Hello guys i have designed 2 different PCB. And This product is gonna be a commercial product so it must be perfect. However i got some bad comments about my PCB design from 2 guys but i am not sure about trusting them. They said it will not work well and have some unstability in the future. Is there any exprienced guy who can check my EAGLE brd files and tell his comments.
Here is the new link there is schematic diagram also photos of layout.
caneradiyaman6:
Is there any exprienced guy who can check my EAGLE brd files and tell his comments.
I'm sure there is, but he'll have a hard time checking it if you don't post your design 
.
Explain why you can't trust them. What are their credentials?
here is my brdfiles and photos of my pcb. They are just telling it is not gonna work not telling the reason ?
pwillard:
Explain why you can't trust them. What are their credentials?
Because they are not telling the problem they are just saying there are errors and it will be many problems in the future
Post images of the board files, not eagle files, not everyone has eagle and image files show up nicely inline here.
Your decouple capacitors are remote from their pins using signal traces not power/ground traces.
You have many traces at random angles - definitely looks sloppy that.
Why have you made it hard to manufacturer by having complex SMT parts on both sides when
there's loads of room?
Without the schematic there's little else I can spot. Expect to make a prototype batch, fix
the issues that they show up and then it'll be good. To maximize chance of success first
time you have to double check every pin out, every trace and footprint. Printout the artwork
1:1 and place the components on top to check they fit even.
If you can place every SMT component top-side you make automated assembly way easier (cheaper).
There appears to be some weird routing, but that in itself is not normally a problem. We need schematics as well though and maybe a PDF/JPG of the traces for those of us that would rather chew there own arm off than install Eagle 
I never expect my hobby boards to be perfect the first time. I've had to have them redone. Occasionally, twice. I don't think people making commercial boards expect them to work perfectly the first time out of the gate either. You make the board, test it, revise it, and repeat that process until you're confident. Anyway, you really should make several and run them full time and maybe in a hot environment to age test them and see how reliable they are after 100, 1,000 and 10,000 hours. I would read up on electronics testing and accelerated aging techniques if I was going to try to make something for commercial purposes.
+1
I don't think I've EVER seen a board work first time without a green wire or two.
I always plan for 2-3 runs before it gets the nod although I admit this one looks pretty simple so that helps.
Here is the new link there is schematic diagram also photos of layout.
MarkT:
Post images of the board files, not eagle files, not everyone has eagle and image files show up nicely inline here.
Graynomad:
There appears to be some weird routing, but that in itself is not normally a problem. We need schematics as well though and maybe a PDF/JPG of the traces for those of us that would rather chew there own arm off than install Eagle
There seems to be a lot of empty space, and you mount the two chips on both sides of the board.
Production is a lot easier if everything smd is on the same side.
If you delete one track at the time, and manually re-route it, you will end up with a cleaner layout.
Order a $10 batch of five from China, and play with it.
Then improve your design further.
Leo..
That G3MB-202P relay is discontinued.
A 1N4004 diode across an opto LED? Not needed.
78M05. Needs at least 7volt. A 1117 has half the dropout voltage.
R3,4,5, etc. = 330ohm will be very bright. I already don't like Arduinos with a 1k resistor.
MarkT:
Your decouple capacitors are remote from their pins using signal traces not power/ground traces.
You have many traces at random angles - definitely looks sloppy that.Why have you made it hard to manufacturer by having complex SMT parts on both sides when
there's loads of room?Without the schematic there's little else I can spot. Expect to make a prototype batch, fix
the issues that they show up and then it'll be good. To maximize chance of success first
time you have to double check every pin out, every trace and footprint. Printout the artwork
1:1 and place the components on top to check they fit even.If you can place every SMT component top-side you make automated assembly way easier (cheaper).
First of all thank you for your all comments Actually that part of board is orginal arduino nano board which i took from this site. I changed it little biy i made the traces little bit wire and increase the clearence between traces. But i did not want to changed it too much. Because İ knew it supposes to work very well. That's why i have complex SMT parts on both sides. However it would be a good decision to change them when i reconsider the cost of them. And sorry i couldnt get the problem about capacitors. It would be amazing if you tell me which capacitors they are. and I mainly understand my problems. But would you tell that "this pcb wont be stable and will not work in the long term" ?
They are called bypass or decoupling capacitors. They're connected across the power rails to prevent noise created by fast-switching chips, and to be able to handle sudden changes in current draw. To minimize inductance from the PCB traces, they should be as close to the chip as possible, otherwise it won't be effective.
Take a look at this thread and the links that were provided by Coding Badly and myself.
Wawa:
There seems to be a lot of empty space, and you mount the two chips on both sides of the board.
Production is a lot easier if everything smd is on the same side.
If you delete one track at the time, and manually re-route it, you will end up with a cleaner layout.
Order a $10 batch of five from China, and play with it.
Then improve your design further.
Leo..That G3MB-202P relay is discontinued.
A 1N4004 diode across an opto LED? Not needed.
78M05. Needs at least 7volt. A 1117 has half the dropout voltage.
R3,4,5, etc. = 330ohm will be very bright. I already don't like Arduinos with a 1k resistor.
Also thank you so much for your warnings.
-i used relay to on/off a boiler. Circuit of boiler connects the relay from connector and when relay is close,boiler will work. I didn't get the meaning of discontinuity if i am thinking wrong please tell me ?
-I used the diode between activating voltage inputs of relay because i saw a circuit like that in internet. But obviously it is useless
-I also checked datasheet of 78M05 and saw the recommended operating conditions which is min 7V input voltage for 78M05 and thought about using 78m33 which has 5.3 min input voltage because i get input voltage from usb so it supposes to supply 5V. But as i said i thought it would be fine because it is orginal schematic of arduino nano. But as i understand i must change it thank you ! Also that regulator circuit has no filter capacitor. In datasheet there is Simplified Schematic and there are two capacitors for input to ground and output to ground. You think Do i also need to use them?
-For resistor values thank you for your advice i will make them bigger !!
caneradiyaman6:
I didn't get the meaning of discontinuity if i am thinking wrong please tell me ?
He means that the product itself is discontinued, it's no longer manufactured.
PieterP:
He means that the product itself is discontinued, it's no longer manufactured.
Okay sorry for misunderstanding. That's sad but i couldnt find any cheap solid state relay working with 5v activating voltage. It would be great if you know one ?
caneradiyaman6:
-I also checked datasheet of 78M05 and saw the recommended operating conditions which is min 7V input voltage for 78M05 and thought about using 78m33 which has 5.3 min input voltage because i get input voltage from usb so it supposes to supply 5V. But as i said i thought it would be fine because it is orginal schematic of arduino nano. But as i understand i must change it thank you ! Also that regulator circuit has no filter capacitor. In datasheet there is Simplified Schematic and there are two capacitors for input to ground and output to ground. You think Do i also need to use them?
The difference is that the nano is a 5V board, so it runs straight off of the 5V provided by the USB connection. If you want to use the onboard 5V voltage regulator (via the Vin pin) you need at least 7V as well.
This board seems to run @3.3V, so you'll need a LDO (Low DropOut) voltage regulator like the 1117 3.3v to go from 5V to 3.3V.
Are you aware that running an ATmega328P @3.3V/16MHz is outside its specifications? It's basically an over-clock. In normal temperature conditions, this won't be too much of an issue, but if you want to create a professional or commercial board, you have to take it into account.
You definitely need capacitors for your LDO. Reason 1 is stability, your regulator may be very unstable without it, check it in the 1117's datasheet, not just any capacitor will do, there are certain capacity and minimum ESR (Equivalent Series Resistance) requirements. The second reason is to filter out ripple from the power supply, and to prevent noise by the chip itself (especially by the ESP, since its RF circuitry creates a lot of noise). Use this larger capacitor together with a smaller one, as mentioned before, and don't use signal traces for your power connections.
caneradiyaman6:
Okay sorry for misunderstanding. That's sad but i couldnt find any cheap solid state relay working with 5v activating voltage. It would be great if you know one ?
That's strange, most SSRs use an optocoupler with some kind of current limiting built-in for the LED, allowing voltages from 3~4V up to 40V.
Edit: I'm sorry, I thought you had the ATmega running off of the same 3.3V supply as the ESP.
PieterP:
The difference is that the nano is a 5V board, so it runs straight off of the 5V provided by the USB connection. If you want to use the onboard 5V voltage regulator (via the Vin pin) you need at least 7V as well.
This board seems to run @3.3V, so you'll need a LDO (Low DropOut) voltage regulator like the 1117 3.3v to go from 5V to 3.3V.
Are you aware that running an ATmega328P @3.3V/16MHz is outside its specifications? It's basically an over-clock. In normal temperature conditions, this won't be too much of an issue, but if you want to create a professional or commercial board, you have to take it into account.You definitely need capacitors for your LDO. Reason 1 is stability, your regulator may be very unstable without it, check it in the 1117's datasheet, not just any capacitor will do, there are certain capacity and minimum ESR (Equivalent Series Resistance) requirements. The second reason is to filter out ripple from the power supply, and to prevent noise by the chip itself (especially by the ESP, since its RF circuitry creates a lot of noise). Use this larger capacitor together with a smaller one, as mentioned before, and don't use signal traces for your power connections.
That's strange, most SSRs use an optocoupler with some kind of current limiting built-in for the LED, allowing voltages from 3~4V up to 40V.Edit: I'm sorry, I thought you had the ATmega running off of the same 3.3V supply as the ESP.
I will consider all your points and fix it !! Thank you so much but why there are so many errors in arduino nano layout ? It is an open source product and there are lots of problems in schematic and layout. If i dirrectly imported the layout, i would have lots of troubles !!
An Arduino pin can directly drive the opto LED of an SSR.
No need to use a transistor.
Don't use a resistor in series with the opto LED if the SSR already has one (most do).
You mention "Boiler".
When I read that, I think of a 10-20Amp load.
The relays you are planning to use can only switch 1-2Amp.
My supplier stocks the FSS1-102Z 5volt.
Many cheap G3MB-202P 5volt on ebay.
Seems the same footprint as on your layout.
Leo..