Voltage regulation circuit 12V to 5V in 5A range

[Ioannis]

You are most welcome! Thats what friends are for, right?

The selected TPS is difficult to handle by hand. Needs heatsinking on the PCB by special design. I do understand why you selected this one over the TPS565208, that is super easy to handle.

Amazing chips TI has...!

Ioannis

[Demon]

Y...The selected TPS is difficult to handle by hand. Needs heatsinking on the PCB by special design. I do understand why you selected this one over the TPS565208, that is super easy to handle.

Amazing chips TI has...!

Ioannis

Definitely, that's why I did my best to mimic the "suggested" layout I posted above. I figure there's countless hours or even days put into that design.

I came up with this 4-layer PCB, top layer:




Both inner layers are identical:




And the bottom layer:




I did my best to use the same outlines, but I didn't have identical sized components, so I had to make due.
- Rpg goes to VCC on the datasheet drawing, but goes straight to 5Vout on the generated schematic.
- they have a single Cin cap, but mine is split into 2 using alternate parts.
- my inductor seems to be twice as large as theirs.

Also, the Webench schematic for 7-12Vin to 5A-5Vout didn't have these resistors:
- Rmode
- Renb
- Rent
So I don't have that trace from PGND going up to VIN.

The last thing I have to adjust is the copper layers; I remember reading something about needing 2 ounces top and bottom, and 1 ounce inners (or something like that - got reading to do).

Looks like this in 3D:

[Demon]

ARGH! Of course it's only now that I notice Webench generated a layout specifically for that schematic.




I couldn't find any mention of copper thickness in the datasheet. No mention in the Evaluation Board for the TPS56637, but it does have a much nicer layout with A LOT MORE cooling holes and a wider area.




I must have read about the copper thickness in the datasheet for another TPS. I just can't remember which cause I looked at so many.


EDIT: No mention of copper in their Quick Reference Guide:

https://www.ti.com/lit/an/slva958b/slva958b.pdf

[Demon]

Bingo, I must have seen this while researching the LM1084. Digikey PDF for the LM76002 on page 43:
https://www.digikey.ca/en/htmldatash.../1/lm76003rnpt

TI recommends using a four-layer board with the copper thickness, for the four layers, starting from the top one, 2 oz / 1 oz / 1 oz / 2 oz.

[Demon]

TI's Eval board for the TPS56637 is 51mm x 64mm. I figure it would be wise for me to use the same dimensions until I have an actual board to check under the infra-red camera.

Increased the amount of cooling VIAs like on the Eval board.

Used a DIP header for the leads for a cleaner look once on the prototype.

Increased thicknesses to 2-1-1-2 ounces and tweaked the trace width/space according to JLCPCB minimum requirements for a 2oz board.




I still have to figure out how I can make my VIAs have large copper rings like the Eval board. I probably have to replace them with actual holes (like I have on the 4 corners - nice visible copper ring).

[Demon]

Had to make the hole a Part, not included in Schematic, BOM or To Be Populated.

Discovered the Create From Selection / Create Array feature; real time saver to make grids of parts.




Starting to look 1/2 decent.

[Ioannis]

Wow! You did a lot of work!

I am pretty sure that the extra layers TI suggest are for less noise ad better heat dissipation. Have you checked how much extra cost is added by JLCPCB?

In general if you want/need to make the board smaller, you can move all componets to the left, connector closer to the inductor and the right board edge also moved to the left. I don't see why this pcb needs to be that large. Saves cost also I guess.

I'd add an extra output capacitor for less noise and better operation without much cost. Parallel capacitors make for lower ESR also.

Nice design. You become an KiCad expert!

Ioannis