Low ripple low noise small power supply design

[BrianHG]

Nice except, I cannot tell where in the schematic one of the 1000uf is connected.
The Dreamcast side 1000uf should be on the linear side...

If both are after the 10uf choke, then both should be on the linear side.
That weird round path the GND need to take through one of the switcher's isn't good at all.
I know you tried to work with a 25x25mm heat sink, but that layout isn't sound in isolating the switching noise from the linear.
You linear GND needs to cross above or circle around below the switchers creating a fairly good antenna.

If you keep your connectors where they are, the only clean solution is having the 2 switchers at the top of the PCB and the all the linear at the bottom row. including the Dreamcast +12v 100uf cap.

There is just no space...

Moving J4/J5 and the power out closer to the edge might help.
If that power connector U plastic finger shape is plastic above the connector, you may over-hang that at the edge of the PCB as long as when being panel assembled, the plastic doesn't interfere with components on the adjacent panel.

You haven't seen any rectangular heatsinks, like the one I mentioned which was 12x25.


If you are trying to keep this layout, the only thing you can do is move C8 right next to C16/ swap those 2 around.
Route the 12v output of the choke around the outside of the PCB to C8.
Also move 1/2 of the output 10uf & 100nf filter caps from the 12v choke where C8 is.

If you are keeping the mosfets where they are, rotate them 180 degrees.

The 2 mosfet load output caps and resistors should be near/inbetween the mosfet and op-amps instead of by the connector.
Maybe even place them on the other side if that is the side you are wiring the output to your power connector.

The wiring between them and the connectors needs to be nothing more than a wire.

That's it for now...

[VEGETA]

I made a rough drawing (using mspaint) on grounds. C16 is for the 5v and op-amp, so it is on linear side.

blue is linear ground, green (and white) is switching ground. I could make another ground just for op-amp and 5v reg.

Opamp and 5v with all their stuff are just under their ground as you can see... I can just put a thick line from 12v to the connector pin and make it as far as possible from linear stuff.

MOSFET taps seems to be the inputs, so is it worth it to make that space under it with thermal vias even with using heatsinks? if 25x25 is too big, then what about those individual heatsinks, the small ones? I still don't know what thermal glue to use in order to stick it firmly.

[BrianHG]

The caps C8 and the ones post L1 are going to the wrong GND.
Especially C8 which may modulate with the switcher it is above.
Those need to be next to the Dreamcast's +12v output.

[BrianHG]

Your caps below the switchers also are painted into the wrong GND section.  Be careful how you pout the GND.  The, the mosfets don't need a GND for their drain.

[BrianHG]

Actually, if you keep this layout, rotating the mosfets 90 degrees may also work.

[VEGETA]

The caps C8 and the ones post L1 are going to the wrong GND.

they should be on the same gnd as the 5v and opamp? or their own?

I will move them to be very close to the output connector to DC (12v).

Your caps below the switchers also are painted into the wrong GND section.

which ones? if you mean those close to the switchers then it is ok, they will go to the switching gnd not the blue one but the drawing here was rough estimate.

The, the mosfets don't need a GND for their drain.

but they will be within the linear gnd plane as shown. I thought about making a small copper area around them with thermal vias to help the heatsink more.

Actually, if you keep this layout, rotating the mosfets 90 degrees may also work.

I will eventually let them face their 3.3v and 5v connector directly.

[BrianHG]

The caps C8 and the ones post L1 are going to the wrong GND.

they should be on the same gnd as the 5v and opamp? or their own?

I will move them to be very close to the output connector to DC (12v).

Moving the cap is more important than the inductor.
I'm talking about the caps after L1.  Their GND should be on the linear GND.
Everything else is ok.

[VEGETA]

Here is the re-arrangement.

- moved 5v\op-amp big elec. cap a little bit to the left.
- placed all the caps after L1 in its place near 12v connector.
- rotated mosfets so that a direct connection is doable.

Notice that under the mosfets still empty in order to make thermal vias... but should I be doing it on 3.3v + 5v rails or where their pads are (the input)? I can make a local copper pour there (even one per mosfet) but to which net? I kinda believe the press-fit heatsinks gonna be enough without any of this, which makes more room to re-arrange bottom parts better.

As for heatsink, I like this 20x20x10 one: https://lcsc.com/product-detail/Heat-Sinks_XSD-XSD271-294-B_C286198.html  what do you think?

can you please link the product you talked about which can stick them and still conduct heat very well without being slippery?

[BrianHG]

Heat Sink OK.

Cheap stuff:
https://www.amazon.com/s?k=Heat+Sink+Thermal+Tape

Better stuff:
Actually, I don't trust that Amazon tape, go for real 3M brand:
https://www.digikey.com/product-detail/en/3m-tc/1-2-5-8810/3M10315-ND/2649860

The heatsink wont slip off the tape (unless you applied it over dust and oily surfaces).  The difference between the cheap and good stuff is the thermal conductivity through the tape.  The really good stuff is cost prohibitive and only necessary to conduct away >25watt <75watt loads.

Some of the Amazon quotes are from people who tried the tape on their PC CPUs not realizing that the stuff wasn't designed to conduct away 150-300 watts of heat produced by a modern CPU.  These tapes should not be used in applications where you need to get rid of >10 watts of heat, they are nowhere near conductive like metal-on-metal with liquid thermal paste.

[VEGETA]

It is nice to know such cheap tapes are good enough, will buy them in time. As for heatsinks, I have many options one of them being individual heatsink per mosfet and the other is one for both. Another one is to locally make them from an Aluminum sheet by cutting it, I guess workshops will do it for very cheap.

Anyway, is the placement of parts ok now? I guess this is the best I can do in such small footprint. If so, then I will start routing.

[BrianHG]

Well, looking at your space constraints, I truly wished the bottom switcher was further away from the linear opamp...

As you layout, you may end up adjusting orientation.

Also, if the traces from the source's to the output pins are short, your opamp may take the feedback from the output pins making them the exact voltage, with the appearance of something like a 0 ohm impedance.

1 heatsink will do as it has a larger fin area and one of the regulators will in general get warmer than the other.  This allows the hotter one to dissipate the extra heat by a larger chunk of metal.

Test the module on a full load output without the heatsinks to see how bad things get first.  You may not need one.

JLPCB & PCBWay's PCB panels are rectangles, not squares.  Adding 10mm width to that PCB will make a nice clear 1cm break between switchers and linear maintaining the exact same layout you already made and you should still get the same 25 boards per panel making the end price identical.

Right now the op-amp is so close to one of the switchers, I hope mere EMI wont affect it.

[VEGETA]

Well, looking at your space constraints, I truly wished the bottom switcher was further away from the linear opamp...

I may be able to move it a bit further.

Also, if the traces from the source's to the output pins are short, your opamp may take the feedback from the output pins making them the exact voltage, with the appearance of something like a 0 ohm impedance.

the 3.3v and 5v. output?

JLPCB & PCBWay's PCB panels are rectangles, not squares.

really? I thought they do all sizes. No sign of this on their site. keeping it small is a feature.

Right now the op-amp is so close to one of the switchers, I hope mere EMI wont affect it.

as I said, I will try to move it away. Maybe under the 2 mosfets since we won't be making thermal pads? how about that? they will be far from the switchers.

[BrianHG]

JLPCB & PCBWay's PCB panels are rectangles, not squares.

really? I thought they do all sizes. No sign of this on their site. keeping it small is a feature.

Look:


You optimize costs by making your panel fit inside that area.
Also, remember you require space between PCBs.

If your PCB was designed with true clearance to have no space between them for V scoring, currently, you can place 8x10 on a panel, or 80 per panel.

Currently, I would expect something more like 7x9 for 50x50mm PCB with 5mm between PCBs, or, 7x7 for 50x65mm PCB with the 5mm spacing between PCBs.  (Careful bending these with V scoring as they will flex an may damage SMD components.  Using cut-able tabs may requires more than 5mm between PCBs.)

In both cases, more PCBs than your original 25 per panel.

Read the panelization tab.  They claim the true sizes of the break-away tabs and V-scoring sizes.

[BrianHG]

Also, if the traces from the source's to the output pins are short, your opamp may take the feedback from the output pins making them the exact voltage, with the appearance of something like a 0 ohm impedance.

the 3.3v and 5v. output?

Yes.  Though, the quality of the solder in the connector's through-hole may add noise to the circuit.

[VEGETA]

I have finished routing it, I hope it doesn't need much modifications.

[BrianHG]

OMG, so messy...

Also, you placed L1 above a switcher, it will act like an antenna and really pipe through some noise, or not.  Cant be sure, but that is not a safe place for it.

Your opamp is in a really bad place.  It is under one of the mosfet drains which contain the bulk noise from the switcher, not to mention loss of PCB heat sink plating area for the mosfet.  I would rather place the opamp in the bottom right corner and place the 5v regulator to the left of it under the 2 1000uf caps.

There should be no GND under the noisy mosfet drains.  They should have a rectangular copper plate via stitched to the surface layer to surface layer to add heat removal.

You are also feeding up to ~15 watts or more power through single vias at multiple places in your design.

You can do a whole lot better...

[VEGETA]

Also, you placed L1 above a switcher, it will act like an antenna and really pipe through some noise, or not.  Cant be sure, but that is not a safe place for it.

I will move it.

Your opamp is in a really bad place.  It is under one of the mosfet drains which contain the bulk noise from the switcher, not to mention loss of PCB heat sink plating area for the mosfet.  I would rather place the opamp in the bottom right corner and place the 5v regulator to the left of it under the 2 1000uf caps.

I thought it would be better to be away from switchers...I will try to put it back where it was on bottom right as you mentioned.

There should be no GND under the noisy mosfet drains.  They should have a rectangular copper plate via stitched to the surface layer to surface layer to add heat removal.

this rectangular copper area with vias... attached to what rail? the smt pad is the input... I can make a small copper area for each mosfet rail 5v and 3.3v.

You are also feeding up to ~15 watts or more power through single vias at multiple places in your design.

you mean the output connector? what exactly.

[BrianHG]

There should be no GND under the noisy mosfet drains.  They should have a rectangular copper plate via stitched to the surface layer to surface layer to add heat removal.

this rectangular copper area with vias... attached to what rail? the smt pad is the input... I can make a small copper area for each mosfet rail 5v and 3.3v.

Ok.

You are also feeding up to ~15 watts or more power through single vias at multiple places in your design.

you mean the output connector? what exactly.

See the attached image purple arrows.

You are driving 6v @ 3 amps through one of those vias, no to mention 4v @ 3 amps.  If you think you can rely on a single tiny via to live through that, you will get some PCB mysteriously dying in the field after a week to a few months of use.

For the switcher, did you follow the datasheet recommended layout?

Also, the red one, hun?  Power to the inductor, but also to the switcher from the inductor's Vin.  I guess thatch ok as well.

Never flood fill when designing you PCB, especially power supplies where current handling matters in some areas.

The flood fill is the last step before the gerber output.

I need higher resolution prints without flood fill and proper net names on as many spots as possible.

[VEGETA]

I removed all tracks and vias so I can start with placement only for now.

I have re-arranged all components and was as faithful to aoz datasheet placement as I can. Now there is enough space between linear and switching, there is no colliding anymore.

if this placement is ok, then I can start routing.

the only downside is that the heatsink now should be a bit smaller, 15mm in vertical length and good length in horizontal position.

[BrianHG]

That looks a lot better.


Rotate C16 so the the GND faces the connector.
Rotate L1 with +12 out facing down.  Feed it with a thick +12v trace following the top/round the corner to the right of the PCB.

The 2 1uH chokes + input side chokes which feed the switchers should be on the top of the PCB while at least 1 of their filter output caps, if not both should be on the bottom.  Those 2 chokes should be above each switcher VCC they feed.  Use at least 4 vias in a square along a thick trace to power the switchers at the output of those inductors.  The output side of those chokes needs to be as short as possible.

As for the moved 1uH chokes to the top of the PCB.  Larger ones here may help as a void for a GND filled path.  You may even consider using the same 10uH (not necessary, there is still routing room with 1uH as the output is a short trace.) from the switchers if you like since they appear to have a nice huge void.  C2 may be moved lower in between the switchers to accommodate the 1uH chokes on top of the PCB.

Rotate and center the opamp & 78L05 regulator portion 90 degrees.  You may need to swap the opamp A&B channel for routing optimization.
You may also need to swap Q1&Q2 as well as the switchers to avoid vias/crossing from their source output and the power output connector.

The switcher's outputs feed should stay on the bottom and feed a big box pad under each mosfet's drain.  That box should have via switching to the top layer under the mosfets to help dissipate heat through copper.

[VEGETA]

I will dig into it tonight.

The 2 1uH chokes + input side chokes which feed the switchers should be on the top of the PCB while at least 1 of their filter output caps, if not both should be on the bottom.

you mean top side of the board and bottom side? Since these are gonna be smt assembled, then they should be on top side.

I can move L4 and L5 to top since I will already hand solder a similar one (L1) there, but the small ones should stay where they are.

The switcher's outputs feed should stay on the bottom and feed a big box pad under each mosfet's drain.  That box should have via switching to the top layer under the mosfets to help dissipate heat through copper.

This was my plan, getting the 5v and 3.3v to have this copper box filled with vias. However, it cannot go under the mosfet since the mosfet has pad which is the input. So i can make it near the mosfet in a way that it doesn't touch the pad.

__________

I am thinking of changing the dimensions since maybe 50mm will not fit properly inside. so maybe 40x60 is a good choice, or even 45x55... the length is gonna get bigger on the expense of the width (meaning the horizontal dimension). this way I must re-arrange the components a little bit.

I hope I can fit the 50x50 one, gonna do some measurements. I could offset it a bit to the side.

[BrianHG]

Don't move the switcher's output inductors.  I'm talking about the tiny ones feeding the +12v.  This is due to EMI noise considerations.

As for the mosfets, yes, the Drain +v inputs at 4.3v and 6v are routed to the switcher outputs through the bottom of the PCB while the source outputs go to the +5/+3.3v output connector on the top of the PCB.  The 12v in to the 10uh inductor is also on top of the PCB with the other 2 input inductor chokes with their 2 input caps.

[VEGETA]

Don't move the switcher's output inductors.  I'm talking about the tiny ones feeding the +12v.  This is due to EMI noise considerations.

I know but the tiny ones supposed to be smt assembled. Is it necessary to move it to other side?

As for the mosfets, yes, the Drain +v inputs at 4.3v and 6v are routed to the switcher outputs through the bottom of the PCB while the source outputs go to the +5/+3.3v output connector on the top of the PCB.  The 12v in to the 10uh inductor is also on top of the PCB with the other 2 input inductor chokes with their 2 input caps.

You mean by top\bottom is the routes themselves not the actual placement of components right?

but why such separation of signals despite being far enough from each other?

[BrianHG]

Don't move the switcher's output inductors.  I'm talking about the tiny ones feeding the +12v.  This is due to EMI noise considerations.

I know but the tiny ones supposed to be smt assembled. Is it necessary to move it to other side?

It's where the source GND is tied to by the caps at the input of those inductors and at the output.  The inductors can be on the bottom.  You want the source caps for those 2 on top and the ones on the bottom feeding the switchers by the switcher's GND.

As for the mosfets, yes, the Drain +v inputs at 4.3v and 6v are routed to the switcher outputs through the bottom of the PCB while the source outputs go to the +5/+3.3v output connector on the top of the PCB.  The 12v in to the 10uh inductor is also on top of the PCB with the other 2 input inductor chokes with their 2 input caps.

You mean by top\bottom is the routes themselves not the actual placement of components right?

but why such separation of signals despite being far enough from each other?

I talking about which side you place the traces.  When driving 3 amps, you try to avoid any vias possible.  They are just too small.  This is why going to the mosfet drains, you get the capability of stitching something like 10 vias around the drain as both heatsink transfer of power to the drain.  Keep the output of the switchers on the bottom of the PCB all the way to the mosfet drains.   Keep the source outputs on the top all the way to the output connectors.  Keep the +12v on the top all the way to the 10uH, then to the 12v power output connector.

Most of the top of your PCB will be GND on the left above the 2 switchers and a separate linear gen from the power input going around the left and down side (top of PCB), opposite the 12v line to the linear section.

Sorry, I got top and bottom.  I know the bottom is your SMD side which will be manufactured up-side-down.
So, when I've been saying bottom, I means the SMD side.

[BrianHG]

Well, how is it going?
I hope my instructions were simple and clear enough...