Transimpedance amplifier PCB layout
It's been a few months and I did another iteration of the design.  Based on what I learned I thought I would answer some of my own questions in case they're helpful for other people.


  How bad is my layout and how can I improve it?


My layout had a few problems.  

First, 1206 resistors/caps are ridiculously large. I ended up using 0603s and while they weren't the easiest thing to solder, even with a half broken iron and lead free solder it wasn't that bad to do a few by hand.  The smaller size made all of the layout much, much cleaner, and while I don't think RF performance was necessarily limited by the 1206 package, it didn't hurt to improve it.  I think the better layout helped a lot, I found the revised design performed better and needed less feedback capacitance.  

Second, I completely ignored the standard advice that you don't run a ground plane under an opamp due to the added capacitance.  It didn't matter in this case because the diode capacitance was ~500x larger, but it was still sloppy design.

Third, I put the 50 ohm terminating resistor very close to the 50 ohm SMB terminal, but farther from the opamp.  At these frequencies it isn't necessary to be only a few millimeters from the SMB connector, while putting the resistor farther from the feedback network effectively extends the coverage of the feedback network, adding both capacitance and more chance for noise pick up.  Switching to 0603 parts and moving the 50 ohm terminator right up against the opamp allowed me to really clean up the feedback network layout and get its area to an absolute minimum. 

Forth, one very minor point, I put SMD parts under the avalanche diode.  This worked ok, but I should have been more careful because the diode casing is grounded introducing the risk of shorts if parts have exposed metal (e.g. taller caps).  I probably should not have put anything but the (very thin) opamp under the diode, as that would have minimized the height of the diode and thus the inductance of its leads.   


  The decoupling capacitors on the OPA847 were copied from another design with this opamp. They seem to work, but I am open to suggestions if they are not correct.


Although it didn't make a big difference possibly due to the high quality power supply I was using, there should also have been some larger (~5uF) caps for low frequency rejection somewhere on the board.  

Anyway, this was an interesting exercise.  I hope what I learned will be useful to other people.