Anyone want to look at my board

Question

I just made my first board and im close to getting it printed i hope..can anyone look at my project and make sure i dont have any messed up traces causing shorts or rendered un printable. Let me know i will send you a link to it. Thankyou 
 Attachments:

rachaelp · Accepted Answer

Hello,

Okay, the next couple of paragraphs will list quite a lot that is wrong, please don't feel disheartened. I'm sure with some help from the community you will get there with this project. It's your first board after all so mistakes are to be expected! Here goes....

I just looked at the first JPG and I can see vias sat in the middle of a bunch of IC pads so you do have shorts which will need fixing before you send it to manufacture.

But looking at the second JPG for the schematic you have other errors there too. It looks like some wires may not be properly connected where you are intending and also the ATMEGA appears to be not connected to power and ground supplies properly. You have the two GND pins connected together but to nowhere else and the VCC pins are not connected at all. Similar issues with the FT232 and your RX pin appears to be connecting via a 1K resistor to the output of the voltage regulator. You've also missed the connection to the ADJ pin of the regulator which is used to set the output voltage and there are no bulk decoupling capacitors on the regulator.

I have stopped looking for errors as they are numerous, probably lots more than I have listed above so far.

Can I recommend you take a step back and tidy up the schematic first and then we can take a look at helping you sort the remaining schematic issues before moving onto the layout. In general running wires overlapping components and squeezing things in between where you haven't left enough space makes it hard to read and easier to make mistakes. If you clean it up and fix the errors I have listed above then repost the schematic and then we can see more clearly what else might need to be done. Look at the data sheets and reference designs for the devices you are using and see how they are done and what additional components they use, that might give you some hints on what else might be wrong in the schematic.

Best Regards,

Rachael

rachaelp · Answer

kizzz ane wrote:

Thankyou i suspected their to be alot of errors. I havnt connected the voltage regulator adjust yet because im not sure what value resostor to use yet. Also i have not cpnnected the remainder of the usb header. Im not sure what bulk decoupling capacitors are. I will correct as much as i see and reposed a new picture of the schematic when im at that point. Thanks again

Bulk capacitors are large value caps placed on the inputs / outputs of power supplies for stability and to give a smooth output and sometimes additionally in other places around the board to provide a reservoir of charge to supply current when part of a circuit needs extra before the power supply and power distribution network around the board can deliver it. Having local "lumps" of storage helps to reduce fluctuations in the voltage under transient load conditions (i.e. when the current requirement steps up suddenly).

Best Regards,

Rachael

rachaelp · Answer

Its better but there is a way to go still You are still missing one of the VCC connections on the ATMEGA. Try and space things out a little more so wires don't have to overlap components, for example the wires running through R7 and R8. Also think about signal flow and try and place the components in your schematic to be conducive to how they are going to be connected. You don't need to have a single point and run a wire around your entire schematic for GND. Better to use GND symbols (they will force the nets to be called GND and will make them connected) at strategic points in your schematic to get all your GND points connected up. Similar with the power supplies. I'm assuming your voltage regulator is going to be set to 5V, you can use supply symbols to connect your 5V everywhere it needs to go. You've not connected VCCIO on your FT232 either, that'll probably want to connect to 5V. Best Regards, Rachael

rachaelp · Answer

kizzz ane wrote: I have not quite figured out how to use the vcc and gnd symbols yet. Do i just search for the symbols in the library and place gnd and vcc where i need it? Thankyou!!! Yes there will be a library with a bunch of standard power and ground symbols. I can't remember which library in the standard EAGLE libs as I don't use them (as I have my own set of libraries I built from scratch) but just off the top of my head I think it might be called supply.lbr or something like that and it'll have a bunch of them in there. Just add them from there and place them where you need them. Once you have them in the schematic if you need extra you can just use the copy command to create extras. Best Regards, Rachael

rachaelp · Answer

Hello, kizzz ane wrote: Hi, ive tried to tidy up the board and im going to share the results, im not sure exactly at this moment what vcc pins on each chip need input, but besides that does this look better what do you think. It's definitely improving a lot, I can read it more easily now I'd have used the +5V symbol rather than VCC as I like to be explicit about what the voltages are on my designs, and I would use a +9V one for the 9V connection you have. If the library is missing the voltage you need you can use this ulp: http://eagle.autodesk.com/eagle/ulp?utf8=%E2%9C%93&q%5Btitle_or_author_or_description_cont%5D=make-supply&button= to create a new one for you. I'd actually recommend you start building up your own library of parts and put any supply symbols you create in your own supply.lbr file separate from the bundled ones. You can create a folder for all your lbr's and add that folder to the list of directories so EAGLE sees them. Anyway, back to your circuit.... You need to look at what is going on with the reset inputs to both the ATMEGA and FT232. I can't remember if they have internal pull-ups or whether you will need to pull them up or if you need to generate a reset pulse to them. I suspect a pull up will be fine but you might want to consider whether you need to be able to easily reset the ATMEGA during software development. How are you planning to program the ATMEGA? I don't see an ICSP or JTAG header on the board for programming. You'll also probably want to add bypass capacitors close to the VCC pins of the ATMEGA and FT232. These are smaller value ceramic capacitors (usually X5R or X7R dielectric) of typically 10nF to 100nF with a rating of say 50V (not because the need to be rated for 50V but because ceramic capacitors have a capacitance degradation with DC bias voltage and the higher the rated voltage above the bias voltage the less the capacitance is reduced). A little more critique on the schematic style, I would try and keep supply voltages nearer the top with the symbols pointing upwards and GND symbols nearer the bottom and pointing downwards. I'd also not have wires at odd angles, normally horizontal and vertical only with 45 degree nets very occasionally when the circuit topology was more clearly expressed by doing so. kizzz ane wrote: So with the vcc and gnd pins the ground and vcc planes will be routed with autorouter? Thanks again You can route them with an auto router. I wouldn't personally use the auto router. You'll learn a lot more and have a much better result routing the board manually. It's a very simple board which won't take long to do manually anyway so there isn't much of a time saving with the auto router. Best Regards, Rachael

rachaelp · Answer

kizzz ane wrote: Thankyou for all of this, only problem i have is this board has to be 1x2.4 inches. I'm not sure what the problem is, 1" x 2.4" is plenty for the amount of components you have on the board. What problem is this size restriction causing you? kizzz ane wrote: i have trouble running the traces with the VIA tools. I dont think i fully understand it. I type name in the command field at the top, then i click the via and name them accordingly. You use the ROUTE command and then when you change layer it will insert the correctly named via for you. You shouldn't be needing to place and name via for normal routing normally. You'd do that for things like connecting polygons to a ground plane or something like that. I think when it comes to doing the layout you need to get a few pointers before you start and it'll hopefully make things go a lot more smoothly. kizzz ane wrote: I plan to upload my code to the atmega via the ft232rl adapter through rx /tx. Right ok so your ATMEGA will come pre-loaded with something like an Arduino boot loader? If not you'll need a JTAG/ICSP header to be able to load up a boot loader initially to then be able to use the FTDI serial connection for programming. Best Regards, Rachael

rachaelp · Answer

kizzz ane wrote: Im going to read more of the documentation on the software. Id really like to know all of these things. Take a look at online tutorials. Jeremy Blum did some EAGLE videos on his YouTube channel and then there are some good basic EAGLE tutorials on Adafruit and Sparkfun too. Look at these types of resources and get the basics from these before delving into the manual as it'll make more sense if you have a grasp of the fundamentals before reading it. If you have any questions on just using EAGLE feel free to create new topics on here and ask kizzz ane wrote: This is not for sales so i am going to desolder a already programmed chip from an arduino and use that. Ok thats fine then, so long as you are happy you can get the chip off the Arduino ok without damaging it. kizzz ane wrote: I also want to figure out how to make parts for the library, This is an essential skill for using EAGLE (or any other schematic/layout toolset) effectively. My recommendation would be, once you get more familiar with doing electronic design, build up your own libraries of parts, including all the basics parts, and avoid the "free" bundled libraries as you cannot guarantee their accuracy so need to spend lots of time checking them anyway. kizzz ane wrote: i would like to just be able to select a blank foot print for ever part i need make the baord that way. Whilst you can do this, its really not the right approach and I wouldn't recommend taking this route for designing boards. For very small boards where you can keep track of what's what then it'll work, but generally its much easier to understand a design and build a bigger design by creating a schematic, especially if you then want to come back to it months or years later. If all you have is footprints connected on a layout the chances of you being able to remember what everything was and be able to start working with it again quickly is very slim. Best Regards, Rachael

kizzzane · Answer

Thabkyou for all of this, only problem i have is this board has to be 1x2.4 inches. Its designed to operate that solenoid about 20x a second on a paintball gun. I will add some bypass capacitors thats a great idea, i have trouble running the traces with the VIA tools. I dont think i fully understand it. I type name in the command field at the top, then i click the via and name them accordingly. I plan to upload my code to the atmega via the ft232rl adapter through rx /tx.

kizzzane · Answer

Im going to read more of the documentation on the software. Id really like to know all of these things. This is not for sales so i am going to desolder a already programmed chip from an arduino and use that. I also want to figure out how to make parts for the library, i would like to just be able to select a blank foot print for ever part i need make the baord that way.

Anyone want to look at my board

Top Replies