You should fix this sharp angle, it could trap etchant and result in over etching . . .
1 Like
I don’t see any problem. The track highlighted by @RaptorUK could indeed be improved by making it enter the pads more straight or adding teardrops. Also rounded pads are nowadays generally recommended, which you could fix by using different U1 and L1 footprints (or changing the existing ones). But this is nitpicking.
That does seem to be problem
I’ll slide that resistor to left a little
Any other points that should be considered related to manufacturing?
What is this about rounded pads ?
Can you explain please
The pads of your MT3608L have a rectangular shape, which means that you have relatively sharp 90 degree corners, that can act as a weak point and would make it easier to start “peeling off” the pad. Compare this to the footprints of your resistors/capacitors, which have rounded off corners. Rounded corner also fit generally better to the shape of the solder.
I don’t have KiCad ready, but compare the standard SOT-23-6 footprint to the handsoldering one. I think the handsoldering ones are older and manually created and the regular ones should have been updated to have proper rounded corners.
Have a read of this thread: Why Rounded rectangular pads in place of rectangular pads - Layout / Footprints - KiCad.info Forums
1 Like
Hm yes that is true that 90 degree pads to peel off
Have seen that many times
Standard SOT-23 ones are rounded edges
As for L1 it straight from manufacturer
Need to see if I can find something similar
You can just drag the track so it exits the pad at the corner . . .
1 Like
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 
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