Please review my first PCB!

[ohfour]

Hi all

I've just finished designing a PCB for an LC meter based loosely on this circuit: http://www.rfcandy.biz/communication/imp_lc.html

Since it will probably take a month to get the boards manufactured I thought it would be wise to seek a little feedback from you guys before I sent it off!

I have built a prototype using leaded components and a breadboard to prove that a) the reference schematic is correct, and b) I can actually use the mega328P the way I had envisaged. I have also double checked the pattern and datasheet pinouts, and physically laid the components out on a printout of the PCB to check sizing.

Since I've never used SMT or made a PCB before it's hard to know whether I have made any bogus assumptions in the translation from through-hole to SMD, or about PCB design in general. Enter EEVblog experts!

The circuitry around U2 is the oscillator and operates at <580kHz. The two relays on the back are used to switch in a calibration cap and change the LC tank configuration for measuring either L or C. I have tried to keep the traces and layout in that area fairly tight to minimise parasitics, though I'm really just guessing at how well it will work (for reference, it works fine on a messy breadboard so this probably isn't actually too critical).

[Charles Creations]

Looks great. The layout is fairly spread out. I think you could definitely make it more compact, and I suspect your board cost is a function of area. You could reduce your price by shrinking it. If you have the extra space, you might also just increase the widths of your traces. Wider traces will always help out if you have the room.

[KJDS]

From a first glance, there are a number of unconnected areas of copper pour wich should either be connected somewhere or removed.

The 14 way connector appears very close to the edge.

It's probably worth adding some copper round the fixing holes.

[ohfour]

Looks great. The layout is fairly spread out. I think you could definitely make it more compact, and I suspect your board cost is a function of area. You could reduce your price by shrinking it. If you have the extra space, you might also just increase the widths of your traces. Wider traces will always help out if you have the room.

Yeah I could compact things a bit more. It's a 60x85mm board and cutting 7mm off the bottom would save me a square inch. I originally decided not to since it seemed like it would be a bit small, but looking at the printout I think 53x85 would be quite a nice size.

From a first glance, there are a number of unconnected areas of copper pour wich should either be connected somewhere or removed.

The 14 way connector appears very close to the edge.

It's probably worth adding some copper round the fixing holes.

I double checked the 14 pin connector position and it was out by 0.33mm. Good spotting

All of the poured areas are connected, although the one under REL1 is only connected via a single spoke. That part of the pour isn't used by any vias though so there should be very close to no current through the spoke.

[KJDS]

All of the poured areas are connected, although the one under REL1 is only connected via a single spoke. That part of the pour isn't used by any vias though so there should be very close to no current through the spoke.

Now you've pointed it out I can see it is connected.

Rel1 looks very close to the two connectors, will be awkward to solder it with the connectors in place.

[G0HZU]

I'd add a few test point via holes in several places. Think of all the places you might want to connect a DMM or scope probe. Also, add a ground test point to allow easy attachment of a scope probe croc clip.

I can't immediately spot any large decoupling caps on the 5V rail. eg 47uF. Is this part missing?

I would also add a few ground 'islands' on the non flooded side in case you need to add a few shunt components during troubleshooting. At the minute it doesn't look like ground access is very good on one side of the PCB if you need to add bits. There's nowhere easy to solder to?

Same goes for the 5V rail. Maybe add a few 5V islands.

Some of the track connections to your connectors look very skinny and weak. Maybe teardrop these?

Can the PIC safely drive the relays without damage from voltage spikes from the relay coil?

The track connections to the 5V regulator V1 look very frail. Especially on the ground pin. If you had to desolder/swap the regulator in the future the artwork looks easy to damage. Maybe beef it up a bit here and maybe have three ground vias to it. Also, have you worked out how hot the reg will get? Does it need a wide copper fill to act as a heatsink?

Add some copper text to the top/bottom layer such that it makes it harder to end up with a PCB that comes back mirrored.  A classic error for a newbie is to send out artwork data that is mirrored and the PCB comes back useless because the artwork is mirrored and the SMD parts will only fit the board if you fit them upside down.