An update on Rev2 status: The schematic is looking pretty good, albeit there are probably still some errors that will seep up to the surface. I’ve started on the board layout, which will also help uncover any schematic errors. Today I’d like to go through the process I usually use to layout circuit boards in EagleCAD.
In case anyone was wondering if I was kidding about the cat and laser pointer thing, here’s a great chance to find out. Download the schematic by itself, open it in EagleCAD, and click the “Board” button (5th from the left on the toolbar), and try laying out the board. Make sure and give yourself some time (a day or two without sleep should do it), and dig in!
So here are the steps I use when laying out a board. After the schematic has been reviewed several times (preferably by someone capable and also familiar with the project, not just by yourself), click the “Board” button (location described above). What Eagle does here is it takes all of your components and puts them next to a random outline.
From here, let’s just go down the list. Note that this is just what I do for boards like this. It gets the job done very quick, with decent quality, but others do things different and may agree or disagree with this approach – I’d love to hear what others do in the comments!
- Draw a circuit board outline
- Group components into proper areas
- Manually route critical traces
- Autoroute remaining traces
- Manually fix autorouter mistakes (sometimes, the autorouter makes no sense!)
- Run Design Rule Checks against the board
- Redo steps 3 through 6 if necessary
- Send design to the boardhouse
1) Draw a circuit board outline.
If you don’t care what size your circuit board is, this is a very easy step. Take the default, and shrink or expand it as you get closer to finishing step two. Chances are, however, you should make careful considerations about your intended enclosure(s) for the circuit board. Don’t skip this step lightly, or you’ll pay for it exponentially down the road. Case in point: ZephyrEye Rev1, from the side as shown below. Originally I thought I would use a different case, but it was too bulky and looked horrible. But it didn’t exactly fit in my backup case, either: I had to cut out the side just to get it to fit.
I’ve downloaded the manufacturer’s datasheet for the enclosure, and following it’s recommendation outlined the board to maximize the PCB surface area – I’m going to need it all to get it all the features packed into this tiny little enclosure. Either modify the existing outline, or draw using wires on the “Dimension” layer 20. The board house will router your PCB following this outline.
Another item I always forget (and actually just remembered while writing this), is mounting holes. Some people use vias connected to ground, while others use drill holes. I usually prefer vias, because you can set the diameter of the copper around the via and avoid routing other traces within range of the head of the screw. It also lets you ground your circuit board to the enclosure, which is common with metal enclosures.
2) Group components into proper areas.
For most components this is pretty straightforward. Put all the schematic elements in the same area: an IC, supporting passives, and related supporting circuitry. But you’ll also need to take into account any special needs of that part of the circuit:
- Sensitivity to noise
- The digital compass would potentially have issues if placed near the transmitter, or near any high current wires due to the magnetic field around a current-carrying wire.
- Proximity to the edge
- The GPS circuit needs to be near the edge because it has an antenna. You can’t trace antenna wires very far without serious signal degradation, so it gets a special spot.
- Most components that need to be near the edge are there because they need to match up with enclosure features – measure these things out carefully when necessary.
- Proximity to other chips it needs to communicate with
- If you can, put inter-communicating chips near each other. There’s considerable flexibility on this point, depending on the protocol, the speeds they communicate at, and sensitive areas that these signals must avoid.
- Example: If you were routing wires carrying USB 2.0 at 480MHz, it would be bad news for both other chips on the board as well as your USB signal integrity if these were long. In fact, at this high of speed, there are very specific routing guidelines that must be followed.
- Speeds of signals that will travel on the signal wire
- Crystal wires should always be very short. Once you get a signal that will be up in the megahertz range, the shorter it can be the less noise you’ll get at other locations on the board. The trace carrying the signal can act as an antenna if it is too long.
- Analog signals need special consideration.
- Usually, you’ll want to avoid routing communication wires (RS232, SPI, or I2C) near analog wires. These communication wires will put noise into your analog signals, causing headaches and very weird errors when debugging the board.
- Antenna signals are analog of the most sensitive kind, and usually need to be a specific width if they travel very far. You may also need to “impedance match” the trace to avoid distorting the signal.
That’s not an exhaustive list, and not detailed by any stretch of the imagination. Google for more details on any above item you fear a board you’re laying out may have issues with. Datasheets will have very specific layout requirements as well, many have a PCB layout guide for the chip. Lastly, check for reference designs. These are great to follow because you know they have been proven.
You’ll notice the schematic is already outlined in this way. For example, the digital compass (HMC5843) should be placed somewhere within the outline that will be away from high-current lines (e.g., lines which may induce magnetism and noise). I picked a corner away from everything else for this guy. It was pretty easy to look at the schematic and see that I needed to pull in C31, C34, C40, R11, and R19. Quickly looking at the air wires, I put them in an order that seemed like would work once the traces were routed. Then I did more or less the same for the remaining component “groups”.
Notice the surface mount components are on top as much as possible – this makes it easier to assemble, particularly for pick & place machines and/or if you are going to bake it in a reflow oven.
3) Connect Vcc, GND, and critical traces
Vcc and ground traces go first. Usually, I go for a ground plane on top. Some people do Vcc planes on the bottom – I’m not a big fan of this, but I have done it. Make sure the traces are wide enough to carry the current they need to (this calculator may come in handy) – in general, they are but it’s better to make wires that carry a lot of current be thicker anyway, no sense having a bunch of fuses around the board. I estimated my max current delivered to this board to be less than 250 mA, but I still use .024″ traces for VBAT, and 0.16 for a few of the VCC traces.
For a few of the components, you’ll also want to trace things out before you let the autorouter have its way. You can also quarantine areas as off-limits to the autorouter for sensitive areas. For example, the GPS circuit is pretty sensitive, especially with regards to the RF ground plane and the antenna trace. I routed this area up ahead of time. To make sure areas like this aren’t touched, you can then place polygons on the top and bottom restrict, keepout, and vRestrict (for vias) layers to manage the autorouter.
4) Autoroute remaining traces
This step has a few tricky items that can make the difference between a successful autoroute and a complete failure autoroute. Pay close attention to the setup! Here are the steps I used:
- Save before you start! You will NOT be allowed to use “Undo” commands after you start the autorouter. I usually save a separate copy before I start just to be safe.
- Make sure your design rules are set up correctly as the autorouter follows these rules while routing traces. Use the toolbar or click “Edit -> Design Rules…” to open the DRC dialog. Set up the rules to follow your intended board house’s manufacturing guidelines and minimum tolerances (check their website). Here are the ones I modified from the default:
- Clearance Tab:
- I set all clearances to 8 mils.
- Distances Tab:
- Copper/Dimension: This is the minimum distance between any copper (whether a trace, polygon, or component) and the board outline on the dimension layer 20. I set it to 10 mils. If you route traces too close to the edge of the board, they may get cut or damaged.
- Drill/Hole: Distance from anything to a hole on the board. Set to 8 mils.
- Minimum Width: This is the minimum width of a trace, and the autorouter will use this for everything. 10 mils is a good minimum if you have plenty of space – I used 8 mils.
- Minimum Drill: This is the smallest drill size available from your board house. 20 mils for me.
- The rest of the defaults generally work fine for me, but make sure you’ve met all your board house requirements before continuing.
- Click “Apply” and then either “Check” or “Cancel”. It’s a good idea to check your work so far to make sure you pass off a clean board to the autorouter.
- Clearance Tab:
- Now click on the “Tools -> Auto…” (or use the toolbar) to open the Autorouter Setup dialog box. Make the following changes according to your design needs:
- Routing Grid: Here’s the deal. The larger the grid size, the less time it takes. But the autorouter will only consider trace joints and intersections every 50 mils. So for surface mount components pins at, say, .5mm pitch (pin centers are .5mm apart), the autorouter will fail to connect most pins. It will also have issues in congested routing areas. On the other hand, using a 1 mil grid will take forever. I used 2 mil routing grid – It took about 30 minutes.
- Change Top and Bottom preferred routing directions if desired. I haven’t found this to make a big difference in actual implementation, just make sure you don’t pick two parallel directions unless you want issues.
- To be honest, I’ve never bothered playing around with rest of the settings, or the optimization settings. I’m sure there are some advantages that can be made here, but I’ve never dove in. Feel free to comment if you know how to change these to some advantage!
Once everything is set up, save again and then hit the “OK” button. Alternately, if you only want the autorouter to work on a particular subset of traces, use the select button and then hit the green stoplight button on the toolbar to go. Be forewarned that the autorouter will ripup and retrace ONLY its own traces, and traces there prior to beginning the autoroute will remain untouched. This can be a problem, especially if you have cut off certain sections of the board with traces on both the top and bottom, or have routed so close to surface mount pins the autorouter cannot place a via to get around it.
In situations like this, and sometimes just due to trace density, sometimes the autorouter just can’t find a path for all the traces. These will be left as airwires for you to manually route…
5) Manually fix autorouter mistakes
Sometimes, the autorouter just doesn’t make any sense. I couldn’t help but post this picture – it’s a classic.
But seriously, sometimes the autorouter just does ridiculous things. Traces have random and startling paths, take weird angles, overshoot and then overcorrect, etc. Check through the history of the Rev2 cad files for examples. You’ll want to shorten most of these traces if you can, take out the weird angles, and fix any traces that went through places they shouldn’t have.
And the autorouter generally uses a LOT of vias. Vias can actually cost you extra if you use too many from some board houses, because they take extra time to drill and plate in the manufacturing process. So minimizing vias is important. You can usually clean a few off manually with a little effort.
It took about 30 minutes to finish the autoroute, because my routing grid was so small. Before the first optimization step, it had around 320 vias. Youch! By the end, however, it was down to around 170. Go optimizer!
It also left about 7 traces for me to finish by hand. Most of them were because the ground plane polygon had “fallen apart”, meaning there were so many traces that parts of the ground plane had become separated and were not longer interconnected. Many were fixed by pushing and pulling vias and traces around. On a few, though, I had to place vias and bottom side traces that jump under traces that cut up the ground plane to make the connection.
6) Run Design Rule Checks against the board
This step is CRITICAL! Don’t even consider sending the board off without checking your board against the design rules. Since you’ve already got the DRC rules setup, just hit the “Design Rule Check” button on the toolbar to run it. It’s pretty straightforward: Anywhere you have traces that are too close or overlap, parts off the boundary, or drill holes that go through traces or components, you’ll get an error that you’ll have to fix by hand.
This isn’t too bad usually, but in densely routed areas can sometimes be a little tricky. Just use your elbows, push things out, and make some room.
7) Redo steps 3 through 6 if necessary
Well, as hard as all this has been, you may find something that needs changing. Say you forgot a critical component, or left off a significant number of traces. Sometimes you can add these things in after the fact, sometimes this is as practical as putting Jabba the Hutt on Jenny Craig.
If you have to, don’t resist starting over. The command to get this to happen quickly can be typed into the command bar: “ripup ! ;”. This will ripup everything, so if there were certain traces you wanted to keep the alternative is selecting the traces to leave alone one signal at a time by leaving off the semicolon, then hitting the green stoplight to execute the command.
If you’re happy with the board, then congratulations! The next step is to get someone to review your board layout. A fresh set of eyes makes all the difference. But don’t be disappointed if, even after several reviews, it comes back with a few hardware bugs. Have Xacto knife and patch wire ready ;)
8) Send board to boardhouse.
There are a lot of boardhouses, each with different pros and cons. Here’s a list of other houses I’ve heard good things about:
- Personally, I use PCBExpress because of proximity – They do small, low-feature two layer boards for pretty cheap, and they ship ground for free. Since they are also located in Oregon, I get them in two days. They also accept Eagle files directly – no need to generate Gerbers.
- I’ve heard good things about Advanced Circuits.
- BatchPCB is related to SparkFun. This one is pretty cheap @ $2.50/sq in (plus setup fee), but takes a while to get your boards back. Time flexibility = lower cost boards.
All of the above have Internet order options. Just upload your file, answer a few questions (usually about layers), pay for it, and you’re done. Usually, this is when I put together my final bill of materials and get the parts ordered so they arrive about the same time as the board.
Well, that just about covers it. I’m sure I forgot something, so as usual feel free to remind me or ask questions in the comments.
There are a few inevitable truths in this world. Taxes will rise, Wookies shed all over the furniture, Luke and Leia are related, and there is no such thing as a perfect first draft schematic.
The Rev2 circuit is nearly complete. It looks AMAZING if I do say so myself. That’s the problem, though: I’m inundated with excitement and therefore am unable to find things that are wrong because I don’t want to find any reason that might delay getting the circuit boards back as soon as possible.
I’m calling out for a few extra set of eyes to look over the schematic If anyone could please go to the Google code, download the Eagle CAD files and take a look, I’d really appreciate it. If you want to make changes, let me know so I can arrange for them to be merged back in properly. Even if you’ve never looked at schematics before, take a look and as always, feel free to ask what’s going on in the comments.
This is also a great chance to give suggestions on functionality. I should add, it may be your LAST chance! Please give some comments if you think you might ever build one, if nothing else just to say you think it works for what you’d like to use it for.
If you’re not familiar with CAD schematics and circuit board layouts, it might be interesting to look at the history of the .sch and .brd files in the Google Code repository. By looking at older revisions, you can see the steps taken along the way chronologically. I commit changes at least at the end of almost every day I work on the project.
The current Bill of Materials can also be found at this Google Docs spreadsheet. It includes estimated pricing – it currently comes in at just under $200. A little bit higher than I was hoping, but about the same cost as Rev1 and Chuck Norris (adverbicized) packed with new extra features!
The schematic is hopefully organized well enough for someone not intimately familiar with this project to try and understand one section of the schematic at a time. The capacitive touch schematic is separate, because it will be a separate board. The way it works is you put copper pads on the board, glue it to the inside of your enclosure, and it senses you touching it on the outside of the enclosure. Pretty nifty, and a great way to avoid milling the enclosure.
Please post comments below, or add to the Google Groups discussion page.
So, the stats tools on WordPress are kind of impressive … and useful at correcting idoits like me. I’ve talked all around it, but I noticed I haven’t released an actual bill of materials and noticed quite a few people have been searching for it. Maybe they want to build a ZephyrEye? I’ll try to do my best to appease the masses. It’s been quite a while since I actually built the hardware, but here it goes…
Lucky for me, and anyone else using EagleCAD, there’s a handy User Language Program (ULP) called bom.ulp that autogenerates a BOM. It only lists items that are actually on the schematic, however, so don’t forget things: the LCD connector denotes you should also buy an LCD display. I’ve never made that mistake though.
Partlist exported from /home/brad/Development/zephyreye/trunk/cad/ZephyrEye Rev0.2.sch at 2/11/10 1:32 PM
|8||TAC_SWITCHPTH||SW_DOWN, SW_IN, SW_LEFT, SW_OK, SW_ONOFF, SW_OUT, SW_RIGHT, SW_UP|
|7||.1uF||C-USC0603K||C3, C7, C17, C18, C21, C22, C23|
|3||1uF||CAP_POL1206||C8, C9, C12|
|2||2.2uF (TANT)||C-USC0603K||C14, C15|
|4||10uF||CAP_POL1206||C1, C2, C6, C10|
|3||470||R-US_R0603||R6, R8, R16|
Most of the “primary” components are from Sparkfun, with most of the passives, voltage regulators, etc. coming from Digikey. So, on top of this list, you’ll also need:
- Case: Pac-Tec PP Enclosure
- 1/16″ Acrylic, available from local hobby shop
- LCD connector
- EM408 GPS module connector
- 2mm headers for the XBee
- An extra 500mA rated LDO regulator for the GPS.
If anybody is seriously interested in making one of these guys, let me know. If at least 10 people are interested, I would be willing to make kits at cost (should be ~10-20% cheaper), and help those wary of the SMT soldering (for a nominal reimbursement). Keep in mind the programming either comes from you, me, or the community and that the software has basic functionality but is not yet complete. Also, you’ll want at least two (unless you want to use it for something other than paintball/laser tag gaming).
Note: I’ve started adding a few product links in. As I have time, I’ll fill in the rest. Feel free to help out in the comments if you find links to products (from SparkFun or DigiKey generally) before I do.
So, how do I get all these different components to play nicely together? Lots of time in the datasheets, browsing forums for tips, and a perpetual lack of anything better to do. That’s because of the inherent coolness of the project, obviously, and not from lack what “y’all call da social skills“…
I’ll be going through each of the components in the chip and talk about how I interfaced them to the ATMega128 AVR microcontroller. I’ll try to give enough detail so that someone could rewrite this in a different language if they felt like it. Once the component interfaces have been described, I’ll go through and describe the remaining functions (menuing, GPS, games, etc.).
This handy little LCD display is pretty easy to use. SparkFun sells them standalone as well as with a sweet little breakout board, which handles the hard to solder connector and funky backlight voltage nicely, allowing just about anybody with a spare micro lying around to use this display in their projects. Here are some simplified pin descriptions (but remember the datasheet is the final reference) for those setting up their own display.
- 1) V_digital: Supply voltage for internal logic circuitry. Should be separate from V_display.
- 2) LCD_reset: Resets the LCD. Necessary for communications.
- 3) DIO: Data input pin, connect to the MOSI line of your MCU’s SPI hardware.
- 4) SCK: Serial clock input pin, connect SCK line of your MCU’s SPI hardware.
- 5) CS: Connected to the chip select line of your MCU’s SPI hardware
- 6) V_DSP: Display voltage. This supply voltage is the one that actually drivers the liquid crystals, and therefore needs to be very solid. The datasheet recommends it has its own voltage regulator, which is not always necessary (it can be tied to Vcc) but I have conceded as it reduces flickering.
- 8 & 9) GND & LEDGND: Connect to ground.
- 10) V_LED: White LED Backlight voltage. +6.8V required to drive these little suckers. I’ve used the TPS61040 boost regulator to do this, it works nicely.
Note that pin 7 is NC. It’s also worth pointing out, since this is a battery driven project, that it’s useful to have enable lines connected to GPIO pins on your MCU. In particular, I’ve been pleased that the +6.8V regulator can simply be turned off when the display is dormant – this saves between 40 and 60 milliamps, which can extend battery life a LOT.
BASCOM-AVR has some very nice routines to use knock-off cell phone displays with the Phillips and Epson chipsets. However, it didn’t quite work with this particular display from SparkFun so well. Luckily, I’d already been using this display for a while before Bascom added a library for it, and by using my init routine after calling theirs, it seemed to work out OK. Here’s the relevant pieces of code (remember, the code can be found on the Google Code repository).
If this LCD worked directly with BASCOM, setting it up would be easy peasy:
'******************************************************************************* 'Configure Display $lib "LCD-epson.LBX" 'Library for LCD screen Config Graphlcd = Color , Controlport = Porte , Cs = 5 , Rs = 6 , Scl = 3 , Sda = 4 '*******************************************************************************
I had to add on my custom init routine to get things to work right, as well as a few helper functions:
'************************************************************ 'Sends initialization data to LCD screen Sub Init_lcd() Lcd_cs = 0 Waitms 10 Snd_cmd Disctl Snd_data &H03 Snd_data 32 Snd_data 12 Snd_data &H00 Waitms 10 Snd_cmd Comscn Snd_data &H01 Snd_cmd Oscon Snd_cmd Slpout Snd_cmd Volctr Snd_data 5 Snd_data &H01 Snd_cmd Pwrctr Snd_data &H0F Waitms 100 Snd_cmd Disinv Snd_cmd Datctl Snd_data &H00 Snd_data 0 Snd_data &H01 Snd_data &H00 Snd_cmd Rgbset8 'Set up the color pallette 'RED Snd_data 0 Snd_data 2 Snd_data 4 Snd_data 6 Snd_data 8 Snd_data 10 Snd_data 12 Snd_data 15 'GREEN Snd_data 0 Snd_data 2 Snd_data 4 Snd_data 6 Snd_data 8 Snd_data 10 Snd_data 12 Snd_data 15 'BLUE Snd_data 0 Snd_data 4 Snd_data 9 Snd_data 15 Snd_cmd No_op Snd_cmd Paset Snd_data 2 Snd_data 131 Snd_cmd Caset Snd_data 0 Snd_data 131 Snd_cmd Ramwr Clr_scr 255 Snd_cmd Dison Waitms 200 For B = 0 To 140 Snd_cmd Volup Waitms 2 Next I End Sub '*******************************************************************************
Wow, I should have commented that a LOT better … bad Brad! (hitting myself with rolled up newspaper)
Here’s the helper functions. Normally I’d just refer you to the code, but for those of you trying to get this LCD to work, using the 9-bit frame is a little tricky. I will refer you to the code for pin definitions and constants, however. I ended up bit-banging it – YMMV. Be careful with the polarity and phase of the SPI signal, it’s very particular. Lastly, note the syntax of BASCOM-AVR for addressing a bit in a byte is the dot operator (e.g. Dab.7 returns the value of the 7th bit of the byte variable Dab).
'******************************************************************************* Sub Snd_data(byval Lcddata As Byte) Lcd_sck = 0 Lcd_dio = 1 'Data = 1 Lcd_sck = 1 Shiftbits Lcddata End Sub '************************************************************ '******************************************************************************* Sub Snd_cmd(byval Lcdcmd As Byte) Lcd_sck = 0 Lcd_dio = 0 'Commands = 0 Lcd_sck = 1 Shiftbits Lcdcmd End Sub '******************************************************************************* '******************************************************************************* Sub Shiftbits(byval Dab As Byte) Lcd_sck = 0 Lcd_dio = Dab.7 Lcd_sck = 1 Lcd_sck = 0 Lcd_dio = Dab.6 Lcd_sck = 1 Lcd_sck = 0 Lcd_dio = Dab.5 Lcd_sck = 1 Lcd_sck = 0 Lcd_dio = Dab.4 Lcd_sck = 1 Lcd_sck = 0 Lcd_dio = Dab.3 Lcd_sck = 1 Lcd_sck = 0 Lcd_dio = Dab.2 Lcd_sck = 1 Lcd_sck = 0 Lcd_dio = Dab.1 Lcd_sck = 1 Lcd_sck = 0 Lcd_dio = Dab.0 Lcd_sck = 1 End Sub '************************************************************
After that, it’s smooth sailing as all of BASCOM’s internal drawing and text display functions work just fine. Here’s all it takes to draw the setup screen. The “splash” picture was included in the program, and is loaded from flash program space. Pixels are set using the Pset command. Drawing text at certain coordinates and with a defined forecolor and background is done using the Lcdat command.
'Display Picture W1 = 0 For Y = 2 To 80 For X = 0 To 127 B1 = Lookup(w1 , Splash) Pset X , Y , B1 Incr W1 Next X Next Y Setfont Color8x8 Lcdat 88 , 20 , "Start Game" , Black , Gray Lcdat 96 , 20 , "Join Game" , Black , White Lcdat 104 , 20 , "Options" , Black , White Lcdat 112 , 20 , "Settings" , Black , White Lcdat 120 , 20 , Unit_name , Gray , White ... (near bottom of program) 'Extra include files - Fonts $include "color16x16.font" $include "color8x8.font" $include "smallfont.font" $include "zephyreyepic.txt"
So there you have it, how to use the SparkFun LCD display. Hopefully that helps somebody understand how to use it.
As I’ve stated before, I also hope the lengthy explanation helps get all this converted into AVR-GCC. As a side note, I would like to develop the component libraries into a more useful place: the avr-libc-corelib project. This would make libraries for all the components readily available for others to use.
As always, if you have any questions about using this display, feel free to leave comments or email me!
To lead up to further descriptions about the firmware, and in order to be qualify for invitation to bodacious Silicon Valley parties, I thought it would be good to release the CAD files and code. Everything on this project is being released under the BSD license.
The code can be found on Google Code under the project name zephyreye. Feel free to check it out. It will likely undergo massive changes as the code is ported to GCC, but the original BASCOM-AVR code will also remain a branch for both reference and for the BASCOM community if anyone wants to hack it up, reference the code, or continue ZephyrEye development in Basic.
If anyone does proceed working on the Basic code, it needs cleaning up and most likely a thorough overhaul as I didn’t originally plan this as a collaborative project. There is no GCC code yet – I’ll get started on some as my other responsibilities allow.
The CAD files are in EagleCAD format. EagleCAD is nice and handy because, even though it’s not open source, it does run natively on Linux, Windows, and even Mac. The CAD files also need some cleanup, and in order to get a version of the ZephyrEye that actually would be usable and durable in a paintball match, there will need to be a revision change because:
- The current hardware construction would be demolished by a direct paintball hit
- A few of the components need to be replaced for different parts to meet the specs better.
So there you have it. Feel free to join the project on Google Code, I think there’s a lot of potential for this fun little project. Also feel free to branch this project if you see other uses for the hardware: cat tracker, robot remote control, whatever!
Now that the code is posted, it will be a little easier to dive into hacking into the code. Over the next few posts I will start describe the lower level functionality to aid anyone attempting to port it, and also to help anyone looking to use these components to understand them better.
So here’s the start of the design section of the project. I’m releasing this project and related information under the BSD license. I’m not into the viral type of Open Source licenses, but if you make a buck let me know about it cuz I’d l0ve to hear about it. And maybe you can buy me some draft root beer … and if it’s a lot of money, maybe a Tesla …
I thought I’d put one of the many logos I made for it here. Amazing what a guy with a hamster wheel in place of right brain functionality can do with a few GiMP filters… Well, maybe not as amazing as I think, considering I am the one with the hamster wheel brain.
Before I dive in too deeply, lemme run over the development cycle that will ensue now that I’ve got my spec:
- Draw up a schematic
- Lay out a circuit board (e.g., place drawings of the parts on a printed circuit board document and draw metal wires between all of the parts that need to be there).
- Break piggy bank.
- Send the circuit board to a “board house” to get it fabricated.
- Purchase parts needed from online electronic component suppliers like DigiKey, SparkFun, and Mouser.
- Assemble the parts.
- Write the code.
- Field test the result at various steps along the way.
I’m definitely a bottom-up developer, meaning I take the skills and parts I know well and attack the given problem with those first, and only add in new skills/parts as my existing skills/parts set prove unsatisfactory. I’ve tried to break this habit, but it gets really cool results really fast and it’s hard to part with that (at the expense of a most likely higher quality project that might be achieved using a top-down approach).
I’ll hit you with a brief overview on the parts that I picked, and then I’ll show the schematic at the bottom:
- ATMega128 from Atmel
- 128KB Flash program space, 4KB RAM
- 54 I/O pins
- 8 ADC channels, for power monitoring and microphone reading
- Clocked at 8MHz and powered at 3.3V (because all cool components run at 3.3V ;)
- It’s one of the easiest microcontrollers to use these days, and ridiculously capable.
- Programmed in BASCOM-AVR. More on that later …
- EM-406 GPS module from SparkFun.
- 20 channel (e.g., can track up to 20 satellites simultaneously)
- 5m accuracy
- Small and works pretty standalone
- Connects through a UART to the Mega128
- Color LCD Nokia Knock-Off from SparkFun.
- 128×128 Pixels
- 4096 possible colors, but only 256 at a time in the palette
- Not that great, but it does the job about as good as an old cell phone LCD display would
- Digi XBee Pro, also available from SparkFun among many other vendors
- 1 mile line of sight range, 300yd urban range
- Easy as pie. And like Jack Handy says, “If you get the chance to choose between regular heaven and pie heaven, choose pie heaven. It might be a joke, but if not, mmm boy!” Mmm, XBee!
- Flexible addressing and self-healing mesh networking capabilities
- FM24C64 chip from Ramtron. I’ve only found it from Mouser.
- 64KB of high-speed, non-volatile RAM.
- Cheap (~$3.50)
- Used to store field and game information, along with user settings
- Every project with small non-volatile needs should use one of these. They’re fantastic.
- 1100 mAh Lithium Polymer battery from SparkFun.
- MAX1555 Li-Ion battery charger.
- This is a pretty good and easy to use combination, and I’ve had great luck with the crazy easy to use charging circuit in the MAX1555 datasheet.
Those are at least the main parts that drive all the primary functionality of the system. Drum roll ….
Schematic time! I use EagleCAD from CadSoft (http://www.cadsoftusa.com) for drawing schematics and laying out PCBs. They have a free version for non-commercial use, which is great for open source and hobby stuff. SparkFun releases EagleCAD libraries for almost all the parts they sell, which kicks development speed up to .5 past lightspeed. Eagle is also cross-platform compatible, for all you fellow penguins out there.
Sorry for the under-impressive image on this page. Click through to zoom in for readability. You’ll notice I organize my schematics by net names rather than running crazy lines all over the page. Please don’t ever make schematics like that. Every time you make a rats nest out of nets running all over the page, a devil gets his horns. Just don’t do it.
Instead, label the crap out of EVERYTHING. It’s best to not leave any nets with a default net name (e.g, N$42). You’ll notice that it’s usually fairly easy to follow the document this way, especially when you’re using a printout, PDF, or some lame JPEG on a blog instead of Eagle to view the schematic.
Rant time’s up. Anyways, I know I messed a few things up. I’ll make an errata list if I can remember what they are … Also, it’s OK if you don’t have a clue what’s going on. I’ll explain most of the connections in later posts, especially once I start talking about the software (because that’s where the pin functionalities and inter-IC signals really get defined).
Also, you may have noticed I like SparkFun (woot!). They’ve got some great stuff that hobbyists normally can’t source, like the GPS module, LCD display, and lithium ion batteries. They also have a lot of great tutorials for beginners, for everything from Arduino to basic soldering. Shameless plug: buy stuff from them. Every time you place an order, a devil gets his horns removed. (No, I don’t work for them … that’s a pipe dream …)
Next time, on Brad’s Projects: Board Layout! Yay!