Check out my schematic!

http://ectoprops.com/gbfans/moviepke-schematic.png
http://ectoprops.com/gbfans/moviepke-board.png

This is the project I’ve been working on the past few months. I’m not quite done with it yet, but there’s only a few more connections to lay out on the schematic before I can start optimizing part placement and then autoroute it. I hope to put my order in tomorrow.

If you spot any glaringly obvious errors, please let me know. That’s why I’m posting it!

I think it’s all fine though. Unlike the last set of PCBs I ordered for another project, this one is based on an actual prototype. :slight_smile:

Oh, and ignore the text at the top of the schematic. I didn’t remember till after I wrote it that header pins aren’t numbered the same in the same order as IC’s.

You see, I’m really boring and am not doing a linked schematic for my board…
It’s only single sided (with jumper wires so no autorouter) and it’s nice to visualise it in my head (even if I haven’t finished that yet! :wink:

Mowcius

A few notes on clarity.

I find some parts of the schematic very difficult to decipher with all the text overlaying components, and what are the circles at every junction, is that an Eagle thing?

Also I don't need to know that a component is CAP_VREG_INPUT or CAP_DAC_AVREF_BYPASS. Almost all that is obvious and irrelevant and as I say these lables overlay other stuff and each other making things difficult to read.

The battery input jack goes to a port which normally means that the signal is used in a few places around the sheet, however it seems to only go to the regulator which is right next to the jack. Connecting the two together would stop me from looking all over the sheet for something else that uses 9v.

There's all sorts of orphaned components, I think they have net names (actually on a second look I'm not sure they do) so the software will put it all together just fine, but they are very small and it's almost impossible to find the net somewhere else. Surely most of the could be connected with a wire so it's obvious where they go.

Most resistors don't have a value, as mentioned there's a nice long lable telling me that it's RES_LED_POWER but no value.

None of this effects the creation of your board of course as the CAD software will be happy, but it will make debugging way harder and also I suspect that's why there hasn't been much response. I gave up a couple of times but then decided to persevere.

Just my preferences though, I don't mean beat on you and others here may disagree. Anyway on to the circuit...

From what I can tell things look OK. I don't think you need a resistor on the SR's G pin, just tie it to GND. Likewise with SRCLR.

What data is the DIP switch providing? If it's a 4-bit number it would be nice to have all bits in a row on a port. If not then it doesn't matter.


Rob

The schematic looks like it has the markings of the library editor and not the schematic capture. Why?

Also I don't need to know that a component is CAP_VREG_INPUT or CAP_DAC_AVREF_BYPASS.

Yeah, I started renaming some of those because I realized it was silly. This is only the second schematic I've done, so I don't know good naming conventions yet. :-)

The battery input jack goes to a port which normally means that the signal is used in a few places around the sheet, however it seems to only go to the regulator which is right next to the jack. Connecting the two together would stop me from looking all over the sheet for something else that uses 9v.

Good point. Doing that would also save me from worrying about whether or not Eagle thinks that is connected to the +5v net.

There's all sorts of orphaned components, I think they have net names (actually on a second look I'm not sure they do) so the software will put it all together just fine, but they are very small and it's almost impossible to find the net somewhere else. Surely most of the could be connected with a wire so it's obvious where they go.

Yep, that was the unfinished aspect of the schematic. I just dropped those in there and hadn't gotten to connecting them up yet. I'll post a new version of the schematic shortly. Unfortunately I've run out of time and will need to submit it for manufacture tomorrow, so I don't know if you'll get a chance to look at it before it goes off to get made.

Most resistors don't have a value, as mentioned there's a nice long lable telling me that it's RES_LED_POWER but no value.

Heh, I'm in a rush, and I didn't remember the values and didn't have time to look up the resistor color codes. But I'll get those entered.

From what I can tell things look OK. I don't think you need a resistor on the SR's G pin, just tie it to GND. Likewise with SRCLR.

I do need those resistors. The sound my DAC was producing was super noisy and I was pulling my hair out over until I realized I hadn't put resistors on those. And as soon as I added them, the sound came out crystal clear. Realtive to what I was getting before anyway. There's still a bit of noise which I hope is due to the fact that the prototype is on a breadboard. Even if it doesn't go away though, the sound effects I'll be making will be noisy, so it's not a major problem.

What data is the DIP switch providing? If it's a 4-bit number it would be nice to have all bits in a row on a port.

Yeah, I saw a tutorial on ports, but I couldn't jusitfy taking the time to figure them out when I have so little time remaining. Also they'd make the schematic harder for a noob like me to read. :-)

Thanks for the input!

The schematic looks like it has the markings of the library editor and not the schematic capture. Why?

I don’t know what you mean.

and what are the circles at every junction, is that an Eagle thing?

Forgot to answer this one.

When you say junction do you mean like a T junction in a wire? That just tells you that the wires are actually connected at that point rather than simply crossing. I’ve seen people use that method in schematics, so it’s not really an Eagle thing.

If you mean the little green circles which are just outlines and next to the components, those are just there to tell me where to drop the wire when I’m making connections. If you drop it in the wrong spot, the wire will still be laid but no connection will be made and there’ may be no indication that there is a break. So yeah, that’s an Eagle thing.

Okay, here's the "finished" schematic and board layout. Unfortunately I just remembered I forgot to put the capacitor and resistor numbers in the schematic, but I'll fix that tomorrow I guess.

http://ectoprops.com/gbfans/moviepke-schematic2.png http://ectoprops.com/gbfans/moviepke-board2.png

If you mean the little green circles which are just outlines and next to the components, those are just there to tell me where to drop the wire when I’m making connections. If you drop it in the wrong spot, the wire will still be laid but no connection will be made and there’ may be no indication that there is a break. So yeah, that’s an Eagle thing.

Most (all?) schematic capture progs have a method of showing when the wire is dropped onto the pin, but once a connection is made the visual indicator gets turned off. Also when you print none of them get shown because the really just get in the way of clarity at that point.

I don’t use Eagle but haven’t seen that on other schematics so presumably it can be turned off.

Things are looking a bit better, the board looks nice, pretty wierd shapes. Good luck with it.


Rob

Well, I checked out your PCB! In general, nothing glaring obvious and it would probably work just fine as drawn. However, I do have some feedback. Don't want you to develop bad habits.

I'm not a big fan of auto-route. It might very well be cause of the some of the following. I would never lay out a board and just hit auto-route. It should be use sparingly and only on specific parts of the board at a time. There I said it. :P Anyway...

You put a via and a trace running underneath your regulator (MIC29150). Even with an insulator there, that's just asking for trouble. It looks very easy to reroute that signal around the TO-220 package entirely. Since the tab is ground why not just put a big ground pour underneath it anyway then no need to worry about an insulator. Put in some extra thermal vias to boot.

I also see several instances of vias close to solder pads. For example the two vias by R5 & R6 or by the ATMEL pin 28. Too easy to solder bridge them during assembly.

In some cases the vias even intrude into your keepout around other traces. In most cases there is no good reason to do this.

Your decoupling capacitor on your shift register (IC2) should be closer to Vcc (pin 2).

I also see a couple of places where you have traces running close to mechanical parts (left and right wings). Reroute them as far from the bolt pattern as possible.

Well, here’s the final board I sent off for manufacture:


Tim:
Yeah, you’re right about that capacitor near the shift register. I overlooked that somehow. Guess I won’t get much noise reduction out of it.

Normally I would take my time with the layout and make it all pretty, but I have to get the boards back by Tuesday morning, solder them together, and ship them out that evening or Wednesday at the absolute latest.

And don’t mention vias! Ugh. :slight_smile: With an hour to go before my deadline, the manufacturer tells me that their site wouldn’t quote me their standard pricing because my vias had holes which are too small… 8mils. Their website said they could handle 8mils for holes and I didn’t see mention that their standard pricing could only do holes down to 10. I ended up having to manually edit each and every via because I didn’t want to try ripping up the board and rerouting becuase the wings gave me so many problems routing and I wouldn’t have had time to double check the traces on the board.

The via under the TO-220 shoudl be okay. I don’t think I’m going to bolt it down anyway. The mounting kits I’ve found are too expensive.

As for the others… I wasn’t sure if these vias are tented or not. I guess I’ll have to be careful when I solder near those. I would have thought Eagle would avoid doing bad things like that.

And the traces close to mehcanical parts couldn’t really be helped. There just isn’t a whole lot of space on those wings, and again I didn’t have the luxury of time to make it all absolutely perfect.

Anyway what’s done is done. I’ll find out shortly (boy is that a bad choice of word) if there are any issues. :slight_smile: Thanks for the analysis!