Hi, I am a student of Electrical Engineering and I designed a pcb required for my project at the University. The board contains Renesas uC (144 pin), two CAN transceivers (MCP2551), PC-104/Plus Connectors (PCI+ISA), four analog multiplexers/selectors (40520). If you can have a look at the pcb and give your feedback, that would be of great help. Please point out even the very obvious mistakes. Thanks!
Sorry, I don’t have time to review properly, but here’s a few points:
-
It would be good to see a ground plane. If you could do a 4-layer board that would be best, but if not I suggest pouring ground planes into the unused space on both layers and “stitching” the top and bottom planes together using vias at a bunch of places. Move tracks around as needed to obtain the most complete ground plane possible.
-
The microcontroller should have decoupling capacitors on every power supply pin, located as close as possible to the pins.
-
It’s hard to tell, but it looks like some of the text on the bottom silkscreen is covering the component outlines on the silkscreen.
-
You have a 100uF capacitors, but they are shown as fairly small (0805?) packages on the PCB. The smallest size 100uF capacitors that I could see were 1206, and they are rather expensive. Either change these to electrolytic types or choose a package size that you can actually buy.
-
Power and ground both need to be much wider to reduce impedance and voltage drop. As mentioned, try a ground pour on one side and minimize routing that cuts the pour, or at least tie sections of the pour together with a number of wide tracks.
-
Check your processor’s documentation on the preferred way to route the ground to the caps on the crystals; many prefer that ground to go directly to the processor before hitting the rest of the board; right now, the LED signals will modulate the crystal ground.
-
Bypass caps really do need to be as close to the pins on the device they are powering as possible with low impedance traces. If possible, the power trace should hit the cap first and then the IC. If it feeds other parts, it should branch from the cap.
-
It’s hard to tell, but maybe rotating the processor CCW by 45 degrees may help.
/mike
I’m certainly not an engineer, but I’ve been designing PCBs for a while. I have to say this is the nicest first board I’ve ever seen. I don’t have much in the way of electrical advice, more just visual.
I think your bDocu layer is blue, which is the same color as the bottom copper layer, so you might want to change that. Not an issue, just a bit confusing at first.
See this image:
You do quite a bit of the first part, where there’s an angle less than 90 degrees. The ones that look like that can mostly be turned into the second part. Always try to avoid acute angles. In fact, you should almost never have to use them. If you need to though, try to put some relief of them like you see in the third part. Some people insist on cornering every right angle on a PCB, but I don’t bother because these days it rarely makes a difference. You may or may not be marked down for not having them though.
These, although they make a right angle, can easily be turned into a “T” which looks better and doesn’t needlessly bend.
There are also some traces on the top that look like you were following the bottom when you routed them, so without the bottom layer visible, they might look strange. One more thing is that the vias on the thicker traces appear to be mixed. Some look bigger and some look smaller, but it’s difficult to tell from the EAGLE rendering.
Hopefully this helps a bit. Keep up the good work! 
@Michael, Mike and Rolf
I could succeed incorporating most of the changes suggested by you. Thanks a lot. I appreciate it. I owe you a treat if I get good grade 
Rolf special thanks to you for the images and your nice words
You have some traces going across a number of pads on the left side of the large IC. I generally try to avoid this as it can look like a short when assembling prototypes.
I agree that this is a nice looking first layout!