SparkFun Forums

[xz124]

Hey everyone,

This is my first time designing a board, and I just wanted to get some opinions on what could be improved or changed before I sent this out to the fab. Thanks!

All Layers:


Top Layers:


Bottom Layers:

[Ross Robotics]

Since we don't know what the ICs are, you might want to post the schematic...

[MichaelN]

Looks pretty good, especially for a first board. I recommend you use the bottom layer as a groundplane as much as possible (i.e., minimise the number of tracks / breaks on the bottom layer). I’d suggest moving the capacitors currently on the bottom layer to the top layer (there is plenty of room). Right-angle corners in tracks are generally frowned on, so I’d suggest mitering these.

[leon_heller]

Ground and supply tracks should be wider, and each Vdd lead on the chip should be decoupled.

[n1ist]

I'd guess the IC is an ATMega328p as this is an Arduino-style board. In addition to what's been pointed out, you have a few potential acid traps (places where traces meet pads or other traces at acute angles).

As for caps, I'd add one more decoupling cap at least on the right side of the chip (possibly a bead and cap on AVcc if you plan to do much analog stuff) and a cap from Aref to ground.

I would also pour a ground plane on the back side. It would improve performance and get a few traces off the front.

You may want to look into rotating the processor 45 degrees; that's common on boards of this type to help with routing.

If your pinout can be changed, you may want to move AR to between 13 and A0 for better routing.

There are a few place where there's silk text over vias. That may end up looking rather messy (if the vias are tented) or not show up at all (if the vias are plated)

/mike

[InactiveUser001]

Move the crystal closer to the IC.

[Mach3Maelstrom]

Right angled traces are very bad, as MichaelN states. Not only are they acid traps (when chemicals are used to etch the board, those chemicals can get stuck in those corners), but also they change the impedance across the trace which can cause signal integrity problems. Always use two 45 degree angles.
As an example, your trace from IC to header pin 5 is good. The trace from IC to header pin A0 is bad.
SOLUTION: Rather than retrace them, use the miter tool in EAGLE. I use 0.01 or 0.02, depending on how much space I need. Then click on each right angle.

The ATmega16U2 requires both crystal leads to be grounded through 22pF caps. Not sure if this is the part you're using (you haven't answered the part number question yet), so just double check in the datasheet.

If I think of anything else, I'll let you know. Good job on your first board!

EDIT: I just saw the two caps & grounding, so nevermind that point.

[winston]

On right angled turns in traces, the trace is 41% wider at a right angle bend (the change in width is what changes impedance). At a mitred bend with the bend at 45 degrees, the trace is only 8% wider at the bend.

Now it's probably not going to matter much or at all if you have no high speed signals, but in any case it's best to use 45 degree bends. It also looks nicer.

[MichaelN]

Right angled traces are very bad, as MichaelN states. Not only are they acid traps (when chemicals are used to etch the board, those chemicals can get stuck in those corners), but also they change the impedance across the trace which can cause signal integrity problems.

Actually, I said they were "generally frowned apon". In reality you'd generally be fine using them - I've seen detailed analysis of high-speed circuits that showed negligible impact to impedance / signal reflections etc. As for acid traps, I'm not an expert on PCB manufacture, but I thought this wasn't really a big issue these days?

[Mach3Maelstrom]

winston: Thanks for the exact figures, that's pretty nifty to know.

MichaelN: We're getting slightly off topic from the OP since digital designs don't usually have as much to fear from impedance changes, but just to answer your post .

Signal integrity *can* suffer due to right angled traces due to the change of impedance down that trace. Perhaps the designs you're referring to weren't affected, but I'd prefer as small a possibility of failure as possible by eliminating trace angles as a possible failure point and use 45 degree angles. It's just good practice.

Also, acid traps aren't an issue when it comes to sending to a fab house. It's usually only a problem if you're etching your own PCB. My warning of acid traps was really a tiny point compared to the signal integrity problem.

xz124 (Original Poster): I'm interested in knowing how this project went. Again, congrats on your first board design!