SparkFun Forums

[henrymound]

Hello! This is my first post, and my first PCB. I created a board that (hopefully) has 12 individually addressable RGB WS2811 LED's (also known as Neopixels). Here is a schematic that demonstrates how the LED's should be connected. I based it off of the Sparkfun breakout board. Here is the LED pin-out for reference.

Here is my board:

And my long Schematic:


Any help, comments, and ideas are greatly appreciated. I am planning on getting 6 made with OSH Park soon.

[Ross Robotics]

You need to post large images if you want a detailed review and attach them to the post. There should be no 90 degree corners on the board. Have you ran a DRC check with OSH Park's DRU file?

Smash the parts so you can move the lettering around.

[henrymound]

Thanks for the advice, I will change the corner angles. I got a quote from OSH Park, and I didn't get an error for the sharp corners. I have posted large images for the schematic here: http://i.imgur.com/NdibXe3.png
And a large image for the board here: http://i.imgur.com/NwRtska.png
Do these have a high enough resolution? Thanks!

[Ross Robotics]

Those aren't much bigger than the ones posted. In Eagle, File>Export..>as image. Browse where you want the image and name it. Set the DPI where the image is higher than 1000px. Then export.

It's not an error that there is 90 degree corners, it's not good practice. 90+ degree corners can cause acid traps, where the copper will fill the gaps. All corners should be 45 degrees or less. It's also good for current flow..

When you upload your board to OSH Park, it will NOT give any errors. It's up to you to check the board for errors. You need to download OSH Park's DRU file. Place it the DRU folder under the Eagle installation and run a DRC check with that DRU file loaded. http://oshpark.com/guidelines. The link to download is under Design Rules. http://www.instructables.com/id/PCB-Cre ... ule-Check/ - instructions for running the DRC check. NOTE: you do NOT need to change any rules once you load OSH Park's DRU file.

[InactiveUser001]

How are those capacitors connected?
I only see connections on one side.

The big thick track, I take it that's gnd? it seems to be going from one side to the other yet could be completely routed on the red side.

The input middle pin appears to go over the thicker track on the red side also. How many layers is this?

Can you explain the differences between the track colours and are the leds SMT versions? (you appear to be connecting to them on different layers yet have blue tracks running under the pins also?)

[henrymound]

Hello again. Thanks so much for replying. I made all of the changes that codlink suggested. I smashed all of the labels, and cleaned them up a bit. I also modified the electrical connections so that they are all under 45 degrees, and I checked the board with the OSH DRC file. I fixed a couple clearance errors, and now the board complies with the DRC restrictions. Here is a higher resolution image with the changes.

To answer mattylad's question, the big thick track is a 5V rail. The capacitors are connected to the 5V, and the rest of the board is a ground plane. Here is an image that has the ground plane visible. The LED's are all SMT, and they are only connected to the top red layer. The input middle pin is connected to the top center pin of the LED. (The data input pin). I hope this answers your questions, if you have any more just ask.

[Ross Robotics]

Getting better. I like mine to be as professional looking as I can make them. I don't ever use rounded corners, but it's your board. You could save some money and make it alittle smaller..

But other than that, triple check everything. Once you order the boards, you don't want coasters..

[n1ist]

The GND pour is cut into two unconnected regions (INPUT and the top row isn't connected to the rest) and what you have is broken pretty badly; try to envision the return currents and how they flow. Since you aren't using the back side for anything other than power distribution, consider moving the data chain to the back side. I'd use smaller vias, right next to the LEDs. That will let the top pour work better.

You don't have any mounting holes; not sure if you need them.
/mike

[qwertymodo]

Personally, I would connect the middle and bottom row of the +5V trace on the left side rather than the right, creating a single continuous 'Z' shape rather than the current '3' shape. That way, you only have a single current path, rather than branching like it currently does along the right-hand side. Also, as n1st said, your Gnd plane is disconnected. See the yellow air wire on the left-hand side? That's telling you that the Gnd signal at the through-hole pad isn't connected to the Gnd pad of the capacitor (it only checks at actual connection points like pads, and it's showing the nearest two points that represent the disconnect, so really, the entire top section of the top-layer Gnd pour isn't connected to either of the other two sections). I'd add a Gnd pour on the bottom layer too, for good measure.