Low ripple low noise small power supply design

[VEGETA]

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

Hello,

I am well 

However, real-life job stuff... and also, the stock dreamcast PSU got broken 

I have been trying to fix it but couldn't after hours of fixing problems one by one, still can't seem to work. So I ditched it and started making one from scratch using the awesome L200 regulator. 2 of it for each rail, DIY project that I will finish tomorrow or so... to be able to play.

The irony is that I am designing a PSU for dreamcast... the the stock PSU got burned 

[VEGETA]

Hello,

I have made some little tweaks:

- Rotated C16.
- Rotated 5v regulator + op-amp 90 degrees.
- Rotated L1.

However, I didn't move input inductors and little inductors to top side of the board since I want them to be SMT assembled. Also, Q1\Q2 placements seem fine to me.

If this is ok as placements, I can start routing next week.

[BrianHG]

Here are some of my ideas...
I pushed up J4 & J5.  Move the +3.3 output cap and R load.  Shifted over the opamp a little.

See the chosen power trace path.

If you do do a linear GND fill, avoid the +12v heading into the 10uH inductor.
On the switcher side, you have generous GND plane fill area as well as room for a hefty 12v trace to the 1uH 12v choke inductors.

!!! The switcher GND fill should not touch the GND trace I laid out which feeds the linear side's GND !!!

These were rough drawings, I'm sure you can make it much nicer in the cad.

[BrianHG]

So?

Did you decide to spend 1 night to finish up this board, make 2 test prototypes so you can get your Dreamcast up & working again the right way?

Or did you scramble and waste more time than that would have taken to finish the small PSU to Gerry-Rig a sub-par temporary fix over a few days which may be dangerous enough to damage your 1 only Dreamcast?

[VEGETA]

So?

Did you decide to spend 1 night to finish up this board, make 2 test prototypes so you can get your Dreamcast up & working again the right way?

Or did you scramble and waste more time than that would have taken to finish the small PSU to Gerry-Rig a sub-par temporary fix over a few days which may be dangerous enough to damage your 1 only Dreamcast?

I will get to do it for sure! no getting back from this, no surrender!

These weeks I've been travelling from work to home back and forth (200 KM) more than ever... this is the cause.

I will keep you posted for sure.

[VEGETA]

Hello,

long time no see!

I finally got the time to work on this, and here is the result.

Obviously I still need to do some polygon pours and vias...etc as well as art stuff. However, I wanna make sure I got the most important stuff done.

what do you think?

regards!!

[BrianHG]

Ouch, kinda messy and you are mixing you switching GND with your linear GND.

Ok, step 1, reset / swap the voltage on both switcher's rewire them to the mosfets.
See attached schematic.
This will get the switcher's output to match my layout recommendations a few posts back.
(See all red text)
(This is only a start, there is a lot to do...)


Please remove all GND traces and see if you can get me a high enough quality bitmap or print to see the more net labels on the pads of the SMD components.

[VEGETA]

So you want to re-locate the switcher circuit for both rails? I can do that but it takes time.

I still need to figure out how to wire the grounds so I will leave it to the last moment.


where exactly did I do wrong in terms of mixing grounds?

[VEGETA]

Here is the update.

I have re-wired the transistors to the other switchers as we agreed. Did the same wirings too but still didn't fully connect all the pads especially grounds... also no ground pours yet.

[BrianHG]

Without a painted rectangle under the mosfets, no heat will be drawn away from their metal drain tabs to the vias to the bottom of the PCB.

More to come.  I need to look more closely of the layout.
There is still too much spaghetti in your layout style.  There is room for much improvement just my moving & rotating a fer smd caps and resistors.

[VEGETA]

Without a painted rectangle under the mosfets, no heat will be drawn away from their metal drain tabs to the vias to the bottom of the PCB.

More to come.  I need to look more closely of the layout.
There is still too much spaghetti in your layout style.  There is room for much improvement just my moving & rotating a fer smd caps and resistors.

I guess I put rectangles in each layer under the mosfets and connected them with vias... or what exactly?

I tried to make the layout as clean as possible with having the same component placement.

looking forward to your further input. thanks

[VEGETA]

Looks like you've been away for quite some time.

I still didn't do further more as nothing is left but to finish the layout itself.

[BrianHG]

You will need to start by redoing the op-amp layout.  It is such a jumble, it has an added chance of oscillation just due to signals going around the IC.

The op-amp's position isn't too terrible maybe center it a little between the 2 mosfets, lower a little.
Place it's decoupling cap above pin 8 and parallel to the opamp.
The termination and resistor divider and feedback resistor for each amp should be on each side o the opamp while the series reference power feeding resistors may be below the opamp.

Your linear regulator mess also needs some cleaning up.
Also, the 5v out's power trace should not encompass the large 1000uf cap's + pin.

See photo, the purple is the switcher's GND fill and the green is the linear's and output's GND fill (All will be on the red layer).  However, do not fill them yet, I just wanted to show you the guide so you know where you will be getting all the GND via points from.  There is still things to clean up on the switcher side after you fix the linear side.

The added red copper by the mosfets is needed for heat sinking.  In fact, there should be a grid of un-tented vias under the tab of the mosfets.

[VEGETA]

You will need to start by redoing the op-amp layout.

Ok, I will do it.

However, why the series feeding resistor must be on the lower side? assuming the mosfets are on the upper side of the opamp?

Your linear regulator mess also needs some cleaning up.

like what? you mean the signals going into vias and long distances?

Also, the 5v out's power trace should not encompass the large 1000uf cap's + pin.

you mean it goes under the cap? if I move it to the left, then it and 3.3v output one will be above some switching components.

The added red copper by the mosfets is needed for heat sinking.  In fact, there should be a grid of un-tented vias under the tab of the mosfets.

I will add more vias there, easy.

[BrianHG]

The congestion around your linear side is making it hard for me to make anything out.
Move the components away from the op-amp and start again.
Do only 1 side at a time as the other side should almost look mirror like.

I'm assuming pins 1&8 should be facing toward the mosfets.  Maybe swap U4A and U4B.

First place D4 vertical next to the input pins.
Place R16 and C38 above next to the output pin, both partway to the mosfet gate.
Place R10/C33 by the input pin.
Place R18 can be a little further away.

See how this looks and see if you can mirror the layout on the other side of the opamp.

[VEGETA]

This is my attempt after hours of doing modifications.

However, some stuff still not connected and kicad shows mosfets square area  being overlapped (top and bottom) + a track (VCC) close to it.

[BrianHG]

You didn't rotate the opamp 180 degrees and swap U4A and U4B to make the routing easier.

Also, why did you change to the green layer for the flood fill GND on the switcher side?

You are also missing heat-sink vias for the switcher regulator ICs.

Also, look at the attached image of example vias under a SMD power transistor.
Use something between pattern 2&3.

[VEGETA]

You didn't rotate the opamp 180 degrees and swap U4A and U4B to make the routing easier.

Also, why did you change to the green layer for the flood fill GND on the switcher side?

You are also missing heat-sink vias for the switcher regulator ICs.

Also, look at the attached image of example vias under a SMD power transistor.
Use something between pattern 2&3.

I sent the response before your response.

what is wrong with the current opamp configuration? I moved a lot of components around to make traces straight and short.

the green layer? i think it is away from the linear gnd so i thought it is ok... I can put the red layer but it wont fill properly.. maybe then I need to put lots of vias to achieve that.

as of heatsinks, i tried putting some of them to make the connection between the red and green rectangle pour... however, i couldn;t place vias in all area of the rectangle. I can add more though.

what more can i do besides heatsink and vias? assuming the op-amp now is good. I really hope I don;t need to change it but i am ready to do so if absolutely necessary

[BrianHG]

There shouldn't be any GND traces on the green layer other than a short hop from SMD pads to VIAs to the red layer which should be a solid GND.

That green GND fill is all chopped and garbled up with no continuous solid 1 piece backbone to it.

Please identify the arrows in the attached image...

Turning around that opamp is the only way to get rid of the clutter of traces under it while eliminating those looping long green traces going in and around the resistors.

[VEGETA]

ok so i will turn the op-amp to try to wire them a better way. however, these signals are on the other side of the board anyway, so a long green wire is a must... just maybe not using red layer is the only improvement to gain.

to make a red gnd of switching side, i need to put lots of vias and connect ground to it from green layer (signals not pour). I will attempt that tomorrow... maybe not a solid perfect rectangle but i hope it is close to it.

i really hope we finish the design soon xD

thanks!

[VEGETA]

I did all of this, it is in attachment.

It is not so tidy, especially the vias under mosfets but tidying it up should be easy.

I have connected both grounds with one trace as agreed earlier.

All traces are as short as they can be, but still some of them had to travel but those are very few.

If anything isn't clear, I will send the project via PM.

[BrianHG]

You didn't swap U4A and U4B in the schematic.

Are you autorouting?  It should not be done for such a simple design...

If you followed all my instructions, there should only be 4 vias in the linear section, 1 for each gate and 1 for each source.

There will be a few vias for GND as well, but no jumpers to the red side.

There would also be 1/2 vias by the 1000uf caps, but nowhere else.  There are 100% complete straight paths everywhere else if you placed the SMD caps/resistors correctly.

Also, what is it with that oddly placed resistor I have the red arrow pointed to?

It beginning to look better.  You clearly have the space for cleaning everything up.  The switching side isn't too bad, though a little adjustment to feedback resistors and maybe a few traces too thick going onto the switcher's SMD pads.  And, the switcher IC's thermal case GND vias in the footprint underneath the IC are missing.

[VEGETA]

You didn't swap U4A and U4B in the schematic

I thought it would be not necessary if I rotate the op-amp. I will try it now hoping it won't require me to re-do everything.

Are you autorouting?  It should not be done for such a simple design...

No, I never did it and don't intend to.

If you followed all my instructions, there should only be 4 vias in the linear section, 1 for each gate and 1 for each source.

one for mosfet gate and one for mosfet source x2 ?? I will swap U4A and B to see this.

There will be a few vias for GND as well, but no jumpers to the red side.

I increased GND vias so that they share the current, despite being so little in the op-amp area.

There would also be 1/2 vias by the 1000uf caps, but nowhere else. 

I didn't understand this.

There are 100% complete straight paths everywhere else if you placed the SMD caps/resistors correctly.

What is wrong with some of the traces going a bit further or bend a little bit? I see it all the time in PCBs. Yes, straight and short is the best though.

Also, what is it with that oddly placed resistor I have the red arrow pointed to?

this one delivers the EN voltage to the switchers. and the pins of the switchers are very far in the next side and cannot be rotated as you can see. either put the resistor in linear side then do the big trace or the opposite.

I will try more now.

[VEGETA]

Here is the said changes, all done.

Now only very few vias exist, but I had to put one to connect the 2 grounds together since kicad keeps listing some of them as not connected.

I couldn't put vias under the mosfets because they will be on the pad itself which is probably not allowed in kicad.

the big cap signal had to go under the op=amp or it would rotate more distance, by this... it is very short distance.

[BrianHG]

I couldn't put vias under the mosfets because they will be on the pad itself which is probably not allowed in kicad.

Maybe you need to do it in the footprint editor?
I don't know since I do not use Kicad.
However, I've attached some additional photos to show you when it comes to 'thermal pads' on ICs and transistors, this is normal in the electronics industry.

also read here, simple google: https://forum.kicad.info/t/pad-holes-under-smt-for-heat-sinking-and-other-questions/3714/3

You are almost done with the PCB.  I need to do some things in the paint software...