Low ripple low noise small power supply design

[BrianHG]

This should help clean up a bit more:

After making my green and red changes, the movement of the mosfet source output traces at the top right should be obvious to get make the GND cover more area and reach that new GND via.  The elimination of the opamp's VCC on the red layer makes all that section 1 solid GND plane.

The red Xs by the lower switcher needs movement and cleaning so that it better resembles the red check marks on the top regulator.  You cant have the protective flyback diode wired the way you have it on the bottom switcher.  It will radiate excessive noise.

Don't forget the Kicad link I gave you earlier where it says that you need a footprint which contains the 'PADs' with drill holes and matching pad number to get the heat-sink relief.

[VEGETA]

I will try to clean it as much as possible, but maybe it will take time since I am busy this weekend.

The red traces on right side (opamp + Vreg)... do you mean they are on the red layer? but the pads are green smt ones, they will need vias to connect to red ground. they are straight connections though, so why do we need to change them?

The rest of your red traces are just re-located ground vias right?

why you put X on the trace connecting the 2 grounds? shouldn't they be connected with a trace? I mentioned that kicad continues to say unconnected traces until I do it.


as for the switcher in the bottom, I will slightly move these parts to the right to make room for all these mods needed. However, these caps and maybe even the diode will be under the linear 3.3 and 5v traces of the red layer... will this make effect?

i will try to modify the kicad pads... I actually thought about this but really didn't think it would be necessary.

I will update you on this once I manage to do it.

[BrianHG]

See my red trace on the bottom, this is a good place to merge the 2 GNDs.
Also, move the V+ trace at the top left so that a little more meat for the GND leaves the power input connector.

[VEGETA]

I enhanced the design further more.

Now I think all are ok.

[BrianHG]

Almost perfect.  I'll upload a few minor patches before I go to sleep tonight.

[BrianHG]

Ok, let's see if you can catch & replicate all my improvements.

(The purple under the mosfets means remove/disable the 'thermal reliefs'.  You want a solid copper fill over those pads.)

I removed some rows of vias around the mosfets.  This will allow you to move the power traces further away from the edge of the PCB.

If you catch every change, and the nets report all connected, after 1 final look over, you will be ready to go.

[VEGETA]

I have removed the thermal relief and it is now solid. I also cut the area so that the traces are not near the board edge.

however, I didn't do the other minor relocations... are they necessary?

I'll see what I can do when I have time.

[BrianHG]

Yes, the minor changes are all necessary.  All those changes concern the series resistance of the vias and the amount of current which you are pushing through them.  So especially on the green layer, take a careful look at my layout changes and the number and location of all the added vias around the switchers, power input, feedback, GND going to the bottom switcher's GND input & also on the +12v going to the dreamcast's +12v power out side.

Do this board right once and you wont have to debug unseen weird things with your scope from PCB to PCB.

[VEGETA]

DONE.

I believe I've done everything.

If all is good now, I will just re-arrange the silkscreen writings.

Then I will try to make a panel so that I can use JLCPCB smt service as a panel (10-30 panels) rather than single ones.

 

[BrianHG]

This should do it:

[VEGETA]

I will do it tomorrow,

by this, the 3.3 and 5 linear power signals will pass under the cap, is it ok?

[BrianHG]

I will do it tomorrow,

by this, the 3.3 and 5 linear power signals will pass under the cap, is it ok?

Yes, this is ok since these signals do not have a high frequency EMI radiating from the switcher.

[VEGETA]

Done.

I thought about doing very small green copper zones around Vcc and 12v pins but I used thick tracks to cover the area properly.

[BrianHG]

I think you got it.
It looks as simple, direct and clean as it will get.

[VEGETA]

Tomorrow I will make a panel of it, suitable for JLCPCB SMT service.

[BrianHG]

Tomorrow I will make a panel of it, suitable for JLCPCB SMT service.

Ask JLPCB first, they may prefer to panel it themselves.  Or, they may tell you how much space you need to place between panels so they are able to assemble the PCB.

Also ask about fiducial marks.

[BrianHG]

1 functional quality improvement.  Take a look at the change I made to R1 and how it's connected to C16.  This is important as the original single via's resistance will determine how well filtered the +12v will be for the linear section in our RC equation where the VIA adds a unpredictable series resistance between the cap's + leg and R1's output.  This essentially makes the cap look as if it has a lower ESR in the filter.

The change makes sure that the +12 goes to the C16 filter cap first.  The that output feeds the linear section off from the cap's + pad through a second via.

[VEGETA]

Done.

I've messaged JLCPCB.

I looked at their site and looks like they updated the service to be able to use black solder mask which is a good thing for me.

also, 50 is the max quantity now.

so I could make 300x300mm panel, get about 10 panels which will have 250 boards! 50x50mm x 5 columns x 5 rows.

I could get just 5 panels though as a start... dunno about the price, lets wait and see.

choosing panel by jlcpcb didn't work on their demo smt board.

btw, kicad penalization is not so smooth, one needs to do some manual stuff.

[BrianHG]

Nice on the cap.  Everything looks good.  Good luck with JLPCB.  I think to get their 5$ special, you have to send the PCB as a single & they will deliver a few PCBs for you.

[BrianHG]

Q: Isn't the vertical portion of that 3.3v and 5v trace a little close to each other?

[VEGETA]

Q: Isn't the vertical portion of that 3.3v and 5v trace a little close to each other?

KiCAD didn't say a thing about them being too close.

[BrianHG]

Don't forget to test with dummy loads of varying current...

[VEGETA]

Don't forget to test with dummy loads of varying current...

Actually my problem is that I don't have an oscilloscope nor electronic dummy load. I plan to buy a scope soon though. I wish if there is a used 1054z available.

[VEGETA]

I have made a panel our of it.

25 single boards with 280x280 panel.

next is dealing with BOM and with JLCPCB format.

[BrianHG]

Don't forget to test with dummy loads of varying current...

Actually my problem is that I don't have an oscilloscope nor electronic dummy load. I plan to buy a scope soon though. I wish if there is a used 1054z available.

A dummy load is a resistor.
Voltage can be measured with a volt-meter, but, a scope would be more useful to inspect everything including noise.

Get 10x 10ohm, 5 watts and 10x 6.2 ohm 5 watts.  Wired...  10 watts may be a better idea.
Get 1x 100 ohm, 5 watts for the 12v.

On the 5v, every 10 ohm resistor you add will add 0.5 amp load, 2.5 watts.
On the 3.3v, every 6.2 ohm resistor you add will add ~0.532 amps, ~1.8 watts.
On the 12v out, place the 100 ohm resistor to load 0.12amps, or ~1.5 watts

The resistors will get hot.
Match and go above the current load of the Dreamcast for each output all running in parallel.
See how hot the power supply board gets.


Note: locally, you cant even find an old used cheap old 10-20MHz CRT oscilloscope for 15$?