Help finishing design of a 3.3V Wii-IR-Cam PCB

Community PCB Design
1

Hi all,

I am really new to all this and need help by you.

I need a PCB to mount/solder the Wii-IR Cam on to get the data via I2C to my Arduino. Apparently there don’t exist any PCB to purchase, at least not a 3.3V version which I would prefer to use with my Arduino FIO.

After a lot of googling I found the spec of the pins of the IR-camera and some example PCBs (5V) and learned that I would need to use a 25MHz oscillator crystal to get it to work. At this point I decided to try to design my custom WII-IR-CAM PCB as a 3.3V version on my own.

Currently I am just happy that I passed the DRM-Check at BatchPCB.

I know that there may be missing some pullup/down resistors and decoupling condensators, too. The placement of the components and routing could also get a review.

Could anyone please help me to complete this design?

Attached you’ll find a ZIP-File containing my *.brd and *.sch file and also the crystal library I am using.

[http://www.mediafire.com/?d4zu8icbateudvu

Kind regards,

Christian

PS:

I didn’t find my fist try to post this topic, hopefully this is not a double post. If it’s actually a double-post feel free to delete this.](wiicampcb)

2

Well, don’t know if there was anything wrong regarding my questions, but I suppose I asked for too much.

I’d like to give my topic another try before vanishing on page two of “PCB Design Questions”.

Assuming that I connected all the nets right, what would be the next logical step to get a “good” PCB?

Adding decoupling caps? Adding Pull-Up/Down resistors? Or am I missing something else?

Kind regards,

Christian

3

To have the best chance of people reviewing things, post them here in pdf form. Many people won’t jump thru hoops to review a board.

I have never used the Wii camera, but here are a few notes:

Schematic:

  • Make a custom schematic symbol for the camera. It’s confusing going from the text notes about camera pin numbers to the schematic showing two 4-pin connectors.

  • Add a 100n decoupling cap for the oscillator

  • Add pullups for SDA and SCL, unless you will count on having them on some other device on the i2c bus. I would add them anyway as you can always leave the parts off

  • The reset pin needs a 22-30k pullup and a 100n cap to ground. In your schematic, the camera is always held in reset

  • QG1 is a crystal oscillator, not a crystal resonator

  • In general. positive power symbols point up and ground and negative symbols point down.

PCB:

  • Check the footprint of the camera; is the row-to-row spacing 100 mils or 150 mils?

  • You have text on pads, text off the board, and text on vias. These should be cleaned up

  • Vias usually are round - they take less space that way and that gives more options of how to hit them with a trace. Square thru-hole pads are usually only used for pin-1 indicators

  • Traces should connect to pads and traces at right or obtuse angles. Acute angles can trap acid during etching

  • Move the pin-1 designator for QG1 off the pad. Ideally, it should be outside the footprint so it is visible after the part is loaded

  • If you plan to hand-solder the board, I would extend the pads for QG1 a bit (10-15 mils) to give you a chance of hitting them with the iron

  • You have no mounting holes

  • If you have the space, add the board name, revision, and date on the silkscreen. Bottom silk is fine.

/mike

4

Thank you.

I will “rework” my board based on your hints.

When I get stuck, I will ask again and make a copy of the board in pdf form.

Maybe this board will get some more attention, when it’s done.

I believe there are a lot of useful and cool things to achieve with the IR-Cam (although one has to break a Wii-Mote for getting the cam).