DC to DC converter

i fixed U1 and L1

as for OC resister which seems good?


Screenshot 2023-09-28 145512

You seem to have done manually what is expected to be done by the zones automatically. This is clearly seen inside the area of R2. You have drawn the zone outline around pads, vias and tracks. That’s not necessary because the automatic zone fill stops before touching them, obeying clearance rules.

yes :sweat_smile:
zone fill is easy to cover entire board but it gets near small gaps which dont looks good

I have never used handsolder variants of footprints. In my opinion there is not a big problem to solder elements at standard footprints and they take less space. Only you need is the soldering iron with a sharp tip and 0.5mm tinol (tin with rosin inside).
I have this one:

It is not soldering station taking a space at desk but only small iron directly powered from AC230V.

And about the project as a whole.
When I use DCDC in my devices I always use input and output pi filters to eliminate voltage ripple at output and current peaks at input. May be it would be good to add filters to your PCB, but it is your choice.

That iron seems decent
right now what i have is not good from SMD very big tip
and another which dont like to heat up well need to invest some decent one if i can find
for now it dont seem like i need any additional filter maybe an extra cap at output
but i can see it can help reduce noise

current design seems fine
DRC is also happy
let’s see how well it would turnd out wen i get the pcb

If you mean too small clearance you can change it. Zone has its own clearance.

my god i forgot that it dose have that
i should be able to use 2 zone with different clearance

1 Like

And solder paste is your very best friend when trying to hand solder SMD. Get a syringe type tube of it with a fine needle nozzle . . .

For example: MG Chemicals 8341 No Clean Flux Paste

1 Like

I haven’t seen anyone comment on the 1st thing that caught my eye. The ground connection for the feedback resistor R2 has a long way to go around to get to the gnd on the chip. I’d run that ground up inside the pins and connect directly to ground on the chip. Now your ground noise isn’t part of your feedback voltage. At 47K there is not much current, even an 8 mil/.2mm would be just fine. .15mm in a pinch.

1 if you have rectangular pads falling off the board, then this is a shitty manufacturer
2 there is no mandatory requirement or standard for ipc there are only recommendations
3 you cannot use rounding on all areas, for example on qfn thermopeds you will get defective
4 Even when drawing a rectangle you will not get 90 degree corners without rounding this is due to the etching method
5 rounding reduces the contact area and solder growth depends more on the type of solder than on the shape of the pad (lead without lead)

I heard without lead ones are not so good
Or I should say good ones are expensive and hard to
find

My local manufacturer is very new to the field that are cheap for me that why I need to take that into consideration

Kicad built in library is very good it have most footprint and symbol that I may need

In my first post I was writing about connection of IC pin 2 under the IC to GND where input capacitors and feedback resistor was connected.

The best connection of R2 should have no common part with current-carrying connections so it is a little different subject but the effect of noticing the same.

1 Like

It would be easier to understand you if you quoted the statements you are referring to. For example for me the word ‘lead’ says nothing. And don’t knowing the meaning of that one word I don’t know about what is the whole sentence.
I had to find that Pb-free was what you had in mind.

Yes yes my bad
This broken smartphone I have can’t select text correctly I really can’t select text at all :disappointed:

Pb is what am referring there

Also I have sent my grb file to manufacturer to check that said it’s ok and I have not butcher the clearance rules :pray:

Thay are the one who recommended kicad to me
" we prefer if you can use kicad or altium"

1 Like

I probably should have been a bit clearer there, the only connection to gnd on R2 should be a trace to chip. This defines the ground pin on the chip as the analog ground If the original layout is kept, and the small trace is added it really won’t help much.
If it’s a switching supply, the 1st order sanity checks tend to be around the high current loops and how to get output voltage feedback to the chip (an analog process swimming in a sea of high power, large volage, high frequency noise).
Not specifically related to this design because how the supply will be used is outside of the discussion, but in the real world both the input and output will need to have some filtering on them for noise. Even a ferrite bead and small cap on each end of the supply can help. Texas Instruments has a lot of good info on switching supply noise reduction. Good reading there. And it’s always cheaper to design in than to add on later. It’s great to see people learning and discussions on all this. Switching supplies and RF are cases where the PCB is part of the design, whether you like it or not.

1 Like

Unfortunately at chip pin2 there are high current pulses together with feedback. So at least the internal connection of that pin to chip inside have to be common for high current and feedback reference.

Have you noticed:

And OPs decision:

Ooops, didn’t notice your comment on filters, sorry. Late night reading of a long post…
w/r/t/ the OPs “don’t see like I need any additional filter”, it is hard to determine what’s going on without spending a lot of money for test equipment. A scope for starters, then spectrum analyzer. When I was starting out (no skill, no money, but lots of time) a short wave radio receiver often helped out. We are all on different points on the same path.

1 Like

The best tool to determine what’s going on you have between the ears :slight_smile:
I spend long time making L and C Spice models to model as close as possibly the charts from datasheet. Then I simulated the filers I planned to use.
My first solution for filter was to design 100uH toroid inductance in a way that no one was doing it. So I had to order it being wound specially for me. For 100uH I got 10 times less (worse) saturation current than typically was possible in the same dimension. That is because I was trying to get as low as possible parasitic C. I have measured this C using only square generator and oscilloscope. As my oscilloscope didn’t had FFT I saved signals in files and used FFT from PSpice. The C was 0.4pF.
Later I got the idea that instead of doing one stage filer to cover low (100uH) and hi (0.4pF) frequances it is better to simply make 2 stage filer using standard elements - one with ferryte bead and one with 100 (or more) uH.

Almost all the cheap ready made DC to DC converter available to buy have issues with noise due to bad layout or bad components selection to prefer cheap prices

This model use the same IC which I am using in this project have tendency to get noisy at high input and output voltage difference

Have not seen much filter related topics on DC to DC

I’ll like to check out some articles that you may prefer

As I already wrote earlier, don’t fill the switch node. It is the biggest source of emissions, keep copper surface small.