First Time Using Eagle & Ordering PCBs, Can Someone Check My Work?

Hi,

I haven’t used eagle before this project, and I’m about to place an order for several hundred small pcbs, is there someone out there that could just look over my setup?

I’m making a pcb to solder 1000 of the SK6812’s (single color NeoPixel).

To save space I’ve made it double sided, putting a 22 ohm resistor and .1uf cap behind the led on the back.

There are also four solder pads that should be through holes.

White NeoPixel Eagle Files.zip (17.7 KB)

Don’t add the 22ohm resistor unless there is a long distance between the boards.
Otherwise the .brd file looks fine.

It's not a long distance between the leds, about 3". I was just following what they had done with the mini neoPixels, they have a 22 ohm resistor there, and similar boards.

Just curious why would I not need or need the resistor?

Resistor is needed for long signal runs to prevent electrical reflections from corrupting the signal.
See page 13 of WS2801 drawing.

Later parts, like WS2812B, do not call for that anymore.

Can’t hurt I suppose.

WS2801.pdf (423 KB)

WS2812B.pdf (381 KB)

I just looked at the files in Gerbv, the drill file ( .TXT) is a different scale and doesn't fit in the board outline.. I don't have eagle so it might be just a issue with Gerbv.. I would but try opening the gerbers with another viewer and take a peek.. might be an issue..

I would give serious consideration to just having say 5 boards built that you could double check before ordering the whole lot. Most projects that I have been associated with get a couple of boards as a prototype verification first then go for the production run (those first boards is where you go to put it together and say "oh crap - I forgot and reversed power and ground there" or something equally foolish (in hindsight).

Always open your gerbers in a gerber viewer (there's an online one, gerberviewer.com I think) and look carefully. This should ideally be repeated the next morning, with fresh eyes.

Always get a small run made first - your Rev. - board is usually going to be unacceptable for some reason, best to have only a few disappointing boards, rather than a ton of them.

If you're assembling them yourself, too, the Rev. - can also alert you to a decision that makes assembly harder, which you can fix in your production version.

Make the power and ground traces wider, especially between decoupling capacitor and the
chip. Low inductance paths are best to allow the decoupling capacitor to do its job best, a
good habit to get into. Low inductance means wide traces and preferrably ground plane.

Put the components all on the same side for ease of manufacture (unless hand soldering).

It you have done N copies in one piece as a line of snap-off boards you will save a lot of
board space in manufacturing and it will be easy to fabricate N at a time.

Ok, advice taken. I’m going to do a small run, get rid of the resistor, and increase the traces.

I uploaded everything to the gerber viewer and it looks okay.

I’m not quite sure how to check the scale of the drilling file though?

BTW, thanks for all the help.

White NeoPixel Schematic.zip (17 KB)

That doesn't look good to me...

You have the gerber export settings screwed up, the board outline seems to be on the top copper layer, not the milling or outline layer. See if you can get a recommended .cam and .dru file from your board house - these make life easier. These are what you're looking for when you check the gerbers. Is the outline layer correctly describing the outline? (no, there is no file in there that described the outline of the board, the layers I'd expect to have that are blank). Is the the copper layer showing the correct copper layout? (no, the outline around the edge connects all the contacts along the edge).

I think if you sent that to the board house you'd either get coasters with no milling and possibly all the contacts shorted, or a "fix your gerbers" email, or they'd mangle your design in some way not specified.

Bummer. I was using SparkFun’s cam file.

I think that the outline was on the wrong layer, I’ve since moved it to the milling layer. The thought with the contacts overlapping the edge was that the circle would be mill away the overlap, and give me a solder pad that went right up to the edge. Are you suggesting that the edge will be conductive?

White NeoPixel Schematic 041516.zip (17 KB)

Just figured everything out, and used this great 3d gerber preview to check it.

Turns out that the cam file had the wrong output for the drilling section. It was Excellon, and it should've been Excellon_24. Everything lines up great now.

Thanks so much for the help everyone - problem solved!