Anyone willing to do a board design check? It’s a small wireless + Atmel board designed in Eagle. Yes, I plan on running everything off at 3.3V and the Atmel processor at 16Mhz. I know it’s not recommended. Any other advice/tips/complaints/suggestions are welcomed.
https://www.dropbox.com/sh/rco08u4monq9 … 91MAa?dl=0
Thanks.
First I don’t understand why people split up circuit diagrams into itty bitty sections that are nowhere near each other instead of having them flow as the circuit should?
On the PCB please recheck your GND return paths, currently its broken & all over the place.
i.e. C4, the GND on this should go directly back to the IC, instead it meanders around 1/2 the board to get back to the IC. Go direct.
Why octagonal vias?
Bottom left of the PCB is a 2 way connector, if that can go up a little then the long connector can be moved left so it is further away from the antenna so will have less affect on it.
Left side of C3 appears to be unconnected?
I don’t use eagle and am struggling making it view how I want to - to be able to see component outlines & names, but your caps etc do not appear to be close to where they should be.
You also appear to have way too many vias where they are not needed, a simple reroute will get tracks in without swapping back & forth between layers.
When I load this there is no copper poured, hitting the ratsnest button shows it? you could do with copper poured top & bottom for the GND.
Mattylad,
Thanks for the responds. I have a few questions/comments before I make some changes.
https://github.com/imagiro1/MRF49XA-Schematics
I don’t understand what you mean about the GND return paths being broken. I agree they are everywhere. But this board is pretty small. I feel like I didn’t have an option when laying out some of these traces.
Is there is a difference between octagonal and round vias? I don’t have a reason for using one over the other.
C3 is connected to ground.
I believe I have the caps close to their respective component. C7 and C13 are close to the micro. C4/C8 are close to the MRF49XA. I can print out a PDF if it’ll help. I also try to layout my boards with the top layer going up/down and bottom layer left/right. I agree this some times leads to more vias. But I find it helps when you have to “hop” over traces.
I’m not trying to argue any of your suggestions (except maybe for number 4). I really want to understand your suggestions before making changes to this layout. It was not a quick board to layout. Thanks again.
My reasoning on the schematic is that if the circuit flows as the signal & return currents then will then it can help you visualize and layout the PCB.
If it’s broken up then the PCB gets broke up, think your circuit is a “whole” not a jigsaw.
The PSU could all run together and into the caps in 1 long run rather than 3, U1 I would put on the right of U3 and connect it up then have the RF section further to the right.
input, process, output - left to right. 
Connectors showing where they are connected to without the reader having to hunt for it.
Re the GND, look at C8 and it’s GND connection, where is the other side connecting? (IC) yet the return path for that GND goes up, right, around the connector, down do C7 etc then back up to the IC in a big loop.
Instead of this big loop C8 could go directly to the IC centre pad in a short connection.
If you can now see what I mean by this, then look around the rest of the board for similar loops (I have not looked).
Vias - no there is no difference really, it’s just odd to see them as I know of no reason why they would be anything other than round (octagonal takes more room).
Caps, C4\C8 might physically be close but think about the signal that goes through them to gnd (as per the top comment about gnd loops).
If you swap C4\C8 positions you will be able to route it better.
C3 must have been a graphic thing because I have not got something turned on.
I have been playing with it but I cannot route in Eagle (IMO it’s horrid) otherwise would repost it with some differences.
Are the positions of the connectors all fixed? you have the USB top left providing power to the bottom of the board and data to the middle where if the USB was in the bottom left\middle then the connections would be shorter with less passing over the whole board.
But if your happy with the placement, I’d simply look at the connection lengths especially for the GND.
Matt