Yeah - Glad they arrived. I may have to sometime set myself up to solder SMD components more easily. I have done some, but some components like the FT2322RL and the USB connector look to be a little more problematic.
Kurt
If you want to hand them to me personally, hmmm…I will probably be getting home late most nights this week, but Tuesday might be an exception. I’ll email and let you know.
Mike
Kurt,
We checked the parts and BOM against the schematic and found some discrepencies.
- C1,C14,… are identified as 100n on the schematic (equivalent to 0.1uF), but the BOM says 100pF. I have some 0.1uF 0603 parts that we can use.
- C20 is identified as a 0.33uF on the schematic but 33pF in the BOM. I thought I had some 1uF parts I could substitute but can’t find them. I am going to throw some 0.33uF 0805 caps in a DigiKey order. For the first board we might stack 3 0.1uF caps in parallel. It looks ugly but works for a prototype.
- C8 (10uF tantalum) is identified in the BOM but is not in the schematic
Otherwise it looks good.
Mike
HI Mike,
Sorry about the ordering mistakes.
The C8 was one that I hoped to sneak in before they produced the boards. It was after I discovered that the USB connector should not have any traces under certain parts of it, I tried to get a change in before they produced them, but they were already started…
Question: On designs like this, when do you use 0805 caps or resistors versus using 0603? My gut tells me it is best to go all possible 0603 as it saves room.
Kurt
Kurt,
No problem, that’s what prototypes are for. I just wanted you to know so you could update the BOM.
0603 are good if you are really trying to squeeze stuff in, but I would use 0805 by default otherwise if only to make manual construction easier. The 0805 packages are also a little more robust. Resistors have higher power ratings, and capacitors have sturdier ceramic layers (less likely to crack under stress). The better performing capacitors (more accurate, better temperature coeff) tend to come in larger packages. So overall I would use larger packages to start and change to smaller if needed.
Mike
I think the update for parts:
c1,c14… Could be:
399-1281-1-ND 6 C1, C14, C16, C17, C18, C6 2 CAP_0603 Murata CAP .1UF 25V CERAMIC X7R 0603 Updated Part
I think C20 could be:
490-1729-1-ND 1 C20 2 CAP_0805 Murata CAP CER .33UF 25V Y5V 0805 Updated Part
Kurt
Kurt,
First prototype finished, being tested. Here are some notes from the build:
- The spacing of the shield headers does not match standard Arduino spacing. In particular, the spacing between the 1x8 headers is not correct.
- The hole sizes for the buttons are too small for the leads. I checked my Eagle library, and it looks like I use a 0.052 inch hole for these switches. We were able to mount the switches, but could not fully seat them in the holes.
- C10 is missing from the BOM.
- It would be good if all the 0.1uF caps were the same package, preferably 0805 if spacing permits.
- There are some vias under the crystal package, and I am concerned about them shorting to the metal body of the crystal. I recommend moving them if possible. (I have never seen a short like this, but might as well play it safe.)
- The JPU, JA, JB, and JC headers are not on a 0.1" grid (spacing relative to each other). This prevents using a 2x4 block for them.
- The various 1x3 headers should line up with nearby 3x4 headers to ease alignment during assembly.
- The ICSP header is just a bit too close to the JPU, JA, etc. headers/jumpers. The programmer can only be plugged in if the jumpers are removed from the headers. It would be nice if it were scooted slightly away (but not so far as to cause clearance issues on the other side, of course
). - The power terminal block silk screen seems to be backwards. If the connector is installed so it lines up with the rectangular outline in the silk screen, then the wires would be coming in the wrong side of the connector.
- It would be very useful to have the VS and VL power inputs labeled in the silk screen.
Testing notes so far:
- Communication with the FT232 works (“new hardware found” message, and we could configure it using the FTDI FTProg utility)
- We were able to download the bootloader and a test app using the ISP header
- We have not yet been able to download an app using the Arduino environment, but that might be the FT232 configuration
- The buttons and LEDs are not in the same order (e.g. button A lights LED B, etc.)
I’ll post more when the testing is complete.
Mike
Thanks Mike,
Sorry about the errors 
. (I am learning). I will play some and try to correct these as you find them.
Kurt,
Like I said, that’s what prototypes are for. Never seen a perfect one yet.
There were a few more things that I forgot to include:
- The polarized cap should have the ‘+’ side labeled on the silk screen.
- I think the USB connector was meant to be mounted closer to the edge of the board. The connector has a little lip right along the bottom edge that prevents it from lying flush with the board unless it is positioned so the lip is over the edge of the board. It’s hard to visualize, but really easy to see when the parts are in front of you. I think the lip on the connector is intended to provide support when the cable is being plugged in. We were able to mount it, but there is a gap between the mounting tabs and the pads.
- I don’t know if this is an issue or not, but the pads for the USB connector tabs are not electrically connected to the board. Are they supposed to be connected to ground? I ohmed out the full-sized USB connector on a normal Arduino and it is connected to grount, but I don’t know if that is standard. I’ll check some boards with mini USB connectors.
Mike
Kurt,
This is a follow-up to my previous post. I pulled up the datasheet for the USB connector and it specifies the layout relative to the PCB edge. So I think the layout should be changed in the next iteration to account for this.
Mike
Thanks Mike,
I have been playing around with the design.
Things I updated:
a)The connectors should be right now
b) Updated hole/pad size for switches
c) I had earlier changed to having 2 large caps, I did not find any of the SMT caps they defined that showed the +, it does have a set of lines in it now? Is this a new way or should I find a way to add the + (make my own symbol)
d) Updated all of the 0603 caps to now be 0805
e) No vias under Crystal
f) moved the JA/JB/JC… jumpers so could now use a 2x4. Also moved farther from ICSP
g) Updated the silk for the Power connector so maybe more correct now. Also added back in the VS/VL ± markings that somehow got lost.
h) Found the A/B LEDs were backwards so reversed.
i) Moved the USB connector closer to edge, not sure if close enough yet? Also wonder about choice of USB connector. My previous Seeeduino Mega boards used this type connector. I had one pull off the board taking the etches with it (may try to fix the board someday). Today I received the 2 new boards which have new type connectors where the edges are not SMT but solder through. Have not found identical ones to this yet. However Molex makes ones that solder thorough as well. Or could bigger type connectors? Thoughts? I would ask Jim but I think they are all on vacation this week?
Kurt
Kurt,
You don’t waste any time, do you? 
This update looks very good.
For the cap markings, you could just add a small “+” character in the silkscreen independent of the symbol. I think that would be more clear than the lines in the symbol.
The datasheet for the USB connector explicitly indicates the PCB edge relative to the pads. I would be inclined to update the symbol to show the PCB edge (maybe in a documentation layer rather than in the silkscreen layer), and use that to help placement. Actually, I would be even more tempted to use a different part if it will fit. The USB connector at Sparkfun (sparkfun.com/products/587) looks more robust (but also a bit larger), and DigiKey has connectors with the same footprint from other manufacturers. A through-hole connector would be fine by me as long as all of the required holes are round. I’ve seen some that need slots rather than round holes.
This part also has a board edge spec in the datasheet, even though it doesn’t seem to have a lip.
Mike
Hi Mike,
I do try 
I added +s to the new CAPS. I sort-of cheated and simply added the + to the silk screen and did not create a new pattern.
I looked at the sparkfun USB connector with their pattern and the like. It is a connector from samtec so should be able to get from other sources. It is for sure bigger, but I do like that there are two through holes to help make sure the component is not ripped off the board when the user unplugs the cable. I also created a fill on the top for the +5v. Not sure if it is needed or if it helps but.
How does this look:
I can also upload the bottom and a zip file with everything if you would like. Have not created and checked gerber files yet.
Kurt
I don’t believe so. My quick look at the data sheet shows it as a 40 pin .6" wide dip vs the 28 pin Atmega 328.
Kurt
Hi Mike,
I am glad we figured out my goof with the connection between the FT232RL and the Atmega and you can now download programs to the board using the IDE 
Glad we are making progress!
I have already updated the Schematic on my side with the fix and I also updated the routing on the board to fix the issue.
Kurt
Kurt,
I knew you would have the board updated already. All the boards now have the fly-wires and are able to download. We have tested with a simple test program that exercises the I/O, and things seem to be working.
Mike
If I went with the hair brain idea of adding I2C to the JR board, it could look like:
What do you think?
EDIT: I updated the board picture as it appears the drill holes were wrong in this version.
Kurt
I like it very much! 8)
Quick question: Are you still doing testing on the current configuration of the board, or should I setup to order a new batch with the current fixes and enhancements?
Kurt