Hello everyone. I set out wanting to create some hardware but I have zero experience on the hardware side (I’m a software guy). I ended up finding an Eagle schematic and board that is exactly what I want for the hardware. I’ve generated the Gerber files, but the problem is I have no idea if I’ll get a workable board out of them. Can anyone take a quick look and see if anything is wrong? All of the files can be downloaded here: http://members.cox.net/fhriley/vpw_interface.zip. Any help is much appreciated.
Can you also post the schematics and a part list? can you buy all of the parts on this board? Parts change fast these days! Do you have the equipment to solder them?
The gerber files, the board file, and the schematic file (all in Eagle format) are included in the zip I linked in my first post. Unfortunately, I don’t have a parts list, but from the schematic I know what parts are needed, and I can get all of them.
I have a friend that has offered to help me with the soldering.
That’s a weird way to do a schematic, it looks like a netlist. Why don’t you connect the parts together, it would make things much easier?
You should decouple both supply pins on the chips.
Leon
Like Leon said, you probably should connect parts together in the schematic.
Saying that, on larger projects I do what you have done quite a lot, but usually only things like SPI/I2C nets or connectors, it keeps the schematic neater.
As far as the PCB goes, by the looks of it you have hand routed it. I ahve to say if this is your first PCB routing it does look very very neat. Nice to see all those 45deg bends. At a glance I think I only noticed one or two 90deg bends I would get rid off, but that’s a personal thing more than a functional thing.
Is there any reason why you have put the PCB on the left side of the 0,0 cross-hair? You must have the professional version to be able to do this… or a “borrowed” copy.
It seems to pass DRC, although I do have my own rule file that I use so depending on where you get it fab’d you may want to check that if you haven’t already.
As far as the circuit goes, you probably want to check the datasheets on the IC’s and make sure you have the relevant passives in place. Meaning those IC’s will probably need decoupling capacitors.
One last thing. You seem to have used quite a few 0402 sized passives. Are you sure your friend can solder these?
You could probably quite easily use 0603 or even 0805 size parts in these places without making the board any larger, and make a much easier job for your soldering friend.
Now a question for you. You have a board edge ISP style pads on the board, I have always been interested in these. Could you post up some details as to the stool/connector you use to “plug” onto the board.
Ditto that comment. 603 are the smallest i can do with whining. i tried some 201's once. that was craziness.gussy:
One last thing. You seem to have used quite a few 0402 sized passives. Are you sure your friend can solder these?You could probably quite easily use 0603 or even 0805 size parts in these places without making the board any larger, and make a much easier job for your soldering friend.
You have three parts on the schematic that are pins only. It works, but is a bit confusing. If you created symbols for those items, the schematic would make more sense.
The board looks like it would work. I don’t see any glaring oversights.
I’d third the thing about component size - it seems to get exponentially more difficult once you start going below 0603 for chip capacitors/resistors etc. Don’t sneeze! (and also, it seems to get exponentially more difficult below 0.5mm pitch on ICs - I find 0.4mm pitch LQFP an order of magnitude harder to get right when soldering compared to 0.5mm TQFP).
The easiest (certainly the tidiest/best looking solder joints) I’ve found with 0603 passives and fine pitch SMD is to use a syringe of solder paste and hot air, rather than a soldering iron.
I’m not the OP…I got bored one day 
and re-drew the schematic so it looks like a schematic and not a collection of parts. I don’t know what U3 is because the original designer didn’t label it. There are also some other “mystery” parts. Then I decided to play with the PCB layout. I changed the 0403 resistors and caps to 0603, because like others, I felt the 0403 parts are too small. I changed the SMD crystals to mini Through-Hole (TH) because the TH crystals use less board space. I added a bulk cap to VCC, and added VCC & GND test points. I moved parts around to reduce clutter and I even have readable part designators on the board. I moved U2 (FT232RL) below the USB connector, but it’s still a tight fit. I didn’t move any of the connectors. The 6-pin ISP connector puzzles me. I don’t know how the user intends to connect to it. Using a 2x3 pin header would be much simpler. I moved the GND plane/pour to the top layer because almost all of the traces are on the top layer. I moved the VCC pour to the bottom layer. I’ve created the Gerbers and it checks out OK. I’d attach it as a ZIP file, but I don’t know if the forum software will let me do that. Note - all work was done with EAGLE v4.16r2.
-Dave Pollum
I just spent a couple of minutes importing the schematic and PCB files into Pulsonix. It converted OK, and I could redo both the schematic and the PCB quite easily if I also imported the Eagle libraries. Here is the imported PCB:
http://www.leonheller.com/Designs/vpw_interface_pcb.gif
I didn’t pour the copper on the top and bottom layers for that version, so it looks as though a lot of parts aren’t connected. I did the copper pour and ran the Net Completion Report - it showed a gap in the ground connections. This might be due to the different spacings that I’m using.
I can’t see why he’s used 0402 Rs and Cs, either.
Leon