[Cryptech Tech] Novena dev-bridge board status

[Fredrik Thulin]

Jacob and Peter, thanks for all your comments. I'll try to respond to them all 
here.

On Tuesday, June 23, 2015 10:28:36 AM Jacob wrote:
...
> I spent some time going over the PDF schematic and Gerber files. Since
> Eagle is not my preferred system, I am not fluent with it so up to now
> I haven't looked at the source schematic and pcb under Eagle for these
> latest files.
> 
> I have some issues with the schematic and the layout. If it was my
> board, I wouldn't feel comfortable to go to production at that stage.
> Will it work if I go? it might, but I wouldn't bet on it.

I wouldn't call this production, but of course I want the board to work so 
I've done what I can to address your issues.

Jacob:
> For example:
> Schematic:
> - R9 is 100 Ohm, meaning 50 mA max power to the design. The consumers on
> the board, especially during switching, require more than that. The
> board is probably starved.

Right - that came with the copying of the significantly smaller novena entropy 
source board. As Peter said, figuring out the right value for R9 can be done 
later.

Peter:
> I took a closer look at the power supply inputs - it seems that the
> Micro-USB VBUS is connected to VCC, meaning 3V3, which isn't right.

No, it is connected to P-5.0V_MAIN. Added missing label in schematics to make 
that clear.

Peter:
> Suggest add schottky diodes, e.g. one BAT54C if 200mA is enough for
> the board, between 5V/VBUS and U1:
>
> 5V ---|>|-+
>           +-- U1 VIN
> VBUS -|>|-+

For protection against back currents? I already have the dual BAT54S in the 
BOM so that would be easy. I measure the STMF429 discovery board to around 190 
mA 5V, but it has that huge display to drive too... the 3V3 LDO is rated at 
150 mA anyways (I have not added diodes yet).

Jacob:
> - Noise Generator: The shield is connected to AGND, but the analog
> power supply (-15V) and the power amplifier are connected to digital
> GND. 

DC charge pump is connected to GND yes - since it lives outside of the 
shielded area. Peter once said the charge pump could/should share GND with the 
noise generator circuit, but I'm a bit reluctant since I think it might 
introduce noise.

The amplifier and digitizer on sheet 3 were mislabeled GND instead of AGND in 
the schematics. Fixed.

Jacob:
> Also, I could not find AGND return in the schematic.

I think I'll blame Eagle there. The only way I found to get a good solid 
connection between GND and AGND (in the one place where they are tied together 
at the boundary underneath the shield) was to make it with polygons of equal 
rank that overlaps. Polygons are just shapes on the board and not represented 
in the schematics, but I'll make a note of this on sheet 3.

Jacob:
> Also, the designed analog plane under the noise sub-system is supposed
> to be decoupled from the digital ground. However the digital ground and
> the digital power are extended under the whole region, coupling unwanted
> noise to the expected analog plane.

Better now? Removed POWER plane underneath the shield. AGND has a polygon on 
GND layer (15) and also on bottom layer. The latter is just to make it 
visible. I'll confess to not really knowing what I'm doing with these separate 
ground planes - just making what I believe are good guesses.

Jacob:
> - I don't see the Ref Des of the decoupling caps of the STM32F in the
> PDF, so it is hard for me to verify association to the layout
> ( I suspect that their placement on board is not optimal).
...
> I opened up the schematic in Eagle to identify the 
> caps, so for example please look at C17 and C33. C17 is a bulk 
> capacitor, - can be away from the chip. C33 is 0.1uF and needs to be 
> close to the relevant pin and if more than 2mm away then it should have 
> good vias to the planes.
> However, in the layout (see attached pic) C17 is near the processor pin 
> while C33 is too far away (yellow path in pic) and without low impedance 
> path to the power plane. The two caps need to be switched around, and 
> the bulk cap C17 needs to have good size vias to the planes (to GND 
> *AND* to PWR)

Thanks for pointing that out. I swapped C17 and C33 locations and generally 
did what I could to minimize the distances between pins and caps. Keeping it 
under 2 mm is a real challenge when the board is 1.2 or 1.6 mm thick, for 
bypass capacitors on the bottom side.

What is a good sized via here?

Jacob:
> If the missing RefDes just a PDF issue or also in the source schematic?
> - there might be other issues - I haven't gone over all sections yet.

Restored the RefDes:es in the schematics.

Attaching new set of files.

/Fredrik
-------------- next part --------------
A non-text attachment was scrubbed...
Name: rev01-eagle.zip
Type: application/zip
Size: 233328 bytes
Desc: not available
URL: <https://lists.cryptech.is/archives/tech/attachments/20150623/1b115a2c/attachment-0002.zip>
-------------- next part --------------
A non-text attachment was scrubbed...
Name: rev01-gerbers.zip
Type: application/zip
Size: 211618 bytes
Desc: not available
URL: <https://lists.cryptech.is/archives/tech/attachments/20150623/1b115a2c/attachment-0003.zip>
-------------- next part --------------
A non-text attachment was scrubbed...
Name: rev01.pdf
Type: application/pdf
Size: 226768 bytes
Desc: not available
URL: <https://lists.cryptech.is/archives/tech/attachments/20150623/1b115a2c/attachment-0001.pdf>