Low ripple low noise small power supply design

[BrianHG]

So you removed the EMI circuit in the bottom for 5v and op-amp? you took them from the 12v output to the DC itself, wouldn't this cause noise and ripple to get into the 5v and op-amp?

There is no EMI there.
And if there were, it would be attenuated by a 100 ohm series resistor while on the other side, it would look like a <0.05 ohm short to GND at 100Hz thanks to the 1000uF cap.  It would look line a <0.0005 ohm short to GND @ above 500KHz thanks to the 10uF MLCC cap in parallel.  The attenuation in the high frequency EMI range is greater than 100000:1 while the regulator's and opamp's PSRR at 1KHz attenuate that by another 10 fold, not to mention at 100Hz they go bonkers and attenuate it by a good 60db (another 1000 fold) each, not to mention the 5v reference goes through a 3.3k series resistor and through another 10uF MLCC cap.  This is utterly insane.  if your current noise on the audio or analog video was 0.1vp-p, a mild visible annoyance, or continuous audio tone with the volume with loud headphones, the supply for the linear reference and opamp will be 5 orders of magnitude less, or 10000 times cleaner.  This is a tactical nuke eliminating a fly.

As for the 1uH, anything 3amps or above will work.
As for the 10uH,  the 1amp I listed will be fine.

As for the 3 or 4 1000uF.  I didn't notice how big they were.  Maybe using double @470uF.  Except for the linear section, 1x 470uF would still be fine as well as 1 at the +12v input.  I would use the extra space for placing additional 470uF caps on the Dreamcast's +12v.

[VEGETA]

There is no EMI there.

But it is taking 12v from a switching supply. Yes it is low frequency but still switching ripple and noise... right?

It would look line a <0.0005 ohm short to GND @ above 500KHz thanks to the 10uF MLCC cap in parallel.

how do you know these exact numbers? I know the RC filter removes ripple and noise to some degree but I cannot know details such as its performance at a certain frequency or so.

while the regulator's and opamp's PSRR at 1KHz

from the datasheet or where?

As for the 1uH, anything 3amps or above will work.

yes it is, but slightly bigger than your suggested one. I think it is the 6 mm package or so.

As for the 10uH,  the 1amp I listed will be fine.

1A? I could use the same part I used for the switching supplies since it is 6mm package... this way is cheaper I guess.

As for the 3 or 4 1000uF.  I didn't notice how big they were.  Maybe using double @470uF.  Except for the linear section, 1x 470uF would still be fine as well as 1 at the +12v input.  I would use the extra space for placing additional 470uF caps on the Dreamcast's +12v.

looking into jlcpcb smt parts, there seems to be all 10x10 mm parts except if you go really low like 100uf or so. 1000uf is the same size as 470: https://lcsc.com/product-detail/Others_Lelon-VE-102M1C1010-TRO_C249474.html/?href=jlc-SMT this one is 16v which is the biggest rating.

Hmmm so getting those 1000uf 10x10 seems to be the best solution since all the same size. getting many of 100uf isn't space-friendly.

[BrianHG]

It would look line a <0.0005 ohm short to GND @ above 500KHz thanks to the 10uF MLCC cap in parallel.

how do you know these exact numbers? I know the RC filter removes ripple and noise to some degree but I cannot know details such as its performance at a certain frequency or so.

This isn't too difficult if you look at the capacitor chart I posted on the previous page:



For simplicity sake, we will use the 470uf and 22uF MLCC caps.  IE, 1/2 the 1000uf cap and 2x 10uf caps in parallel.
The chart labels these as separate impedances, not both components in parallel which would be similar to adding 2 resistors in parallel.  I assume you know how to add 2 different parallel resistors together.

Let's concentrate on just the 22nF cap, the cyan-blue line on the left chart.
At 100Hz, you can see it is 100ohms.  This means if you place this cap after a 100ohm resistor to GND, feeding a 1v 100hz sine wave signal into the 100ohm resistor means on the other side, 100ohm -> cap which = 100ohm to GND @ 100Hz, your 1v 100Hz signal will now be 0.5v.

Now say we feed a 10Khz 1v sine wave into the 100ohm resistor, well now, the cap at 10Khz looks like a 1ohm resistor to GND.
The formula here is the same voltage attenuation formula, 1ohm/(100ohm + 1ohm)= 0.0099v 10Khz sine wave at the output of the resistor, or we can call that 0.01v.

Do the same for 1Mhz and it's 0.001ohm/(100ohm+0.001ohm) = 0.0000099999, or we can call this 0.00001, or 10000:1 attenuation.  Assuming I didn't get my decimal places incorrect.

For the purple 470uf trace, a 1000uf cap would run a little lower in resistance in the middle, but be ~half the resistance down at the 100hz location.

As for the regulator and opamp, there is a specification in their datasheet called PSRR, or power-supply-rejection-ratio or sometimes called 'Ripple Rejection'.  This tells you how much the device attenuates down the input signal at a given frequency.  The on-seminconductor MC78L05 datasheet says it's PSRR when powered at 10v driving 40ma is 49db @ 120hz.  (Not the best one, but ok.)  So going to this site, I put -49db into the calculator:

http://www.sengpielaudio.com/calculator-db.htm

And get: 0.00354.
Looking at an 100ohm to 1000uf cap at 100hz, it's a little less than 0.01, multiplied by that regulator's -49db PSRR 0.00354 gives you 0.0000354 of your original 100hz signal before all the in place filters to after the regulator.

If you old circuit generated a 1v 100hz hum, after all this, that 100hz hum would be ~0.00004v.
So, a 0.1v 100Hz hum would become ~0.000004v.

[BrianHG]

LM358 datasheet PSRR: Worst case 65db, normally 100db (between 0.00056 and 0.00001) :

[VEGETA]

I made the changes.

I hope I can fit all of those 1206 10uF caps + 1000uF elec. caps on that tiny board... and most importantly, leave place to mount the heatsink on the mosfets. Once we finish modifying everything I will think about the heatsink, most probably it is going to be press-fit. I just hope it conducts well and doesn't get loose over-time.

My understanding of PCB layout is this:

I put all switching stuff on one portion of the PCB, like the upper side... make its ground pour on its own. Then make the same for linear regulator mosfets, and another private gnd pour for the 5v regulator. Then  connect all grounds together via thick traces (since some will carry big current right?).

I guess by this we ensure switching current and its noise stays on its ground and never make it to linear side since it is lower resistance there than the trace to other grounds.

[BrianHG]

My understanding of PCB layout is this:

I put all switching stuff on one portion of the PCB, like the upper side... make its ground pour on its own. Then make the same for linear regulator mosfets, and another private gnd pour for the 5v regulator. Then  connect all grounds together via thick traces (since some will carry big current right?).

I guess by this we ensure switching current and its noise stays on its ground and never make it to linear side since it is lower resistance there than the trace to other grounds.

Everything looks good.

Excellent, you are aware of the impedance of the GND layer itself.
You got the right idea.

On the switching side, you need to keep that GND & VCC path from the switchers diode & Inductor as tight & well thick as possible while all the feedback and control paths can be thin.

Make sure when you order the PCB, choose 1.5oz or 2oz copper thickness.  If I remember, from JLPCB, on 10 PCBs, the price increase was only around 25c per PCB, but, that's more than double the thickness compared to the standard 0.5oz.

The thick copper means trace spacing, via angular ring and drill size needs to be a bit larger.  Something like 12 mil drill instead of 8mil.  (These figures are a few years out of date.)

For copper fills, I usually tend to make the clearance of 12-15mil.  Don't be the one who sees the PCB fab says their trace-trace clearance needs to be at least 7mil and the copper flood fill to that tiny 7mil.

The rest of the PCB is so few in traces that you cannot do wrong if you manually place & route the thing.

Remember to stitch GND vias all around the bottom fill and under the switchers & decoupling caps.  Some vias, occasional partial lemmons can have as much as a >1ohm impedance and pass QC test unless you have specified specific impedance matching quality PCB, not the cheap quick ones.  Having a bunch eliminates this threat as such a high impedance via is rare, but grows if you are pushing the drill hole size down to the lowest limit.

I like 1 side = switchers, 1 side = linear.
Try to get most tracing on the top of the PCB except for some extension to the bottom.

On the top switchers, you want to also try to get their GND trace to be 1 solid piece as well when concerned with VCC, IC, diode & coil caps.  Then via-stitch along the entire central mass.  As for any components or feedback signals which need to be tied to GND, you may tap the GND place below if so long as it is not a power switching load.  The AOZ1284PI datasheet should provide an example layout.

[BrianHG]

Have you looked at 47uf 16v X5R 1206/1210 caps?
You could use half the number of 10uf caps.

[VEGETA]

I like 1 side = switchers, 1 side = linear.
Try to get most tracing on the top of the PCB except for some extension to the bottom.

component placement will all be on one side, which is say top. However, traces can be of different planes. My suggestion meant that at the top face of the board where components are sitting... I could gather all switching stuff on one area while all linear stuff on the other one... and also do the switching traces on top and linear traces on bottom.

Have you looked at 47uf 16v X5R 1206/1210 caps?
You could use half the number of 10uf caps.

There are some options but double the price. I will see, if the 10uF ones fit the board then ok.

________

I want this to be fully functional using JLCPCB service... then when I plan to sell them I will look into making a small volume maybe from a different manufacturer and assembler. How much do you think it would cost approximately?

Like a panel of 280x280mm can have 25 of it. Let's make say 10 panels (can be done through jlcpcb service if you notice). This means 250 boards!

[VEGETA]

To make you laugh, please look at the PCB. Still nothing done but look at component size xD. what a joke... all components on one side 

[BrianHG]

  That's MAD! 

You will probably have to live with only 2x 1000uf.

Maybe cut the 10uf in half.

[BrianHG]

The linear and switching sides just need to be separated -(good luck)
Having the bottom almost all GND is your bigger + with regard to EMI and noise.
You just want a separate GND path from the +12v in and the linear GND and output power.
Basically a 'crack/channel' in the GND and the 10uH inductor sitting over that gap, with both decoupling caps on each side.

Same thing for each switching supply with their 1uH inductor.

It not about reserving a layer for linear/switching, it's just separating/channeling out each parts GND to make them appear as a separate module.

Also, just painting the entire bottom as GND may be the best solution if you cant do the channels.

[BrianHG]

Just in case, make sure the positioning of the 2 mosfets and other components around them will allow that 1 wide heatsink you found to be taped on-top.

[VEGETA]

I removed a lot of 10uF caps while converting the rest to 22uF using 1206 package + removing about 2-3 1000uF caps... STILL no way near fitting them as you can see!

I started thinking about putting all small components on one side of the board and let that be the one JLCPCB assembly service take care of... while I solder manually the big components on the other side of the board. How about that?

Gonna take a lot of time obviously but for 50x50mm board this is the only solution. TBH, the small components are too much, they are the ones clogging the board not the big components.

So stuff like 1000uF caps, 10uH inductors, even some 1206 caps can all go to the other side of the board while everything else can be SMT assembled.

BTW, do you know about PCBWay SMT assembly service? I saw people say it is like JLCPCB but better. Like getting colors and both sides assembly...etc but they source the materials.

[BrianHG]

Strategically, I would place the 10uH, 1000uf  and the 12vside 10uf associated with that 12v side filter on the bottom.
Maybe place that Dreamcast power connector on the bottom right, or move it down a bit so the the 2 plastic fingers may slightly go over the edge.

JLPCB were to wave a panel, then only wave compatible SMD components may go on the bottom.  You cant do that with the 1000uf caps.

As for the switchers, make sure both look wired equivilant.  I see their 10uh wired on different sides.

You can also go down to a SOT23 78L05 which only can drive 35ma if memory serves, but, you are only using a fraction of that.

Cutting 10uf in half is ok, except for the output of the switchers.  Keep 2 of them there instead of 3 of them.

[BrianHG]

A more sane solution would be to slightly lengthen the PCB so you get 4x5 = 20 on a panel.
Remember, a panel is 400x500, not 400x400, so in theory you can still lengthen the PCB slightly and still get 5x5 or a good bit larger 4x5 panel.

Also don't forget the 2oz on top and bottom layer is you want extra low impedance traces.

[VEGETA]

Strategically, I would place the 10uH, 1000uf  and the 12vside 10uf associated with that 12v side filter on the bottom.
Maybe place that Dreamcast power connector on the bottom right, or move it down a bit so the the 2 plastic fingers may slightly go over the edge.

JLPCB were to wave a panel, then only wave compatible SMD components may go on the bottom.  You cant do that with the 1000uf caps.

As for the switchers, make sure both look wired equivilant.  I see their 10uh wired on different sides.

You can also go down to a SOT23 78L05 which only can drive 35ma if memory serves, but, you are only using a fraction of that.

Cutting 10uf in half is ok, except for the output of the switchers.  Keep 2 of them there instead of 3 of them.

JLCPCB lets you decide which side you want to assemble... I will put all small stuff on bottom layer and let that be assembled.

Top side will have my logo and name..etc + 2 mosfets with their heatsink + all large caps and inductors. notice that 1uH inductors are 0603 so they are on bottom.

with this approach I can put more caps like before.

There are no 10uF caps now, all 22uF as you can see. output of switchers is now just x2 22uF 1206 ones. EMI filter now using x1 22uF before and after the inductor instead of x2 10uF.

As for heatsink, is the one I posted good enough? also, what should I buy to be able to stick it firmly so that it conducts well and doesn't get loose by time or by movement.

If we finalize this, I can start doing the PCB. If I wanted JLCPCB smt service only, I will be forced to put everything on one side + make the board taller which is not nice. hand solder stuff is easier, and I will get them in reels in quantity.

I think the only stuff needed to be hand soldered are:

1000uF caps (I can put more now xD).
2 mosfets (I can put them on assembly side but heatsink should be on top to get more air).
10uH inductors

Also don't forget the 2oz on top and bottom layer is you want extra low impedance traces.

isn't it 1.6 by default.

[BrianHG]

isn't it 1.6 by default.

Make sure.  I think that's 1oz copper + .6oz plating.
I was asking for 2oz copper + 0.6 plating.
The last PCBs I made had little impact on the price of double thick copper, something like 50cents a PCB.  However, they were 4 layers.

[BrianHG]

I hope you are testing a 1 or 2 PCBs before building 250pcs...

[langwadt]

isn't it 1.6 by default.

Make sure.  I think that's 1oz copper + .6oz plating.
I was asking for 2oz copper + 0.6 plating.
The last PCBs I made had little impact on the price of double thick copper, something like 50cents a PCB.  However, they were 4 layers.

so we are past the tactical nukes, Tsar Bomba is what it takes

[BrianHG]

isn't it 1.6 by default.

Make sure.  I think that's 1oz copper + .6oz plating.
I was asking for 2oz copper + 0.6 plating.
The last PCBs I made had little impact on the price of double thick copper, something like 50cents a PCB.  However, they were 4 layers.

so we are past the tactical nukes, Tsar Bomba is what it takes

I once got quoted on a 4oz copper PCB.
Pricey and the PCB fab recommended clearances >10mil, but, you better believe those traces where low in impedance.
It was a high power PSU & Stepper motor and solenoid driver board.

[tszaboo]

1 last addition, I would add 3-4x more 1000uf caps on the Dreamcast +12v side + a single 1000uf cap at the V+12 input.

Nah, he should add a bunch of 100.000 uF caps everywhere with a load of 1000uH inductors, because that schematic is not too big of an abomination already. And please make it star ground.

Seriously, can you guys please use some common sense?

[BrianHG]

1 last addition, I would add 3-4x more 1000uf caps on the Dreamcast +12v side + a single 1000uf cap at the V+12 input.

Nah, he should add a bunch of 100.000 uF caps everywhere with a load of 1000uH inductors, because that schematic is not too big of an abomination already. And please make it star ground.

Seriously, can you guys please use some common sense?

LOL.....
I only helped out with someone who 'Asked' for the death of all outputs...

Too bad those ultra-low EMI switchers from TI I listed 2-3 pages back weren't available.  Used with the 1uH emi filters at the input + another at the output would have been enough as their load regulation and ripple far out-performs the AOZ switcher almost 10fold even without the additional output filter.

[langwadt]

1 last addition, I would add 3-4x more 1000uf caps on the Dreamcast +12v side + a single 1000uf cap at the V+12 input.

Nah, he should add a bunch of 100.000 uF caps everywhere with a load of 1000uH inductors, because that schematic is not too big of an abomination already. And please make it star ground.

Seriously, can you guys please use some common sense?

https://images-na.ssl-images-amazon.com/images/I/61yK53-z0CL._AC_SL1004_.jpg

[BrianHG]

1 last addition, I would add 3-4x more 1000uf caps on the Dreamcast +12v side + a single 1000uf cap at the V+12 input.

Nah, he should add a bunch of 100.000 uF caps everywhere with a load of 1000uH inductors, because that schematic is not too big of an abomination already. And please make it star ground.

Seriously, can you guys please use some common sense?

https://images-na.ssl-images-amazon.com/images/I/61yK53-z0CL._AC_SL1004_.jpg

They didn't install one of these:
58f 16v cap
So it's pure junk...

[VEGETA]

I managed to place the components as discussed. I think now it is time to route.

The white square on top side is where the 25x25mm heatsink will go, I drew that to make sure no component come inside that area. I still need to fix the silk screen components of a lot of parts!