My PSU design ripple and noise with picture measurements

[VEGETA]

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

done.

- 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.

[BrianHG]

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.

[VEGETA]

done.

[Faranight]

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.pdf

Cheerzies!

[T3sl4co1l]

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

[sandalcandal]

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.

I actually saw a masters thesis presentation earlier this year where coupling from a shielded inductor 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

[VEGETA]

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.

[T3sl4co1l]

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.

I actually saw a masters thesis presentation earlier this year where coupling from a shielded inductor 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

Hah, 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

[VEGETA]

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.

[VEGETA]

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 check


to do list:

- silkscreen stuff like component tags and so on.

[VEGETA]

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?

[BrianHG]

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.

[VEGETA]

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.

[BrianHG]

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_Kd54g tears 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.

[BrianHG]

Just in case you want in the future:

http://electronoobs.com/eng_arduino_tut155.php

Aduino 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.

[VEGETA]

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/

[VEGETA]

I have arranged the silkscreen stuff properly now. Currently doing the BOM.

[VEGETA]

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?

[BrianHG]

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.

[VEGETA]

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.

well, 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.

[Vovk_Z]

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).

[VEGETA]

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).

sub-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.

[BrianHG]

well, 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.

Yes, 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=1046.7uf
Divide 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.

[VEGETA]

well, 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.

Yes, 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=1046.7uf
Divide 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.

I 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.

[Vovk_Z]

what is your recommendation then?

I 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.