I want to ask if someone would help me with my PCB

[Jambul46]

Hi i would want to ask if someone could make 2-layer PCB (and small as possible) for me and check my schematic if all is connected correct if possible. Thanks!




Attached zip file is EasyEDA schematic

[Jambul46]

My current proggres

[VinzC]

Hi Jambul46 and fellows.

Here are annotations I made to your project, which I'm sharing for review as well so anybody can comment on that.

In essence, here are my recommendations for a 2-layer board:

• shortest traces as possible and avoid long detours and loops
• avoid crosstalk between traces and pads/traces so have some copper in between
• have copper pour on both sides, stitching ground planes/pours with vias, more than one if possible
• functional blocks packed together with shortest traces as possible between functional blocks

You might have to move around components to fit those recommendations.

Source: Proper PCB grounding by Rick Hartley (https://youtu.be/ySuUZEjARPY)

[jpanhalt]

The negative terminal of your battery does not seem to be connected to ground.  What is the return path for components connected to Vcc?

[Jambul46]

it's in the schematic. the battery has chrg IC protection

[mariush]

Not a fan of the layout, sorry.

If possible, I'd shift the SD card slot a bit to the left.

I'd rotate the U7 90 degrees and move it a bit to the right and move  its crystal between the SD slot and the chip.

Don't break the ground fill under the card slot with that trace going to U3 . Either route it on the edge of the board (leave a few mm between the edge and the ground fill, make the trace thicker, or route that trace below the card reader and on the other 

Move U3 much higher, maybe where the RESET button is.  The RESET button could be moved to the left of the OFF ON switch , or between the OFF / ON switch  and the card reader.  You'll want the buttons near the edges anyway, to be easily accessible by your fingers if you stack boards.

Your Arduino chip could go a bit to the left  and maybe even rotate it to the right 90 degrees so that the crystal isn't so far away
Speaking of crystals, you really couldn't find some smaller ones, with smaller footprints?

Then I'm looking at U6, your 3.3v linear regulator?  Did you have to use such a small chip? Why not some sot-223 or something, so that you'd have better heat dissipation into the circuit board and the package. You'll be converting 3.7..4.2v or 5v down to 3.3v, so there's gonna be some heat.
I don't see any decoupling capacitor on the input (probably not needed but wouldn't hurt to have a 0.01 uF ceramic there)

Also, on top layer, I see the output voltage go to C3 and the ICSP pin and that's all. Assume there's a via to the back layer and going to Vcc ?   Also, took me a few minutes to scan the schematic for C3 only to see it separated on the side.

What's R7 and R6 doing by the ICSP header, if it's very close to the SD card in the schematic? Don't do that ...  move the U3 chip away from the SD card and you have room for the resistors there.

Also, it's a good opportunity to use resistor networks, both for those 4 x 10k resistors and for those 4 x 1k resistors for the CH340g
Here's some examples, 4 resistors in 1206 footprint  :
1k : https://www.digikey.com/en/products/detail/stackpole-electronics-inc/RAVF164DJT1K00/1744131
10k : https://www.digikey.com/en/products/detail/stackpole-electronics-inc/RAVF164DJT10K0/1744119  or https://www.digikey.com/en/products/detail/bourns-inc/CAY16-103J4LF/431579


That trace going to C8 around the hole is silly. Experiment with rotating Q2 and U2 so that you don't have to go around the hole with that trace - maybe see how you could route that trace around the right edge of the board.
 R4 can be much closer to U2 , and then the trace could go straight to R16 from the right side of the pcb.

Overall I'd make the 3.3v traces and the input voltage traces thicker. No reason they should be as thin as the signal traces.

R2 footprint seems to be much bigger than other resistors for some reason?  Is that on purpose or what.  ... R13 , R9 , R10 ... the text of R13 is screwed by the via there... The R13 is pointlessly shifted to the right when it could leave space so you could have R9 text printed vertically like the other resistors.

Maybe have TX and RX text  to the LEFT instead of between the LEDs

I'd also like to see the leds have proper naming, like D1, D2 etc   and you have plenty of space to say "CHARGE" instead of pointlessly short it CHRG

Pay more attention to direction of text ... ex R12 can be read straight forward, R1 and U1 and R5 is flipped vertically.

Traces going to U9 (the crystal for the CHG chip) should be about the same length though in practice won't matter that much here. Also, no reason why you should route that trace so close to the pad . Again... super big footprints for these crystals... you should be able to find smaller crystals.
And better layout would save you from routing the trace between the pins.

May want to consider if it's a good idea to have the Q2 and U2 chips so close to the edge (for example what if someone drops the pcb on the floor, could those chips be damaged or could the solder crack and get intermittent results?)





To be honest it looks like there's enough space that you could fit the battery on the top edge and have everything below the battery

[Jambul46]

Ok, thanks and for the battery i want it at bottom it will stand on 4 computer standoff's

[Jambul46]

and for the ressistors i can't use array's because 1. i don't have any proffesional tool's only cheap soldering iron and 2. i won't order stencils they are expensive

[Jambul46]

And like i said if someone would make the PCB for me it would be huge help

btw my experience with creating PCB's is one little audio amplifier and this (this PCB/schematic is v2 of original) PCB with pre constructed modules (arduino nano,sd card reader,charge IC)