Here are the updated schematic/drawing from the previous comments. Not sure what else to do at this point:
Kurt
Propeller with Analog.zip (109 KB)
I will see if Mike has time to look at it. You ready to make a board? 
It might be fun to see how much of it works and what we need to update…
Kurt
Got your message Jim. I will take a look, probably not tonight, but I will have some time tomorrow night.
Mike
Kurt,
OK, I finally got a chunk of time to look this over. It’s looking really good. Just a few comments.
There is not much to say about the schematic. My only concern is the FT232R connection. The schematic doesn’t show a ferrite bead on the power input, as recommended in the FTDI documentation. That is there for EMI, but I am not sure if it is intended to improve emissions, susceptability, or both. They are available in SMT packages at low cost, so it might be a good idea to put one in to be safe. The power connection doesn’t exactly match any of the “cookbook” circuits in the datasheet, but it looks reasonable. I am not certain how it will behave in the different combinations of logic power and USB power. The only change I might consider is to connect it more like section 6.2 of the datasheet, with RESET# driven by USB power, and VCCIO driven by the board’s VCC. Caveat: I have not designed with this chip yet and my knowledge is all theoretical, so I may be all wet.
On the layout side I have a few items.
- The mounting hole diameters are a bit small at 0.039 inches. The BotBoard has 0.125 inch holes to allow 4-40 screws.
- You might want to consider using thermals on the ground plane to make prototype soldering easier. Probably won’t be an issue for production boards made with a reflow oven.
- The speaker silk screen has a polarity marking (a ‘+’ sign by one pin). The connection is backwards relative to this marking. I don’t think it makes any difference for this type of speaker, but I would still turn it around.
- The 3.3V power takes a roundabout path across the board before getting to the header for P16/17/18/19. I would try really hard to route 3.3V to that header separately from the rest of the logic (i.e. use a star connection rather than a daisy chain) in order to minimize noise being coupled to the logic from whatever load is connected to those pins. Same comment for the 3.3V power to the PS2 header.
- Similarly, the 5V power to the A/D converter should be routed separately from the rest of the 5V bus in order to minimize noise on the A/D reference. (Ideally it would have its own separate ground plane too, but that is pretty difficult on a 2-layer board.) I would be especially concerned about electrical noise from the buzzer when it is operating. The current drawn by the buzzer will cause voltage swings in the 5V reference when the buzzer turns on and off.
- In general, I would beef up the power traces as much as possible. Also, the traces to the decoupling caps on the I/O headers could be thickened without causing any layout issues. That would reduce the inductance slightly and make the caps a little more effective.
- The three switches are very close together and are pretty close to nearby headers–they might be awkward to press. That is probably unavoidable given the amount of stuff on the board.
- Very nit picky. The bussed power connections for P8/9/10/11 and P16/17/18/19 are routed on the top of the board, but the others are routed on the bottom. I would route all of them on the bottom unless there is a specific reason not to. No need to change layers. Similar comment for the PS2 connector.
I am very impressed at the amount of function you have managed to fit on this board.
Mike
Thanks Mike,
I will try to fix all of these over the next few days…
Kurt
I have made a pass through your list and hopefully have made some progress. I added a ferrite bead to the FT232RL connection. I sized it for 0805SMT like ones mentioned in document. I have not changed the rest of the FT232RLs yet, still not sure the best thing. The current stuff was based off of board sold by Parallax: parallax.com/Portals/0/Downl … ematic.pdf
And a Parallax made board: parallax.com/Portals/0/Downl … ematic.pdf
Your suggestions on this would again be greatly appreciated.
I did not put a picture of the schematic here as not much yet changed…
But I made quite a few changes in the board:
a) Mounting holes updated
b) Thermals on ground layer
c) Speaker I thought I updated but not sure now will check again…
d) Tried to route through more 3.3v and 5v Busses and less dasy chaining, also took care of the nits of some of the powers/grounds were on top layer…
e) beefed up power sizes - I an wondering if that also should imply some more clearances…
f) tried to give the buttons slighly more room. Could probably gain some more if I move J4 farther right/down and thne shifting the Analog/PS2/… pins over some more… What do you think about edge mounted switches?
Edit: I redid the placements I mentioned, which now gives .2" between switches. I moved the smaller power capacitor for power regulator as I thought it was too close to screw hole. Now cleaner connection.
Propeller with Analog.zip (112 KB)
Kurt,
I hadn’t seen the Parallax schematic. As far as I am concerned that makes your design a “proven” design and I wouldn’t change it.
The layout changes look good on the image you posted. (I’ll open the file in Diptrace when I get home and look a little more closely.) I think you have addressed my concerns about power routing. There is only so much you can do to free up space for the buttons, and I think you might be at the limit. It seems like edge mounted switches might be limiting for some board mounting arrangements.
One new thing to check is the clearance near mounting holes. Is there enough space for the head of a 4-40 screw? Specifically, C6 and the VSVL and P0/1/2/3 headers. I’ll check tonight to see how much clearance I allowed on the BotBoard. I think Jim had some requirements in this area, but don’t remember details.
Mike
Thanks Mike,
I updated the drawing after and documents after I think you downloaded. I thought C6 was bad as well and has been moved. As you can probably see in the updated drawing above.
Kurt
I have been out sick for about a week. I never miss work… I’m swamped. The tops of the screws we use (4-40 hex socket head screws) measure about 0.181" so make sure no components are closer than 0.205" on the top or the screws will not fit. On the bottom there needs to be at least 0.285" to clear the 1/4" hex spacers, so maybe 0.305". That’s all I got for now. 
Hope you are feeling better Jim.
I thought I remembered that there was more clearance required on the bottom than the top, but couldn’t remember why. Makes sense.
Mike
Ok, as I sometimes like to stack boards, I took it that it would be good if nothing on either layer were with an a radius of .15" from the center of the mounting holes on either top or bottom. I think I was pretty close to the BB2 on the bottom with the 20 pins, but found it had about .1" on left and .2" on right. So I shifted everything right .05. I move the cap associated with pins 16-19 to the left of the group on the bottom so it wont be there. On top Moved everything such that Analog group leaves .o15 on right, moved jumper for Analog reference down as well. On top Left moved large cap to right slightly, plus then moved all of the buttons…
Also moved power regulators down some… So should be more clearances all the way around the screws.
Kurt
Propeller with Analog.zip (113 KB)
Looking really good. A few more things caught my eye.
- There might not be enough clearance between R8 and the PS2 header.
- There are a number of cases where silk screen seems to overlap SMT pads. This should be avoided. Examples are the USB connector, reference designators for R1, U8, J1, D5, R2, R3, R4, R7R17, C9, R13.
Mike
Thanks Mike. I missed the R8 one last night, I moved/rotated it and gave it more clearances. I took a pass through this morning with updating the silk screen stuff (makes sense). I hope I did not miss any…
Kurt
Propeller with Analog.zip (113 KB)
Kurt,
I think you got them all, except maybe for the USB connector, but that is no doubt in the library component. I am not very experienced with Diptrace. I know Eagle has a “documentation” layer that shows up on the display, but is not by default included in the silk screen Maybe the library component for the USB connector uses something like this, and the lines will not show up in the actual silk screen. The way to tell is to use a Gerber viewer on the generated files. I have used Viewmate (a free download from Pentalogix) for this purpose, but there are other products out there as well. It’s amazing what you can find this way that you totally miss in the PCB editor. I highly recommend this step before sending the files off to be built. And of course run the design rules check on the board if you haven’t done so lately.
One final step I often (but not always) do before ordering boards is to print the board 1:1, tape it to a piece of foam core, use an ice pick to punch holes for the through-hole components and mounting holes, and put on as many components as you have on hand. This is a good way to catch clearance issues that don’t show up in the layout software (usually due to inaccurate library components). I have had issues with screw terminals taking up more space than I thought in previous designs.
I’m trying to think of other things that have bit me, usually when I create my own library components. Hole diameter is one–I have made boards where the holes for some through-hole components were too small for the leads. But your board looks good on that front.
I think it might be about time to dive in and get some boards made. I have had good luck with Olimex (inexpensive but 3-week turnaround with shipping) and PCBFabExpress (their “standard technology” boards are good quality with reasonable turnaround).
Good luck!
Mike
Thanks Mike for all of your help!
I found the mini-usb from a different project, so now I imported it into my custom library and edited the top pattern so it no longer overlaps the pads. I did not upload a new set of files yet as that was the only change.
Jim, what should I do next!
Kurt
Get a few boards made and I will reimburse you for all costs. It is up to you where to go. When we get them I will get some chips to populate them. We will have to find someone to assemble them. This is exciting!
I downloaded the Gerber viewer that you mentioned and I did a first pass Gerber output… I viewed them and my gut tells me that I should change some of the rules for the paths to give some more clearances to the etch, especially for some of the larger ones… Here is a bitmap of the current bottom…
I will try playing around with the clearances and see if it makes my gut feel better. I am guessing I will go with the Olimex as you say you have had good luck with them… Will try to order early next week. I think they are closed this week anyway
Kurt
Kurt,
I agree with your gut. One thing I didn’t do in my review (but should have) was check the design rules. You are currently at 6 mil (0.006 in) clearance for most things. I would go with minimum 8 mil, and prefer 10 mil. For copper to board edge, 40 mil is what I have used. (I got my design rules files from Olimex. They are pretty conservative.) A good board house will be able to handle 6 mil clearences, but they might charge more, take longer, and/or have a greater probability of defects.
After changing the copper pour clearance, check the ground plane and make sure it doesn’t have any breaks or lengthy paths. It doesn’t look to me like you will have any problems.
For this order I would probably go with PCBFabExpress since they are not much more expensive (besides, Jim is paying 
, with quicker turnaround and generally higher quality. I have never had a defect in an Olimex board, but the PCBFabExpress boards look better. The alignment is better, the silk screen is cleaner, and the edges are neater because the boards are routed apart rather than sheared. Olimex is very Eagle-centric, which worked great for me since I use Eagle. The best thing about them is that you can send them multiple designs, and they will put them all on the same panel and route the different boards apart for no extra charge. Also, you can send them Eagle files and they will do all the post-processing for you. Neither of these is an advantage for you in this case.
Whichever board house you go with, let me know and I will send one of my submissions. They both require “readme” or similar files with instructions, and it is easier to pattern it after a previous order.
Mike
Hi Mike,
I will go with your suggestion. PCBFabExpress… I have been playing around with the design and clearances and the like and have uploaded a new set of files. I have most things up to the 10mil. I am having some difficulty getting that much with the pads of some of the components. I was having problems with the patterns used for the chips: TXB0104PW/TXB0108PW, so I edited them and I think they are now to the TI specifications for pad locations and sizes.
I imported the generated Gerber/drill files into viewmate and tried running their DFM stuff and a lot of it is good However it does
Error: on the mounting holes not having min copper rings. Not sure what to do here
Warnings: I think I have hand edited out most of the routing warnins…
Warnings: on silkscreen stuff.
Any suggestions?
Thanks
Kurt
EDIT: I made a second version of it layout file where I replaced the mounting holes with static Vias with hole .125 and external .165. I converted to Gerber and ran through the viewmate DRM stuff again with no errors. Is this a reasonable way to go.
Propeller with Analog.zip (261 KB)