Feature #3313
closeddesign simple SFP breakout board
100%
Description
- SFP cage + connector
- 4x SMA for RD+/RD-/TD+/TD-
- 2.54mm header for accessing I2C of SFP
- 2.54mm header with all the misc signals (LOS, etc.)
- power supply (5V input, DC/DC to 3.3V, 300mA max, filtering as per SFP MSA)
Basically we want the inverse of https://shop.trenz-electronic.de/en/TE0422-02-SFP-2-SMA-Adapter
There seems to be a board close to what we want, but USD 495 is ridiculous for something that has a parts cost of USD 30: https://hitechglobal.us/index.php?route=product/product&path=59_90&product_id=124
The resulting design should be something small which we can easily hand to prototype manufacturers. Staying within 10x10cm might be a good idea, if possible.
In terms of the SFP connector and cage, I would suggest to use- https://www.digikey.de/products/en?keywords=U77-A1114-100TCT-ND
- https://www.digikey.de/products/en?keywords=UE75-A20-6000TCT-ND
both are relatively low cost and available in quantity from stock.
Files
Related issues
Updated by laforge almost 6 years ago
- Precedes Feature #3314: design simple SFP experimentation board with LVDS transceiver added
Updated by tnt almost 6 years ago
I just did a footprint for SFP cage and connectors referenced above. I'll upload it this afternoon (couple of tweaks left :p)
Updated by laforge almost 6 years ago
mschramm please let's keep the related eagle library / design files in @osmo-small-hardware.git
http://git.osmocom.org/osmo-small-hardware/ and make sure to commit frequently. thanks!
Updated by mschramm almost 6 years ago
- Checklist item schematics set to Done
- Checklist item board layout set to Done
Updated by mschramm almost 6 years ago
- % Done changed from 0 to 50
A simple PCB has been committed, derived mainly from SFP exoperimenter PCB (see #3313).
Remarks see ticket #3313, some apply here too. - The break in the GND plane under the diff signals of the SFP receptacle is not nice and should be improved on both PCB - if we don't go to a 4-layer PCB (and remain w/ 1.55mm FR4) for a 'closer' GND plane.
Updated by laforge over 5 years ago
13:25 < tnt> Any "real" design using the SFP would be 4 layer, so I guess it's an argument to make the experimentation board as close to what a final product would use.
so let's go four-layer. mschramm: please change layer stack-up, add gnd/vcc planes, and adjust trace widths for "usual" four-layer stacking.
Updated by laforge over 5 years ago
let's please also add some form of polarity protection to the DC input. A regular series diode would be the simplest approach, but the TLV1117 requires up to 1.4V drop-out voltage, which makes the budget for 0.7V quite tight. (3.3+1.4=4.7V). Even a shottky diode is unrealistic at that point.
So either we use a different approach for polarity protection, or a different voltage regulator with lower drop-out voltage. Moving away from nominal 5V DC as input voltage is not really a good idea, IMHO.
There are LDOs with built-in reverse polarity protection. However, we cannot use electrolytic caps at the input (C3) in this case. But 10uF at 5V is definitely possible to get as ceramic?
Updated by laforge over 5 years ago
MCP1825ST-3302E would have a maximum drop-out voltage of 0.35V, i.e. allow a series diode. It's readily available and we have used it before (and hence it's in our eagle lib). maybe worth a thought?
Updated by laforge over 5 years ago
for the record: EAGLE designs are in http://git.osmocom.org/osmo-small-hardware/tree/sfp-breakout
Updated by mschramm over 5 years ago
- Status changed from In Progress to Feedback
- % Done changed from 50 to 80
PCB revised
- 4 layer stack
- LDO is now a MCP1825
- input protection w/ Schottky series diode and TVS
Some suggestions by tnt still pending (see #3314#note-12), trying to integrate them today.
Updated by mschramm over 5 years ago
- % Done changed from 80 to 90
added features asked by tnt - see #3314#note-15.
Updated by laforge over 5 years ago
- Status changed from Feedback to Resolved
- % Done changed from 90 to 100
Thanks. I extended the default clearance from 0.15mm (was looking quite small in getbv) to 0.25mm, re-ran the DRC and now ordered 10 boards from Seeed.
The clearance change + exported gerber has been committed.
Updated by laforge over 5 years ago
- Related to Support #3524: assemble + test SFP breakout board added
Updated by tnt over 5 years ago
The boards that I have don't have the 3v3 connected on the bottom pin header.
Eagle schematic and board file look fine, but the gerbers are not ...
Also check on the -experimenter board and on that one, the 3v3 is connected.
Updated by laforge over 5 years ago
tnt wrote:
The boards that I have don't have the 3v3 connected on the bottom pin header.
Yes, I'm sorry, that's indeed a known bug :/
Eagle schematic and board file look fine, but the gerbers are not ...
See "git log", the error was fixed after the gerber/boards were made/tested.
Updated by laforge over 5 years ago
- Subject changed from design simple SFP experimentation board to design simple SFP breakout board