Yes! I assumed they were unnecessary but left them there.
Ill remove them and order this PCB and give it a try, thank you again!
wait! don't hurry!
Take a little time to think about any other modifications that can be made before ordering the PCB
same case with ALL the GND connections. It’s not neccesary to put traces.
I assume the main polygon pour is connected to GND right? In both layers, like this
to make a connection between both coppers pours only place vias
Did you make that connections manually? The tracks are too thick
If you are going to use relief connections this width is ok
and the result would be
I was a little bit too fast, but I was able to pause the order 
Ive now removed all of my GND traces, and re-routed with auto-routing everything except the GND layer, and have quite a lot to fix and route manually for the GND to pour connections.
Do you recommend doing auto-routing when theres quite a lot of connections or should you always do it manually yourself?
Thanks!
I have now rerouted all of the traces, I am not sure how to setup the “relief” connections in EasyEda.
Here is my full PCB layout now:
Does too big GND connections cause trouble?
Ive now removed all of my GND traces
good! Looks better.
Do you recommend doing auto-routing when theres quite a lot of connections or should you always do it manually yourself?
This is a personal opinion: I don’t trust auto-routing and I don’t use it. I always use manual routing.
I have never used EasyEDA, I just donwloaded it, so to fix these connections you must do the following
Please tell me if you did it like this:
Imagine this is you design and you want to add a cooper pour connected to GND:
step 1: make sure you are on top layer
step 2: Go to copper area
step 3: select rentangle (or polygon in your case)
step 4: select the region you want to fill with copper
step 5: make sure to select GND in “net” field and press “Confirm” button
you will see this
copper pouring automatically connects the PADs to GND
step 6, Informative only: to change this conductor width (I don't recommend it)…
…select the copper puor and press the gear icon
change the “spoke width” field (remember, informative only, don’t change it) and press confirm button
step 7: select “Rebuild Copper Region“ button
note how the track width changes. (keep it at 0.254 mm)
Or you can select a direct connection
oh… repeat the same steps for bottom layer
you can use another polygon to connect the pin 1 of your inductor with the pin 8 of U3 (you will need to move the capacitor C8 a little and maybe also C52)
like this
connect some vias to GND pad of U3
like this
Check the width of this track (you can use another polygon in U12)
This track and many others:
I mean, this:
or this
instead of
this via is very close to the other pads, you have a lot of space
1 Like
Thank you! It feels like you almost helping me way too much, but its very appriciated! 
I see that my “spoke width” default setting was at 0, so it probably did the connections as big as possible, I changed it to 0.254mm now!
(Did it for both layers)
Something like this?
I have thought about this, but I wasnt sure if it was possible, added now!
Is this enough?
Ive made sure that the main-power trace is pretty wide on the bottom layer:
And that small trace is just powering my EEPROM memory.
I have also added a polygon here to the capacitors for the ATmega2560 processor, but I think that they will increase the stability of the 5V line for the entire board since everything goes through that?
Thank you again!
I changed it to 0.254mm now!
Perfect!
(Did it for both layers)
great!
Something like this?
beautiful
I have thought about this, but I wasnt sure if it was possible, added now!
Is this enough?
My recommendation is that you do not place ant track under the thermal pad. just move the tracks
Haven’t you changed the location of this via?
Regarding the voltage regulator U12, you can do this
Do you need a connection through the bottom layer? Then put some vias
is this pin not connected to anything? What is the part number of U12
I have moved it now, tought I moved it, but maybe tha autoroute moved it, and I missed that, sorry, my bad..
I also moved the powertrace underneeth and added some more vias to the thermal pad!
Also looks much better and a lot cleaner.
Ive now changed the layout to look like this:
I think that Ive now officially fell in love with polygon, they look so good in combination with the copper-pour!
I have no connections to 3.3V on the bottom layer anymore, I moved a lot to the first layer instead to make thing easier. I wanted to move all of the “general” components to the bottom layer, and just have the “cool components” on the top layer, but that will be something that Ill start working on once this version works as it should!
This component had two VOUT connections, so I just used one, but Ive now also added that other VOUT to the 3.3V net.
Thank you for all of the help!! Do you have any other comments before I update and place my order?
pefect, good job! And yes, looks cleaner
Regarding this polygon, I see it is VERY close to the edge of the PCB, modify a little bit the shape of this polygon
with a diagonal line so that it is not so close to the edge
Beautiful, just move this GND via up a little bit
also this one
Be very careful also with this pads that are very close to the edge
Is this component (U11) the ESD protection diodes for the USB connection?
If so, make sure it is close to the USB connector (Although the space between the USB connector and U2 is very small, it will be difficult to work there)
otherwise, ignore What I said
regarding this track
check the clearance of these two lines
increase the gap between these two tracks
too close!
this another thack is very close to the pad
Wouldn’t it be better to rotate R4 and R5 180° in order to make a straightforward line?
too close
these thre lines
I mean
No:
Yes
Fixed!
Fixed!
U11 is actually a BMP280 air preasure/temprature/humidity sensor.
That looks weired, I will have to stop with the auto-router now I feel like, but fixed this too!
Increased the space a little bit now since I got plenty of extra space.
I saw that I got DRC errors for those, fixed now!
Yes! Fixed, I also modified theese to get better routes:
I have also done the rest of the modifications, except at SW1 since those pads that they cross arent used, only one side of the button is actually wired.
This part still gives me anxiety..
Here is the fill PCB layout now:
For someone with not as much experience in PCB design/layout, it starts to feel pretty good!
Good, although I still see some tracks that are very close to others pads.
This part still gives me anxiety..
Yes, but without a schematic of that part I can’t help much. I need to know the part number of the components
1 Like
I have now received the PCB and soldered it and it works amazing! Solid 5V on the 5V line and 3.6V for my 3.6V line!
Thank you so much for the help!
All of the I2C devices works too, but I am struggling to solder a solid connection for my IMU (BNO085) which is also at that “anxiety” part of the PCB, but it works very short in bursts right now every now and then, so the schematic should work, I have copied the components and wiring from the BNO085 development board. But its very very tiny to solder, and has quite a lot of pads. But that Ill work on myself!
Thank you again!
1 Like