Please help me avoid a disaster with my first pcb

[spicy_coder]

Hi, first of all, hi to all as i am new on this forum.
I am Computer Science student and electronics hobbyist and i´m trying to make my PCB first board.
I have made a little electronic circuit and electronics schematic to make a little plant grow light controller,
i have not enough experience/confidence on my design and tried to make it as simple as possible, but still i have a feeling that is going to be a big fail, so if somebody with experience could give me some advice and at least help to me make it safe and avoid burning my house down it would be awesome.

Description of the device
- 24v input drives two power converters, MP1584 Buck converter board from china for 5v electronics and meanwell LDD-700L, this driver is used to drive two BXEB L0280Z led light bars.
- esp32cam board used as MCU, to take photos of the veggies, control and take data, show it a oled screen and upload it to a linux server.
- DHT22, 2 i2c lines for i2c devices (oled screen and one to expand in the future) and onboard ftdi, and boot pins to flash the esp on the go.
- I am trying to make it as cheap as possible, so its as small as i could do it and i am avoiding using smd components and use only through hole components to be easy soldering.

Questions
- i used 0,8mm separation between traces, 0,15 mm width for signal lines, and 0,8mm for power lines, as it is a bit more than the values that i get in a this trace width calculator using 18micrometers as Cu thickness, 24v and 1A, could be this the layer thickness or i am messing numbers from the fab page?
- i saw that the bottom part of the esp32 antenna should be outside of any pcb and preferably without any traces underneath, because of interference, but i plan to use a external antenna, should be concerned about interference anyway?
- Should 24v GND, MP1584 input and output share the same GND? i think so because 24v input is input for ldd driver, and i plan to dim the driver with the MCU so they should share the same GND, but this makes connect input and output ground of MP1584 directly, and i don´t know if this is safe.
- should be there any resistor between the ldd driver dim and the esp32 output?
- Is there anything dangerous because of crossing lines between positive and negative 24v 1A in top and bottom layers?
- Is there anything apart from the listed in the questions on the schematic or board that doesn´t make sense or it´s dangerous?








Thank you in advance for your time and help

 

[andre_luis]

Regardless if there is any issue at the PCB layout, I would thoroughly review the schematic diagram; at a glance we can note the lack of pull-up resistor at the DHT22 sensor, as well using a lot of pins shared with the SD card, so is it supposed you will not use it?

- - - Updated - - -

In my oppinion, the width of 0,15mm for tracks is too thin, consider increasing by 2x or 3x.

Side note: In general, routing dimensions are depicted in mils ( 1.000ths of inches )

 

[wwfeldman]

Your board looks like it has two layers of copper
it also looks like all the components are through hole
it also looks like you have components mounted on both sides.
DHT22 and ESP32-CAM on the bottom
LDD-700L and MP1584 on the top

that generally doesn't work
especially if the leads from one side protrude into parts on the other side
which appears to be the case

i suggest that you follow andre's suggestion and
that you make the board bigger and put all the components on the top

 

[KlausST]

Hi,

I agree with the others.
For a first PCB layout it's not that bad.

I'd add power supply decoupling capacitors. SMD.

Regarding THM components on both sides: It could be possible with stand-offs and hand soldering in the right order. I didn't check it in detail.
But debugging and repair is difficult.

GND plane.
It's not that bad .. but with some simple modifications you could avoid the lengthy traces within the plane.
* MP5184, pin1, left trace: remove it, route it to the right, and route it between pin2 and pin3 to the left side.
Then you are able to make the upper blue trace red.
* red trace left from the "F" of "FTDI": make it blue (only very short trace).
Then you may reroute the blue +supply trace on the red side between the connectors.

Klaus

 

[FvM]

MP5184, pin1, left trace

Not completely clear which net is addressed.

Regarding the double side population, I understand that it can be only realized with hand soldering. The components placed on top of through hole pins must be mounted in a lifted position, possibly using spacers to avoid shorts with conducting areas on their bottom side. I presume it's nevertheless possible.

Apart from the challenging double side assembly, the board looks fine to me.

0.15 mm trace width is standard at all PCB manufacturers. With plenty of room, you may consider to increase signal lines to 0.2 or even 0.25 mm. Parasitic capacitance will however increase too.

- - - Updated - - -

it is a bit more than the values that i get in a this trace width calculator using 18micrometers as Cu thickness

I would consider 35 µm (1 oz) as standard technology, e.g. for prototype PCB. 18 µm would be specifically used for HDI PCB with line width < 0.1 mm.

 

[KlausST]

Hi,

Not completely clear which net is addressed.

Oh yes, thanks.

Indeed it´s the (red) "VCCIO" net connected to pin1 (square pad) of DHT22 (I was confused by the double side assembled parts ... and the picture showing both sides at once)

Klaus

 

[FvM]

VCCIO is the 5V output of DCDC, I think it's o.k. to route it this way.

 

[spicy_coder]

Thank you all very much to all for your help!
Sorry my delay answering but there´s a ton of new info for me and i am trying to digest it all,
also sorry, maybe i should have added at first post more information,

24v-to5v converter and esp32cam are going to be put on raisers (i don't know well how they are called, i think ¿female pin headers?), i thought it would be better because as i am going to use cheap china components that i have at home, in case of fail in any of them, i want to avoid re-soldering them.
That´s also the reason because i thought putting things soldered through on the other side, as the components are raised, there shouldn't be any problem with the components protruding and touching the ones on the other side, as pointed, i know it should be a bit more difficult to solder but you can't have all.
This also looked a good solution for me because i want to have the esp32 camera and dht22 pointing downwards (to the plants) and have the i2c ports on top letting me connect the oled screen on the top without having to extend i2c cables from the bottom part, and also, let me make the board smaller and thus cheaper, and as i expect this project to be a complete fail (Hope for the best case, expect the worse case), cheaper fail is a better fail, but if still with this in mind most of you think its risky or pointless, i haven´t any problem to redesign the board, as my main interest is to learn from this project.

So with al your suggestions in mind i modified the layout.

Respecting what Andre commented:
- I use esp32cam microsd ports, because i am not planing to use it, and you are true about pull-up resistor used for DHT22, i got to at home DHT22 sensors and also DHT22 "arduino expansion modules", that come already with that on board, for convenience i will use the seconds, so i changed the 4 pins for a 3 pin header and avoided adding more components to the PCB.
- I also increased all tracks to 0.6mm (24mil) for data pins and 1mm (40 mil) for power tracks.

Respecting Klaus comment:
- It took me a bit to figure out the modifications, but i got it and with your help and some minor changes i was able to let the GND plane free of any tracks, which is i think the goal you was pointing out.
- I looked out this "decoupler capacitators" concept, where you think i should put them? they are not already integrated in the buck converters? I havent the soldering skills for SMD components, but i could savage some throught-hole cap from any old breaked electronic board, if it´s better to add it i will do it, but i try to keep the components used at bare minimum.

Respecting FvM comment:
- I added in the my design wider tracks before reading your comment, but now i don't know it was a good idea, as now there is less space between tracks, so parasitic capacitance will be also increased.
- I took 18 µm because its stated as "base copper thickness", but there is another field called "Min. processed copper thickness" which is 35 µm, i don´t understand the difference, and i still don´t know which one is the one that i should put on the calculator as the field "Cu thickness".
- PCB fabric spec page link (I am not endorsed in any way with this company, it´s just the more convenient for me, and if any moderator thinks link should be removed i have any problem with it and posting a photo or something)

Apart from the stated i also did some minor changes and the board and now it looks like this:



The only tracks that don't look good to me now are the tracks under LDD-700L, and the output of this converter, i tried to avoid using the top part of the pcb just under the converter so i put both output lines on bottom part, making me connect one of the screw terminals be connected indirectly, also i took out all tracks that where intersecting with ground plane, so i neeed to take UOR and UOT tracks directly under this converter, is this a good solution or was better before?


Thank you again all for your time and help, it´s helping me a lot to make something better and to understand better what i am doing, i hope my questions don´t annoy you.
Best Regards, Niko

 

[FvM]

I took 18 µm because its stated as "base copper thickness", but there is another field called "Min. processed copper thickness" which is 35 µm, i don´t understand the difference, and i still don´t know which one is the one that i should put on the calculator as the field "Cu thickness".

Processed copper thickness is the relevant parameter for trace resistance and current rating. Outer layer copper is build by electrolytic deposition on the etched base copper structure when through plating the holes. The base copper information is often omitted in a simplified description of the stack-up because the processed thickness matters.

 

[KlausST]

Hi,

I looked out this "decoupler capacitators" concept, where you think i should put them? they are not already integrated in the buck converters?

As a raw rule: put a decoupling capacitor at each power supply pin of every IC.
For sure, if the modules have integrated Cs, you may omit additional ones.

And a capacitor on one end of a power supply track does not replace a capacitor on the other end. Any track - almost independent of width and thickness - is an impedance. Especially at high frequency signals (better say: signals with high rise / fall rate) will cause significant spikes on traces.

SMD soldering: 0805 size should be hand solderable, you may also use 1206. There are online video tutorials on how to SMD hand solder.

Klaus