Sanguino based game pad

Ok, so I got bored of making kits quite quick, once they began working reliably... I'm a teenager, what do you expect? Anyway, I decided a cool project over the summer would be to design a board from scratch, get it etched (Mum doesn't like the idea of me doing it my self, something about an ecological hazard?) so, before I go too far down the design process this is what I have so far (dropbox link) is this OK? Is there something I should change? Because of the spacing of the pins on the FT232RL chip I used a 10mm routing grid, is this OK too.

Also, any ideas of hardware to add to the board would be appreciated, not a ADC chip though, those things are remarkably expensive :P

Things I may / may not add: - SD Card slot - EEPROM - RTC Chip - a bit dear, but could be worth it. - RAM? - PS2 Port, for using a mouse or keyboard (I have seen a xxDuino do this before, and I think it is in the playground, it could be quite cool. - Composite out port - Extra control options, ie, Pots, LDRs, (not a accelormeter, I'm not made of money)

any thoughts are welcomed. If I get it made at sparkfun I may have some PCBs to sell back to you guys to help fund it ;)

Regards, /me

I had a brief look at this, I can't see what the clock & data pins on the PCF8574T are connected to?

Edit

I'm a teenager, what do you expect?

I expect you to sit down, be quiet, study hard and listen to your mum :)

jabber, I saw that shortly after posting, I made some other "minor" changes too, these are the revised files.

I would maybe try something a bit less ambitious on a breadboard first. Trying one step at a time. Going with an untested pcb design straight off will lead to expensive problems.

Do you have a link to a pdf file?

(* jcl *)

PDF of what? The schematic / board files?

Both.

(* jcl *)

Sorry, I should have mentioned that the 20 pin header is for the GLCD. It has an odd pinout.. I was too cheap to buy the normal one so spent the time decoding the chinese datasheets... I've tested the pin out with a normal Arduino.

Disclaimer 1: I'm still pretty new to all of this and have only started serious tinkering 6 month ago Disclaimer 2: I etch my boards myself, therfefore i tend to not use anything less than 10 mil

Couple of thoughts on the pcb: I can't see myself etching anything like this at home, so if at some time you might persuade your mom to let you do it, you will need to adjust quite a bit.

If you stick with one trace width, make it thicker. You have a 500mA fuse and the trace leading to and from it are 6 mil. This will work, but the traces might already start to heat up by 5-8 degree Celsius (10-15 F), before the fuse blows. I usually pick something pretty thick as a standard (32 mil for self etched, maybe 16 mil for professionaly made) and only decrease trace width when necessary. You can change the width of multiple traces by selecting them (one by one, or with the "selection rectangle") and using the wrench tool. Also 6 mil trace might cost extra.

Do you know where you want to manufacture your board? If so look up there rules regarding thickness, spacing, etc. Maybe they even have DRC (Desing Rule Check) settings, which you can use to check your board before sending it to them.

The idea of the capacitators C1 and C5 is to smooh any irregularities in the power supply for the ICs, therefore they should be as close as possible (in terms of electric connection) to the respective power pins. As it is, they are all pretty much near the power regulator.

You have some very tight areas, and some very roomy ones, use your space! For example below the ATMega you have four traces running in 0.7mm distances. You even have dents in one to make room for a via. But to the right of it you have 50 mm of completly free space. This will also help with manufacturing tolerances and might make soldering easier.

Be carefull what you finally use as the silkscreen. If you print over any pads you might not be able to solder to them later on.

In general you should avoid sharp edges in traces. This isn't really a problem for anything on the scale of an arduino, but it might be a good thing to start doing this early on.

Just to make clear: This is not bad for your first board, there are a few neat areas in there. I just agree with jabber that it might be to ambitious. If i design a shield, i usually got through 3-4 prototypes, before i'm happy. And even after that i still find ways to improve it. I have the advantage, that i can make one prototype Friday evening, test it on Saturday, make some changes and etch a new one on Sunday. If you make new revisions, you will have to pay and wait for it each time.

I would recommend always testing a circuit on a breadboard first (depending on the complexity this can take days), and for smaller things even using stripeboard or perfboard for the first few prototypes.

Sorry for the long post, i hope i didn't sound to negative. Bye, NsN

If you're looking for a (more) inexpensive method of fabricating PCBs professionally, you may want to take a look at DorkBotPDX's group orders:

http://dorkbotpdx.org/wiki/pcb_order

What they do is panel all of the PCBs together, then order a giant board. They then separate the individual boards and ship them off to the correct people. It comes out really cheap ($5 per Square Inch for 3 boards; including shipping!)

Just an idea :).

Tchnfl that is awesome! I was going to go with something like what seeedstudio does, it is for 10 boards, I know, but $40 is dear. I would get more PCB for the money though... 160 Sq inches... 4*4x10. (I think thats right..)

It depends on whether the is interest in the board..

Check & double check the schematic. What is the top end of F1 connected to? How do you set the address of the PCF8574? Are the SDA & SCL pins connected to the correct pins on the MEGA644?

Try these things on stripboard/perfboard before spending any money on pcb's. Also thicken the trace widths as well, and autorouters are not always a good way to go.

Just a few things to check :)

Thanks, Jabber!

A couple of notes —

  • I would do the reset different. 10K pullup.
    If you are not planning to high voltage program
    the uC I would add a protection diode.
    There is no internal protection diode on the
    RESET pin. For noisy environments Atmel
    also recommends a cap. This is usually not
    required and will break the /RTS reset trick.

  • I would add a low-pass filter for AVCC.
    10uH inductor and 0.1uF cap.

  • The decoupling caps were mentioned. I would
    also place the various peripheral parts that
    each chip require close to the chip. Matching
    the schematic if possible.

  • For fuses I usually use a 500mA PTC
    It is an 1812 package and very easy
    to solder. Personal preference.

  • Are you sure you need the pulldown resistors
    for the PCF8574T? It looks like there is an
    internal pullup current source that can be
    connected to the output (100uA). If
    this is not true (or you are unsure) I would
    leave the resistors in.

  • For the FT232RL I would use 10K resistors in series.

  • I also like to add transient suppression on
    the USB interface.

(* jcl *)


www: http://www.wiblocks.com
twitter: http://twitter.com/wiblocks
blog: http://luciani.org

Wow, jcl, I have some googling and revisions to make and do. Thanks so much, really appreciated.