: T3sl4co1l on September 09, 2021, 09:45:36 pmthey are in description.it will be smt assembled not hand soldered.do you think this will eliminate most or all cm noise?

author: T3sl4co1l
author_rank: Super Contributor
timestamp: September 10, 2021, 01:14:24 pm
content: Hmm, still can't figure it out, like why does the top copper not seem to pour over the bottom side traces? They're both green, it's very ambiguous.Tim

author: VEGETA
author_rank: Super Contributor
timestamp: September 10, 2021, 01:32:25 pm
content: Quote from: T3sl4co1l on September 10, 2021, 01:14:24 pmWhat connector exactly?I chose "solid" for copper pours, so all pads will blend in with the copper pour without thermal relief stuff. top side is red while bottom side is green.I can make more photos if you want but kindly mention what exactly is the thing you want to see.Also, will this solve the noise problem? the layout is good now? I am interested in those more.

author: T3sl4co1l
author_rank: Super Contributor
timestamp: September 10, 2021, 02:01:44 pm
content: I mean, like if I zoom in over here, the via seems to be completely surrounded by black. Which is obviously absurd, why would it dead end?Ohhhh, zooming in, and cranking the shit out of the brightness -- I can see what's going on. The connecting trace has RGB 33,0,0 against a background of black 0,0,0 (original levels). Your eyes must be much better than mine (or your monitor is, or, it's a whole lot worse..!), to actually be doing work like that?Tim

author: T3sl4co1l
author_rank: Super Contributor
timestamp: September 10, 2021, 02:02:50 pm
content: Aha, amping up the red channel, and narrowing green a bit, gets something that looks a lot like old school Ultiboard.Why can't they use these as default settings though?Tim

author: T3sl4co1l
author_rank: Super Contributor
timestamp: September 10, 2021, 02:17:16 pm
content: So here's what I'd like to change:- Move the traces to the blue paths. This keeps ground solid under the regulators.- Add vias where shown (blue circles). This keeps top and bottom ground solid, stitching around traces.Note that the inductor is not a high-current switching path, it's fine to run traces under there, within reason. No problem from cutting the ground (i.e. the negative space created by pouring around a trace). And this trace isn't sensitive to noise.- Remove a couple caps (blue X's) and add a series inductor (purple). This filters the 12V passthru/out.All the filters are clustered around the bottom so the output connector should be nice and quiet. The input connector is across the board so can pick up some switching noise, but at least the switching currents should be tightly contained, and are surrounded by lots of ground copper, keeping the voltage drop small. And there's a CMC, which helps.The overall number of capacitors is... rather obnoxious, but they don't hurt anything being there, they can always be depopulated on assembly. Do check for compensation / stability (load step test).The layout could be smaller, I suppose, for example if less space were taken up where 12V is routed around one regulator to the other; they could just be chained on the same trace, no problem.Tim

author: VEGETA
author_rank: Super Contributor
timestamp: September 10, 2021, 03:10:34 pm
content: Hello,- I re-arranged those traces to make better grounding. I should not get feedback circuit under the noisy inductor, therefore I made those routes and re-routes. However, the other resistor is for power good function which doesn't care about noise but still managed to get it without going under the L.- I didn't remove the 12v filter caps since I don't know the inductor value and therefore I could use 4.7uH which I used here. Plus I already put 4.7uH one as seen in schematic and layout (upper right). Do you mean I remove 22uF+47uF caps and put a 4.7uH instead just for output connector? since they won't be feeding the switchers.- added more vias in different places.number of output caps for each switcher stages are correct. I need total capacitance to be less than 200uF, here it is about 201uF or so... 1206 package is good for that despite they are putting 0805 in datasheets but that is mainly because they were interested in showing how this part actually reduces space. I have enough space therefore I can put such caps. They only recommended ceramic caps but I added an electrolytic 47u at the end.It is possible to eliminate all 47uF elec. caps and just use 22uF ceramics since 1206 is kinda good with 3.3v and 5v. but 47u ensures more capacitance rather than get reduced by dc bias. plus, 12v is very harsh on ceramics due to dc bias.from this and your opinion, how much noise\ripple can we get as a total figure? I really want it to be so low even if it is not fully needed to be so. perfection is always desired xD. Previous comments suggested that CMC is the key to reduce all this which is why I added it + the layout note about vias. I hope now it is done.problem is I can't order this again due to high cost of assembly for mere 5 boards. JLCPCB doesn't have all the parts either, the TI switcher is impossible to hand solder! I am trying to have a solution which ensures very little cost to try at least 1 board fully assembled.

author: T3sl4co1l
author_rank: Super Contributor
timestamp: September 10, 2021, 09:18:05 pm
content: Yes, 4.7uH is fine. You're not filtering the output from the input, you're filtering it from the switchers, which throw quite a lot of noise upstream. It would likely be fine also to bypass it all, loop the raw input (after the CMC) around the side, down to the connector.Tim

author: VEGETA
author_rank: Super Contributor
timestamp: September 10, 2021, 10:19:34 pm
content: Quotemeaning what exactly? putting ceramic caps around CMC?I will put 4.7uH instead of those 2 caps next.

author: T3sl4co1l
author_rank: Super Contributor
timestamp: September 10, 2021, 11:00:55 pm
content: Bypass in the plain meaning, run the trace around the right edge, ignoring the internal 12V pour.Tim

author: VEGETA
author_rank: Super Contributor
timestamp: September 11, 2021, 11:45:23 am
content: Quote from: T3sl4co1l on September 10, 2021, 11:00:55 pmyou mean give it a separate path? this way it won't benefit from the huge 1000uF capacitor.

author: T3sl4co1l
author_rank: Super Contributor
timestamp: September 11, 2021, 03:01:11 pm
content: Who cares, don't need it anyway. Or put it on the other side of the 4.7uH.Tim

author: VEGETA
author_rank: Super Contributor
timestamp: September 12, 2021, 06:06:58 pm
content: Hello,I have done it.- re-arranged 12v stuff.- added another 4.7uH inductor, now has 2 separate paths of 12v... one for output connector, one for switchers. Both stages supplied by 1000uF+47uF capacitors.- each 12v stage has 22uF ceramic + 47uF elec. cap.- layout is done where the 2 inductors are on the side.is it good now? does it need anything else?what noise\ripple expected now?regards!

author: T3sl4co1l
author_rank: Super Contributor
timestamp: September 13, 2021, 03:49:47 am
content: Nice!Hm, I would add one via:That should do it.Tim

author: VEGETA
author_rank: Super Contributor
timestamp: September 13, 2021, 05:24:25 am
content: Nice?! you should say "marvelous" hhhhh xDI will add that via today when I get back.First time for me to know that adding vias like this is vital in PCB design. Also, that doing ground pour on both layers is the best way to go. However, in 4 layers stack, I guess I should have signal-gnd-gnd-signal stack right? since the 3rd layer can be a power layer but sometimes I would have multiple power rails which makes it difficult to put them all on one power plain, therefore making it gnd is better right? I could just route power on signal layers.I understand that vias are short path to gnd which makes it easy for current to go to ground instead of travelling long distance, therefore noise will be significantly reduced overall. is that correct?what is more to learn about this? what more improvement I can do? is the CMC part suitable and how to choose a suitable one?most importantly, do you think I can achieve < 1mV total noise\ripple this way? maybe at least < 5mV p-p? how much exactly?

author: T3sl4co1l
author_rank: Super Contributor
timestamp: September 13, 2021, 06:18:42 am
content: Oh, one more thing but it's unrelated to electrical performance per se. With all that copper, and via stitching, and direct-pour pads, you may find soldering is quite difficult. Especially on those undersized pads for the CMC. Basically the whole board needs to reach soldering temp before anything will melt. And the direct-pour pads have extra surface tension that tends to lift components, leading to tombstoning, particularly when the other pad just has one or two traces leading out of it. (Tombstoning isn't much of a problem for 0805 and larger, but is a concern for smaller chips.) If nothing else, you'll have a hell of a time doing any rework with a soldering iron; hope you have a hot air machine.2-4 spokes (thermal relief) drops just enough thermal resistance to make soldering a little easier, while having essentially no electrical impact, and for thermal dissipation purposes (at regular component-self-heating power densities) has little effect as well. (That is, because soldering is done with more heat, the temp drop is higher, so the spokes are helpful there, while also being mostly inconsequential in operation.)5mV is probably in the right ballpark. I'd have to do some calculations to give a better guess.Note that we still have not resolved whether your power adapter in the first place is the source of noise, nor of what the spectrum looks like (just a forest of spikes, modulated at 50Hz). If it is the adapter, the CMC will at least help a bit, but you may still not observe the noise floor of the board itself, if this is the case.Tim

author: VEGETA
author_rank: Super Contributor
timestamp: September 13, 2021, 06:30:38 am
content: Quote from: T3sl4co1l on September 13, 2021, 06:18:42 amYou mean choose "thermal relief" in Kicad instead of "solid" for ground pours? I can also make CMC pads bigger.I won't be doing any rework stuff anyway, but adding thermal reliefs seems reasonable enough.I hope I can get below 5mV if possible, how can you calculate that now?there is nothing else besides the power adapter anyway. I used a reasonably-good one, I have worse. users might have better or worse too. the forest of spikes at 50 hz seems not good to me since this is not the switching frequency of the power adapter. therefore, we concluded here in this thread that it is CM noise. I think you can still see the ripple waves caused by the power adapter in the pictures.

author: T3sl4co1l
author_rank: Super Contributor
timestamp: September 13, 2021, 08:08:49 am
content: Yes, thermal relief.Oh, and keep vias direct, thermals there just take up space.Calculations require building a model, which will take several hours to do; I'm guessing you don't have the budget for me to do that, but if you like, references can be found for using simulators, and building EMI equivalent networks. Which, without starting knowledge, it will take some, probably weeks to get up to speed -- well worth it if you're planning on making more supplies and stuff though. Well... weeks, more like months including background material like how to setup and measure networks, RF port theory, CM/DM etc...Tim

author: VEGETA
author_rank: Super Contributor
timestamp: September 13, 2021, 06:09:25 pm
content: Done. I had to re-arrange stuff around switchers when making thermal reliefs.I may increase the pad sizes of CMC if it is necessary.

author: BrianHG
author_rank: Super Contributor
timestamp: September 14, 2021, 04:48:07 am
content: You have 1 trace which may be damaged by the mounting screw and the same thin trace right at the edge of the PCB. see photo for fix...

author: VEGETA
author_rank: Super Contributor
timestamp: September 14, 2021, 04:57:01 pm
content: Quote from: BrianHG on September 14, 2021, 04:48:07 amI fixed it, plus added some vias under inductors.

author: T3sl4co1l
author_rank: Super Contributor
timestamp: September 14, 2021, 06:42:31 pm
content: The reliefs seem pretty large, just 7 to 10 mils is enough expansion / clearance. And similar for spoke/web width.Which, huh, a few look super thick, like the uh, whatever the row of capacitors is above the middle regulator, I can't read the silk from here. Looks like there's fat ass traces hidden by the polygon or something? If those are required for connectivity / pouring, I'd shrink them, and align them with the spokes so you aren't creating extra or thickened ones.Tim

author: VEGETA
author_rank: Super Contributor
timestamp: September 14, 2021, 08:42:19 pm
content: Quote from: T3sl4co1l on September 14, 2021, 06:42:31 pmkindly check attached images. first one is for ground pour settings so you can see and advise which ones to change, the 2nd one is for showing the traces (blue arrow, red arrow, black arrow) to see which ones you mean.if you mean blue arrow, this trace size is 2 mm which is the biggest since it is the main power input for the regulators as you can see... came from 12v rail. Should I shrink it a bit, to be 1? since there was nothing around it I thought of making it big.

author: T3sl4co1l
author_rank: Super Contributor
timestamp: September 15, 2021, 09:20:27 am
content: Yes the traces are too fat in places, they can be necked down locally, or for just an ampere or two they don't need to be very wide at all, 0.5 to 1mm. And you can get 2oz copper for extra handling.Yeah thermal relief and clearance, 0.254 mm will do.Tim

author: VEGETA
author_rank: Super Contributor
timestamp: September 15, 2021, 07:04:24 pm
content: Quote from: T3sl4co1l on September 15, 2021, 09:20:27 amdone.- I have adjusted it to 0.254mm.- I removed all GND traces under the vias which connected caps together, now only thermal reliefs are there.

author: BrianHG
author_rank: Super Contributor
timestamp: September 15, 2021, 10:49:02 pm
content: Via 'A' may cook/fail if port 'B' draws above 250ma at 5v. (I do not know drill size, so I'm uncertain.)You may move that entire trace to the bottom layer, no need for a via.

author: VEGETA
author_rank: Super Contributor
timestamp: September 15, 2021, 11:22:53 pm
content: done.

author: Faranight
author_rank: Unknown
timestamp: September 21, 2021, 07:10:46 am
content: Hello.I skimmed over this thread since I was doing a buck PSU design myself recently and I have some remarks. One thing I noticed about your design is that you're running copper traces underneath or very close some inductors. For example, L2 and L3 seem to have a trace or two going back to the IC. Several papers on buck design that I've read advise against this practice because the inductors will introduce noise in whatever lies beneath and around them. The TPS6291x datasheet shows the two pins should be connected directly to an inductor, so I'm not sure, if that's going to be a problem or not. The buck feedback traces should also be routed away from inductors - you're running one such trace very close to L3.See this document for example:https://fscdn.rohm.com/en/products/databook/applinote/ic/power/switching_regulator/converter_pcb_layout_appli-e.pdfCheerzies!

author: T3sl4co1l
author_rank: Super Contributor
timestamp: September 21, 2021, 02:45:18 pm
content: I don't worry too much about trace proximity to inductors. First it depends on shielded vs. open: if the latter, give more weight to the consideration. Also, while you can't really figure it at design time, you can at least measure it in the prototype: just hold a loop nearby, approximately where the trace would be, and measure the induced voltage. Intuitively, even for unshielded inductors, it can't be more than a N:1 fraction of the switching waveform, and falls quickly with distance. Most inductors have a fair number of turns (for something like in this thread, say 10-20t; but it does go down to 1-3t in high current, high power inductors) so that's on your side.For my part, I prefer putting pours around the inductors rather than thin connecting traces, simply to increase the power dissipation of the component. Some heat may be sunk out of the regulator by the same means. (Other likely routes are GND and VIN, one of which (GND most of all) is likely to be substrate and therefore thermally important.)And with inner planes, proximity on opposite sides is irrelevant: even 0.5 oz copper planes are adequate to block 100kHz+.Tim

author: sandalcandal
author_rank: Unknown
timestamp: September 22, 2021, 09:19:40 am
content: Quote from: T3sl4co1l on September 21, 2021, 02:45:18 pmI actually saw a masters thesis presentation earlier this year where coupling from ashieldedinductor was actually causing significant EMI issues and change in behaviour of a buck converter eval board. Despite multiple other theories, the cause was tracked down to be coupling into a nearby voltage sensing pin. Quite the journey to track down and 100% confirm the root cause.https://www.psma.com/sites/default/files/uploads/files/Impact_of_Power_Inductor_on_EMI_Performance_of_DCDC_Converters_Ammad_Javed_Ernst_Abbe_University_of_Applied_Science_Jena.pdf

author: VEGETA
author_rank: Super Contributor
timestamp: September 22, 2021, 12:27:53 pm
content: I actually had the feedback pin from another path away from inductor, but got the suggestion here to route it this way near the inductor due to making a split in ground plain. should I get it back? maybe it is safer under the switcher than near L.

author: T3sl4co1l
author_rank: Super Contributor
timestamp: September 22, 2021, 02:56:28 pm
content: Quote from: sandalcandal on September 22, 2021, 09:19:40 amHah, neat. Their fault for cramming the pin so tight I suppose, and also putting more than just an error amp on it (who knows what's in that "Direct Control and Compensation" box). Note the problem would've been lessened if they had simply poured ground around the inductor (preferably with stitching)!Irony being, the "problem" is advantageous, at least at the particular conditions measured; free spread-spectrum broadens and lessens the peaks. What's disadvantageous is it's dependent, going away at higher input voltage evidently.Tim

author: VEGETA
author_rank: Super Contributor
timestamp: October 05, 2021, 05:09:27 pm
content: I have re-allocated the 3.3v feedback from being near the inductor to being from under the regulator... the only place available.I also added more ground stitching vias on top near connectors, that area had 0 stitching vias.I also made the pads of CMC bigger, now 1mmx1mm instead of 0.55mm or so.

author: VEGETA
author_rank: Super Contributor
timestamp: October 05, 2021, 06:45:13 pm
content: EDITS:1- downloaded and used the correct CMC footprint, it is DLW5BTM501SQ2L which is available cheaply on LCSC.2- added more vias under caps and inductors.3- added 3D models for all stuff to look fancy.4- CMC has weird pads shape, which kicad doesn't add thermal reliefs by default. thus I added them manually to the best I could. please checkto do list:- silkscreen stuff like component tags and so on.

author: VEGETA
author_rank: Super Contributor
timestamp: October 13, 2021, 09:58:59 pm
content: what do you guys think now? I still have to clean up the silkscreen stuff.I am interested in the final ripple and noise p-p figure, what to expect here?plus, do you know a pcb house that can do only 1 or 2 assembled boards cheaply?

author: BrianHG
author_rank: Super Contributor
timestamp: October 14, 2021, 06:00:45 am
content: Looks good.If you if you want to go through the trouble and you have the parts, you can setup your own small SMD lab with a flat iron and arduino board, thermo couple and solid state relay. Handy allowing you to make small PCB anytime:I still prefer to use a stencil and old credit-card to apply the solder paste. Using a stencil with the iron can get you to the edge of what will look like a professional SMD assembly job.

author: VEGETA
author_rank: Super Contributor
timestamp: October 14, 2021, 10:40:33 am
content: I cannot do such setup right now unfortunately. Plus, some of these items are very very small (2mmx2mm for switchers). I hope there is a company which has small setup fees or so.Do you have anything else I can do or add to make the design better?Can we get < 5mV p-p total noise\ripple figure? I hope so.

author: BrianHG
author_rank: Super Contributor
timestamp: October 14, 2021, 12:39:02 pm
content: Unfortunately, without PCB and a measuring scope, there isn't much that you can play with other than try to match the IC manufacturers recommendations. If your inductors are a good match for the ones in the TI data sheet, you should get a clean output. It is the question if your new source power-supply choke is big enough to isolate switcher noise from that 12v supply going throughout your system. The other problem is that this noise can be down in the low KHz region. Your PCB may be clean, but noise looping though even the ground of your source 12v supply can create a problem in the dreamcast where using a battery or linear 12v DC supply will be completely isolated from your AC wall outlet in a way no cheap Aliexpress 12v AC adapter switcher would be. That is unless you make sure such a 12v switcher came from a reputable design.(Youtube channel DiodesGoneWild ->https://www.youtube.be/channel/UCQak2_fXZ_9yXI5vB_Kd54gtears apart many of these switchers, he opens and unwinds the transformers themselves, and except for top name brands and an occasional fluke, most of them are garbage and fail on many levels.)As for the switcher being 2x2mm. Yes that is a headache, though when ordering PCBs with a SMT stencil, the paste application is easy. Especially on small PCBs. And when placing a device with tweezers, you do need to get it close, but not perfect as the device centers itself as the solder paste melts.I've seen youtube videos of those using a frying pan with sand to spread the heat evenly before it reaches the PCB, but, the iron has a thermocouple right on its surface with precise temp control so nothing will get burnt.Having mounting hardware means if you make a mistake or blow the component, or need to change a component, you can remove the part, clean it, and try again. Though, I cannot blame you about wanting to have someone else already equipped and experienced to do it.

author: BrianHG
author_rank: Super Contributor
timestamp: October 14, 2021, 01:26:34 pm
content: Just in case you want in the future:http://electronoobs.com/eng_arduino_tut155.phpAduino base hotplate with source code.He used the stencil method of applying solder paste.His resulting PCB looks better than some of the Aliexpress junk pre-made PCBs I have seen in the past.

author: VEGETA
author_rank: Super Contributor
timestamp: October 14, 2021, 04:05:41 pm
content: Right now I am searching for cheap oscilloscopes. Here in Jordan we have picoscope 2204A but it is out of stock, and Hantek 6022be which doesn't have ac coupling and seem a bit bad.I am thinking of asking here in the forum if anyone willing to giveaway or sell digital scopes at very cheap price so that it doesn't cost a lot in total. Best Amazon deal was this:https://www.amazon.com/Oscilloscope-Channels-Bandwidth-Portable-SDS1102X/dp/B089GG14BP/for 230$ including shipping + 0$ import fees which I kinda doubt.EDIT: I found this isolated one for 145$ total including shipping and import fees:https://www.amazon.com/OWON-VDS1022I-channels-Digital-Oscilloscope/dp/B07CNP2CJY/

author: VEGETA
author_rank: Super Contributor
timestamp: October 14, 2021, 06:54:28 pm
content: I have arranged the silkscreen stuff properly now. Currently doing the BOM.

author: VEGETA
author_rank: Super Contributor
timestamp: October 27, 2021, 06:16:44 am
content: I ordered Owon VDS-1022I USB scope, will arrive next week or so.I am contacting my PCB assembled to make only one assembled board for testing purposes, this time I hope I get it correct. I hope noise and ripple are < 5 mv p-p total.do you think I can achieve such a low level?is there any modification to do before sending the gerbers?

author: BrianHG
author_rank: Super Contributor
timestamp: October 27, 2021, 06:52:15 am
content: The 5mv will be difficult to measure as it will be within the noise range of the scope input.And you may be reading noise just through the probe's GND clip or even local AM radio broadcasts.Using the scopes input filters and running the probe in x1 mode will help here.Also, remember that your goal is this low noise level when actually loaded by the Dreamcast, playing a CPU intensive game. You should do fairly well. I can only imagine needing to add a huge electrolytic cap on the 3.3v rail-gnd to help if the Dreamcast current load modulates like hell.

author: VEGETA
author_rank: Super Contributor
timestamp: October 27, 2021, 03:32:50 pm
content: Quote from: BrianHG on October 27, 2021, 06:52:15 amwell, adding another big cap will be bad since it will exceed the maximum capacitance allowed by the switcher. it strictly advised to stick to it. I am at the top of it now. I am doing 201 uF instead of 200uF maximum... most of them are 22uF 1206 caps which will dip a bit to allow < 200uF effective capacitance. this is the total before and after ferrite bead exactly as datasheet wants.I previously used 0805 caps but now 1206.AllPCB are doing free assembly these days so I will definitely use it.The scope sensitivity is 5mV/Div, so even at 10 mv setting I can see the 5mv i guess. plus, this time common-mode noise should be gone or hugely eliminated which is always a plus.

author: Vovk_Z
author_rank: Super Contributor
timestamp: October 27, 2021, 04:45:20 pm
content: It is good to have an oscilloscope because id is a universal device. And it definitely will help to fight with a ripple of any switcher. But be ready that it can't help much if you are interested in low-noise measurements (sub-millivolt).

author: VEGETA
author_rank: Super Contributor
timestamp: October 27, 2021, 05:01:05 pm
content: Quote from: Vovk_Z on October 27, 2021, 04:45:20 pmsub-millivolt? well, if I can get to 1 mv I consider that fantastic, this project is targeting about 5 mV which is in the range of the scope which people report it is clean in terms of inherit noise.what is your recommendation then?right now at this stage VDS-1022I is the best choice for me.

author: BrianHG
author_rank: Super Contributor
timestamp: October 27, 2021, 05:17:12 pm
content: Quote from: VEGETA on October 27, 2021, 03:32:50 pmYes, right at the switcher, the low impedance direct connection in the feedback path and GND.But remember, in your Dreamcast, you have a ton of caps from VCC to GND throughout the PCB. Your total is probably exceeding that 200uf limit by a few fold.Just counting the electrolytics and tantalums in a photo of the dreamcast motherboard I see:10+10+10+10+22+22+4.7+47+220+100+47+100+47+100+150+47+100=1046.7ufDivide that by ~2 so you have half on 3.3v and half on 5v.That's another 500uf not counting the sum of the tiny stuff.This should not be a problem as you have a enough of a series resistance between your power supply PCB and the dreamcast itself in the power cables alone.Yes, if you place a 2200uf cap on your PCB right where your other caps are on it, the switchers may oscillate and their mosfets and your inductors may get a huge current spike at power-up since it will look like a short to GND for a small instant if those caps have a low ESR. This gets worse with a nice huge 22000uf cap.

author: VEGETA
author_rank: Super Contributor
timestamp: October 27, 2021, 06:10:33 pm
content: Quote from: BrianHG on October 27, 2021, 05:17:12 pmI guess the dreamcast board may have your suggested amount but it is not direct at the rail itself like my caps. they are spread in the board in many stages and ICs, after and before other stuff. So I guess they don't count as mine or nearly.I have another PSU made by someone else which is kinda the best in market, it only has 100uF elec cap at the output of each stage.. just that, no ceramics no others. I tested playing on it for hours and hours different games but still didn't notice any degrade in performance. I have double that capacitance.the PSU and dreamcast are connected directly using pins, no wiring at all.I think I will go with this current design. I do have extra 220uF through-hole caps (and other values) in hand so I can also test adding one of them in case something like you suggested happened. My scope will arrive in 7-10 days or so but the PCBs will take more.

author: Vovk_Z
author_rank: Super Contributor
timestamp: October 28, 2021, 02:42:58 pm
content: Quote from: VEGETA on October 27, 2021, 05:01:05 pmI use an oscilloscope plus AC true-RMS microvoltmeter with 5 MHz range to work with sub-mV levels (It is simple and quite cheap old Soviet В3-57 microvoltmeter).If you are fine with "near-1mV" RMS noise lever then an average oscilloscope itself possibly should be fine.

author: Vovk_Z
author_rank: Super Contributor
timestamp: October 28, 2021, 02:52:16 pm
content: Quote from: VEGETA on October 27, 2021, 06:16:44 amIt is good that it has galvanically isolated power lines. So you wan't have an excessive induced common mode noise.

author: VEGETA
author_rank: Super Contributor
timestamp: October 28, 2021, 03:10:58 pm
content: first time I know about microvoltmeter but it doesn't look like it draws like an oscilloscope but rather a value like multimeter.I think there are reasonably cheap or affordable oscilloscopes which can do 500uV/Div but are they good enough?VDS-1022I is isolated yes, which means no common-mode from source.

author: VEGETA
author_rank: Super Contributor
timestamp: November 21, 2021, 08:00:20 pm
content: I've got OWON VDS1022I and the attached images are taken by it for 3.3v and GND of both my PSU and other PSU. Notice that my psu is the old version which I posted its measurements before... the new improved version with proper grounding + CMC + better filtering + bigger sized ceramic caps is going to start being manufactured in 2-3 weeks due to chip shortage. will need time to arrive though.summery of pictures:My PSU:ground noise floor: about 14 mv P-P with some noise on top.3.3v regulated rail: about 17-20 mV P-P ripple with nearly no noise on top, just ripple.Other PSU:ground noise floor: about 5 mV P-P ripple with more noise on top.3.3v regulated rail: about 11~12 mV P-P ripple with a lot of noise (40~50 mV P-P) on top of it.Please check the images and tell me what do you think?

author: T3sl4co1l
author_rank: Super Contributor
timestamp: November 21, 2021, 10:38:53 pm
content: What does the power supply and probing setup look like?Tim

author: VEGETA
author_rank: Super Contributor
timestamp: November 21, 2021, 10:45:53 pm
content: I have it in attachments... just regular scope probing directly at rail itself.

author: T3sl4co1l
author_rank: Super Contributor
timestamp: November 22, 2021, 12:45:09 am
content: What about the power supply?The loop area of the probe, and it laying over the input cable besides, may be picking up much more than you wanted, even with the CMC at the input there.Another way to tell is if the spikes drop in level when you put multiple turns of ferrite bead on the scope probe.Tim

author: BrianHG
author_rank: Super Contributor
timestamp: November 22, 2021, 03:41:54 am
content: You need to use 2 channels on your scope in differential mode to get the authentic noise output of your PSP.Here's how: Channel 1 on your test VCC (right on your power supply's GND output) and Channel 2 on GND (right on your power supply's GND output). Both scope probes should be calibrated and both channels should be set to the same voltage and same bandwidth options. Then you need to select the scope's math function and select channel 1 'minus' channel 2. The math result display, sometimes it's a new third trace on the display, will be the true voltage noise coming out of your power supply. Just move the VCC probe to test both rails.To verify that you are setup properly, if you move either probe, tying VCC to GND, or vice-versa, (IE: Both probes on VCC or GND) the math output should read 0mv noise. (Or, at least as close to 0mv as your scope's input and sampler can get.)Move your 2 probes connections to the Dreamcast's power input and you will get the true noise as the Dreamcast's input.Your 2 probe's GND clips should be connected together to a common GND point on your PCB or Dreamcast.

author: VEGETA
author_rank: Super Contributor
timestamp: November 22, 2021, 07:30:43 am
content: Quote from: BrianHG on November 22, 2021, 03:41:54 amI will do that today, I think this owon scope supports math functions for sure.Quotepower supply is external laptop-style power brick. it is connected directly via the connector at the white plastic part, then 2 wires (red and black) goes to dreamcast. i guess i could move the scope probes a bit off it but even at current setup i think they are away enough not to pick up anything major but will try tonight.notice that this design doesn't have a CMC and also with the bad grounding we talked about above. new design will arrive in a month or so.but besides all this, what do you think of waveforms of both PSUs? which one is better?

author: VEGETA
author_rank: Super Contributor
timestamp: November 22, 2021, 09:04:38 pm
content: please check setup and results of differential probing in attachments.

author: BrianHG
author_rank: Super Contributor
timestamp: November 22, 2021, 09:25:07 pm
content: The connection and math look correct.2 tests to make sure everything is ok.1. tie the 2 GND scope probes together and to a different GND point than the power connector.2. Tie the both probe's tip to the same VCC. In your scope capture, channel 1 and channel 2 should both show the same signal exactly, but, the math channel should be flat with no signal at all. If the math still shows something then double check your scope settings, or re-orient the probes so that they approach your PCB from the other side. EMI may be entering through the probe casing and probe coax.If in case #2, your you see the math channel flat with no signal, then once you move one of the probes from VCC to GND, the output you see on the 'math' channel will be authentic power supply noise at the connector.

author: BrianHG
author_rank: Super Contributor
timestamp: November 22, 2021, 09:28:51 pm
content: CORRECTION:Channel #2 looks delayed compared to channel #1. This should not be. The spikes in channel #2 should line up with the spikes in channel #1. The 2 should cancel each other out in the math channel.Is there some sort of setting in the scope which delays the sampling of channel #1 and #2?Is the sampling set to be simultaneous between both channels?Do you have a bandwidth limiter, IE 20Mhz bandwidth set on one channel but not set on the other?Like what I said in my test #2 above, tying both channel inputs together should show you the exact same signal on both traces and the math output should reveal a flat 0 signal.Is it possible that your scope may sample the entirety of channel 1, stop, then sample the entirety of channel 2 at a different time instead of simultaneously sampling both channels? This would be bad and make the differential measurement setup fail.

author: T3sl4co1l
author_rank: Super Contributor
timestamp: November 22, 2021, 09:40:57 pm
content: I think it's just aliasing from the super zoomed out view. Try more like 100ns/div, trigger on a spike.And you can take a closer look at that, see what (if anything) in the circuit correlates with the spike rate, and ringing frequency.Tim

author: BrianHG
author_rank: Super Contributor
timestamp: November 22, 2021, 09:49:29 pm
content: Another snapshot showing the exact same 2.25us delay on Vegeta's PCB.That is such a huge delay for a scope, maybe it is a bug on the Owon software/firmware.I cant imagine it being a circuit design delay in the scope's electronics as 2.25us would require a huge amount of wiring. But in software, we are talking about having a bad relative sample offset, or, one channel is going through a software filter and the other isn't.The samples speed is set to 50msps. Maybe is Vegeta turned up the sample speed to the high MHz, maybe he can bypass the bug, but you would still need to check.Though, connecting probe #1&#2 to the same point with these settings doesn't produce 2 identical readings, we know something is wrong with the scope, most likely a software or firmware issue.There should not be a 2.25us skew between channels. Maybe Owon didn't test this specific setup. I wonder is turning off the 'math' may fix the problem and align the spikes, or choosing a different timebase. If so, it is clearly a programming bug in Owon's software. Unless you are experienced, you have no clue how many bugs I've been running into in recent years compared to the days of the old-fashioned CROs with regards to component datasheets and modern test equipment which haven't been properly tested with all use case scenarios.

author: BrianHG
author_rank: Super Contributor
timestamp: November 22, 2021, 11:26:25 pm
content: Quote from: T3sl4co1l on November 22, 2021, 09:40:57 pmYou could be right, but the timed pairs coming out which I pointed to.He is running the scope at 50msps for 2 channels but the scope is capable of 1ghz with 1 channel, 500msps with 2 channels. Vegeta needs to increase record length to get the full 500msps as the expense of the USB display refresh might slow down, but with much greater precision display. Though, if doing this shifts the timing of the 2 samples from 2.25us to 0.225us, it shows there still is a fundamental bug in the scope's software and it needs to be fixed to get the true Channel 1 minus Channel 2 view.

author: BrianHG
author_rank: Super Contributor
timestamp: November 22, 2021, 11:37:52 pm
content: Found the 'problem', see image: (It's in you scope settings...)Error: You should not be triggering on both channels 1 and 2. Only trigger on channel 1 exclusively, otherwise, channel 2 will randomly or find the next trigger event and re-align to a non-parallel position based on its waveform completely screwing up the whole purpose of the differential measurement. (IE, the scope is waiting for a trigger on channel 1, then it waits again for the next trigger on channel 2. You do not want that. Channel 1 and 2 need to be aligned in parallel, so, you should only be triggering on 1 channel.)This is assuming using 2 separate triggers on 2 channels simultaneously does the same thing as it would do on my Tektronix scope. With this setup, my scope would generate the exact same error and doing this when attempting the same A-B 'math' differential common-mode measurement, the 2 channels are no longer aligned giving me a flawed result. The math is being done on the sample data in the window with the relative alignment position you see, not like an old cathode ray tube analog scope where the input A-B function is done at the analog stage in the probe input amplifiers where such an alignment error could not be made.Once again, if set correctly, my test#2 above, with Channel 1&2 on the same VCC should generate an identical signal on each trace while the 'math' channel should show dead flat 0.The 50msps should also be able to be increased by using a longer record length as the Owon scope in use can do 1ghz, with a 10 million sample record. Increasing this setting would generate a far greater refined scope shot and more accurate measurements even if you keep the horizontal zoom level at the current 5us/div. (Assuming the Owon has enough ram, otherwise, the only way is to zoom in the time-base.)

author: VEGETA
author_rank: Super Contributor
timestamp: November 23, 2021, 07:18:42 am
content: So to sum up, I need to disable channel 2 triggering while keeping channel 1 triggering? so channel 2 can be active but take triggering from channel 1? I am new to using the scope so I would need some assistance. I will try that tonight when I return.Also, you recommend changing sampling to just 50 instead of 500?

author: BrianHG
author_rank: Super Contributor
timestamp: November 23, 2021, 08:21:29 am
content: Quote from: VEGETA on November 23, 2021, 07:18:42 amPoint #1, you are correct.Point #2, since I do not know about your scope, this speed might be a hardware limitation. If so, zooming in on the horizontal time-base will improve the speed. Or, you may be able to increase the sampling setting at the cost of the on-screen display refresh running slower. This you will have to find out on your own. 500msps means the sampler is running at 500MHz instead of 50MHz, but, there will be 10x the data to send to your PC to display the same amount of width on the scope display.

author: VEGETA
author_rank: Super Contributor
timestamp: November 23, 2021, 09:11:03 pm
content: i did this, please see.i couldn't modify sampling, it is auto

author: BrianHG
author_rank: Super Contributor
timestamp: November 23, 2021, 09:37:34 pm
content: In this snapshot: both_channels_on_3.3v.PNG, if both channels were on 3.3v, how is it possible that channel 1 shows the ripple and channel 2 is flat? Could you have disconnected your probe? If both probes are on the same source signal with the same settings, they should show you the same image.Also, because of the sampling frequency, you should set channel 1 & 2 bandwidth limiter to 20MHz. The view will be cleaner and for this level of zoom, probably more accurate.

author: VEGETA
author_rank: Super Contributor
timestamp: November 24, 2021, 12:16:08 am
content: Quote from: BrianHG on November 23, 2021, 09:37:34 pmI have re-taken the images right after I named them, so this picture is ch1 on 3.3 and ch2 is on gnd.I have searched for limiting stuff but couldn't find, maybe I should search more, please tell me if you know the option. but what is your opinion on the waveforms regardless?I have now modified the picture to have correct name.

author: BrianHG
author_rank: Super Contributor
timestamp: November 24, 2021, 12:59:10 am
content: I don't see the both channels on VCC 3.3 screenshot.You wont find the limiting stuff, your scope is already only 25MHz analog bandwidth anyways.

author: VEGETA
author_rank: Super Contributor
timestamp: November 24, 2021, 07:09:53 am
content: Quote from: BrianHG on November 24, 2021, 12:59:10 amI can take this picture for you if you need to see it, but I remember it was like the grounds one.I feel like it didn't really make the subtraction, or am I wrong? the resultant waveform seem nearly identical to 3.3v one, I don't feel there is a reduction based on ground signal. what do you think?based on waveforms for both PSUs, what do you think of each?

author: BrianHG
author_rank: Super Contributor
timestamp: November 24, 2021, 07:19:38 am
content: It shouldn't be like the GND snapshot.Channel 1 should have the pulsing noise.Channel 2 should have the same pulsing noise.Channel M should be flat, assuming your setup is correct.Your GND snapshot has 3 channels, #1 & #2 & #M all flat.We are verifying to see if your measurement scope setup and probes are all setup identically and properly. 1 mistake, and the result will not look as I described above. 1 mistake and what you see in the 'M' channel is useless for this type of measurement.

author: VEGETA
author_rank: Super Contributor
timestamp: November 24, 2021, 09:01:18 am
content: Quote from: BrianHG on November 24, 2021, 07:19:38 amyes this is what i meant by line grounds... ch1 and 2 are similar and the result is flat.I will see tonight, will replicate the test again. but for now please assume it is correct. so, what is your opinion on this?will proper grounding and separate paths for 12v + 1206 caps + ground stitching done on the newer version (still not arrived).. will this make it better by noticeable amount? at least better than other_PSU

author: BrianHG
author_rank: Super Contributor
timestamp: November 24, 2021, 09:26:07 am
content: Quote from: VEGETA on November 24, 2021, 09:01:18 amI believe the other PSU is just operating at a much lower frequency, hence using larger inductors and larger caps makes the signal softer.Yes, at higher frequencies, the choice of inductors and cap quality will play a part in the output ripple.Your first measurements from 2 days ago show a leakage on both PSUs, a set of dual pulses at 50Hz. This is usually a bleeding ground loop from the AC mains from your source supply and it Y1 cap and primary rectifier diodes. It typically causes a faint buzz in the audio and hum-bar scrolling through the picture. If this is part of the problem you are getting, no small switching supply can fix this as different measures are needed to get rid of this. This would be an annoying AC mains looping frame ground problem I've seen with some 12v supply, perhaps like the one feeding your switcher when you have the output of the Dreamcast attached to another device like the scope GND clip, or your TV's video input. If this was the actual problem, you would not see this with an analog power supply feeding the 12v input or using an isolator transformer on your AC mains feeding the 12v supply. A proper differential measurement of the output on your switcher will determine if it is reacting to such a problem, but, we need to know the measurement you are making is true.As for the 2MHz ring, yes, with a scope, we can sniff some of your PCB and find a solution.

author: VEGETA
author_rank: Super Contributor
timestamp: November 24, 2021, 10:11:57 am
content: yes the other power supply uses lm2596 which has 150 khz switching frequency, with big inductor has "330" label on it, but output caps are just 100uF elec. caps per rail. it has solid ground plain though.Mine runs about 2 MHz switching, therefore smaller inductors. I assume solution is already done on the newer version, perhaps check the previous replies to find it. we put CMC + one ground plain with lots of stitching + short loops for switchers + bigger ceramic caps + more input filteration + making 12v output using a separate path with separate filters than the 12v fed into the switchers. I think we all agreed back then that it would be good to solve all issues but we are waiting the PCBs which will take 4 weeks.So lets discuss the benefit of choosing slow frequency vs fast frequency switching here... what could be the best to use? faster switchers seem more desired these days but what in terms of noise\ripple?

author: T3sl4co1l
author_rank: Super Contributor
timestamp: November 24, 2021, 01:30:32 pm
content: Best for what? Ripple? Non sequitur -- ripple can be made arbitrarily low, given adequate filtering and shielding. It's the other constraints that limit performance: size and cost primarily, with efficiency, component selection, V/I range, etc. also being relevant.Tim

author: VEGETA
author_rank: Super Contributor
timestamp: November 24, 2021, 01:44:36 pm
content: Quote from: T3sl4co1l on November 24, 2021, 01:30:32 pmi mean for my application, 50x50mm board, low noise\ripple requirements as much as possible.my switchers promised < 1 mV of total ripple and noise but the case in real life is not like this. we addressed this to be a grounding problem with what I explained in the previous post. so the new version of the circuit is on route.down through that we landed on the idea that it is also common-mode noise, so CMC is added. I guess CMC can also help in regular noise suppression since it is a big L after all right?however, low frequency stuff could have less worse ripple\noise if filtered through large L and C right?I didn't address the PSRR of the switchers, which is a good value really. but the < 1mV is supposed to be assuming no ripple\noise on the input to begin with. but in my case and most cases, there are a ton of ripple\noise. So I needed to use more filters, bigger caps, better grounding to address this issue.I am hyped about the new design, hoping to be the last one.

author: VEGETA
author_rank: Super Contributor
timestamp: November 24, 2021, 08:30:29 pm
content: this is both channels on 3.3v for my psu

author: BrianHG
author_rank: Super Contributor
timestamp: November 24, 2021, 09:37:04 pm
content: Ok, you have proven that your scope can properly do a differential measurement.Meaning if you place channel #1 on the VCC and #2 on the GND with this setup, the MATH channel will show your true noise at the output.Also, looking at the current background noise in the MATH channel, your scope's approximate background noise level is ~15mv p-p. It might be possible to turn on the scope's measurement stats for the MATH channel as well.Now, your scope's timebase is 10ms/div and the waveform is approximately 2 divisions long.IE: 1s/0.020 = 50Hz. Is this correct?If so, this interference is not your switcher oscillating, it's a leakage from your AC mains bleeding into/through your circuit. Changing a tiny output cap or inductor on your PCB will not solve this problem. (Those changes are to correct problems at the 2MHz switching speed which we cannot currently see.) Now that your scope is properly setup, please do the differential measurement of the rail, with both probe GND clips tied together, then clipped to the dreamcast's GND through a series 100ohm-up to-1kohm resistor. The purpose of this measurement is to verify that the route of this 50Hz interference isn't coming from a looping GND throughout your multiple AC main power supplies throughout your measuring scope's GND. Verify that with the same time-base setting that your competitor's board doesn't bleed through the same 50Hz.(You might as well test the 12v rail too. This interference may be coming through there.)If your video output is 50Hz, this may be CPU processing load once every V-sync. To verify this, load a different game and this waveform's duty cycle should change or disappear. If this is the case, then we need to look at the regulation feedback filter on your PCB and again, the same test is worth looking at on your competitor's PCB. Also, this 50hz signal may not be on the 5v rail if it is due to CPU processing modulating current draw when rendering each frame.

author: VEGETA
author_rank: Super Contributor
timestamp: November 25, 2021, 11:34:11 am
content: Quotethis was the case in previous images. last image was just because I forgot to do it with the rest.QuoteI didn't find it, but since all channels are the same vertical resolution (20mV/Div)... I just use ch1 measurement to measure all waveforms.QuoteI wasn't paying attention... perhaps the pictures above contain this info.QuoteWill do it soon.QuoteSo i should do this measurement setup for both my psu and the other one?ok but what to expect in both cases? I mean why the resistor?Quotethis is interesting.I cannot do it now but will find an SD Card to load games on it then use it since I have gdemu not a gd-drive.

author: BrianHG
author_rank: Super Contributor
timestamp: November 25, 2021, 05:24:55 pm
content: Quote from: VEGETA on November 25, 2021, 11:34:11 amYes they do.QuoteOk.QuoteThe resistor separates the scope's GND from your PSU GND just in case the 50Hz ripple is running throughout the GND. It may also be useful to check if with the Dreamcast disconnected from any TV if it is currently wired there.QuoteYes, if the Dreamcast is currently rendering a really simple scene, IE drawing 3 amps for part of a frame, then going down to 0.5 amps for the rest, this 50hz ripple we see would be within the regulator's transient load response and would probably only show on the 3.3v rail. The other PSU you have may be doing the same thing, you just need to measure that supply with the same scope settings.Typically, this type of problem would be solved with either a low esr bulk capacitor on the 3.3v output right at the PSU power connector, or, modification of the feedback filter for the regulator's 3.3v sense circuit, or use a heavy-duty over-current regulator which wont react to such a transient. However, now with a scope capable of a differential measurement, you can now measure ripple on the feedback resistor network VS the output to trace the problem.

author: VEGETA
author_rank: Super Contributor
timestamp: November 25, 2021, 07:10:17 pm
content: So to sum up, which test should I do for now without the game? which ones with the game? so I can do it.

author: BrianHG
author_rank: Super Contributor
timestamp: November 25, 2021, 09:06:07 pm
content: You may skip the game for now if you like. Just measure the 2 PSUs with the same settings on the scope.If you are going to test a game:Does the Dreamcast have a demo or power-up test mode?Look for a game with just a still intro screen which stays on.We just want to see if it changes the waveform you see now because a 50hz signal can be coming from the AC mains, or, just the right CPU intensity processing in a PAL vidoe system.

author: BrianHG
author_rank: Super Contributor
timestamp: November 25, 2021, 09:47:32 pm
content: Also, if it's power sag or interference from your power source, have you considered it's your input power choke?Did you try shorting it out?Also, what about placing a 2200uf cap on the power output connector? (When powered off of course, the powering on.)What does your scope output look like with the probes on the cap?In your scopeshots, I didn't see anything saying that the probe was set to 10x or 1x. Do you have a 10x/1x setting on your probes?

author: VEGETA
author_rank: Super Contributor
timestamp: November 25, 2021, 10:12:33 pm
content: Quote from: BrianHG on November 25, 2021, 09:47:32 pmI got the probes to x1 to be able to measure beyond 50mV/div.I don't have a CMC in this circuit, please remember that this is the old circuit... CMC and grounding solution is on new circuit which is on route.you mean putting very big elec. cap on 12v input from the ac-dc power brick? since I cannot put that much capacitance on 3.3v or 5v output since switchers specify 200uF maximum capacitance as a must... I am about 20uF away from that on this board and about 200uF on new board.so the tests i should do for now includes this resistor from DC ground to my scope ground leads for both PSUs right?

author: BrianHG
author_rank: Super Contributor
timestamp: November 26, 2021, 12:33:27 am
content: Quote from: VEGETA on November 25, 2021, 10:12:33 pmYes on the resistor PSU tests.The elect cap should be on the 3.3v.Yes, I know you exceed the recommended switcher's rating. If you are afraid of oscillation due to a lemon value of cap, going to 4700uf or 10000uf cap should be too high to allow the switcher to inject odd oscillations into the 3.3v rail.

author: VEGETA
author_rank: Super Contributor
timestamp: November 30, 2021, 07:32:24 pm
content: Hellodone the resistor test for my psu, check it in pictures with names.Here are some comments on pictures:- odd behavior picture:this happened after testing several caps to get results for other pics, such as 220uF, 1000uF, and 2200uF. then I noticed the waveform is flat with periodic bump as you see. I hooked up the video output and saw the picture completely messed up!! please see it in detail. it blinks each half a second or so while the colors are messed up a lot... slow functionality too like some delay until it registers a button move. I really regret doing the cap thing now since it ruined my dreamcast for reasons I don't know! messed up screen picture is in 2nd post.

author: VEGETA
author_rank: Super Contributor
timestamp: November 30, 2021, 07:33:15 pm
content: here is the messed up screen.any way to know the issue or fix it?

author: VEGETA
author_rank: Super Contributor
timestamp: November 30, 2021, 09:24:25 pm
content: helloafter disassembling it and re-assembling it, it stopped turning on! it turns on for a brief moment then shuts off.. i measured about 86 ohms from 3.3v to gnd unlike 5v which is open load, so suspected something wrong.checked many components which deals with 3.3v, left pins, etc.. but still 85 ohms... to make it worse I destroyed a sharp 07vz1h regulator! even after this regulator is out, still 85 ohms.check pics:https://slow.pics/c/JOSrApgaEDIT: it now powers on completely with fan and so on, voltages are ok but there is no output picture. I measured voltages on caps and found the cap highlighted in picture to have 0v on its + side and about -0.5v on its negative side:https://slow.pics/c/PGsUaNuKEDIT 2: that sharp regulator takes 3.3v and outputs 2v according to this schematic:https://archive.org/details/Dreamcast_Schematics_Uwhat is going on? could it be that that regulator supplies power to output video?

author: T3sl4co1l
author_rank: Super Contributor
timestamp: November 30, 2021, 11:30:32 pm
content: Yeah, it's a good idea not to plug in capacitors randomly to powered circuitry.Toasted regulator? Ah, seems likely the large capacitor effectively shorted out the main supply, reversing the regulator, with more current than it can handle. Lucky it wasn't something much worse? Or maybe that's just the first thing of notice...Tim

author: VEGETA
author_rank: Super Contributor
timestamp: November 30, 2021, 11:45:56 pm
content: Quote from: T3sl4co1l on November 30, 2021, 11:30:32 pmmost of the times i shut the system off, then plugged the cap and turned it on. but yes did put caps while it was working, just not many times.I still don't understand what went wrong till now. the regulator made by sharp wasn't bad or at least I didn't verify it. I went along the board trying to disconnect all 3.3v related regulators and destroyed it by being a super saiyan in a wrong time and place.but even if without destroying it, the picture was distorted. but now it works and turns on but no picture at all... which makes me thing the video circuitry got the problem. don't know if it is the analog video or the gpu itself.that cap is showing reversed voltage which is very weird. it needs more investigation but now I ordered a new dreamcast locally which I learned to be more careful.

author: BrianHG
author_rank: Super Contributor
timestamp: December 01, 2021, 03:59:18 am
content: I so sorry to hear your dreamcast got damaged up. Like 'T3sl4co1l' and what I wrote in my original post:Quote from: BrianHG on November 25, 2021, 09:47:32 pmThe cap had to be secure and not attached/detached while powered on as it may appear as a short, or, a voltage surge if the cap had a charge.Quote from: VEGETA on November 30, 2021, 07:33:15 pmIt looks like a data bit in memory is stuck low.This is odd because corrupt memory usually means the CPU wouldn't be able to do anything at all.And yet your CPU is still working and executing code.When you say it may be in the video output section, it is rare that this could be the video DAC, but not impossible.Does anything else work?Is there audio?Were you able to replace the busted regulator?Looking at the schematics, can you probe IC 401, with your probe in 10x mode for the high frequency, and check the data line inputs to see if any are stuck as well as the outputs?Found cleaner scan of schematics here:https://console5.com/wiki/Dreamcast

author: VEGETA
author_rank: Super Contributor
timestamp: January 05, 2022, 04:04:55 pm
content: Hello,new boards have arrived, and looks like we nailed it perfectly this time!I probed using differential probing of 2 channels then math function as done previously, also using the same 12v regulator. Now on a new dreamcast which is working fine. no game used though, and has its gd drive in place while the previous one used a clone gdemu.Here are the details:- org: original PSU from SEGA.- mine: 2 pics, one measuring ripple only and one including noise spikes.- competitor: 2 pics, one for ripple only and one including noise spikes. this one similar to the one used before.Results:original: about 65-70mV p-p ripple with no noise spikes. I kinda expected better.mine: about 9mV p-p of ripple and about 31mV p-p noise spikes which are not a lot.competitor: around 20mV p-p ripple and about 45mV p-p noise spikes.please check the waveforms and tell me your opinion.I conclude that CMC + grounding enhanced the design significantly, it is now more than 2 times better than best competitor. certainly more than good enough as a high quality product. Stock PSU still excels more at grounding as seems from the yellow noise or maybe that it doesn't use any high frequency switching (fly-back) plus its own CMC made it better to suppress noise, or more clearly it doesn't make noise.Looking forward to your feedback!

author: T3sl4co1l
author_rank: Super Contributor
timestamp: January 05, 2022, 05:54:53 pm
content: Shrug, that's just output resistance. Well within limits it seems. What about the switching ripple, what's it look like around 1us/div?Tim

author: BrianHG
author_rank: Super Contributor
timestamp: January 05, 2022, 06:52:46 pm
content: Zoom into and trigger/capture the spikes.They are too high frequency and being mucked up by the slow sampling rate and 10ms/div speed.Your new supply seems immune to that 50hz buz in the signal.For the high frequency spikes, if they are there in the differential when zoomed in on the time base, then they are authentic.Because of their high frequency, strategically placed 1-10nf caps in the right place or strategically positioned ferrite bead should get rid of them. Then you will be pretty much on par with an analog supply.

author: VEGETA
author_rank: Super Contributor
timestamp: January 05, 2022, 07:37:56 pm
content: Quote from: T3sl4co1l on January 05, 2022, 05:54:53 pmI don't understand what you mean by just output resistance.I probed exactly like all previous times, literally the same. the psus are on the actual device and it is running. now gd-drive instead of gdemu. gonna try gdemu next time which will add a small loadQuotearen't the spikes fully visible hear? or you want the trigger level to be on them so that normal signal is not triggering?QuoteI will try that next week (tonight is just this) but I think I changed to different time bases and saw nothing hidden or special. same method for other supplies as well.Quoteadding a small 10nf ceramic on each rail is doable but where? the space is limited, and I think I have some small through hole ceramic caps in this range available right now... so I could use them in this current circuit without building a new one. next pcb should be a small production batch not a test one.Quotecan you kindly explain?so assuming this psu still the way it is here, is it good in your opinion? what specs should I write for it in its product page besides (high quality low noise PSU...)?

author: BrianHG
author_rank: Super Contributor
timestamp: January 05, 2022, 08:47:34 pm
content: Quote from: VEGETA on January 05, 2022, 07:37:56 pmThey are 1 pixel wide. What is their shape and frequency?Spikes seem to exist on both the GND and VCC channels, and with 1 pixel wide spikes, maybe you are seeing a sample on one input channel and not the opposite one due to the sample being missed as it is 1 pixel wide.As for analog power supply comparison, most switching supplies have a continuous ringing on their output when under load. Since you are not zoomed in, I don't see this interference problem. Though we still cannot also see perhaps an EMI coming out of your switcher. Most likely, you will need to run your probe in 10x mode with the scope time-base set to the sub uS range to see anything there as your new supply operates in the 2MHz range and if switching noise is getting through the output filter, that signal will have edges up in the 500-200ns range. An analog linear supply will not generate this type of noise.

author: T3sl4co1l
author_rank: Super Contributor
timestamp: January 05, 2022, 09:07:37 pm
content: Quote from: VEGETA on January 05, 2022, 07:37:56 pmMeasure load current. I think you will find it's pulsing up and down at the vertical refresh rate. (This will be a PAL or SECAM model, I expect?). Thus, the voltage is changing in relation to load current: output resistance.This has nothing to do with the converter's switching cycle, at some 100s of kHz.QuoteBeats me. I don't know your scope. Is it aliasing the spikes? Are they really spikes? Is it switching ripple? Ringing? Lots of things it could be. No way to tell from a 10,000m view.QuoteA linear supply only rectifies mains voltage, filters, and regulates it if applicable; they have no switching noise besides the diodes, and that's at mains frequency and harmonics so is easily handled by a regulator.There's nothing inherently impossible about a quiet SMPS, but they do take more effort to make quiet: you can't be lazy about layout, and may need shielding.Tim

author: VEGETA
author_rank: Super Contributor
timestamp: January 05, 2022, 09:28:37 pm
content: so I just hook it up as usual then zoom in to 200us or so range?I mean, what do you really want to see or verify? 2MHz switching frequency (exactly the same as previous design) is big enough not to be shown and therefore it didn't need big inductors, yet we used 4.7uH main inductors. It also has ferrite beads integrated inside the feedback loop itself as explained later.it is quite difficult to measure the current, i mean i can not break the circuit to insert the current measurement. and since there is nothing to see for current then maybe no need to do it.I just don't want to do more pcb revisions for now.I do report that the device works perfectly fine and image is very clear with no problems. 3.3v and 5v are spot on as value too.looking at the images above, how do you compare between the 3 PSUs?

author: VEGETA
author_rank: Super Contributor
timestamp: January 05, 2022, 11:36:55 pm
content: HelloI have done extensive tests as required and here are the pictures:https://slow.pics/c/tXFqHF3rplease notice picture's name under it, which signifies measurement parameters.I have added some capacitors directly at 3.3v rail output pin to gnd pin as indicated by pictures, values like 4.7n, 47n, 2x47n, 22p, and 10u elec, as well as 33u elec. It doesn't seem to have done a noticeable effect.what do you think?

author: T3sl4co1l
author_rank: Super Contributor
timestamp: January 06, 2022, 12:39:16 pm
content: Quote from: VEGETA on January 05, 2022, 09:28:37 pmWhy guessing? I gave a number earlier?~200us/div may show insight into control loop compensation, or the like. Not that you're doing a proper load step test, it's just whatever the console draws, which... who knows, it could be doing anything? Wouldn't it be nice to know what it's doing?QuoteI didn't say it was going to beeasyto measure -- or necessarily that you have to measure it at all, but if you're looking forcause and effect, y'know... wouldn't that be a good thing to know? Worth cutting a wire and inserting a probe, current shunt, sensor, whatever? Or testing with an independent load of known behavior?QuoteWell, on what basis should they be compared? Evidently they all work; is that sufficient? What things would your potential customers want to see before buying? What things can you test?If I were considering buying such a thing, I would want to know that it's followed good practices. Now, I don't expect to see a product description claim that; it should be safe to assume. Customers have that expectation, and they're relying on your good will that it does what it says, and doesn't blow up their hardware or whatever. It's a lot harder to test for good will, or not blowing up, but you can invest in preserving your reputation by doing electrical tests that exercise the extremes of electrical and other conditions, which should have a strong correlation with also not blowing up.For my part, I would do at least:- Supply voltage range test: make sure it meets or exceeds ratings, over the full input range;- Protection, if applicable: for example if the device has reverse polarity protection, check that it works down to the rated reversal. Similarly with transient or overvoltage protection, to the extent I need to/care to/can test it.- Load current range test: meets or exceeds ratings, while at supply min/nominal/max; characterize the current limit / foldback / hiccup / etc. behavior;- Load step test: output ripple voltage is within tolerance for typical load conditions e.g. 50% base, step to 100%, step back to 50% of rated output;- EMI/RFI emissions: set up the device in a testing jig, to measure RF emissions from input and output ports. This is particularly important for things connected to long wires/cables, AC mains, or low-noise systems. If it's just some internal part, maybe it doesn't matter; this isn't a required step for any particular module or subcircuit (like a DC-DC converter, say), but in that case, the things that do reach those paths (long cables etc.) should have their own filtering to deal with it. Or it can be dealt with in a case-by-case basis, perhaps the module is too noisy for the filtering in one particular system and does need to be improved, etc.I happen to have test jigs (or know how to make my own if needed) for that last one, so it's feasible for me; conversely, I don't happen to have the equipment (signal generators, RF amplifiers) to do RF immunity testing, or transients (EFT, surge, etc.). So for those, I follow good design practice, and hope that it works out. (Which, I have the benefit of calibrating that experience by testing commercial products in the lab; that would be hard for you to do on this project, unfortunately.)The next best thing, that you can do presently, for that item, is at least just looking at it on the oscilloscope. It has the frequency response required (well, some of it anyway). It doesn't read signals the way an EMI receiver does, but still, it's something. Even without a test jig, the fact that when you're clipped onto it, you're seeing tiny (~us) squiggles, is proof that something's going on in there. How many mV tall are those squiggles? Would it be enough to interfere with a nearby radio? (Mind, you can only test for radiointerference when you have A. a radio that operates at some frequency, and B. a radio station at that same frequency, to potentially be interfered with. Or at best you pick up the pilot tone or buzz of the SMPS, on a dead channel, not needing B. Trouble is, maybe you can pick up the AM and FM commercial broadcast bands; maybe you even have a SW receiver too. But beyond that? I mean, it's still something, but it's very spotty coverage, not representative of the full 1 to 200+ MHz range we expect an SMPS to produce.)And no matter how hard you squint at it, you're not going to tell what's going on at those frequencies, looking at a 50ms/div trace.Tim

author: BrianHG
author_rank: Super Contributor
timestamp: January 06, 2022, 04:40:43 pm
content: Those pulses are approximately 20ns wide, or in the 50MHz region. The right series ferrite/rf choke would prevent the propagation of that switcher EMI interference as we see the GND input trace is clean.

author: VEGETA
author_rank: Super Contributor
timestamp: January 06, 2022, 06:36:54 pm
content: well thanks for your feedback, here is what I think I should do:label it as "high quality low noise power supply replacement for dreamcast". it is of high quality for the job as it uses good parts and good design practice, went on many revisions..etc and low noise since it is noticeably less noisy than the best alternative (about x2 times) and a better than original PSU as well. I also tested it for long play hours and it went fine with very clean picture which is the ultimate purpose. not to mention that it does have a lot lower temperature than stock PSU, and it has 12v rail properly loaded in case of removing gd-drive.as of protection, this is a duty for the used 12v wall adapter not this device. this is the case for all designs as well. also short circuit protection the same. I could design a "pro" version of it later on which takes ac directly using recom or meanwell 12v power modules but this will be very expensive and not the scope of this board. such power modules have everything inside and all protections.I am interested into the potential issue inside the switchings... aren't they just the switcher switching itself? and since this was tested to work properly without problem we can assume it is not going to be one.I maybe can add one ferrite bead right before the output pin which is the same type used here... but isn't adding 10nf caps better? like adding them before and after the inductor, plus the ferrite bead, and at the load pin itself?I am open to do any change which is easy to implement in the upcoming 20 boards production batch, which won't do any problem... meaning if it didn't enhance the system, it won't break it. i believe adding ferrite bead and 10nf caps as mentioned won't make the circuit broken or unstable if it didn't enhance it.the project should be easy and specs are simple, it works and produces low noise and low ripple when using normal 12v power adapter. that is it for me... so that people can buy it knowing it is the best choice as replacement for the original one.

author: VEGETA
author_rank: Super Contributor
timestamp: January 09, 2022, 09:44:09 pm
content: hello,kindly check the attached picture, it has small changes which can be done without fearing of circuit getting broken.it is just replacing 47uf input filtering for each switcher with 1000uf, plus adding small 10nF in 3 places for extra filtering for higher speed ripple if necessary.I can relocate stuff to fit these easily, on expense of removing some silkscreen.i figured that ripple is coming from input side rather than the switchers themselves since they are about 2mhz while ripple is slower. so, having a significantly larger input cap (while keeping some 22uF ceramic input caps) should enhance the signal.right now i can modify the circuit i have to add these and test them next 1-2 days since i have a lot of 1000uf smd caps, it doesn't have a footprint for sure but can be installed using very short wires and so on.i just like to hear your opinion.EDIT: hmm i could replace 4.7uH inductor which is the input to the 2 switchers with 10uH one (not shown in this pic), also the other 4.7uH which is the filter of 12v output rail. i found one with same footprint. however, switchers inductors should still be 4.7uH

author: VEGETA
author_rank: Super Contributor
timestamp: January 10, 2022, 10:22:58 am
content: just a side note, i've found some small footprint 1uH inductors with high enough current.Would it benefit if I put one of 1uH L on the output of the rail, just before one 22uF ceramic and 47uF elec. cap? plus one at the input of each switcher to act as a small pi filter with either the currently installed 47uF or the suggested 1000uF?also, adding either 4.7uH or 10uH inductor right after the CMC and before the global 1000uF elec. cap?oh fk! i am fking redesigning it again despite it worked fine and delivered better results than the others!!! am I ill?

author: BrianHG
author_rank: Super Contributor
timestamp: January 10, 2022, 06:41:33 pm
content: Do not change you output circuit. You board is working fine. It is the 25-50MHz band switching pulses you want to filter out.For this, you do not want to add inductors to the middle of your circuit or even add caps. What you want is a series ferrite bead choke right at the output of your PCB before it feeds the Dreamcast. You want a ferrite bead with as low as possible impedance to make sue you do not loose any voltage or regulation at the output, plus, a ferrite which has a significant -db signal choking capability between 25-50MHz. This one component, I'm guessing 2 of them on the +3.3 & +5v out will prevent the migration of those tiny pulses from your PCB to the Dreamcast.The source 12v power supply would not be the generator of these spikes as they are too high in frequency/narrow to make it down the long power cable in tact as we see in your scope shot.

author: VEGETA
author_rank: Super Contributor
timestamp: January 10, 2022, 07:21:29 pm
content: So not even an extra 22uF ceramic cap at the output?The ferrite beads I am using is Würth Elektronik 7427922808, it is already there and inside the feedback loop itself (the feature of the switching IC). how does it compare here?from its datasheet I see it is about 8-10 ohms @ 100 MHz, but only 5 ohms at 50 mhz. it was recommended by the switcher datasheet itself.the other recommended ferrites are: BLE18PS080SN1 and 74279221100.which parameter in datasheet should I look for in ferrite beads to know the suitable part for 20-50 mhz attenuation? and what about my current one's capabilities?EDIT:I searched and found these alternatives:Z0603C280APWST -> very cheap (30% of the one used currently). about 28 ohms @ 100 MHz, estimated of 21~26 ohms from 20~50 Mhz.BLM18KG300TH1D -> very cheap as well, labelled as 30 ohms @ 100 Mhz. website shows 15-22 ohms from 20-50 mhz.FBMJ2125HS420-T -> probably cheapest. 42 ohms @ 100mhz. 32~38 ohms at 20-50mhz. is this the best out of these suggestions? however this is 0805 which requires some modifications to fit it... original one was 0603if these are accepted, can they replace the one already used inside switching regulator's loop? this will enhance the price and looks like it will also enhance performance.

author: T3sl4co1l
author_rank: Super Contributor
timestamp: January 10, 2022, 08:51:27 pm
content: None of these specify DC bias, so it's not obvious if they would be suitable.At such frequencies, layout is critical. It's very difficult to say offhand how much is present by inspection alone. Why do you refuse to measure it?Tim

author: VEGETA
author_rank: Super Contributor
timestamp: January 10, 2022, 09:43:19 pm
content: Quote from: T3sl4co1l on January 10, 2022, 08:51:27 pmcan you show me where is the dc bias in another one if you know?how can i measure it? didn't i take all measurements?

author: T3sl4co1l
author_rank: Super Contributor
timestamp: January 11, 2022, 04:18:19 am
content: Apologies, I had checked your last link after your last reply after it but it seems either it wasn't updated by then, or my cache didn't update, in any case I only saw the 50ms/div measurements.So, the thing about the ~10ns pulses. Do they show similar magnitude when probing ground to ground? Any ground, any connector? If so, it's more common mode than the differential mode you think it is. For which, differential filtering will accomplish nothing, and the question of ferrite bead is moot.At a guess, the input won't have much of this noise (at least when probed by itself), due to the CMC. The question is then, which connectors/grounds is the noise between, and should that be solved by cutting ground, rerouting traces, adding CMCs, etc.?Or it may still be differential, suggesting fairly poor performance of the inductors I think, as the layout isn't that bad. Maybe you just need better inductors, or another LC stage with a smaller value like 0.47uH then some 0.1uF's, say.Bias curves are shown in the datasheet, or mfg supplementary (characteristic) curves, if available. Most do not provide them. Laird is the most reliable, having bias curves on almost all beads in their catalog. Wurth sometimes does, as was in this case:https://www.mouser.com/datasheet/2/445/74279221100-1720641.pdfTim

author: VEGETA
author_rank: Super Contributor
timestamp: January 11, 2022, 06:35:57 am
content: so I should go and do the same probing but try to probe another ground points? like the negative of ch2 is on output ground pin while positive of ch2 is on other ground pins of the circuit?you can see all pictures here:https://slow.pics/c/tXFqHF3r> there is a 500ns/div picture and others, please re-check. name of each picture is under it.inductors are the maximum size for the switchers, 4.7uH. suggested inductors in datasheet are very very expensive.I can add an extra stage as suggested earlier, will be 1uH inductor + 22uF + the 47uF elec cap since it should be the final one before the connector. or add another ferrite bead just before the connector. if 22uF is not suitable, I have 1uF ceramic used elsewhere, so I can use it here. such components are very cheap and can be added easily. but why very small inductor and cap size for extra LC stage?I still want to think about making input filtering to the switchers a bit bigger... or add an inductor right after the main CMC, or making main inductor filter for the switchers input 10uH instead of 4.7uH...etc. what do you think? a better way is to remove 2 of 22uF ceramics and replace them with 47uF elec. this is half the price and better performance since input voltage is 12v and the 22uF 1206 ceramics will surely suffer from dc bias. then add another 47uF to be the total input filtering per 1 switcher is 3x 47uF elec + one 22uF ceramic + 10nF (bypass at pin). instead of 3x 22uF ceramics + 1x 47uF elec. + 10nF. how about thatwe already used a CMC at the input and it did great to suppress much of the earlier noise and it helped eliminate 50hz stuff. adding another one will be expensive unlike the extra LC stage.so maybe it can be like this: switcher -> 4.7uH (main L) -> 4x 22uF -> main ferrite bead -> 3x 22uF ->1uH (extra L) -> 1uF -> 47uF elec. -> 10nF (already exists). with an optional ferrite after this.still, what do you think about the suggested ferrite replacements? they are cheaper and still have more Z at frequencies.

author: VEGETA
author_rank: Super Contributor
timestamp: January 12, 2022, 04:35:54 pm
content: the funny thing is that TPS62913 is out of stock and will be in stock in September!!

author: VEGETA
author_rank: Super Contributor
timestamp: January 17, 2022, 06:59:56 am
content: I would like to point you to this image:https://i.slow.pics/31fiYciR.png(taken from all photos here:https://slow.pics/c/tXFqHF3r)it is 500nS time base, and shows about 2 MHz pulses of about 17 mV p-p. this is clearly the switcher's switching frequency which is about 2.2Mhz.hmm can we choose a ferrite bead which has a lot of impedance at 2 mhz to solve this?this one (https://www.digikey.com/en/products/detail/w%C3%BCrth-elektronik/78279221281/14669530) seems nice with lots of impedance but the dc bias makes it about 1 ohms @ 2 mhz frequency when current is about 3 amps. so it becomes useless?

author: BrianHG
author_rank: Super Contributor
timestamp: January 17, 2022, 09:45:29 am
content: Quote from: VEGETA on January 17, 2022, 06:59:56 amThose pulses are in the ~50MHz frequency range. They may be happening at a period of the switcher's 2.2MHz, but as you can see they are tiny single cycle ~50MHz oscillation happening twice every 500ns, a single pulse going up, and a single pulse going down.If it was a 2MHz signal, you would see a single fat sine wave going up and down, where each pulse would be a fat wide 250ns high and 250ns low. This is not what we are seeing. This is why choosing the right filter is important here and optimiziog your output filter for 2MHz might end up filtering nothing letting that higher 50MHz pulse go right through. You want a filter where the '50MHz' component will be something like 100 or more ohms series resistance so any 0.1uf output cap will divide that component by a factor of 100 or more while the lower frequencies like below 2MHz will be a short of 0.01 ohms or less.

author: VEGETA
author_rank: Super Contributor
timestamp: January 17, 2022, 05:25:14 pm
content: ok so adding 100nF cap can solve it? I will try that soon, I have some 0.1uf elec caps around

author: BrianHG
author_rank: Super Contributor
timestamp: January 17, 2022, 08:05:06 pm
content: Take a look at your capacitor impedance charts. You want to choose capacitors with the lowest impedance in the 20-50MHz range. This may be a smaller value than 100nf. You need the true specs from a cap company with true readings.The same goes for the series ferrite bead or inductor before that cap. You want as close to 0 ohm as possible, but, at 20-50Mhz, you want as high impedance as possible.

author: KubaSO
author_rank: Contributor
timestamp: January 17, 2022, 08:59:28 pm
content: For supply evaluation, I always add an AC-coupled noise amplifier on the board – say x20 or x50, and an active rectifier and active peak detector. That way it’s easy to see ripple on any oscilloscope, and measuring peak and average ripple/noise can be done with a multimeter. But those three circuit functions need to be also well designed and fairly broadband (say 100MHz bandwidth) – and their layout is critical too. So it’s a chicken and egg problem: you have to already know quite a bit to design all that. For ripple itself, you’ll do fine with a lower bandwidth amplifier, since otherwise the scope isn’t sensitive enough, so even 10MHz is better than nothing. That still calls for an op-amp with 100Mhz GBW, and you’ll need two stages of gain. And it that opamp is quite hot when idle, you know you got oscillation – then just compare the op amp’s supply current with the quiescent value in the datasheet. You’ll want current measurement shunt resistors installed on the PC board to avoid messing with multimeter’s ammeter series connection. Heck, that amplifier could be discrete, to save on cost. But without a scope it’ll be hard to make sure it all works. All amplifiers can oscillate and their DC readings taken with a multimeter will look great, but it’ll be misleading. And some wideband amplifiers just run hot by design – especially the older video amps.You’ve got many pointers from other replies. One thing I’d add: whatever “layout examples” the manufacturer provides don’t mean that you can just copy them and are guaranteed stuff will work. It still takes understanding of what the layout decisions mean and why they were made. Those are handy “sanity check” references for experienced engineers. For novices who can’t but copy without understanding, they are only mildly helpful.Furthermore, in switching supply design, the non-ideal properties of components do matter, and things like ceramic capacitor dielectric type and ESR and SRF (self resonant frequency) of any capacitor type do play an important role.And then, just looking at the size of that switcher chip: the inductor physically looks like it’s way too big. Those things usually scale together, so the physical size of the switcher chip and that of the surrounding passives go together at least roughly. Not always, but such big disparity is a red flag.

author: VEGETA
author_rank: Super Contributor
timestamp: January 18, 2022, 10:21:52 am
content: I didn't quite understand last point about capacitors ratings of impedance vs frequency. But know that I opted for caps from Lelon brand since they are good well known and available for JLCPCB, that is for elec. caps. for ceramics, I get what is available on LCSC and JLCPCB SMT service.However, for ferrite bead, I get it from Digikey\Mouser from well-known brands... I posted few suggestions which has quite good impedance at 20-50mhz which could replace the originally recommended by chip manufacturer.as for inductor size, it is 4.7uH and no way I can find one 2x2mm (size of the switcher). Recommended inductor is smaller than what I got for sure but physical small size isn't important to me, but price is. LCSC inductors are a lot cheaper than say Pulse branded ones and do the same. I got ones with greater ratings than required to eliminate any chance of margins.I didn't blindly follow the example layout but rather did my own using best practices. You can find pictures of it in previous replies, people here helped doing it.So to sum-up, here are some suggested solutions:1- keep all the same, and go for a 2nd ferrite bead using one of the suggested above after the final 47uF elec. cap. a bead which has good impedance at 20-50mhz as the parts I listed above.2- add another LC circuit comprised of 1uH inductor (small size) + 22uF caps as PI filter. meaning, split the output caps to be before and after the added L. ensure 47uF elec. cap to be the absolute final before the connector.3- same as 2 but also add another ferrite bead.4- same as 3 and 2, but add 10nF or 100nF caps next to big caps.note: i am ok for getting one nicely branded cap but it should be say 0805 so I can hand solder it. one extra BOM line won't ruin the entire design economy. Please check the inductor I chose too.which do you think should we go with? if not, please suggest a practical move i can use.Notice that I am fine with <9mV of total ripple but just wanted to filter out the high frequency noise spikes. I don't think it will affect the final output of the system but still should be solved if possible. this design is already x2 times better than all other solutions. also, better in terms of ripple than original one, but worse in noise... original one doesn't have any noise spikes at all.

author: VEGETA
author_rank: Super Contributor
timestamp: February 13, 2022, 07:37:06 am
content: Quote from: BrianHG on January 17, 2022, 08:05:06 pmI wanted to make a final revision (hopefully) so I am interested in your suggestion, which is after the final 47uF elec. cap... adding a series ferrite bead and a 100nF or so to ground.So I am trying to search for values similar to what you have explained, so can you help?I found thiscapandhereis its data. click characteristic graph -> frequency graph -> |Z|I found its lowest Z is at 25 MHz, but this is the resonance frequency right?what do you think?Also, here is another one which is 10nF: GCM155R71H103KA55D this one has 0.5-0.2ohms at 25-50mhz and its resonance frequency is about 90mhz.

author: VEGETA
author_rank: Super Contributor
timestamp: February 23, 2022, 11:15:10 am
content: I posted the question to TI support to see if they have a good recommendation, plus asked them about exceeding maximum output capacitance of 200uF.Looking forward to your comments on my previous reply.

author: Vovk_Z
author_rank: Super Contributor
timestamp: February 23, 2022, 03:04:05 pm
content: Quote from: VEGETA on February 23, 2022, 11:15:10 amI'm not sure simple increasing a capacitance at the output will help with noise or spikes. It doesn't work like that in real life. You just have to make some experiments with different types of caps of a low value (1-47 uF), consider playing with electrolytic caps of a general type with high ESR too.

author: T3sl4co1l
author_rank: Super Contributor
timestamp: February 23, 2022, 06:07:24 pm
content: And like I said. It might be common mode noise still. It is impossible to tell without a proper setup, free from conflating sources (from the power adapter, load, etc.), and preferably in a jig that gives standardized conditions (typically LISNs over ground plane).Tim

author: VEGETA
author_rank: Super Contributor
timestamp: February 23, 2022, 06:39:37 pm
content: Quote from: T3sl4co1l on February 23, 2022, 06:07:24 pmI do appreciate your pro tips and setup but I am not that advanced nor the product itself. I mean, we came a really long way to achieve this low noise level after much help... just one more issue remained. I will be very happy if we could attenuate it by any factor for now.TI chip will be in stock in May but my PCBway can get them now for 10$ per IC... so I can make one more prototype and 1 assembled board.

author: VEGETA
author_rank: Super Contributor
timestamp: March 20, 2022, 05:23:17 pm
content: Hello,I have been idling for a long time, I thought of some minor changes could be done to enhance the thing with little to no cost. I thought of changing the CMC to a better one, here are the candidates I searched for:https://www.digikey.com/en/products/detail/pulse-electronics-power/PA4339-102NLT/9659623-> 1.02k ohms @ 100MHz, about 600 @ 20mhz and 1000 @ 50 mhz. this is a massive upgrade of attenuation from previous one (DLW5BTM501SQ2).https://www.digikey.com/en/products/detail/tdk-corporation/LCV70-701-2PL-TL00/11682555-> 700 ohm @ 100 MHz. Upgrade from old one but the first candidate is better IMO. Unless Z @ freq. is not the only factor.https://www.digikey.com/en/products/detail/w%C3%BCrth-elektronik/744237152/14011659-> better than both but higher price.^ all this assuming 12v @ 3amps of absolute maximum, reality is less.original CMC was noticeably cheaper, these are easily 0.5~0.8$ more in price. So I thought of removing some inductors and caps here and there to save some cost, and put only one big main filter inductor instead of one per switcher. What do you think of that? so something like this:12v -> new CMC -> elec. caps (47uF x 2) -> big inductor (cheap one but big) -> 1000uF elec cap. then input to each switcher will get 2 or 3 47uF caps + 2 22uF ceramics. while the 12v output only has like 1 47uF since it is not really used much.or instead of one main filter cap I put one per regulator but leave the 12v without inductor?I thought of this due to the harmonics seen are mostly common-mode as many here agreed, plus getting more diff. inductor filtering should help.I am open to suggestions.EDIT:inductors selected for now:100uH:https://lcsc.com/product-detail/Power-Inductors_TAI-TECH-TMPC1206HP-101MG-D_C357256.html33uH:https://lcsc.com/product-detail/Power-Inductors_PROD-Tech-PSPMAA1040H-330M-ANP_C436575.html10uH:https://lcsc.com/product-detail/Power-Inductors_PSA-Prosperity-Dielectrics-MCS0630-100MPY1_C2937094.htmlso putting one 100uH as main filter, then just bulk caps before regulators seem good or putting 33uH per regulator without main L. what is best? the 33uH is slightly more expensive than 4.7uH one! still gonna need a 4.7uH for the switcher itself as indicated by datasheet.

author: VEGETA
author_rank: Super Contributor
timestamp: November 13, 2022, 12:44:27 am
content: Hello,boards arrived, tested and it works perfectly fine as intended except for one thing.Well, ripple for 3.3v is about 5mv p-p which is awesome! you can add the noise sparks and it become less than 10mv p-p. I consider this a win!however it is not the same for 5v rail, which can go to 40mv p-p sometimes!I figured it could be due to layout, therefore I attached the layout pics...any suggestions??I will make another board for more testing, which originally was to test putting 3 vias for routing the 5v signal as seen in attached image but now I need to see what to do really.I highly appreciate your suggestions

author: VEGETA
author_rank: Super Contributor
timestamp: November 13, 2022, 06:41:44 am
content: here are the problems which I think might have caused this bad 5v rail despite 3.3v is perfect:1- long travel of 5v signal from first stage filtering (C9 and others) to ferrite bead FB3:as mentioned, in manufactured design the signal goes under 3.3v signal by only 1 via not 3... I made them 3 vias later on.however, 3.3v signal is very short and direct as seen.TI rep engineer didn't like placement of the ferrites and their signals being under one another, basically that whole area. they called it "cross talk" and "overlap" due to high frequency resonance of the ferrite beads.what do you think?2- the 5v rail filters are near the 12v rail which is minimally filtered:not so much there but still listed this as a possibility. the 12v rail signal is at the very right of the board but somehow near the 5v filters.I will post waveforms soon but trust me that 3.3v total ripple noise figure is about 3-10mv p-p which i assume the best one can get from such buck designs.my possible solution which I started to accept is to make the board 70mm length x 50mm width instead of 50x50. the 20mm of length will help me re-distribute the ferrite beads and final filter caps to make connections to 1st stage extremely short and direct + very far from each other. so no cross talk or anything to be feared. also, will make me shift the entire thing to the left side which makes everything very far from 12v signal lineis my analysis good?what do you think?I was very happy for 3.3v rail results but got disappointed for 5v ones... really thought i was ready for production...! very hyped! now more testing boards and time has to be consumed but I ask all these questions to make sure the next test board is the final one.best regards

author: T3sl4co1l
author_rank: Super Contributor
timestamp: November 13, 2022, 06:58:47 am
content: Possibly this is a candidate for a slotted ground,Pink arcs: switching currents circulate under the regulator. This is mostly local, but some leaks out into the surrounding ground plane -- no conductor is ideal.Pink 'U': a slot here would prevent currents from flowing into the connector and filter area.Downside: the plane suddenly stopping here, means whatever current would've been carried by it, is instead wide open and exposed in the slot. This can make induction worse, for example. (Keep traces at least a board thickness away from the slot.) Maybe there's more voltage across the slot, than there was across the plane before. This could increase common mode noise (even given the input CMC).The extra 12V trace would be spanning across this slot, carrying 100% of the voltage on one side of the slot, across. It must be filtered locally, with an inductor to absorb that (AC) voltage drop, and a capacitor to firmly  ground it again.To explain further: the pink arcs represent current flowing under the regulator, at least very vaguely. Normally, that current is "shorted" out (no short is ideal, but copper is nearer to a short than say air is), so the voltage drop is small, and confined locally (read: dropping inversely with distance from the source, or probably faster than that, up to an exponential drop with distance). With the slot, the voltage drop is not shorted out, but left hanging. Which puts some voltage on one side of the slot, that isn't present on the other. Hence, common mode voltage appears between the two sides.But the best solution is to optimize out all the extraneous capacitors (I think you will find you get the same noise level with a fraction as many), place the regulator off to the side or in a corner where its currents can be better localized (using the natural board edge as a slot, as it were, but more to the point, also routing in/out from just one side of the region), and joining the connectors as well as possible (solid ground plane between them) and filtering local to them. Such a layout will take more blank PCB space for noise separation, which will be obtained by optimizing the filter components.Tim

author: VEGETA
author_rank: Super Contributor
timestamp: November 13, 2022, 07:29:19 am
content: I didn't really understand all that you said but I kinda understood that "U" that you put made a slotted ground meaning 2 ground plains separated which prevents currents from circulating properly which forces them to travel near or under the 5v rail signal (= along the slot).however, the arcs you put are not an issue IMO because most of them are feedback resistors network and one for some internal regulator cap... all grounded properly as seen while switching currents should come only from one pin per rail and as seen coupled to ground with multiple vias. how can this be an issue?there cannot be any modification to the 12v long trace since this is how the board and product shape is. assume we got the ground plain to be properly done, will this trace do any harm without putting an extra inductor to it? I can put caps though.I'd like to remind you that the bottom layer is all ground with minimal traces so i think even if the slot exist on top layer, the bottom ground should be there. or am I wrong?I have followed datasheet and rep engineer layout guidance for the regulator, besides the issues i spoke of. I don't know what caps you speak of, do you mean first or 2nd stage filtering?my next plan is to make length 70mm and change the layout as drawn in attached image.this way there will be no ground slots or disconnections but rather very short and direct connections for the rails with 0 cross between them as they will be very far.is this what you meant?note that the capacitance are sized according to design and datasheet calculations and so on, don't really recall exactly but be sure they are correct value.what do you think?

author: T3sl4co1l
author_rank: Super Contributor
timestamp: November 13, 2022, 09:17:45 am
content: Quote from: VEGETA on November 13, 2022, 07:29:19 amNot really two. Different regions of the same. The pour will still be solid around the left (where the 'U' does not extend).QuoteYou "don't really understand", yet you deny the possibility? (Namely, that currents flow over an extended range, a fuzzy, broad path, not a straight line.)Wait, do you think current follows the "path of least resistance"? As in, the infinitesimal narrowest and shortest possible path between two points? Fucking hell that phrase is so harmful. It should not be repeated, it so easily leads to such conclusions. I wish people would expunge the phrase from history itself!Needless to say, current does not follow such a foolish path. It's a field, it spreads out along conductors, particularly between their facing sides (at AC).Current flow in the area has little to do with which exact components are there. I don't care about the feedback resistors. They're irrelevant to this flow. The primary switching loop is between the chip and the bypass caps (above it). Currents can nonetheless extend down even below the chip. It is my guess that this is the effect at work here.There are other tests that could be done to confirm this, but I'm remembering now, it's training cats to pull teeth to get you to test anything the least bit confusing... so, nevermind.Quote...All layers...As in, you could literally saw through the board, and maybe actually demonstrate exactly this with the PCB you have. I might not recommend that, for a variety of reasons, but from such a process, that's where the copper would be (and wouldn't). Removing copper on all layers, and leaving PCB material (FR4), is fine there.But if you're going to the trouble of a new board, I would again suggest a better layout emphasizing the grounding between connectors.QuoteReps don't know anything, it's blind luck if they are helpful at all with EMC issues.More exactly, they aren't particularly different, as a class, from any other EEs. Among which, EMC knowledge is rather spotty at best, and full of partial or mis-conceptions.QuoteI can't tell what components are supposed to be here. I guess the one connector is shown. Where are the others?Tim

author: VEGETA
author_rank: Super Contributor
timestamp: November 13, 2022, 10:00:15 am
content: Quoteit is that I understood you meant something related to feedback resistors since arcs were on them... now i know you only meant switching node currents from switcher to inductor. this I agree with you on it for sure.QuoteI know this famous line is not really that straightforward. I saw many videos on return path current and so on and how to optimize layout for it.Quotethis is good and practical to do, can you tell which connectors exactly? I can start tonight especially if I extend the length of the board by 20mm which will make really nice space to work.Quotethis was my thought as well but at least I wanted to involve someone to take a look at my layout. she did emphasize on the "cross talk" between the two rails due to overlap of the ferrites as i mentioned above. do you think it is an important issue?Quotehmm i guess I put arrows to tell which is which. it is a mere rough drawing... for example that half-T shape is for first stage capacitors, I draw it like this since it is the same way I layed them out if you return to the layout picture. the bold line indicates power signal path... now it is straight and short with no cutting of any ground or making slots (to my knowledge).FB is ferrite bead, 2nd stage is for 2nd stage filtering caps which originally were at the bottom left of the design... now in this suggested drawing they are spaced well to ensure no cross talk.. etc.any suggestions?QuoteI have owon isolated usb scope and nothing more.i was thinking to make some tests like putting extra elec. caps, or remove the 12v rail trace (scratch it from its origin) so that I see if it is the one affecting the 5v rail... also thought of removing 3.3v rail ferrite bead to make only 5v rail exist to see if ferrites affect each other... hmm also maybe take scope measurements at the end of stage 1 filtering caps for both rails to confirm that the problem happens in later stages as i suspected, namely the long 5v trace from 5v first stage filters to 5v ferrite bead.. the one which made the slot to begin with.I am open to suggestions... to make sure the new test board is finally the last revision. and always thanks for your continuous support.EDIT: I made another rough drawing for the suggested new layout. sorry right now in work i don't have my laptop to do proper kicad layout.

author: VEGETA
author_rank: Super Contributor
timestamp: November 13, 2022, 05:49:56 pm
content: I've been thinking if instead of the 5 2nd stage 10uF ceramics... I put 4 ceramics the same + 1 22uF elec. cap + 1uH inductor to further smooth it out. is it better? ofc, using the better layout.so it becomes:1st stage caps -> the ferrite bead -> 2x 10uF ceramics -> 1uH L -> 1x 10uF ceramic + 1x 22uF elec. cap near the output pin.for your opinion.

author: VEGETA
author_rank: Super Contributor
timestamp: November 13, 2022, 08:35:03 pm
content: I have done extensive measurements as seen here:https://slow.pics/c/NlypkqhLeach picture has its own title so you can know what it is.I noticed it delivers 25mv p-p at full load for 3.3v which is, unfortunately, similar to another cheaper PSU on the market... so it would not make sense to make this one. I wonder why really... that psu is very basic without filtering at all just 33uH + 100uF or so at the output of a generic buck regulator. previously I said 3.3v delivers 5mv but that was at very light load.one thing I noticed with this design is that signal before inductor is better than after 33uH inductor, which is weird really. it is supposed to be better and smoother.also it gets worse at the switcher input pins themselves, which is after the ferrite beads and some filter caps.so assume i removed the 2 input ferrite beads and the inductor, then tested it... do you expect better result overall? since input noise is a critical figure and main cause for output noise level. but most importantly i wanted to understand why this happened in the first place.for your kind help, I am a bit frustrated after all that huge effort.Notice that this design uses TPS54394 instead of the TPS62913 initially used with first version of this circuit.

author: T3sl4co1l
author_rank: Super Contributor
timestamp: November 13, 2022, 09:03:09 pm
content: Quote from: VEGETA on November 13, 2022, 10:00:15 amAh, OK.QuoteAny connectors with wires.Which... is what connectors are usually for.But more particularly, connectors with grounds connecting to other things. Outside environment. Floating fan connections, say, probably not so much, but input and output, especially yes.QuoteExternal field of ferrite beads is small.Beads per se, are probably not what you want here anyway (they saturate under DC bias), but ones that big are probably okay. A regular inductor like 1uH or so would be more compact.Coupling between the beads is irrelevant; what matters is their absolute impedance, and some coupling between those impedances makes no difference. Well, if it was like 50%+ coupling, that'd be weird and probably bad, but that's not going to happen on board even with unshielded spool style inductors.Coupling between beads and switching inductors, more important. I'd keep at least one inductor width between the inductor and the filter ones. Which is a fine place to put capacitors.Like, this would be feasible:All the switching currents cluster tightly around the regulator, at great distance to the connectors; probably the slot is still better to use, and that keeps current away from the between-connectors path. Think in terms of a 'T' section, with the top of the 'T' being the path between connectors, and the regulator being placed on the stem. One side of the 'T' just happens to be bent around (towards the bottom, with the long connector), but topologically that makes no difference.QuoteOh, so like as-is, but in a more vertical section. Yeah, that avoids the slot for example. It still puts the regulator between connectors though.Quote from: VEGETA on November 13, 2022, 08:35:03 pm"Extensive" yeah but they're all at uselessly large scale (10ms+) so I don't have a clue what the actual EMI is like. And you didn't take a common mode measurement (between connector grounds, or ground and oscilloscope) so it's impossible to tell how much the CMC is doing, or how much DM or other filtering is really needed.Unless those have been added, I haven't checked since last time.Tim

author: VEGETA
author_rank: Super Contributor
timestamp: November 13, 2022, 09:46:38 pm
content: Quotehere i have that bottom right connector which is board-to-board connector. nothing else, besides the one in left side which is just the 5v rail as an extra connector for modding.what is my mistake here and how you suggest i fix it? does it have to do with bottom right connector having bad ground path to the regulator ic?____your suggested layout might not work due to the regulator IC itself having the 2 output stages on opposite sides, please check it up: TPS54394.so to sum up your suggestion, you want me to keep L and its first stage caps near the IC which is already done... however, you want me to move the 2nd stage (starting with bead) away from the main inductor... as far as possible so that no field or coupling happens... correct?? hmm I think the beads and 2nd stage are kinda far from main L... but do you mean that L and first stage itself are close to the output connector itself??are you sure 12v trace won't cause problems despite traveling all that distance under the filtered clean rails? also the 3.3v and 5v themselves, is it ok to travel that long?btw here are pics for the actual board:https://imgur.com/a/6ANuRwu< now you see everything.and here are the key components:common-mode choke: PA4339.132NLTferrite beads: Fair-Rite 2773021447main filter inductor: inductor_MCS0630-4R7MN2_7.3x6.6 (4.7uH from LCSC since the ones in datasheet and eval board are expensive)33uH inductor: LCSC C182163now for the slot, it kinda makes sense. i can just make a no copper zone in kicad. but we still need to see how the switch ic to be placed since as i said its inputs are from both sides not like you drew it. the slot you suggested forces the current not to go from switcher ic to the connector.do you think I need to get the eval board (https://www.ti.com/tool/TPS54394EVM-057) and test its actual performance? or make another version myself with your guidance? I saw the eval board give about 15mv p-p which is still not 10mv i want.since the main L is our biggest problem, they have2.2uHand I havethis 4.7uH. is mine that much worse?actually if this is the main cause, I can invest in getting a really nice coilcraft\tdk\pulse-electronics\etc.. inductor and shave off some unnecessary stuff like maybe the input 33uH inductor and the 2 input ferrites... this could be kinda financially ok if it boosts performance.___as for measurements, kindly tell me what to measure and at which conditions and I will do them tomorrow.

author: Mechatrommer
author_rank: Super Contributor
timestamp: November 14, 2022, 07:28:36 am
content: Quote from: VEGETA on November 14, 2022, 05:16:16 amread jim william's app note, tektronix probe primer abc etc on how to deal with low level noise measurement. use 1x probe, short cable etc is key.. as jim said, the best probe is no probe.. there is no such thing as to cancel noise of passive probe, you probably started with unshielded, hence crappy passive probe in 1st place, solution is get decent brand probe. I saw earlier suggestion to use diff probe, i dont know how that helps as diff probe is such noisier in itself. And with cmrr and phase mismatch issue, you probably get junk reading, as i believe you already figured out. Ac coupled 1x probe to dso is the key when 10x passive probe is not reading it anymore, no need fancy or active probe.. btw I'm also working on similar smps noise issue and carefull pcb layout, except mine is variable output for preregulation purpose. I'm getting there, after changing inductor value, i get 40 to 60mVpp on linear output during switching. I'm spinning another pcb version with more carefull layout hopefully to get better noise performance.. i have this hypothesis of 'the rain of noise bandwidth' where each bw will take different path from hi freq returning along signal path (least reactance) to low to dc freq returning in straight path (least resistance) or rain of 'coupling' or 'crosstalk', electromagnet 101.. when current move in circle, em induced and hence current on the other intersecting tracks... gnd plane is a 'circuit', not a 'plane' as we might have think. if you can avoid this 'rain in the return paths' in pcb layout, then its better, if not, i think i need to provide umbrella, ie slot(s) in gnd plane to steer away this rain of noise.. but care not to run signal or power on top of this slot.. you can google rules on slot in gnd plane. Ymmv.

author: VEGETA
author_rank: Super Contributor
timestamp: November 14, 2022, 08:23:18 am
content: Quote from: Mechatrommer on November 14, 2022, 07:28:36 amI think my Owon VDS1022I came with these along the probes themselves:I mean the spring ground item (don't recall its proper name).I guess this is the best I have right?in my design I got final 3.3v output of about 25 mv p-p ripple which is similar to another cheap design, which frustrated me since I wanted to do better... to reach <10 mv p-p. the 5v rail is worse, it is +30 mv p-p with lots of noise rather than ripple.weird thing is that the other cheaper design showed similar behavior of 5v rail being noisier while 3.3v rail just ripple.the PSU is for Dreamcast and the main power is for 3.3v rail (2.5~3 amps) while 5v rail not so much (maybe < 0.5 amp).what do you suggest for routing and other optimizations?

author: Mechatrommer
author_rank: Super Contributor
timestamp: November 14, 2022, 08:57:11 am
content: Quote from: VEGETA on November 14, 2022, 08:23:18 amyes thats your best at cheapest cost and easiest quick way. probe very close to output node and ground plane. herehttps://www.analog.com/media/en/technical-documentation/application-notes/an101f.pdf(read carefully Appendix C) jim is using single ended pre-amplifier to make measurement, so you may want to build your own or find equivalent of HP461A if you are really serious looking into uV range.Quote from: VEGETA on November 14, 2022, 08:23:18 ami'm also learning and its hard to see whats on your pcb... i may give you useless advice anyway, so imho its not worth it to act like clever guy. imho you have to work yourself based on advices you received so far.. but i wonder why you want to still fight if its like an impossible battle? its like large promising market for Dreamcast PSU? many people in your place play Dreamcast? that you have to nail down other competitors in market? how about i give you advice, stop playing Dreamcast?or does it need so low noise to work properly? i say thats a bad design for game console. or is it only yourself that want to challenge yourself? 30mVpp for smps is good output already imho. ymmv cheers.

author: VEGETA
author_rank: Super Contributor
timestamp: November 14, 2022, 09:05:36 am
content: QuoteI will try to use it soon and write feedback here.QuoteI am into retro gaming and it has nice community of people. yes, 30mv is fantastic but I still want to do better. the market for alternative PSUs exist but I wanted to make one that beats the others... if so, people will buy it for sure. Plus, the challenging thing you spoke about.the lower the noise the better for retro consoles since it is all about analog video which gets affected by noise... 30mv or so is not bad really but as i said, i wanted better.actually, all i wanted is to have better noise figure than others. that is all. later on i will create a mains powered psu to act as full replacement of the original psu... this will be based on this design but have something like meanwell ac-dc module as input.i am fine with your advise since i am not an expert. i have done several revisions already but i cannot beat the 20-30 mv limit!

author: VEGETA
author_rank: Super Contributor
timestamp: November 14, 2022, 10:54:51 pm
content: Hello,I have used the spring and isolated the scope and stuff from other mains chargers as much as possible, here are the images:https://slow.pics/c/0H7FqG0jall images are for my design except for when labelled "competitor".any more images at certain time bases you need me to take?^All this for the newer design using TPS54394 dual buck.However, as you know, I started this project using TPS62913 low noise buck regulator, I have dug it out and tested it as well... here are the pics for it + schematic attached:https://slow.pics/c/gQsPrODG(layout picture available too, 3.3v rail is the first pin from the left of that 6-pin connector).I switched from that IC due to price + it is almost always out of stock.we used DLW5BTM501SQ2L common-mode choke, then we wanted to search for one which is better at attenuating 20-50 mhz noise... then i found PA4339.132NLT but I never used it in that "older" design due to out of stock IC but rather in the new design.weirdly enough, the 5v rail of the older design is very clean, much better than newer design. but both suffer from 3.3v...how do you think i can improve the new design taking all these stuff into consideration?

author: jonpaul
author_rank: Super Contributor
timestamp: November 14, 2022, 11:51:20 pm
content: bonjour à tousSeems a classic case of poor measurement and probing techniqueSuggest use BNC >>RG174/U coax, >> 450 Ohm series R make Zo probe with very short shield to plane loop. Dump the Chinese clone probes.Check à good text on high frequency PCB layout and SMPS design and theory.Do not depend on the TI application notés as gospelJust the ramblings of an old retired EEj

author: T3sl4co1l
author_rank: Super Contributor
timestamp: November 15, 2022, 05:23:00 am
content: Take a picture of how and where you're probing.Take waveforms at,at most,5µs/div. Zoom in during the load pulses. I don't care what the load is doing on the order of 100s of Hz. Your power supply should be (and is!) at least good enough not to have the least care what's going on at such boring frequencies!Preferably, replace the Dreamcast withan actual load resistor,so you aren't seeing those damn load cycles as it's running. What is it running, anyway? Home screen? Is a game loaded? Is it rendering a lot or just a little? Who knows. The load is probably inconsistent and not reproducible. Get it out of the lab!Build your own step load generator to do that in a better controlled fashion.Or, if this is actually what you are concerned with -- low frequency or DC response of the supply, not the filtering you've been concerned with for the last, this thread -- then realize that that is where you must focus your attention, (almost) no amount of capacitors will affect this aspect of the response!Label your figures properly:"3.3v competitor with spring" -- with spring where? How is it wired, where is it probed? Who is the competitor, how did they lay out their circuit, what other relevant points should I draw from this, etc.?"both channels loose with spring math" -- loose how? Floating in space? Are the two probes' springs tied together or loose (open) as well? What math? I don't see a function anywhere on screen!"both channels with springs-ch1 for 3.3v and ch2 on ground" -- with math I guess, but again, what function? Add? Subtract? ch2 is ground but how? Is there significance to the distance or direction between probe and spring contacts, how could I know?Mind, I enunciate these comments not to offend, but to emphasize and reiterate the importance of clarity, precision, and thinking critically about what you are doing, what you are saying. Think about what someone else may read your comments as -- or what they won't know (because it's been omitted), that they should!Tim

author: Mechatrommer
author_rank: Super Contributor
timestamp: November 15, 2022, 05:57:55 am
content: If the 100hz is due to digital load its subjected to, then you have finite (non zero) impedance output psu... if its under dummy or passive resistor load i'll check for gnd loop/common mode error in probing. Gnd spring must be near power output, and then put probe tip on the same gnd spot where your spring lands, if you can still read the boring 100hz then you have gnd loop/common mode error in probing, else i think you have heavy current flow switching somewhere. In my psu i got 0.5Vpp after bypassing many high impedance nodes, it was 5Vpp spikes before! The loop controller went heywire.. and then i changed to significantly larger inductor for smps than whats i installed earlier ie recommended by 34063 app, then spikes went down to 60mVpp, it was current ripple! thats what my critical thinking tells me. The easiest imho is to sim the inductor switching and look at current ripple, not easy to do on real pcb..

author: VEGETA
author_rank: Super Contributor
timestamp: November 15, 2022, 06:19:11 am
content: QuoteI will take those picture tonight. but i was probing the 6-pin connector with a spring grounded probe, not alligator ground. so path is very short.Quoteso, time base in the nano seconds to 10us is the range you want? ok.QuoteI wait until it loads the main screen or main screen of a game, then took those measurements so they are consistent. I have some load resistors (50W) but since the final application is DC I thought using it directly is better.QuoteI want to buy some more advanced gear such as electronic load and so on in the future. However, as mentioned, right now the application of running this PSU on DC is what I want.Quotewith spring = spring grounded not alligator clip ground. probed the 3.3v or 5v (depends on label) and gnd pins of the 6-pin connector. 3.3v pin is pin 1 from the left, 5v is pin 2, pin3 to pin5 are ground, pin 6 is 12v.competitor isthis.12v power brick used with all isthis.Quoteloose means they are not connected to anything, just on the bench and not connected to each other. math is channel 1 - channel 2.Quotemath here is channel 1 - channel 2.channel 2 probe to ground and ground to ground via spring ground. so this is a differential measurement. all of this is probing the 6-pin connector. shortest ever distance between all those measurement points.QuoteI told you my main goal for this device, it is to have the total noise and ripple figure to be < 10 mv p-p.taking pictures of each frequency is fine by me too since it may help reduce the ripple.so judging by these figures, how do you analyze what type of filtering required? I mean, it is obvious that adding bulk caps does not work as I tried putting some 220, 1000, etc elec. caps at the final load pins (6-pin connector) for 3.3v but had no effect. I also tried adding another 22uF ceramic but also didn't help.so this leaves us with what conclusion?I mean that ripple is about 50-60 hz or so... I have put CMC filter according to our mutual decision back in the mid of this thread. shouldn't bulk elec. cap reduce such low frequency ripple?I do have another power brick but it is noisier, also a DIY bench switch mode psu that I built myself as other alternatives. the final product must be used with a 12v power brick so I picked the current one I linked above since it is better than the crappy noisy one. anyone who uses such a device will have a similar brick.the point of CMC and input filters is to eliminate the ripple and noise generated by 12v power bricks as much as possible to have clean input to the switcher. however, as mentioned previously, the 33uH inductor and the following ferrites have increased amount of noise!I made 2 units assembled of this design, i can for testing purposes, remove the 33uH inductor and the following input beads and just use the input bulk caps as main filtering caps, then see how it affects the overall system. but i am interested to know why this happened... especially that 33uH supposed to filter low frequency ripple.what do you suggest?best regards and always thanks for helping.

author: VEGETA
author_rank: Super Contributor
timestamp: November 15, 2022, 07:17:46 am
content: Quote from: Mechatrommer on November 15, 2022, 05:57:55 amwell, I also suspect it is due to high current ripple switching but I am already using 4.7uH inductor which is on the high side + using 7x 10uF ceramics X7R which are also the maximum.I started to suspect that choosing Chinese inductor + ceramic caps can be the issue due to, well, being not so good.datasheet says this:Quotemy inductor is:https://www.lcsc.com/product-detail/Inductors-SMD_PSA-Prosperity-Dielectrics-MCS0630-4R7MN2_C385253.htmlit has dc resistance of 37 to 40 mOhms, rated current is 5.5 amps which is way more than needed, saturation current is about 7 amps. and it is 4.7uH.their suggesteddatasheet inductor is CLF7045-2R2N -> 14 mOhm, 5.5 amps, 2.2uH.evaluation board inductor is SPM6530T-2R2M -> 19 mOhm resistance, 8.4 amps. but this one is 2.2uH.one thing to notice is their inductors are of lower dc resistance. my initial thoughts were that this can cause more heat. but can this really affect ripple performance?my caps areCL31B106KAHNNNE-> 10uF X7R, ESR shownhere. lowest is about 4mOhms at <1Mhz, at 700 khz it is about 4 mOhms... graph is just a picture, you can't check the actual data.datasheet caps are C3216X5R0J226M which datasheet says 2mOhm ESR. atproduct pageand datasheet I couldn't find such info. there is though a graph showing ESR, lowest is about 3.16mOhms at 525khz. for this 700 khz switcher it would be 3.3 mohms,evaluation board caps areGRM31CR70J226KE19having about 3mOhms at 700 khz.hmm not so far away but still 1 mohm difference... is it worth it to get higher quality caps + inductors to enhance ripple noise performance? then other cheaper caps can be used in 2nd stage filtering + input filtering.

author: Mechatrommer
author_rank: Super Contributor
timestamp: November 15, 2022, 09:08:13 am
content: Yeah order from digikey dont buy from china, punch in the spec and you will get legit stock. in the end you'll have better performing but more expensive productwhy do you care about brand? Inductor is an inductance you can even make your own.. your 1mVpp speced converter ic will take care of volt drop in control loop due to mOhm resistance, no? btw i got my stock from lcsc and its in china, why do i care? What i know is its inductance because thats what affects di/dt.. and they are cheap.. cost is another factor to fight for.. no? i'll say.. experiment with larger inductance, recoil your own if you have tocheers.

author: T3sl4co1l
author_rank: Super Contributor
timestamp: November 15, 2022, 09:32:12 am
content: Quote from: VEGETA on November 15, 2022, 06:19:11 amHow can you say your application is "DC" if your waveform is not DC? Clearly something is wrong with your assumptions! Be critical -- always check your assumptions!QuoteNo need to buy, there's no end of threads here alone from people building electronic loads, or step generators. The most basic case of the latter is a 555 timer into a MOSFET and load resistor. It's quite far from rocket science!It seems, then, your primary failure is not testing at DC. Your load is not DC and you have been, apparently, unaware of this. Cure this discrepancy, and I think you will find your noise is in the single mV. And that it will be predominantly high frequencies (actual ripple that your filters are handling).The remainder, then, will be due to dynamic loading, and this in turn is limited by loop gain of the regulator, among other things. Apparently it's not very high, or there's enough DC resistance between the feedback point and load to produce your observations.What importance is gain? Well, if the regulator is an error amp, which senses some difference between ideal (setpoint) and actual, which is then multiplied by a gain factor, then wouldn't a higher gain produce a lower error (input difference) -- it's more sensitive to differences in the input? Exactly! An excellent point to introduce control theory, at least at its most basic. Further reading recommended!QuoteHmm, hard to say how noisy it is. Any random thing off Amazon is about meaningless with respect to EMC. They have the regulatory logos but that doesn't mean they actually tested to them, they could be improperly applied. They don't appear to have any information to support that (but that's not surprising, who goes on Amazon looking for EMC certificates anyway).At least the measurements so far don't seem to be grossly out of order, so it's probably not too bad. But without the paperwork, who knows.QuoteThe waveform is clearly not mains ripple (not sinusoidal), and you shouldn't expect such a waveform from an SMPS anyway (if it has 60/120Hz ripple, it is likely a fraction of overall output). This is easily verified by looking at the input voltage, which likely is not varying much.It is mere coincidence that your load draws current on a similar schedule. See the earlier point about poorly defined loads? If it's confusing you, making you think mains when it's in fact completely unrelated? That'd be a bit of a problem, right!? Isolate and identify!Namely, NTSC, and PAL 60Hz, run at 60Hz, so it makes sense that the graphics operations of a console have a similar heartbeat. Game loop calculations are typically done on the same schedule, or perhaps every other frame (30 FPS) depending.Tim

author: VEGETA
author_rank: Super Contributor
timestamp: November 15, 2022, 09:40:49 am
content: Quote from: Mechatrommer on November 15, 2022, 09:08:13 amso you aid the idea of getting better ceramic caps?however, for inductance you think they don't affect ripple performance by being lower resistance, correct?I noticed something I have done which may have an effect, which is that I didn't put much ceramic caps on the input of the switcher IC.I only put 1x 10uF cap with another smaller one, plus the 220uF bulk cap... according to some readings including this:https://www.ti.com/lit/an/slta055/slta055.pdfi should have put multiples of that ceramic cap to tame down the input ripple which will further enhance the system's final ripple value which is my goal.what do you think?

author: VEGETA
author_rank: Super Contributor
timestamp: November 15, 2022, 10:30:41 am
content: Quoteall my waveforms and testing were on the dreamcast, i never said otherwise. however when you said i should get elec. load to step load testing, i then mentioned that i have a 50w load resistor that i can use.Quoteactually, i saw these that i think are fine for my needs:https://www.amazon.com/Electronic-Battery-Capacity-Constant-60mmx88mm/dp/B082F36D3T/https://www.amazon.com/MakerHawk-Electronic-Adjustable-Intelligent-Resistance/dp/B07F3NHHSTthere are other better ones but price jumps from 50$ straight to 300$I was just waiting for december to consolidate my amazon purchase, that is all.QuoteAs mentioned, it was all Dreamcast with all those tests and waveforms.Quoteyes games are either ntsc or pal for it, but i never thought this would reflect back to the power supply itself! i mean as long as we provide enough capacitance and filtering, it should not dip much.hmm... so now i may test the 1 ohm load resistor and see how the waveform looks like then compares it with dreamcast. you note about ntsc and pal made me remember that the other PSU also showed similar pattern of ripple... all at 3.3v while 5v didn't have any pattern of ripple but just continuous spikes as seen in images.assuming this is a fact that it draws its power mainly in this pattern, is there anyway or method to eliminate such a ripple? or it is simply unavoidable?I also connected this to the input caps of the regulator ic which I didn't really put anything besides 1 10uF ceramic with 100nf cermic close to the input pins + 220u bulk nearby. meaning, the lack of enough ceramic caps could in fact make input ripple higher and the bulk cap being slow with much esr will not be able to filter out the huge current ripple... therefore putting more ceramics right at the input pins seem good solution?if so, then i can start putting ceramics even before... like with the 2x 1000uF bulk caps right after the main CMC. this could reduce the total input ripple significantly, don't you think?>

author: Mechatrommer
author_rank: Super Contributor
timestamp: November 15, 2022, 12:25:15 pm
content: Quote from: VEGETA on November 15, 2022, 10:30:41 amimo your load is DC (Digital Current), something is demanding current (or pumping it) at 50-100Hz (that mVpp square wave). have you point out what causing it?Quote from: VEGETA on November 15, 2022, 10:30:41 amthats what we call, R&D one-time investment. it will worthy to buy if you think you are going to design many other PSUs in the future, but for your case, you can easily simulate the "Digital Current" by building a very quick low side n-mosfet, power resistor on high side and your PSU supplying the power, $1-5 worth of parts, you can control the gate switching by square wave generator or by hand. you choose power resistance value based on what you want to test. real life current demand from your Dreamcast? or how strong is strong your PSU is by choosing lower and lower resistance. btw i recently purchased few bunch of power resistor at $25 cost for real DC load..https://www.eevblog.com/forum/beginners/4r-and-8r-100w-resistors-from-ali/msg4484695/#msg4484695i also have home made e-load but maybe i'll use later for transient testing. my newly built passive 500W resistors load doesnt need power or anything to setup, i just move the wiper/clip by hand along the winding and i can change load level at an instant.

author: VEGETA
author_rank: Super Contributor
timestamp: November 15, 2022, 12:51:42 pm
content: Quoteby DC in that reply i meant dreamcast.I pointed out that I hooked the PSU i made to the dreamcast, started the dreamcast and waited until gdemu title screen appears (or a game, same result), then took the measurements on 3.3v and 5v as mentioned above (spring ground, etc..).what did you expect or assume?the waveform is taken by ac coupling 1x probe setting.Quoteyes, i will certainly get a nice unit for this purpose but not immediately now... will need some time.___so my application being dreamcast is taking big current at 50-60 hz periods which caused this waveform performance on 3.3v rail... correct? how can we fix this if it is fixable?

author: Mechatrommer
author_rank: Super Contributor
timestamp: November 15, 2022, 01:45:36 pm
content: Quote from: VEGETA on November 15, 2022, 12:51:42 pmnot necessarily big.. to know if its fixable, we need to sim, to sim... we need to know...1) average current consumption by dreamcast on both 3.3 and 5V rail2) your smps ic average switching frequency? Ton and Toff? if you got some picture.3) better if we have ballpark value of your PSU's output impedance, you can build a test rig as mentioned, and give it a good stress loading..low side switching.. on your left side..then i think we can snap some simulation.. as i remember my Snr.Eng scolded me 20yrs ago its still fresh in my mind.... nothing is impossible!... but implicitly in behind... its just a matter of cost and spacei can think of one "active" way to deal with this, if you really want to fight it... cheers.

author: VEGETA
author_rank: Super Contributor
timestamp: November 15, 2022, 02:29:14 pm
content: Quotecan't be for sure since i didn't measure myself... but 3.3v is about 3 amps or a little less. someone posted it is 2.8 amps. 5v is < 0.5 amps.Quoteit is fixed 700 khz.i guess ton and toff are taken assuming input and output voltage. input voltage is 12v, output 1 = 3.3v, output 2 = 5v. now we know the duty cycle for each rail and can conclude timings.Quotei don't know how to measure it really. what test rig are you referring to?remember that this device will be used with different types of 12v power bricks, each its own quality. what solution do you have in mind?i don't mind little cost up if it is gonna significantly enhance the output.

author: Mechatrommer
author_rank: Super Contributor
timestamp: November 15, 2022, 03:52:30 pm
content: Quote from: VEGETA on November 15, 2022, 02:29:14 pmtest rig picture shown above. by using voltage divider (psu internal resistance + Rload + mosfet Rds on), we can work out what is the "virtual" internal resistance.https://www.science-campus.com/engineering/electrical/dc_theory/chapter6/dctheory_6_7.htmlQuote from: VEGETA on November 15, 2022, 02:29:14 pmthe solution to isolate input power source's noise has been proposed to you earlier by using slotted gnd plan. not much we can do if variant is the input source as different user will use different source hence different noise profile. maybe another easy fix is wind the input's wire into toroidal ferrite core/ring, ymmv.https://my.rs-online.com/web/c/passive-components/emi-filters-protection/ferrite-rings/other thing i noticed... analyzing your schematic and pcb, it seems you installed C37 and also maybe C38? (C22, C23 in earlier design? not sure which pcb you are testing now) are they important and recommended by manufacturer? i cant see it in tps62913 datasheet other than Cff = N/P (not populated) have you tried removing them? sometime bypass across either feedback voltage divider can make regulation worse. ymmv. reference:https://imgur.com/a/6ANuRwu

author: T3sl4co1l
author_rank: Super Contributor
timestamp: November 15, 2022, 05:43:17 pm
content: Quote from: VEGETA on November 15, 2022, 10:30:41 amIt necessarily reflects to the power supply, of course!Indeed, if you've ever had the experience of a poor quality or failing adapter, you may've noticed this as the consumption of your PC/laptop/phone/widget varies with function. Or, I had one occasion I was running my laptop off this shitty inverter thing I made,The output filter inductors and/or capacitors vibrate slightly when switching (it's a "modified sine" output), and more when under load. So the laptop's variable load is almost immediately (within 10ms or so) reflected in the sound of the inverter. It's audible, responding faster than Task Manager's CPU gauge does.Indeed, a power converter is a lowpass filter of sorts; it might add some noise, too, but to the extent we can null that out or otherwise ignore it, its behavior is dominated by the energy storage components that make it up. So, input and output filters, and whatever the conversion mechanism is (usually a switched inductor, but sometimes capacitors are used, or a combination thereof).An ideal power converter, I suppose you could say, stores no energy and transforms input to output (or vice versa) instantaneously. Converters have certainly improved along such a trajectory, over the years: going from low frequency switchers and huge inductors (low ripple fraction), to higher ripple fractions (peak current mode, resonant) and higher frequencies.Note that ripple fraction basically says how much energy is stored, or how many cycles it takes to build up / release the full energy of that element. A ripple fraction of 30% means that about 30% of the energy is circulated each cycle, so takes about 1/x or 3 times that (3 cycles) to fully dis/charge that energy.And doing that at higher frequencies, then, simply goes faster. Your regulator might be around this level. So, at 700kHz, that's a power bandwidth, so to speak, of ~230kHz. The input and output filters cut generally lower than this, but this would be the limiting case, if you for some reason needed fastest response from load to source.Some converters intentionally store energy, for safe keeping (hold-up time), or because the source itself is intermittent (single phase AC). Note that 3-phase AC needs very little energy storage, because power is available continuously, and indeed many industrial converters only use modest filtering, to take advantage of this.In any case, sooner or later, change in load must be reflected by change in draw from the source. Even a battery isolated system must be charged sooner or later, and the amount of charge equals (well, modestly exceeds, due to losses) the load consumption over that time.This is even relevant for SIGINT purposes. The power consumption of a building or room can be monitored, and information can be leaked out as a result. (A battery-isolated design might be required to help mitigate such attacks, even if power is generally available at the location!)Tim

author: VEGETA
author_rank: Super Contributor
timestamp: November 15, 2022, 09:27:58 pm
content: well I have got some updated measurements, this time at no load to see if the spikes and ripple really exist in the power supply itself or from load.here are the images:https://slow.pics/c/BIaB5avOolder design is the one used tps62913 and newer design using tps54394, competitor using lm2596 with 33uH inductor as main filter, 220u cap as input, 100u cap as output... very simple.notes on new pics:1- older design have about 3mv total p-p, no load.2- competitor have about 2-3mv p-p which is very good. at no load of course, when loaded it makes those 50-60 hz ripple.3- new design have good input ripple, about 7-10mv p-p but with huge spikes... but output ripple increased in magnitude. why is this?4- there is some ringing effects as seen in images. I can hear very tiny sound from the board when my ears are like very close. could this be that switcher is not stable enough?for your opinions.

author: T3sl4co1l
author_rank: Super Contributor
timestamp: November 15, 2022, 10:08:37 pm
content: Burst mode operation. Looks like the filter is very poorly damped, hence the ringing.Tim

author: VEGETA
author_rank: Super Contributor
timestamp: November 15, 2022, 10:20:33 pm
content: Quote from: T3sl4co1l on November 15, 2022, 10:08:37 pmI have followed design guidance, also it has internal compensation.I didn't find burst mode but rather eco-mode in datasheet:https://www.ti.com/lit/ds/symlink/tps54394.pdfit says it is for light loads, which our latest measurements are.so what are the damping needed and where?I have followed their datasheet and eval module precisely, especially in placement of caps and L. how could that go wrong?

author: T3sl4co1l
author_rank: Super Contributor
timestamp: November 16, 2022, 12:15:06 am
content: Quote from: VEGETA on November 15, 2022, 10:20:33 pmHow? Appnotes aren't generally well written, mediocrity is the norm. Very little understanding is promoted, or used in the writing process.In particular, take the inductance of the ferrite bead. Resonate it with the capacitors on either side of it, in series. Get the impedance Zo = sqrt(L/C). Ideally, add this as a resistor in series. But that would worsen DC performance. So instead, put it in an R+C in parallel with one of the caps (probably the output side). Use C > 2.5 times the total output capacitance.Tim

author: VEGETA
author_rank: Super Contributor
timestamp: November 16, 2022, 05:25:17 am
content: Quote from: T3sl4co1l on November 16, 2022, 12:15:06 amno app note was used, only datasheet and eval board + direct support.so you think the output meaning stage 1 or stage 2 after ferrite? the datasheet and eval only have stage 1, I added stage 2 for better filtering.this is the ferrite bead:https://www.fair-rite.com/product/sm-beads-differential-mode-2773037447/I could not get the inductance value. however it does have impedance curves. judging from the 2nd graph in "electrical" tab, the impedance is a little above 0 at 3 amps. first graph shows Z=38 at 1 MHz, our 700 khz would be maybe 35 but it is outside the drawing.anyway, stage 1 has 7x10uF = 70uF (not calculating effective one due to dc bias), 2nd stage has 5x10uF + lower value ones = 50uF.so I need something like 150uF elec. cap with a resistor in parallel? I read that elec. cap alone can do the job since it has high esr, but here may need more. how much resistance to add?I actually added 220u elec cap at 3.3v output directly but it didn't enhance the performance during full load... however, this may be due to the 50-60 ntsc pal thing we talked about. I didn't try it without load though. that was for stage 2. also, each rail have a load on it, maybe 1k or so in parallel with output caps.as for stage 1 they didn't recommend elect cap to begin with and they specified a maximum capacitance of 68u... so what do you think?so by having Zo=sqrt(L/C) for stage 1 and 2, what are we looking to do?I have different types of resistors I can use in parallel with 220u cap, what do you suggest?and one more thing, does this R+C for damping actually act like other caps in terms of filtering ripple or it is just for damping because of very high R?

author: Mechatrommer
author_rank: Super Contributor
timestamp: November 16, 2022, 05:43:14 am
content: How about another revision? Trash all those redundant smd caps thats taking up spaces, smps only act as preregulator, nevermind worse performance.. put linear ldo regulator 3.3v and 5v at the front end and let the psrr do its magic, so if you are still not satisfy, nobody here will be able to help you anymore

author: VEGETA
author_rank: Super Contributor
timestamp: November 16, 2022, 06:03:04 am
content: Quote from: Mechatrommer on November 16, 2022, 05:43:14 amldo will have heat issues and will require me to put heatsinks and so on which originally i didn't want.however, having too many 10uF caps is troublesome, I can use 22u caps instead. maybe one of those higher quality low esr ones i linked before.also, ldo psrr is usually good for lower frequencies and won't do much for high or mid frequency noise. could they enhance the low frequency ripple though? i don't know.if we are going this route, then we would need like really low drop voltage... mabye 100mv? i bet the ldos which could do that are very expensive xD. however at 100mv dropout for 3.3v at 3 amps = 3x100 = 300mW dissipation. it won't need a heatsink. having to install heatsinks are kinda no-go for me.i am easily satisfied.. xD i just need that nice juicy <10mv p-p full loadlol i found lt3033 which can do 100mv dropout but it is 9$ per one IC hhh.

author: Mechatrommer
author_rank: Super Contributor
timestamp: November 16, 2022, 06:52:54 am
content: Look again, your problem is 50hz, far from hi freq region.. its some low freq loading that either feedback control unable to compensate, or you have significant resistance in your output tracks.. increase your track width.. and add filter/capacitance.. very near to power connector.. thats what it takes if you want to improve things... more space, more components, more cost, more heatsink... thats engineering.. for 0.3w you can let the pcb spread the heat ymmv..

author: VEGETA
author_rank: Super Contributor
timestamp: November 16, 2022, 07:09:26 am
content: Quote from: Mechatrommer on November 16, 2022, 06:52:54 amwell, lt3033 won't need any heatsink but it is massively expensive. more realistic LDOs would be ones reaching 1-1.5w dropout dissipation, i guess heatsink needed for that right? gonna be very hot.look at my tracks in some of the layout images above, i actually used zone copper filling so that it is way wider than tracks.so the ldo can actually attenuate the 50-60hz ntsc pal power sipping pattern? i don't know about that. problem is that the smps ic here still even at no load has some ripple and noise which is not 50-60hz. maybe i should be trying a load resistor to see the actual performance of that ic since no or light load is using eco-mode.hmm it is getting a bit more complicated and way expensive that i needed...I mean see that competitor I spoke about, using the very cheap switcher IC LM2596 operating at 150 khz... at no load it achieves very small ripple and noise <5mv but at full load still has that pattern. could this actually be the better alternative?? it uses very large 33u inductor as main inductor while my ic uses 4.7 max since 700khz.

author: jonpaul
author_rank: Super Contributor
timestamp: November 16, 2022, 07:34:51 am
content: Bonjour, after 9 pages of comments, perhaps 100 messages, looking at the breadboard photoI think the OP needs more research and experience to do this PSU.The breadboard technique is not useable to debug these issues.Jon

author: VEGETA
author_rank: Super Contributor
timestamp: November 16, 2022, 07:40:05 am
content: Quote from: jonpaul on November 16, 2022, 07:34:51 amwhat breadboard? i never used any breadboard in this project so far. all manufactured PCBs. are you referring to probing technique? still, i didn't post an image for it i think.thanks

author: Mechatrommer
author_rank: Super Contributor
timestamp: November 16, 2022, 08:09:00 am
content: Quote from: VEGETA on November 16, 2022, 07:09:26 amthats a strategy right? Start cheap, optimize later. if he revise and add post-reg, what hope do you have? Probably still cheaper or same cost as your latest version. Didnt we mentioned try larger L? dont make my mistake of following recommended L.. we'll never know..

author: jonpaul
author_rank: Super Contributor
timestamp: November 16, 2022, 09:09:58 am
content: Mistook photo in the post of T3sl4co1Sorry.J

author: VEGETA
author_rank: Super Contributor
timestamp: November 16, 2022, 03:29:27 pm
content: Quote from: Mechatrommer on November 16, 2022, 08:09:00 amhmmm I always get warned about using more than recommended inductor size, it happened twice. so my 4.7u is the upper limit, i can now stack another one on top of it to be 2x 4.7u in parallel for the sake of testing. do you think it might work?what is you test about this? you mentioned you had a mistake following recommended L.hmmm... I would stick to pure switching design for now... really don't want to have extremely costly device as well as more complicated. I found LT3033 which can work for 3.3v and ADM7171 (ADM7171ACPZ-5.0-R7) for 5v. both can handle about 100mv dropout which is fantastic without heating. 5v rail can tolerate more since it has less current demand. However, these are not cheap. taking also that we need a switcher or 2 switchers... the problem is that I want this device to be sold at 40$ retail price, I can bump it up to 50$ at absolute most if it is really lower noise and ripple but choosing such high cost stuff will make that near impossible. There is TPS7A53 too but it also will increase cost.+ 91 weeks lead time xDanother approach is the cheaper LM1085 (3A) and LM1086 (1.5A) regulator but this would require a heatsink for sure, which makes it kinda worse that original 20-year old PSU which has a lot of heat.

author: Mechatrommer
author_rank: Super Contributor
timestamp: November 16, 2022, 04:06:47 pm
content: Quote from: VEGETA on November 16, 2022, 03:29:27 pmthe recommended L is 22uH, big spikes on output, changed to 470uH, spikes went down almost 100%. it wont hurt trying 10 minutes stacking them together in parallel to get 9.4uH, if it doesnt make any different call it failed and remove back to original 4.7uHQuote from: VEGETA on November 16, 2022, 03:29:27 pmsometime we have to pay the price to get better performance. after the other cheaper solutions failed. ymmv.

author: VEGETA
author_rank: Super Contributor
timestamp: November 16, 2022, 07:29:16 pm
content: Quoteoh so they told you 22u is the recommended, what was the upper maximum they told you about? but 470u is too much compared to 22... assuming modern switcher which has fast switching like 1-2 mhz, having smaller L is doable but it would not hurt to use very large L right?what mV p-p you had before and after? do you have some waveforms?Quoteyou are correct but also there are limits to how much you can increase price... the other cheaper solutions are working fine especially the not-so-crappy ones... I just wanted like a "premium" version which has truely better performance... so from 38$ for the best one to 50$ for my solution seem nice... just not much more.testing L is one last hope I can cling to. but i try with others here to have another solution using the same parts if possible

author: Mechatrommer
author_rank: Super Contributor
timestamp: November 16, 2022, 08:16:28 pm
content: Quote from: VEGETA on November 16, 2022, 07:29:16 pmyou can look my psu herehttps://www.eevblog.com/forum/projects/voltage-spikes-on-the-linear-output-in-split-rail-smps-pre-regulator/msg4495825/#msg4495825you can read my tuning/debug process if you are interested. but different requirement as yours, i will be happy if it can do 100mVpp. and i start with the cheapest jelly bean 34063 so i dont expect too much when starting this project knowing people like to bash 34063... this is for personal use, and as an exercise and learning too. i didnt report my last result (by increasing L from 22 to 470uH) which is somewhere 60-100mVpp ripples/spikes on the linear post-regulator output (still nasty ripples on smps pre-regulator, dont ask!). in the mean time i will wait to send the revised pcb ver4 to jlcpcb... i'm doing other project now.

author: VEGETA
author_rank: Super Contributor
timestamp: November 16, 2022, 08:30:07 pm
content: I tried putting 2 10uH inductors on top of the 4.7u one so now they are all in parallel not in series... so 10 | 10 | 4.7 not a full 26.7u. the result didn't really change. so i think maybe series is the way to go?i am really confused to what i should do now...

author: Mechatrommer
author_rank: Super Contributor
timestamp: November 16, 2022, 08:57:41 pm
content: yup inductors should be in series to increase inductance, not parallel. i was having a brainfart momentyou should be able to google this easilyhttps://www.allaboutcircuits.com/textbook/direct-current/chpt-15/series-and-parallel-inductors/so then you have to do dead bug style inductors on your shiny pcb

author: VEGETA
author_rank: Super Contributor
timestamp: November 16, 2022, 09:21:26 pm
content: Quote from: Mechatrommer on November 16, 2022, 08:57:41 pmhere is what i did:https://imgur.com/a/UD88Rdqthose are in parallel... I remember reading that in parallel does provide benefit of sharing the load for sure, but in our case the load is fine for one inductor. it is just the ripple performance that we need.i will have to remove the 4.7uH inductor and replace it with 10uH one... it should provide some visible benefit being more than 2 times bigger. if so, then it makes sense to install a bigger one like 100uH or so but I actually don't have one. maybe salvage from other boards that have 33uin your design you seem to use a very generic and low quality IC, having 60mv could be a good result.

author: Mechatrommer
author_rank: Super Contributor
timestamp: November 16, 2022, 09:55:09 pm
content: Quote from: VEGETA on November 16, 2022, 09:21:26 pmyes they share load but reduce inductance just like parallel resistors. reduced inductance than recommended means increased current/voltage ripples and also make converter works harder (hotter).Quote from: VEGETA on November 16, 2022, 09:21:26 pmditto! before the era of mVpp smps... but they are few cents ICs..

author: Vovk_Z
author_rank: Super Contributor
timestamp: November 17, 2022, 10:11:55 pm
content: To TS: I guess you want 10-22 uH main inductor. It depends on a datasheet of cause. My guess goes from some 'average' DC-DC convertor IC design.You dont have to go too far from datasheet value.Linear post-regulator will improve ripple too (about 10x). Some LDO should do.

author: VEGETA
author_rank: Super Contributor
timestamp: November 18, 2022, 10:09:50 am
content: Quotewhen I return to lab in 4 days I will try putting 2 10uH in series to form 20uH, on a perf board and hooked in the place of 4.7uH one. we'll see. 22uH seems realistic but TI keep telling me it might cause instability. output caps too.Quotethat is a valid choice too but unless I go for expensive stuff, I would need to use a normal LDO which has some edge of dropout... then I would need a heatsink. this is what I didn't want to begin with but I will see if it is a valid choice.

author: VEGETA
author_rank: Super Contributor
timestamp: November 18, 2022, 12:20:18 pm
content: speaking of LDOs, I found this:https://www.ti.com/product/LP38503-ADJexact part number is LP38503ATJ-ADJ/NOPB which has thermal junction to ambient of 33 degrees and junction to case of 22 degrees which I think very good. not cheap by any means but still can make it.if this choice was taken, then I can get local aluminum sheets cut to specific size to be fitted on top of both regulators... any Aluminum sheet heatsink can do such low requirements. I need this heatsink to be dirt cheap, so no buying and shipping!meaning 0.55 maximum dropout * 3 amps = 1.65 -> 1.65 watts * 22 = 36.3 degrees + 25 for ambient = approximately 60~65 degrees total. any heatsink can do it right?if paired with switcher IC which can deliver relatively clean signal, then i think we can make it to <10 mv p-p under full load right? current switcher is dual output which is fantastic but needs more tweaking to get better noise output.looking forward to your opinions.this creates another issue which is how to stick the aluminum heatsink to both of them? I see such products use thermal adhesive but i don't know any good brand or the cost.

author: Mechatrommer
author_rank: Super Contributor
timestamp: November 18, 2022, 12:28:21 pm
content: since you are not happy with 5V rail, maybe you can only use linear post-regulator on that rail only.. doing homework for you... LM1085 maybe a good choice. 5mVpp load regulation, 1V dropout x 0.5A = 0.5W should be manageable pcb as heatsink. $2.5 in digikey, cheaper in ebay china. who knows that knock off can do 10mVpp? should be good enough if so...Quote from: VEGETA on November 18, 2022, 12:20:18 pmtry avoid ADJ version if you are tight on space, that will need more resistors divider. but thats your choice.

author: VEGETA
author_rank: Super Contributor
timestamp: November 18, 2022, 01:17:39 pm
content: Quoteit is for both. I need top performance on 3.3v more than 5v since 3.3v is the main one which powers everything.QuoteI originally thought about this but the high dropout voltage kinda made it not the first choice at least for now.dropout is 1.5v * 3 amps = 4.5 watts. meaning about 100 degrees, but with heatsink is about 70. very high IMO right?if i ever go heatsink route i will never get anything from outside... but rather as i said, locally cut from big sheet with nice thickness. after that stuck or glued to the IC.Quotethis particular IC does not have fixed version.. adding 2 resistors is very easy even on tight places so no problem for me.do you know any thermal glue or anything that can stick the heatsink on the surface of the IC? this is the only way I want to achieve it.

author: VEGETA
author_rank: Super Contributor
timestamp: November 18, 2022, 02:35:49 pm
content: Possible other LDOs alternatives:RTQ2533W-> cheap. PSRR is 60db for lower frequencies at 3 amps but still promise 10uV noise somehow. junction to ambient is 35 degrees. dropout max is 180mv max which is fantastic. so assume 200mv -> total 0.6 watts -> maximum of 20 degrees raise -> 45 degrees total! does this seem too good to be true? 45 degrees (including ambient) does not require heatsink right? i am worried that it only purchasable from digikey.its junction to case is worse than junction to ambient, why?a similar RT9059 available but 450mv dropout max at 3 amps. -->0.45*3= 1.35 watts on vqfn package. 1.35*32.8 c/w = 44.28 == 45 degrees above ambient... +25 = 65 degrees. can this be without heatsink??MIC35302WD-> cheap but very high dropout which requires heatsink.MIC37302-> good overall but 0.5v dropout. however, it states only 5.5 C/W junction to case.NCV59745AMW180TAG-> not cheap, 100mv dropout typical, 200mv maximum. 0.2*3 = 0.6 watts * 40 c/w = 18 degrees above ambient. this is without case. PSRR seems interesting as the curve displays high value for lower frequencies up to 10khz. I just noticed it cannot output 5v!MIC68400YML-TR-> expensive, 500mv maximum dropout at 3 amps. psrr less than others. 30 c/w to ambient.MIC47300WD-TR-> 400mv max dropout.MIC69302-> 0.5v dropout, 38 c/w ambient.ISL80103-> not expensive, 120mv dropout, but kinda limited availability

author: VEGETA
author_rank: Super Contributor
timestamp: November 20, 2022, 12:34:18 pm
content: Hello,I've been thinking and iterating this design for a while now seeking more options... and I came up with this in the attachments.key points:1- using 10uH inductors instead of 4.7u as main switching inductors... as well as using one 10u instead of 33u as main input filter.2- settle on RTQ2533W as LDO since it ticks all boxes. 200mV dropout will ensure maximum of 0.6 watts for 3.3v 3 amps rail which I think won't need heatsink. if heatsink needed, I can cut 10x25mm aluminum piece and stick it on top of both LDOs.3- made the design 60mm x 50mm instead of 50x50. this made more room.4- arranged components to allow the slot, please check it out.5- switcher now has 22uF 1206 caps, 5 of them instead of 7x10u.please check for any info or suggestion.i am still far from lab, need 2 days

author: T3sl4co1l
author_rank: Super Contributor
timestamp: November 20, 2022, 11:09:18 pm
content: You're gonna change those FBs (they saturate) to inductors proper (saturate at rated current) right?Add some R+C or electrolytic footprints to dampen the LC sections.Add a bypass resistor (optional 0 ohm jumper) to try it without the LDOs first.Tim

author: VEGETA
author_rank: Super Contributor
timestamp: November 21, 2022, 06:50:55 am
content: Quote from: T3sl4co1l on November 20, 2022, 11:09:18 pmhere are the ferrite beads:https://www.fair-rite.com/product/sm-beads-differential-mode-2773037447/the reason to include them was to do some filtering of noise, this particular one can do for lower frequencies. putting inductors will cause drop voltage, and I don't know what value inductor to use. thus, thought that FB was a better choice since its resistance is like 1.2 mOhm.however, if you mean like small 1uH inductors which have so small DC resistance then yes maybe I can replace the beads seamlessly. LCSC has a collection of such smaller and high current L.quick edit: hmmm since i won't use the switcher as final stage, then I can afford some dropout since it will already have 200mv max dropout before the LDO. actually, the LDO says 180mV as max dropout at full load so assuming 5mR inductor at 3 amps will have 45mv dropout. so maybe I can just put 250mv total dropout and be safe... or just rely on 200mv total since the rated LDO dropout is 110mv. what do you think?assuming maximum dropout of 270mV, it will result in 0.81 watts at LDO which makes about 30 degrees temperature increase over ambient = about 55-60 degrees total which I think requires a heatsink. always wanted to get away without oneQuotewhere exactly? at which stage?if at LDO stage which has 5x 22u ceramics... is it ok to add another 22u ceramic in series with say 100R resistor as a damper instead of an elec. cap? or better yet 1uF cap with 100R or so? since I do have 1uF in design and it is small and won't take space.elec cap will be huge capacitance value which will affect the stability of the switcher, or so TI recommended. I am already exceeding maximum allowed capacitance of 68u.Quoteat the output of switchers? I can add a load resistor, say 1k ohm to ground.if 0 resistor is used, then it will be like a connecting bridge between switchers output and LDO stage. is this what you want?On another point, do you find this layout good? knowing that i am simply adding footprints and so on, not a real design yet but just a rough layout.

author: T3sl4co1l
author_rank: Super Contributor
timestamp: November 21, 2022, 08:52:13 am
content: Quote from: VEGETA on November 21, 2022, 06:50:55 amYou can get inductors like that you know...Look at the impedance curve. See the 1A curve. See how it's so depressed? How much filtering value do you think you're getting in that condition?Better yet, don't think -- calculate! What is the attenuation for such impedance at 1A and 1MHz? 10MHz? (Bonus points: include capacitor ESR and ESL too!)(That we should be so fortunate as to be able to model and predict everything we do in EE. Not always easily enough to be worth doing, but in principle at least. But this case happens to be one of the easiest to model.)QuoteYes. (Inclusive-or. All of them, most likely.)QuoteWhat the heck will 100R do?...And how would one figure it out?R = sqrt(L/C), for C being total capacitance (may be the series equivalent of caps on either side of the inductor in question), and L the inductor between it. Cbulk >= 3C.You propose R = 100 ohm and Cbulk = C/5. Even at best, with L(FB) being, let's see, about 40 ohms at 1MHz (zero DC bias) or ballpark 6.4uH, and assuming the capacitors don't drop under bias (they certainly will -- check the characteristic sheet), you'll have 5*22 = 110uF, or Zo = sqrt(6.4/110) = 17 ohms. 100R will reduce the ringing moderately, but won't bring it down to zero (well damped, or overdamped).(Normally, this kind of connection does not give an overdamped condition; much more Cbulk is needed to get there. Somewhere around slightly underdamped to critically damped will do fine, anyway.)Inverting the capacitor counts is more likely to be helpful. Say just one or two 22uF in parallel, then an R+C using 3-4 in parallel, plus whatever resistance is appropriate.The fact that Zo is so high, has substantial implications for the load step response. This impedance has physical meaning. It represents the peak change in voltage, from a step change in load current. If you want 10% regulation at 3.3V, for a step change of say the full 2 or 3A load (whatever it was?), that's 0.33V/3A = 0.1 ohm. Evidently for C = 110uF you need L < 1.1uH. But for C being smaller as described above, L will be smaller still.You can measure all of these quantities with a suitable setup.I don't know how many ways I can emphasize this, by the way.You can, physically, practically, in a couple of minutes, set up a test to measure all of these parameters. Impedance, time constant, step response, output DC resistance.You can do it with an automatic pulse generator, like a 555 into a MOSFET and resistor.You can do it with a resistor and a wire in your goddamn hand -- you have a DSO more than capable of capturing single events. You can touch a wire, get the single capture, and inspect the waveform at your leisure! Very handy indeed.Anyway.To do that RC with fewer components, an electrolytic will have about the right ESR, or can be chosen nearby at least. So, 0.1 ohm ESR, 0.1 ohm Zo, and the output doesn't do any ringing, no nasty step response shenanigans, nice and solid.Matter of fact, go ahead and do the all-ceramic thing. Set yourself up for another mess of waveforms. Do the tests. See them ring. See the steps.Then glom on a big fatty sloppy ESR-y electrolytic.See it all go "thud".See it fix all the ringing.Tweak some other component values. Goob in a smaller inductor.Then see what the step response does.You can do all of this so so easily.I don't know what I possibly have to tell you to get you to do this.It's so painfully easy and pleasant to do.You just have to be willing to grab a few damn resistors and sit down at the scope.And zoom your scope in once in a while.What time constant is this all happening at, by the way?We know this, precisely, as well!The LC time constant is pi sqrt(L C)/2. The RC or L/R time constant is, well, exactly those. Any of those pairs of variables will get you something of interest.QuoteYou don't seem to be too concerned about that given the other poster suggesting you exceed the recommended inductance value as well...QuoteBypass, as in, to short from SMPS output to LDO output, with LDO removed (DNP = do not place). To pass it by. By-pass it, as it were.Or you can jumper over it with a stupid bodge wire, that's fine too, but as long as you're going to the trouble of making another board, why not make it easy on yourself?QuoteThe placement should be a significant improvement. I would not bother with the LDOs at all.Mind, it's still not clear how much of any of this actually matters, because even just your waveforms and testing are woefully insufficient. Some combination of these mechanisms (filtering, LDO, CM) will have effect atsomepoint, but how much of one kind of filtering you need to employ before the other comes to dominate, isn't clear.Somewhat aside, the LDO idea itself is bothersome:So many people say "just add postreg to clean it up!!", completely ignorant of:- LDOs have shite PSRR in general, particularly at modest to high frequencies (>10kHz), and at low Vin-Vout (with some standout exceptions);- A better differential filter and higher Fsw is cheaper and more efficient;- An LDO does fuck all for common mode noise, which can't be helped by ANY amount of differential filtering. CM is dominated by layout alone, and some use of CMC, but also more layout.I think the idea of a postreg mainly persists (i.e.it meets the definition of a meme) because:1. It's just complicated enough for one to feel proud of building/designing, while still being easy enough to succeed;2. It sounds good / has a believable function (but as mentioned above, it need not actually succeed at that goal!!),3. People see a lot of others doing it so it must be good right??!?3a. ...Nevermind *who* they see doing it. Or not doing it:Few professionals use postregs (read: very often, or at all). And for the occasions that that additional filtering really is well and truly necessary, and where burning that little voltage overhead really is worthwhile (e.g. smaller than the DM filter components), not just any damn LDO will be used, but a type with especially good PSRR (some are in fact available, targeting RF equipment for example), or a discrete circuit such as a "capacitor follower" (taking advantage of BJT characteristics to get exceptional performance).4. And most especially of all: nevermind if they know they need it in the first place -- or can verify (or have any way to verify!) that it's doing ANY of the claims set out in whatever they saw that inspired them to build it!Few professionals likewise use them, because there just isn't any damn point to it. I regularly measure single digit mV output ripple on point-of-load converters, running typical things, you know, an MCU, a few interfaces and peripherals (amplifiers, RS-485 transceivers, etc., you know, the usual add-on junk).For something like your load with large and frequent fluctuations (variable CPU and GPU activity during a frame, and between frames), 10s of mV would seem normal, and perfectly acceptable. I have no idea what that system actually specifies (you'd have to see their internal design documents, or at least the data of everything that's running from those direct rails), but I would be shocked if it even cares about 100s of mV. Perhaps some random glitches would start to occur at that level, who knows.And then, anything less than that [some 10s of mV], it... simply doesn't matter. It's meaningless. It provides no performance or reliability improvement. It's an internal connection (at least, I assume this connector and cable is short and internal?), it likely doesn't affect EMC. (Emissions up the power-input cable may be relevant, which will be affected by emissions on the output connector, by the principle of reaction ("..equal and opposite force.."). But no further than that.)As for just getting it low for, shall we say, academic purposes -- well, now we're measuring something. So get to measuring. Do the step load tests, see the transient response. Zoom in and see the switching ripple. Zoom in further and see the CM noise.Can even set up a LISN and measure emissions. Wire up a ground plane with a few bias tees dotted around, wire up the connectors, and see what noise is present on each one. Can be used as an introduction to RF theory and EMC testing too. Lots of academic value we can explore around a humble power supply.Tim

author: VEGETA
author_rank: Super Contributor
timestamp: November 21, 2022, 10:17:40 am
content: Quoteaha, so at my 3 amps it won't do much if any, therefore this bead is only suitable for lower power consumption circuits right?thus, we need to get an inductor which is rated at say 4-5 amps with saturation current more that this, but still has relatively low resistance.the inductor won't be saturated if choose one more than 5 amps.Quoteif we go with this, we have 17 ohms as our impedance.how did you conclude that 100R will not be enough using these calculations?Z=sqrt(L/C)assume C=110, for Z to be 0.1 ohms we need L=1.1uH so 1uH is suitable.if we added another 220u elec, for z to be 0.1R we need L=3.3uH, correct?Quotewell, putting elec cap as a simple solution will be ok for me except for the maximum capacitance we talked about. yes i exceeded it but not by much, having 5x22 = 110uF caps instead of 68u is kinda accepted but if i have to put 330uf don't you think it is too much?they recommend low esr ceramics for switcher operation to be fast and so on...if you were to design this stage of filtering what would you put?if we go elec. route, meaning just put the elec. cap without a resistance in series right? or should we?QuoteI do have a switch to the whole thing. I can hook the scope to the final 3.3v rail, then power on the system with scope at single shot mode to see the step it takes from off to fully on. is that what you suggested? here no need for resistor. unless you mean hook-touch the resistor-wire to another point in the design.or you actually mean I disconnect the psu from dreamcast and power it, then use different resistors to see the response? like 1 ohm resistor for 3.3 amps or 1.1 resistor for 3 amps. put scope into single shot mode, then wire the wire-resistor to ground then touch 3.3v rail and see what happens?I need to know what setup you mean exactly and will do it tonight for sure. so please state it.I can then as you said save the waveform and measure + zoom to stuff.Quotewe were speaking about the inductor, which I will test a 10u instead of 4.7u. however, I already put 110u capacitance instead of 68u. in your experience, does it really hurt going much more? i mean, using elec. cap will surely be a lot.. like 220u at least.actually, i once soldered a 220u elec cap to the first stage (in parallel with ceramics) and it didn't do damage but still didn't enhance the system performance.Quotethen i would need the ldo to be not installed as you mentioned. installing it myself later on will be hard for me. it is VQFN-20 pins 3.5x3.5mm... very small. I only have soldering iron and some thin solder. will get more stuff like hot air later on but certainly not now.so maybe having the ldo installed is a good choice for this matter.QuoteRTQ2533W LDO seem good and cheap enough, so any improvement they provide is nice and will be easy. i have put 3x22u on LDO input, and 5x22uF at LDO output.I guess for our damping we need to be concerned with 5x22u of first stage switcher filters + small inductor which replaces ferrite bead + 3x22u ceramic caps at LDO input. anything else I missed?and I asked a question but no one seemed to notice: if putting 220u elec cap with say 1k ohm in series while both in parallel with other caps, will the 220u be counted with the filtering caps themselves? I mean, would it do good for filtering or just for damping purposes?Quoteyou could say that. other psus already have "just working fine" to their marketing and I was happy using them.however, originally, i wanted to achieve like premium quality or let's say a perfectionist approach to product design. maybe i look silly saying it but this is something i like. therefore, i thought nothing is bad if i designed my own solution which delivers very low noise and ripple at full load despite all these frequent simps of power. less noise and ripple is always better, despite sometimes some noise is ok.original psu 20 years ago was fly-back design, if you dig in previous posts here you may find its output waveforms.besides the perfectionist stuff, yes, i want to learn how to actually design good stuff. the problem is that patience is not my best feature and wanted to go to market fast since this project got changed a lot and took much time...etc._______okaction plan:you kindly specify exactly what and where should i do the resistor-wire measurement as proposed above.I will do these measurements and report back with nice waveforms. then we analyze them to figure out what to do.analysis needed: calculate output impedance, figure out L needed in order for Z to be 0.1R, then see which resistor and capacitors value we need.best regards and always thanks for all this. no scope can measure how appreciated i am.

author: Someone
author_rank: Super Contributor
timestamp: November 21, 2022, 10:35:57 am
content: As these specific questions with values of capacitance/resistance/inductance come up, it simply sounds like you're missing the point of engineering: a high dimensional problem, a designercanchange just about any parameter/value but other things would have to change too.TI provide all the information needed to simulate the design, then you can quickly try the results of varying different component values. But it seems like you aren't taking that engineering design approach, and are reliant on others to do that work for you. Just using off the shelf design guides will lead to the performance that any other person could do, low barrier to entry, no advantage over competitors. To have a unique product that surpasses the competition the designer needs to add something (effort or special knowledge).

author: VEGETA
author_rank: Super Contributor
timestamp: November 21, 2022, 11:24:51 am
content: Quote from: Someone on November 21, 2022, 10:35:57 amactually, i worked with TI support on simulating it and we did. I don't quite remember results but I still have the file somewhere. TI ran it on their PC since it is better than mine, but I can still run it fine. check some of the images attached. as you see, we added every detail about components used to have perfect representation. >> I will post sim file once i return home, now just these 2 snipsHowever then we talked about how big inductor filter at 2nd stage (my idea) was causing 200mv drop...etc and they directed me to the ferrite bead solution which as we saw here was not correct.I will re-install PSPICE for TI software and try to re-create everything to test.I am doing effort but i still need more learning. trying the simulation file maybe a good first step + help of this thread. do you think after doing this I can achieve what I want? or simply unrealistic to get down to <10mv p-p at that periodic full load?thanks

author: Mechatrommer
author_rank: Super Contributor
timestamp: November 21, 2022, 12:55:30 pm
content: Quote from: VEGETA on November 21, 2022, 11:24:51 amimo at this stage, simulation is useless. you need to rig yourself up with necessary knowledges and skills for psu design, such as resonant freq, Q etc mentioned, so you can make educated guess when you want to make component selection, know what the effect of ESR ESL if it really matters, and know why different valued mlcc have different cut-off/notch frequencies thats why people use different valued caps several decades apart instead of many same value.http://axotron.se/blog/decoupling-primer/then you should know which part to simulate, your area of interest you want to tackle, or make bode plot on some components, etc etc. knows what happens and its effect on control, ripples and stability if you overshoot the recommended L in dc-dc converter's datasheet. and then your pcb is a part of the equation even yourself (or me to my pcb) wouldnt know.Quote from: VEGETA on November 21, 2022, 11:24:51 amthat depends on your skills... read this...https://caxapa.ru/thumbs/348441/Switchmode_Power_Supply_Handbook_3rd_edi.pdfhttps://designers-guide.org/design/bypassing.pdfhttps://www.comtest.ro/biblioteca-tehnica/5952-4020-DC-Power-Supply-Handbook.pdfsince you are dealing with pcb (1oz or 0.5oz) layout, impedance and parasitics could be the issue...CHAPTER 12: PRINTED CIRCUIT BOARD (PCB) DESIGN ISSUESPCB layout guidelines to optimize power supply performanceyou can google related topic for more...and many others reading materials and yotuubes.. and become the master of your own fate... cheers.

author: Vovk_Z
author_rank: Super Contributor
timestamp: November 21, 2022, 04:26:34 pm
content: Quote from: VEGETA on November 21, 2022, 06:50:55 amThey mainly help at the output. There is much less need for them (R+C) at the input. (I mean we talk about steady-state pulsations, but not about transients).

author: VEGETA
author_rank: Super Contributor
timestamp: November 21, 2022, 09:46:55 pm
content: I have added the simulation of the circuit as basic as it is. no parasitic stuff added so you see it delivers about 1.5mv p-p which does not comply with real circuit.I am doing another simulation after putting all parasitics but speed is 3 instead of 0 since my laptop is very poor core2duo. will post it once it is finished.

author: Someone
author_rank: Super Contributor
timestamp: November 21, 2022, 10:02:04 pm
content: Quote from: VEGETA on November 21, 2022, 11:24:51 amPerfect, but not correct. Instead of knowing the problem or finding out what it is you build more PCBs with different architectures, learning little from the process. Simulation will not match reality perfectly but it can get close enough to answer most of the questions you keep posting.Which is quicker?Simulating 100 timesorBuilding 2 PCBsNormal engineering practice is to stop when something is not working as expected and test/measure/learn to understand why. Then you only need to fix that, not the 6 new problems created with another guess. But as the incredibly patient T3sl4co1l has brought up many times, you are designing toward a marketing number (p-p noise) without first:having a specification or model of the loadormeasuring the separate contributions to the noiseThis seems to be way beyond your capability, with no evidence of you going back and learning the fundamentals. Damping a resonance or changing the value of an inductor might be one of the very many steps and changes needed to end up where you want, but you need to understand those contributions rather than expecting everyone else to contribute the engineering work. As an example: I've not seen any evidence that damping is needed as this looks like more fundamental issues, but only measurement can confirm that.

author: VEGETA
author_rank: Super Contributor
timestamp: November 21, 2022, 10:31:17 pm
content: Quote from: Someone on November 21, 2022, 10:02:04 pmuntil now I have built maybe more than 5 boards, but right now I want to make improvement before making another board. because i want to base my new board on something, rather than just try stuff, don't you agree?it was not perfect or so but maybe close as you said.I have listened to Tim's words but still waiting for him to respond with the test i need to do so i can do it. his suggestion will let us see the step load response. then we can see what to do or put.this project is above me but I am learning as I go and I really made lots of new gains and info along the way. I also want to learn the engineering stuff more so I can rely less and less on other people's help.So I will be waiting Tim's comment on the exact test method, and I will do it for sure.do you have any suggestions? you speak about an issue of fundamentals, so kindly inform me where exactly.

author: T3sl4co1l
author_rank: Super Contributor
timestamp: November 21, 2022, 11:12:09 pm
content: Quote from: VEGETA on November 21, 2022, 10:17:40 amCorrect. Or 3A. Check the datasheet, it will say how much inductance has dropped by, at the current. Usually like 20 or 30%. Which is fine.Make sure it's rated for DC current as well (thermal limit, usually 40C temp rise). Your demand for low resistance will probably make this trivial, but check anyway.To emphasize: there are two current ratings.One is purely thermal. It has absolutely nothing to do with the electrical characteristics of the component. This is the only current rating ferrite beads carry.The other is saturation, which inductors typically bear. Ferrite beads, you have to discover through the characteristics (if provided at all).For example, the bead in question is approx. -30% impedance by 200mA. Pretty pitiful as an inductor.But it's also a pretty pitiful inductor in general, since much of that impedance is resistance. That is, it has a low Q (quality) factor. Indeed resistance dominates above 2MHz. This makes it great for damping resonances; but not when significant DC current also flows.Ferrite beads are most often applied to low current loads when a minor amount of filtering is required (and a whole inductor is unwarranted, and a resistor would still drop too much voltage), or signals from connectors to filter picked-up RFI, or to dampen cable resonances, etc.; external connection stuff.QuoteNo, use the bare (low ESR) capacitance only. The ESR makes the rest looks like a resistor, at least for middle frequencies (around Fo = 1 / (2 pi sqrt(L C))).This will still affect the control loop response, and it could be that the loop gain is higher, or phase margin lower, below those frequencies, where the capacitances do apparently add (F << 1 / (2 pi ESR Cbulk)), and you get poorer transient response, or oscillation. In that case, reduce all values closer to nominal and see how it works.Most likely the ESR acts to stabilize the loop and the permissible amount of (bulk) capacitance becomes unlimited. But this would have to be tested.QuoteThe electrolytic has ESR. Shop for specified ESR.External resistance would be required if you're using something that doesn't have enough. Aluminum polymer easily go that low. Ceramic certainly do. The electrolytic will be smaller than a fat stack of ceramics.QuoteNo, that's just power-up transient. That tells very little about performance (it does, but not enough of it).QuoteYes!Also test with some idle load, so it's not going from 0-100% each time. Maybe a 10 ohm always connected, then pulse a 1.2 ohm across it. Or 2 and 2 ohm (50-100% step).And take the falling edge (100-50% or etc. load step). In general, they will not behave the same! The controller is nonlinear. The closer together the states are, the more similar their responses will be, but you also want to see what happens when transitioning from, or to, light load conditions, or burst mode.QuoteMore is permissible if compensation is adjustable. Which... I guess I should actually look at the TPS54394 anyway......Oh it's a hysteretic control, lol.Yeah it doesn't give a shit what you hang off it.I would keep the switching inductor small to keep frequency high, and use a modest amount of capacitance at the output. See Fig.24:https://www.ti.com/lit/ds/symlink/tps54394.pdf?ts=1669071182112Just do that (left side), then tack on another 1uH, then 2 x 22uF || 100uF electrolytic.It will generate ripple at light load, anything with burst mode will anyway but particularly being hysteretic type, it always will, proportionally. If you must, this can be smoothed out with an LDO.The LC filter deals with switching noise, the LDO does not. Note the datasheet:https://www.richtek.com/assets/product_file/RTQ2533W/DSQ2533W-02.pdfindicates a mere ~30dB above 100kHz (page 11), give or take the peak there, and whatever happens above 1MHz. And that's with an obscene amount of output capacitance: most specify 1-10uF, they're calling for 67!QuoteOh then add in two more, at input and output of LDO, and disconnect it completely, no problem?QuoteWhat is 1k going to do with respect to the fractional-ohms of capacitors already there? It's just some load. 1k*220u = 220ms, a time constant so glacial it might as well be a DC load, as far as the control is concerned.Strictly speaking, it would improve damping -- but by an imperceptible margin.You should ask the inverse question, too: what if too little ESR? Then it looks like it's parallel with the low-ESR caps already there, and doesn't dampen as well.Best damping is achieved for ESR = Zo.Quote from: Vovk_Z on November 21, 2022, 04:26:34 pmConsidering the input already incorporates electrolytics, I felt safe using the [all encompassing] inclusive-OR.Tim

author: VEGETA
author_rank: Super Contributor
timestamp: November 21, 2022, 11:31:50 pm
content: HelloI have done the simulation with parasitics and more components like my design:- capacitors are 10u with 10mR esr, along with 5nH parasitic inductance... dc bias also taken into consideration thus i lowered the values.- added the same amount of caps in all places like the pcb.input ripple is measured to be 400mv p-p with 50khz but actual psu used is about 100-200mv with maybe as i remember 300khz switching... output ripple is the same magnitude though, plus voltage regulation is not accurate (not an actual issue on real pcb).meanwhile, I will be reading more material suggested by mechatromer and other materials... also trying to think for more additions and modifications which I never tried yet.i am really motivated to do the work so that the next pcb is better than this one.QuoteI will read and respond to your kind post tomorrow.however, i am glad i understood this portion xD.I will invest some time into making these resistor loads beforehand, THEN start doing the measurement. I have small perf boards of different types and shapes, will solder resistors on it and make it as neat and practical as possible.I guess using regular resistors is fine, no need for big powerful power resistors since it will be 1 second or so... except for the continuous one. I may make a DIY power resistor by putting them in parallel. will post you on it for sure with pics.good night for now and will report back soon.

author: Someone
author_rank: Super Contributor
timestamp: November 22, 2022, 01:50:25 am
content: Quote from: T3sl4co1l on November 21, 2022, 11:12:09 pmWith fixed internal compensation, hence the datasheet giving rather narrow ranges of L and C values. That control scheme has average models so it is possible to design an external compensation solution, but without that it will easily become unstable.

author: T3sl4co1l
author_rank: Super Contributor
timestamp: November 22, 2022, 02:22:04 am
content: I can hardly make out any labels on that schematic. It's crammed into the corner of the sheet, labels are overlapping all over.What th... why do the inductors all say "L = 4.7u / DCR = 5n", did you mix up which field is which?Miracle the sim runs at all..!Quote from: Someone on November 22, 2022, 01:50:25 amThat would be true if it used an error amp, but the block diagram clearly shows a comparator and no time constants.Think more along the lines of MC34063 ....but, needless to say, much more advanced, so it actually performs well.The "adaptive on-time" seems to be more the secret sauce. Whether that 'adapts' as part of a control loop, I don't know, at least at a glance. Although there's no indication on the diagram of what that actually means; alas, TI has had poor (inaccurate, or outright disingenuous) diagrams before, and it wouldn't surprise me if that's the case here too.Tim

author: Someone
author_rank: Super Contributor
timestamp: November 22, 2022, 04:04:07 am
content: Quote from: T3sl4co1l on November 22, 2022, 02:22:04 amNot sure I would trust any vendorssimplifiedblock diagrams, even when they claim to show the entire system, unexplainable behaviour shows up in testing (regulators in particular).If you'd like to lift the rug, TI have some ancillary publications SLVA546, SLVAF11, etc

author: VEGETA
author_rank: Super Contributor
timestamp: November 22, 2022, 05:37:23 am
content: Quoteweird, the pdf seems to zoom nicely with me.Quoteall parasitic inductors are 5nH but the outside label is not correct since I copied the inductors from the main L=4.7u, and when modifying it from the model it does not seem to update the outside label.however, maybe you are correct and i didn't update the correct field, I will check again because maybe i didn't update the fields properly.

author: Mechatrommer
author_rank: Super Contributor
timestamp: November 22, 2022, 06:53:45 am
content: Quote from: T3sl4co1l on November 21, 2022, 11:12:09 pmit has been proposed earlier with low side switcher rig, hopefully this time you got his attention. Looks like he's into finding the solution in simulator..

author: VEGETA
author_rank: Super Contributor
timestamp: November 22, 2022, 07:22:10 am
content: Quote from: Mechatrommer on November 22, 2022, 06:53:45 amOriginally I didn't understand that he wanted me to do this test on a separate load... but rather thought full load is only the dreamcast itself. now I know exactly what to do.I will do a very simple rig. just some little boards with resistors on them, hook them to the supply with the scope using alligator clips after preparing it to do either single shot or continuous as agreed.as for simulation, it will go in parallel to all this. won't hurt to try and won't delay the progress.

author: Mechatrommer
author_rank: Super Contributor
timestamp: November 22, 2022, 06:04:09 pm
content: It needs sharp eyes to see mV differences between 20% load and say 80% load if you do switching with hand. If you switch the low side nmosfet with function generator or mcu programmed to output 100hz signal to the nmosfet's gate, you should be able to see that mVpp 100hz on your psu output, then thats your psu load regulation problem. If psu is stable, then problem is something else. If you do the test, post pictures on psu output and what kind of load you are giving it. Then we have better picture what your problem is.

author: VEGETA
author_rank: Super Contributor
timestamp: November 22, 2022, 07:33:43 pm
content: I have finally done all resistor mini boards and here are the tests:https://slow.pics/c/Di7BsJkHeach picture has its name for it, all done via 3.3v rail.quick notes: some readings of multimeter does not match the current, meaning i say 0.5R load and it gives 2.2A @ 3.3v while it should be 1.5 ohms. my multimeter is Aneng8009 and maybe it is not good after many years despite not used a lot.for example, it gives around 1.5 ohms for that 1 ohm 50w resistor.still, i think we have achieved our goad having these figures. however, I don't see much wrong when stepping up or down even when zooming.for your kind review.

author: T3sl4co1l
author_rank: Super Contributor
timestamp: November 23, 2022, 01:45:10 am
content: Sanity checks:- What rail is being tested?- What is the other rail doing?I have no idea!test08_0.5ohm_2.2A_stepdown, test08_0.5ohm_2.2A_stepup: why is this so chunky? Sanity check: real waveforms aren't made of line segments. This is clearly a sampling error. (You can further confirm by changing display mode to points instead of vectors, or enabling sinc interpolation, if these options are available.) Perhaps you took an acquisition at very low sample rate, and zoomed in?Hm, also very visibly aliased. The mostly-flat parts dither between discrete values. Surely the scales used during acquisition are completely different from what's shown (500mV/div, 1 / 2 ms/div).Also, you're saying this thing steps ~3V with a 0.5Ω or 2.2A load? No, that must be power-on/off. So add that to the list:- What test is being performed?I assumed these were all load-step tests, because that's what we were talking about.You can never provide too many details when documenting things!test01_20ohm_130mA: OK so this will be a light-load (burst mode) waveform? Why is the amplitude so unstable? Is that an aliasing problem (too zoomed out), is it interference from the other channel (what's it doing? -- hence why that is important to note!)? Does it change if the other channel is disabled (remove EN, or bias V(FB) up with a resistor, setting its output to 0V)? Does it change if you touch anything in the circuit (maybe it's an instability or sensitivity)?Be suspicious of inconsistencies. Investigate. See what affects them, what correlates with their appearance (did the other channel fire a burst at that moment?), what affects their frequency (repeat rate, wave frequency, pulse length, etc.) and amplitude?test02_1ohm_1.3A: That looks more like the switching ripple I'd expect to see, though it is square not triangular, implying induction from the switching inductor (it's the same shape as the square wave applied to the inductor), or maybe ground-loop voltage. But what the hell are the bursty things? Are they present on every edge, or just erratically? Does anything affect their presence?test03_1ohm_1.3A_stepup: I guess this is 1.3 to 0A step? Why does it rise so far? Or, not very far at all, it's DC coupled and only 0.8V tall? Wait is this V(FB) startup or something?!test04_1ohm_1.3A_stepdown: I guess this is the shutdown then? Why is it slow (an RC exponential, as one would expect!) when test08 is ~instantaneous [as far as the scope can tell]?test05_10ohm_240mA: This is the first one that looks like real actual output ripple voltage. It's smooth, reasonably periodic, a little lopsided as one might expect from a filtered square wave at some odd duty cycle.test06_2ohm_875mA, test07_0.5ohm_2.2A: Essentially identical, but like test02, what are the spikes/bursts? Why is the switching ripple square?Tim

author: VEGETA
author_rank: Super Contributor
timestamp: November 23, 2022, 04:08:57 pm
content: HelloQuotethe rail tested is just the 3.3v rail as I mentioned somewhere above. the 5v rail does nothing but has on-board load resistor of 10k (same as 3.3v), while 12v rail is taken from the input itself, no other load is on it.QuoteI have never missed around with sampling. it says 250KS/s on the scope software for this particular shot for 1ms/div. when I lower the time base, sampling increases. for example 2us/div has 100MS/s.kindly inform me which to choose for such shots.Quotehere is the procedure I went with:I powered the PSU, hooked the scope, and prepared single shot mode. Then I hooked the resistor first lead on 3.3v, then the other lead via a multimeter in current mode. Now I hold this lead and quickly hook it to the GND pin of the PSU , which makes the scope get the reading.Here is a simple diagram for simplicity:3.3v ------ Resistor+ ------ Resistor -----||GND --- multimeter- --- multimeter + ---So it goes from low load (only the 10k on-board resistor) to the specified load. this is the case for all stepup\down pictures.QuoteI assumed it is the case for such low loads too. the amplitude is not constant maybe because I have chosen low time base, but if increased time base will show the full pattern. and no, nothing changes by touching, actually even if kept for minutes it will not change. so stability is ok.Quoteyes I noticed the weird squares and no idea why it is like this. just notice it is 5us. bursty edges are maybe due to low timebase, when bigger time base it may not look the same.QuoteI assure you it went to 3.3v as usual but maybe this is one of the pictures which was not correct. I had ones which went to 3.3vQuoteI zoomed in that is why it looks slow.test08_0.5ohm_2.2A_stepup is for 2.2amps step up, and another test8 is for 2.2amps step down.the only continuous ones are the ones not labelled stepup\stepdown.Quoteif I zoom out, all of them appear constant amplitude.Quotespikes are maybe more visible if we zoomed out, I don't know really.___so after all these measurements, what can we conclude? for me I saw no ringing on step up and down despite sampling wasn't perfect. but they exist on actual Dreamcast load.I am ready for more tests if needed.

author: VEGETA
author_rank: Super Contributor
timestamp: November 23, 2022, 10:49:08 pm
content: Hello,I have checked simulation, and all those parasitic L were 5nH inductance but also 5n DCR. I changed this DCR to be 1m, and done the new simulation. Results here:https://slow.pics/c/SUiVWKDVwaveforms:yellow -> input 12v, has 200mv ripple p-p.green -> 3.3v @ 3 amps.red -> 5v @ 2 ampsI have noticed the exact same square pulsing on the output! is it a coincidence?

author: Mechatrommer
author_rank: Super Contributor
timestamp: November 27, 2022, 11:23:01 am
content: what is this? (A and B) A is about 150Hz 3-5mVpp (also can be seen in test06_2ohm_875mA and test07_0.5ohm_2.2A), where is that coming from? you must figure out where is that coming from. the switching IC? your room? or some ground loop caused by another device in your lab? turn OFF other devices, lamps etc you measure in dark room if you have to. but since your using PC connected DSO, so its difficult to rule out your PC noise. B is what? related to IC switching? or what? you must find it yourself, we cant access your circuit, maybe better to turn on dso channel 2 and see simultaneously the IC switching or Vinput noise (like i demo'ed in my thread linked earlier) thats why many channels dso is important in diagnosing this kind of circuit. does your simulation shows exactly like in the picture? if not, your simulation model is not good enoughymmv.

author: VEGETA
author_rank: Super Contributor
timestamp: November 30, 2022, 10:20:51 pm
content: Quote from: Mechatrommer on November 27, 2022, 11:23:01 amas for A, please check the simulation pictures I linked in previous post. they look very similar, almost identical (check sim last image). we can guess they are related to switching ic.From scope pictures, A is about 1.5uS period = 0.67 MHz, therefore I conclude that it is the switcher since the switcher has a fixed frequency of 700khz. very close so it has to be it, especially that it exists in simulation almost identically.imagine that it is the only thing that exists... I will be overjoyed by 5mV p-p total figure!however for B, which is about 20-30 mV and it happens not in a regular pattern but overall slower frequency. could be the input 12v supply itself since I suspect its switching frequency to be around 300 khz or less.I am out of home for now, will return in days. I will conduct new tests where I will put high continuous current and measure both 3.3v output and the input on the switchers + switchers output directly at inductor (before or after?).then I will remove 4.7uH main L and install 10uH in its place, then repeat the tests as well.so we need to take care of 2 switching frequencies: 700 khz one from the switcher, and the low frequency one from unknown source till now. plus, the 50-60hz due to actual final load as discussed.as for loads in my house, only laptop with PC monitor + mobile chargers (hooked to power strip but no mobile was connected) + neon light (no switching lights). these are the ones in lab room, rest of the house is the same but with an old fridge. no effect is expected.if the 12v source itself was the problem, then why the other psu delt with it correctly? I can use a chinese lab power supply that i got to see if it has other effect.what do you think of this till now? waiting my return to lab + teslacoil's response.current discoveries and discussion seemed to result in making 10uH instead of 4.7u, with a second stage of 1uH instead of the ferrite bead followed by filter caps (including 1 electrolytic). adding to all that a good LDO to deal with 50-60hz stuff if possible. making 2 versions will not be easy but I can manage to put them next to each other and then mouse-bite them together... making 2 versions one with LDO and one without can be time saving. but as agreed, first we need to understand more.thanks

author: VEGETA
author_rank: Super Contributor
timestamp: December 12, 2022, 08:31:29 am
content: I am home and I can resume testing soon.I will perform these tests:1- Remove 4.7uH inductor and put 10uH in its place, then see what is the final result is.2- Use another power supply source, plus measuring ripple and noise of it (and the currently used one). this is to see what type of noise is related to the input source.On another level, I will get this soon (1-2 months):https://www.amazon.com/dp/B082F36D3T/I think it is enough, 60 watts and 10 amps are very good for my needs. there are others available but higher wattage is not required for me at this stage. what do you think about it?

author: VEGETA
author_rank: Super Contributor
timestamp: June 21, 2023, 03:21:52 pm
content: Hello,I have made a new update on this as follows:since I the demand (and my ultimate goal) was to have a true universal AC power supply drop in replacement to original, I decided to do just that. so I have changed the design to take universal AC with the following changes and design choices:- usingRecom power moduleas AC-DC converter which delivers 12v. its size is more compatible than meanwell module but it is not as cheap. it should be better quality.- I addedRC212-0.5-10Mcommon-mode choke since I got advised by many that such AC-DC modules probably do not have enough CMC filtering.- the AC-DC module is filtered by 2x 330uF elec caps + 1uH inductor (similar to 2nd stage one mentioned below) + 2x 1210 22u ceramics + 1u ceramic.- main 12v filter before each switcher is filtered by one 22uF elec cap + 2x 1210 22u ceramic + 1uF 0402 (very close to pin)- switcher IC used isAP62600SJ-7, very cheap and capable.- main inductor used isTaiTech_TMPC1265which has very low DCR of 1.7mOhm which should give excellent ripple performance, it is better than eval board choices. huge size but I managed to make it fit as seen in images. 1uH is supposed to be enough especially that I will operate the switcher at 1.2 MHz.- main filter caps are all X7R ceramics 10uF 0805 and 2 1210 22uF ones as seen. layout made them very close to SW and GND to have good coupling.- 2nd stage filtering also using 1uH inductor but not as good, it is MWSA0603S which has 7.4 mOhm DCR. I compensated for this when choosing switcher output voltage.- all ceramic caps are X7R, elec. caps of 22uF were put in every stage to help dampen the stages according to advice I got. Final output cap of 2nd stage, besides the 2 1210 ceramics, is a330uF solid polymer capwith just 9mOhm of ESR. should give better performance than regular elec. caps for sure while having huge capacitance._________i have made the layout as recommendation, but i am worried about if some of the pours i mentioned in pictures won't solder properly due to large copper without thermal reliefs.for your kind opinion.

author: VEGETA
author_rank: Super Contributor
timestamp: June 22, 2023, 09:21:49 pm
content: Edit: I have modified all zones to have thermal reliefs suitable to each pad... only switcher IC pads have solid connection due to limited space.

author: VEGETA
author_rank: Super Contributor
timestamp: June 24, 2023, 09:18:13 pm
content: I re-arranged some components in a minor way and added proper silkscreen stuff.any comment before sending it to create a prototype?

author: VEGETA
author_rank: Super Contributor
timestamp: August 07, 2023, 05:31:30 pm
content: Hello,I have got the design and tested it. please check images here:https://imgur.com/a/3Lqw5NZI also attached the images with this post. + pictures of it installed.measurement results (ac coupling, short scope spring ground):3.3v no load:mine: 29mV p-porg: 70mV p-p5v rail:mine: 7mV p-porg: 33mV p-p3.3v full load - main menu screen:mine: 47mV p-porg: 70mV p-p3.3v full load - crazy taxi game (should be max it can take in its operation):mine (ripple only): 26 mV p-pmine (ripple + noise spikes): 65mV p-porg: 90mV p-pthe one and only thing that needs changing is ac connector mechanical holes... need to be 1 mm bigger. I filed them to fit this time.honestly, what is your opinion overall?

author: VEGETA
author_rank: Super Contributor
timestamp: August 09, 2023, 08:32:36 pm
content: I wish to remove the 50-60hz big noise spark which is due to the console operating at those frequencies. if these big spikes removed, I will consider the design to be perfect.I will try increasing the output capacitance since original PSU had much more capacitance than this, will see if it works.output currently have 2x22uF ceramics + 330uF solid poly cap as final output caps + 22uF elec. cap for damping.

author: Vovk_Z
author_rank: Super Contributor
timestamp: August 10, 2023, 09:38:42 pm
content: Quote from: VEGETA on August 09, 2023, 08:32:36 pmIDK why your oscilloscope says frequency is 50 Hz or 60 Hz if as I can see pulsations have 100 Hz frequency (10 ms period), which is typical for 50 Hz mains and not enough 100 Hz main filtering capacitance after rectifier (otherwise it's just a pure PSRR of your regulators due to not ideal PCB wiring).For test you may add the same capacutance (or about 50%) in parallel to existing main filter caps and look at those output voltages under load again.If pulsations drop proportionally to increased main filter capacitance - then you see that it must be increased. If it doesn't change pulsations then you have fine filtering but pure regulator PSRR (pure PCB design/wiring etc, IDK).Upd: I see now, main filter capacitor I'm talking about is a high voltage one in that Racom RACM-30 power module. And it has glued case, hard to disassemble...This module gives you a lot of 100 Hz pulsations and it seems to me your posr-regulators don't do much with it.

author: T3sl4co1l
author_rank: Super Contributor
timestamp: August 10, 2023, 11:13:52 pm
content: I think you're misunderstanding (you're not alone, the same confusion was had much earlier in this thread). It's not line frequency, it's update rate of the console -- he's done (almost?) all load testing with the real system. So you're seeing the pulsing load as the CPU/GPU prepare a frame, every frame.Scope appears to be 10ms/div and pulses repeat 20ms or 50Hz, must be a PAL 50Hz version?Edit: a bit less, 6 cycles in 5 divs = 60Hz.Tim

author: Someone
author_rank: Super Contributor
timestamp: August 10, 2023, 11:30:32 pm
content: Quote from: T3sl4co1l on August 10, 2023, 11:13:52 pmThat's this thread 100%, no 200%. It's trivial to simulate what more capacitance will do for the 50/60/100/120Hz noise/ripple, and experienced people already know exactly where this is headed. But the OP is set on their methods and isn't planning to expand their skills/knowledge.

author: VEGETA
author_rank: Super Contributor
timestamp: August 11, 2023, 09:57:25 am
content: Hello,I wanted to do this update yesterday but couldn't because forum didn't work on my browser. Now using portable browser.I added 3x2200uF at the final filtering stage to get rid of that low frequency spike and it worked as intended. please check the attached image which is full load while running a game.Now only the 50-60 hz ripple or power sips which are as previous reply mentioned, just the console update rate which is typical and is seen on the original power supply itself.Yesterday tried many many capacitance variations and looks like the key is high bulk caps at the very end to deal with power sipping demands. today if I get time I will try and add more caps at different stages especially after the module itself to see what difference will it make overall and how the module will tolerate it. the result in this image looks like the perfect form already, I don't think we can get rid of these cycles right?next and final revision is where I will add the new caps to 3.3v rail and this time will make them through hole caps to save space (and cost), will add another low esr solid cap as well. so it will be total of 3x2200uF elec + 2x 470uF solid + 2x 22uF 1210 X7R ceramic. as for 5v rail it is good the way it is now.

author: VEGETA
author_rank: Super Contributor
timestamp: August 11, 2023, 04:54:37 pm
content: Here are some new measurements.I probed the module output after filter stage (just before the switchers), and as it seems even adding many capacitance didn't remove the 50Hz component. I tried adding 4400u and 6600u caps but no use either on its own measurement or at final 3.3v.I also added 8800u for 3.3v rail (full_load_game_3v3_8800u picture) and as it seems a maximum of 20-25mV p-p total figure with 0 noise of any kind. I also tried making it 9800uF but didn't improve much, 6600uF also was slightly worse but overall similar. main menu is 50Hz since the console is PAL but game is NTSC crazy taxi thus 60 Hz.therefore, I have made the following changes to be done on upcoming test sample:- use 3x 220uF caps for main module pi filter instead of the 2x 330u ones.- use 1x 220uF cap for each switcher input instead of 22uF elec one while keeping everything else.- use 3x 2200uF caps for 3.3v rail final output + 2x 470uF solid polymer caps (instead of 1x 330uF).caps are Lelon through hole RXW series which are low ESR and long life:220uF elec.:https://www.lcsc.com/product-detail/Aluminum-Electrolytic-Capacitors-Leaded_Lelon-RXW221M1CCC-0611P_C916211.html2200uF elec.:https://www.lcsc.com/product-detail/Aluminum-Electrolytic-Capacitors-Leaded_Lelon-RXW222M1ABKF1020_C2920647.html470uF poly:https://www.lcsc.com/product-detail/Solid-Capacitors_Lelon-ORZ471M0JBK-0608_C434469.htmlorhttps://www.lcsc.com/product-detail/Solid-Capacitors_Lelon-ORK471M0JBK-0608_C176697.htmlthese caps are certainly better for SMPS (labelled this way from manufacturer too) than previous SMD ones, and for sure better than the crappy ones I tested now (with very dirty soldering job).I am confident that this will keep it (and maybe make better than) maximum of 25mv p-p absolute full load. I mean, realistically can't be better than this TBH. I consider this the best available design from my side, extremely low ripple due to console itself and 0 noise. even by its current no big bulk caps readings it is already 2-3x better than original PSU.I remember once that we spoke about LDO capability to eliminate such 50-60hz but now I am satisfied with this. I may try making an LDO version as a future testing and learning project though.for your kind opinion.

author: VEGETA
author_rank: Super Contributor
timestamp: August 12, 2023, 08:33:39 pm
content: Hello,more interesting tests.I have done 2 tests tonight:1- using DC load itself, not the final console.2- using a 1 ohm power resistor.as seen below in images (with description)... the design looks very good. the measurements showed 2mv p-p final noise and ripple figure at full load, even similar reading on previous stages like 1st filtering stage and 12v rail.however, in dc load 3.3v and 5v @ 3 amps measurement pictures you seem some random (yes random, did it many times to verify this) spikes and stuff happening above the 2mv p-p figure. this is for sure due to long wiring from the device to the dc load connection + input connection (lots of wiring). notice that switcher is running at about 1.2 MHztherefore, I wanted to do a pure resistor load with short wires (and no input to AC power outlet, no noisy psu supplying it...etc) and the results were very nice! 2mv p-p on 3.3v and about 3v p-p for 5v.notice that 3.3v rail has the extra 3x2200uF caps while 5v does not. these caps are necessary for final connection of the device on the console to be able to supply the huge power sips mentioned above. they are only required for 3.3v not for 5v though which is nice!I attached the pics of my setup for reference.I am very satisfied with this result, especially when I see it on the final design (with new elec caps mentioned before).what is your honest opinion after this marathon?

author: Vovk_Z
author_rank: Super Contributor
timestamp: August 15, 2023, 04:19:38 am
content: Power rails look nice and clean now. (Working with pure resistive loax with short wires). Using just pure resistor you may identify pulsation and noise of you power supply more esily. Addind your pulsating load you'll know output impedance of your power supply.Those spikes can be not connected with your power supply. It can be anything like WIFI or LED lights or IDK. But it is good to investigate and find a reason otherwise you can't call your design 'low nose one'.

author: VEGETA
author_rank: Super Contributor
timestamp: August 15, 2023, 05:17:40 am
content: Quote from: Vovk_Z on August 15, 2023, 04:19:38 amyes after putting the resistive load I saw the waveform as mentioned, just about 2mv p-p. the 50-60hz ripple is just the console sipping power at those rates which can't be negated, at least with conventional means.By "pulsating load" you mean what exactly? the 50-60 hz stuff is the console as mentioned.I don't have LED lights, and for wifi it is not so close to the setup too. the same result is using the original power supply, meaning showing the 50-60hz cycles but at higher amplitude than mine.I put a big common-mode choke on the ac side before the power module (which has its own), this was the key to filter all noise from the source. in previous designs, i couldn't beat the original power supply in this particular area. the original power supply always looked cleaner due to big and good CMC but after adding it to my design, it got the same.what do you suggest I test next?

author: Vovk_Z
author_rank: Super Contributor
timestamp: August 15, 2023, 06:46:04 pm
content: Quote from: VEGETA on August 15, 2023, 05:17:40 amYes, the pulsating load is your console.

author: Vovk_Z
author_rank: Super Contributor
timestamp: August 15, 2023, 07:09:51 pm
content: Quote from: VEGETAThis topic became qute large so I don't remember if there is a suggestion for you to read some helpfull books about noise and related things.1. Highspeed digital design. A handbook of black magic. Howard Jonson, Martin Graham.2. Noise Reduction Techniques in Electronic Systems. Henry Ott.Those books give you a full.picture.

author: VEGETA
author_rank: Super Contributor
timestamp: August 15, 2023, 09:11:31 pm
content: Quote from: Vovk_Z on August 15, 2023, 06:46:04 pmOk, but you saw the pictures right?I mean, I tested it on the console with different capacitances and this is the result which is about 6600u is more than enough.the original power supply (schematic here) shows similar result but higher amplitude. Meaning no noise or spikes...etc which means the setup or power grid is not an issue.However, original one for 3.3v rail has 1800u + 1000u + 470u + 6.8uH in between for PAL PSU, linked schematic is for NTSC PSU. this is a bit different than mine since I used 1uH inductors and higher frequency.so the key was higher bulk caps since the pulsating load is very low frequency. Previously, it had another problem of high frequency noise and common-mode noise, this got fixed after using very good power module AC-DC with very good CMC + nice layout.I have made the changes to add 2x3300u caps+ 2x470u polyto 3.3v which should be a lot better than currently added bulk caps (crappy chinese + ugly solder job).Such very low ESR bulk caps should give very fast response... I am hoping that it could enhance it even further, we'll see.3d image is attached, those are very huge caps for sure xD. 16mm diameter.as for further reading, yes will do it in future. but i feel this psu is already very good in terms of noise and ripple don't you think so? further readings will be for my own development and knowledge.

author: Vovk_Z
author_rank: Super Contributor
timestamp: August 16, 2023, 11:40:25 am
content: I see your 3300 uF caps are much larger then 2200 uF (16 mm vs 10 mm?) So, then 3x2200 uF may have sense. I have used 2200 uF x 6.3 V (for 3V3 rail) and they have 10 mm diameter. That's much smaller then 2 x 16 mm 3300 uF caps.

author: Vovk_Z
author_rank: Super Contributor
timestamp: August 16, 2023, 11:44:15 am
content: Quote from: VEGETA on August 15, 2023, 09:11:31 pmIf it is now better than original then ok. With proper knowledge taken from those books you may do even better.

author: VEGETA
author_rank: Super Contributor
timestamp: August 16, 2023, 04:49:35 pm
content: Quote from: Vovk_Z on August 16, 2023, 11:40:25 amafter reading a lot and changing my mind a lot, I came to love Samyoung NXH series of elec. caps. they do have 2200u ones but they are 12.5mm, having 3 of them costs more than double the 2 of 3300u. 3300u now fits ok as seen. LCSC does not have much of this series unfortunately.I do have 2x470u polymer ones which will assist a lot, so all and all it should be better than I got now.QuoteI will continue to learn for sure. the noise book from 1988 seem nice but old, surprise to see nothing new written on the subject.

author: T3sl4co1l
author_rank: Super Contributor
timestamp: August 16, 2023, 05:23:30 pm
content: Quote from: VEGETA on August 16, 2023, 04:49:35 pmAge means nothing -- the theory of electromagnetism was well developed within a handful of decades of its discovery; the only thing that has changed is the ease with which, and the means by which, we are able to interact with the EM field.There is very little in this book that wouldn't be familiar to, say, the eggheads at Bell Labs wholly a century ago (Zobel, Campbell, et al.), or to even more rarefied groups almost as long again prior -- physicists, or more generally "natural philosophers" as it was at the time: Hertz, Helmholtz, Maxwell, etc.. Even Faraday, despite his reluctance (or perhaps ignorance) for mathematics, probably would've understood much of the concept, purpose and method of the book, perhaps inbetween marveling at the depth of modern technology of course (that we have to deal with waves on a regular basis, not just the E and M separately, that concerned his experiments; not to mention the ease with which we generate said waves).In other words -- the enduring value of books like this, are the fields (literally, in this case) they deal with. EM itself does not change, only the technology we use to interact with it; and our analytical methods to approach it.If you compare to a book like Terman'sRadio Engineer's Handbook, or F. Langford-Smith'sRadiotron Designer's Handbook, the mathematical approximations used were much cruder -- the engineer might be working on pencil and paper, slide rule in hand -- and plotted data (nomographs) and empirical measurements were the tools of choice when blindingly-simple equations didn't suffice. Whereas today, not only are more complicated formulas feasible (consider the formulas in common circulation for microstrip impedance, for example), but algorithms entirely, since everyone and their dog has a computer available at all times.Which are still excellent references, by the way. The simplicity with which they approach problems is refreshing, and the results are no less effective -- we just might have tighter performance demands nowadays (squeezing out every dB of SNR and DR, while minimizing circuit size and power consumption, say), which sometimes suggest alternative solutions, but generally the conventional topologies work fine, or at the very least as starting points.A contemporary case being the development of electric wave filters, at first single-pole (RC or LR), then k-derived (using a transformation that's easier to work in, resulting in circuits containing poles and zeroes which hampered performance but made them easier to work with), then m-derived (a more general method), and eventually analytical theory (by the... 40s or so, I forget? Crowned by Zverev'sHandbook of Filter Synthesispublished finally in 1967), which in sense fully and completely perfected the art. Since then, optimization tools have addressed minor and more practical aspects of filter design: accommodating component selection by commercially available values; ensuring performance over component tolerances; and reducing engineer time by automating much of the process. Not to mention incorporating transmission lines or full field simulation into the process, a critical step for microwave circuitry.Or for a more direct case: not that exceptionally low power supply impedance was much of a concern back then (tube circuits are fine with some ohms), but most any of these authors would see your optimization problem, and a system diagram, and ask: why not simply increase error amp gain? Or since you don't have control over it (internal to the IC), why not choose a regulator with higher gain? It's surely cheaper and more compact than trying to stuff oversized capacitors into the box!They would also have the wisdom to ask: do youreallyneed this? An intrepid one might even perform measurements on your load to see how much ripple it can tolerate before malfunction occurs, and set a maximum at the power supply of a modest fraction below the critical level.Tim

author: Sniper1
author_rank: Regular Contributor
timestamp: August 16, 2023, 05:40:22 pm
content: Maybe the ERS to to low and it is not properly compensated for modern caps .SMPS need some compensation, well basically if the output caps are very low ESR they may respond to fast and that messes up with the FB loop and it picks random noise and amplifies it (or potentially osculates)

author: VEGETA
author_rank: Super Contributor
timestamp: August 16, 2023, 05:55:45 pm
content: Quote from: Sniper1 on August 16, 2023, 05:40:22 pmall of these are for 2nd stage filtering. I do have first stage filtering after switcher which has a 22u elec cap (high esr) to act as damper as agreed in previous pages.so, having low esr at final output should not affect anything badly in terms of stability. feedback loop is taken from 1st stage not end of 2nd stage.Quotewell, as you saw in waveforms everything looks fine now with 2mv p-p ripple except that 50-60hz power sips which as it seems can't be fixed. I have no problem with it also since it exists on the original power supply itself, mine is actually better. those caps now fit nicely, the system seems to need such caps due to its power sipping at low frequency, original psu also has big caps and bigger inductor as well.

author: Someone
author_rank: Super Contributor
timestamp: August 16, 2023, 10:52:15 pm
content: Quote from: VEGETA on August 16, 2023, 05:55:45 pmWhich is trivial to fix, and the answers have been provided several times in the thread.

author: VEGETA
author_rank: Super Contributor
timestamp: August 16, 2023, 11:39:15 pm
content: Quote from: Someone on August 16, 2023, 10:52:15 pmI believe previously we mentioned that an LDO can fix this issue, but I didn't want such solution and still don't.Besides that I assume I have followed everything else. Like, first I changed the entire design and used a complete solution with AC-DC power module + good CMC to ensure input power is good since this was an issue before or at least uncertainty.previously it had ringing + noise, we reached a conclusion of using 22uF elec. caps on everywhere possible to dampen the system... which I did and looks like it proved its worth. Now there are zero noise spikes or ringing of any kind. especially after adding bulk capacitance on 3.3v rail. the 5v rail is fine without anything extra.adding the elec. caps (with higher ESR) is the replacement solution of adding snubber circuits, as it does the same job. but a quick rough calculations on 3.3v rail for the new modification: it has a total of 7690uF capacitance and 2uH inductance for the total of both stages assuming no capacitance dc bias.for that, Zo= sqrt(L/C) -> sqrt (2/7690) = 0.016R. Previously got mentioned that after calculating this, it should be added in series with one of the caps at the output. I can add it in series with an extra 22uF elec cap but since it is so low, I assumed that elec. cap ESR will do the job just fine and this was the recommended solution.for the recent test, I put 3x2200u bulk caps which did the trick of removing the last power sip spike and now it is just regular 50-60hz consumption.I want to emphasize that this 50-60hz thing exists in original psu itself despite being made professionally by sega themselves. do you think they could have fixed this or is this the way to go? actually, its amplitude in original psu is worse than mine.so in your opinion, I need to do what besides all that? should I specifically add external snubber circuit using the data from the newly chosen elec. caps?

author: VEGETA
author_rank: Super Contributor
timestamp: September 24, 2023, 05:11:59 pm
content: pics:https://imgur.com/a/Cyt5WCpmeasurements:https://imgur.com/a/IbU18zAnew and final model arrived, tested to be fine and according to expectations.