Hello! I’ve completed a pretty simple layout for my first board; it’s an overblown breakout board for a PIC 18F2550, with a crystal, programming header, reset button, etc, and would like some feedback on it, if you wouldn’t mind.
I’ve:
Run SFE’s DRCs, with no errors
Done a 1:1, and verified components
Viewed the Gerbers
I may run this all the way through fab, just to get the kinks worked out on something simple, so please give me what you’ve got!
Thanks in advance!
Robert
Supply and ground tracks should be a lot fatter.
Crystal capacitor grounds should be connected to the nearest ground pin on the MCU.
Right angles in tracks should be mitred.
Tracks should connect to oval pads at the end.
Tracks aren’t centred on pads.
Leon
Thanks, Leon!
I’ve made some tweaks, but I have some questions as well:
Supply and ground tracks - I upped them from .01 to .024. For a PIC, what do you recommend as the min?
Crystal cap grounds - They were/are connected to the nearest ground pin on the PIC, or am I missing something?
Right angles should be mitred - Check! 
Tracks should connect to oval pads at the end - Is it ok to come in at an angle, or should they be redirected to come in straight to the end?
Tracks aren’t centred - Given the grid size I’ve got set up ( 0.05, as per Sparkfun’s tutorial), Eagle doesn’t want to allow me to move the tracks in small enough amounts to center them. (See the track for RB0, for example). Suggestions? Shrink the grid size? The SF tutorial indicates that could cause some issues…
Thanks, again for your advice; I appreciate it!
–Robert
I missed the ground pin connection for the crystal capacitors.
Tracks shouldn’t connect to pads at an angle, it can cause etching problems.
I don’t use Eagle, but there is a way to ensure that tracks connect to the pad centres. I think that you have to start routing from each pad and connect the tracks in the middle. The software I use does it automatically wherever I start from.
Leon
IMO, if you are using double-layer, you should have one of the layers as ground plane if you can. I’m quite sure it will work anyway. But you said it yourself, you’re doing this to “to get the kinks worked out on something simple”.
The input power and ground traces should be increased as well.
Is that a regulator? Shouldn’t it have a filtering cap before it?
If you have two pads that you want to connect that are off grid, you’ll need to start the trace from one pad, cancel it half way, then start it again from the second pad and connect your trace in order for both ends to be centered on the pad. Or you can change your trace bending option to turn before the drop.
Since this is a double-sided board, I’d add a ground trace from the input connector directly to the regulator (and its caps when you add them).
/mike
Hiya -
the square pad of the component on the right (voltage regulator?) seems a bit close to the RC7 trace (I assume the square pad is on both sides of the board…) Likewise some of the traces around through-hole pins seem a bit too close to other pins. Apparently not so close that they fail DRC (since you say it passes DRC) but I’d be wary of getting traces close enough to solder pads that there’s a possibility of the trace leaving the solder mask area and potentially getting bridged by a solder connection… Likewise for some of the traces at the ICSP header - probably they’re safe, but personally I find them (like the PGD trace that wraps right around the PGM pin) too close for comfort. You’ve got tons of board space here, there’s plenty of room to spread some of these things out.
Also, the PIC datasheet says that if you use a strip-cut crystal you may need a series resistor on OSC2. Don’t know if it’s worth including on the board layout, but it’s easier to include it on the board and jumper it if you don’t need it than to stuff a resistor onto a board with no pads for it… It also might be worth providing a footprint for a ceramic resonator (either a ground pin in between the two pins for the crystal, or else a footprint somewhere else for a resonator…)
Regarding the power switch - aren’t the labels backwards? The power from the jack is connected to the board’s power bus when the middle pin is bridged with the one on the right, but the “on” label is on the left…
Why the via between the power jack and the “P-IN” pin on the right side of the board? Seems like you could just make that a top-side trace.
And - all this and no footprint for a USB connector? I mean, I guess if you’re just planning to hook this up to a USB cable or use the pins on a solderless breadboard, then the footprint for a USB connector is just wasted board space you need to pay for. But it seems like one of the main advantages of working with the PIC 18F2550 is to use the USB features - I’d at least throw a mini-B connector on there.
FWIW - I recently designed a small breakout board for the surface-mount version of the 2550, [here. (Warning - I have not yet tested the boards since receiving them… Link is FYI only) I designed the board primarily for converting existing I/O devices to USB. In retrospect, there are a few features I wish I’d included on the board:
I probably also could have included the PGM line as you did, to do low-voltage programming - but I never use LVP…](OSH Park ~)
Thanks for everyone’s feedback! I’ve got to do “real” work tonight/tomorrow night, so will be updating my layout later this week.
Thanks again for everyone’s input!
Robert
