My First PCB Design

[MrAureliusR]

And I did most of it myself, just learned the basics of Eagle and away I went. I have a pile of ATtiny13A's sitting around so I wanted a breakout board, and figured I may as well design it myself.

I'm open to being torn a new one, I really need to know what I did wrong and what I can improve. The big thing I'm wondering is if you should ground plane both sides or not. I'm fairly sure most designs I've seen only have one side planed.... or am I totally off there?

There's a couple small mistakes I've noticed but mostly I'm proud of my first design

[free_electron]

-it is a bad idea to have a larger cap AFTER a regulator than before. at poweroff current can reverse and destroy the regulator. put a diode in reverse from out to in.

-100nf cap around regulator ?
-via holes are too small
-holes on bridge are too small
-CN1 . what is with the elefant holes ? can we have slots please ?

- kill two vias from + of c1 on top layer go directly to LED1. that kills two vias below C1.

ISP1 connector.
-the trace from bottom left going inbetween : rout that down , right and up to the right of the 8 pin header.
the trace from left colum middle pin , go left, down , right , up and connect o pin 3. that eliminates the via at PB2
now pb3 trace can be routed left and down to pin 1 of JP2. eliminates a via.

you can get rid of all vias.

[MrAureliusR]

Excellent, this is exactly what I need to hear. Are you saying I should have a 100nF cap across the reg?

Going to start making changes now

[c4757p]

The big thing I'm wondering is if you should ground plane both sides or not. I'm fairly sure most designs I've seen only have one side planed.... or am I totally off there?

At lower speeds like this it doesn't matter. Usually, I fill just the bottom layer with ground plane, then try to route the top layer like a single-sided board as much as possible so that the bottom ground plane is mostly unbroken. I could add ground plane on top too, but usually the bottom one is pure enough that it's not required, and I think it looks better without (as well as giving fewer places for shoddy PCB makers to bridge traces to the plane).

I've been doing a lot of boards lately that have relatively high frequencies at relatively high impedances, so that's part of why I keep the ground plane away on top (reduces capacitive coupling). Sometimes I will add it back in sections, after finishing the layout, in areas where I know it won't be a problem.

[free_electron]

here you go

[MrAureliusR]

Thanks free_electron! I actually made one of those changes on my own! (At least my grey matter does it right sometimes  ) Thanks c4757p as well. I ripped up almost all the traces and am re-routing. Going to add the extra caps now (already swapped the 1000/470)

[mariush]

I was just about to say that ... the 1000uf capacitor after the regulator is a bit silly.  It would make more sense to have there a diode between output and input. 10-47uF 10-16v electrolytic capacitor on the output should be enough.
Add a 0.01 uF capacitor in parallel with that 470uF capacitor. Speaking of which, it may be too small.

The 7805 needs about 2v above 5v to output your 5v... so you need a minimum of 7v on the input. 

Now I don't know what AC power source you have... assuming 7.5v ac , you'd get after rectification and considering the drop on the rectifier about 9v DC max. If your board is going to use let's say up to 0.25A (the controller and a few leds or something) then to have 7v DC to the 7805 you'd need  C  = ( Current ) / ( Vripple x 2 x ac frequency) =  0.25 /  (9v dc in - 7v dc minimum) x 2 x 50 Hz = 0.3/200 = 0.00125 or about 1250 uF

With 12v AC or higher, the 470uF capacitor would be enough.. but anyway.. it won't hurt to go higher in capacitance at input.

One more observation... I don't understand why you'd use that footprint for the bridge rectifier. You don't need a bridge rectifier in such large package - those through hole rectifiers are usually for several amps of power ... your 7805 can barely do 1.5A or something like that, and the microcontroller itself is unlikely to use more than 0.5A. It will just make your board tall for no reason.
So why not just put 8 holes for 4 plain 1n400x diodes, or footprint for a bridge rectifier like one of these:
1 : http://uk.farnell.com/multicomp/w01mg/bridge-rectifier-100v-1-5a-wob/dp/1861435
2 : http://uk.farnell.com/multicomp/di152/bridge-rectifier-1-5a-200v/dp/9380760
3 : http://uk.farnell.com/fairchild-semiconductor/df02m/bridge-rectifier-1-5a-200v-4-dip/dp/1467465
4: http://uk.farnell.com/vishay-general-semiconductor/df01m-e3-45/bridge-rectifier-1ph-1a-100v-dfm/dp/2101159

All perfectly good choices.

Same with the 7805 linear regulator. It's unlikely you'll need a heatsink for it, but it may be a good idea to flip it the other way around so that you could bend the leads 90 degrees and have the regulator use less space vertically.

With a bit of effort you could also make the board one sided instead of double sided.  Worst case scenario, you could simply use some 0 ohm resistors as jumpers over other traces.  May not look as nice but it would be a board cheaper to make.

[MrAureliusR]

The reason I used the through-hole rectifier is that I have a shit ton of them in a few tubes here. I put the 1000uF after the rectifier, and 47uF after the regulator. Added the diode and small cap per free_electron's comments, re-routed quite a few traces, and eliminated all the vias.