Frequency distribution amplifier

[awallin]

I made some draft plans for an SMD version of the tried and tested TADD-1 frequency distribution amplifier:
http://www.anderswallin.net/2015/11/frequency-distribution-amplifier-plans-a-k-a-smd-tadd-1/

constructive comments and suggestions on the schematic and layout welcome!

I hope this will be a prototype during this year and a small series produced early next year - including 1U 19" enclosure for two of these side by side.

thanks,
Anders

[analogNewbie]

the gnd is not connectted to any of the output transformer pins.

[awallin]

the gnd is not connectted to any of the output transformer pins.

Thanks! Fortunately this was fixed before I ordered 2 boards.

One channel assembled today and tested:
http://www.anderswallin.net/2015/12/frequency-distribution-amplifier-first-tests/

Anyone have experience with the LP38798 linear regulator? Recognize a 'fingerprint' of some known noise-source in the phase-noise plots?

I am looking at the ADA4899-1 datasheet - might be worth a try!?!
That one should have an input voltage noise density of around 1nV/sqrt(Hz) instead of 6 nV/sqrt(Hz) for the AD8055 used now.

Any other op-amp suggestions? Should be unity-gain stable, low noise, low distortion. +20dBm 10MHz sine-wave slew rate is 200 V/us so more than that.
SOIC-8 footprint could be easily tried on the current board.

[awallin]

A time-nut should never be satisfied with a sub-par noise-floor, so I did some SPICE simulations and came up with a v2 design:
http://www.anderswallin.net/2015/12/frequency-distribution-amplifier-v2-simulations/

I'll think about this for a few more days and then order boards and parts for the next prototype.

[awallin]

Well bummer  , I assembled my v2 board with an ADA4899-1 and the simulation shows >10 dB better phase-noise floor but in reality it is worse than the v1 board with an AD8055 

The 6502B is the best distribution amplifier I measured so far, so we apply: "Don't turn it on, take it apart":
https://www.dropbox.com/sh/3vxyu87ax5cqjyf/AACQWDG3lN5lpnvTAqRXKW9ia?dl=0
Update: here is the latest schematic I have https://dl.dropboxusercontent.com/u/5709522/6502B/6502B_schematic_v2.pdf

Anyone see the same circuit in the pics as I tried to sketch? Or something I interpreted wrong or missed?
kicad schematic available by e-mail/PM.

Anders

[awallin]

I removed the files from dropbox, and instead posted them on my blog:
http://www.anderswallin.net/2016/02/symmetricom-6502-distribution-amplifier/

The op-amps used are:  (GBW, Slewrate, Voltage-nosie)
input-stage: LMH6702 1700MHz  3100 V/us  1.83 nV/sqrt(Hz)
output-stage: LMH6609 900MHz 1400 V/us  3.1 nV/sqrt(Hz)

I'm thinking of maybe trying the AD8000 also:
AD8000 1500MHz 4100V/us 1.6nV/sqrt(Hz)

Earlier I tried an ADA4899, but the limited slewrate creates lots of distortion with anything above maybe -4 dBm signal, so it can't really be used 
ADA4899-1 600 MHz 310 V/us 1 nV/sqrt(Hz)

The powersupply in the 6502 is very simple: transformer, rectifier, caps. Then adjustable regulators LM317/LM337 (two in parallel I think). Each op-amp has both and RC-filter and an LC-filter on both power-supply pins.

Suggestions for other op-amps to look at, as well as low-noise regulators worth looking at are welcome!
Related to this, Charles Steinmetz recently posted a PDF on distribution amplifiers on the time-nuts list:
http://www.ko4bb.com/manuals/62.78.147.191/Tutorial_Distribution_Amplifier_Architectures_STEINMETZ_rev1.pdf

[TheSteve]

Looking forward to further updates, I'd quite like to build a nice distribution amp.

[uncle_bob]

Hi

Op amps are not really a good way to do this. (as you have found).

Is this a single frequency application (as in 10 MHz distribution)?

Bob

[Jay_Diddy_B]

Anders,

I have had a look at your schematic. I think you need to use dual power supplies. Here is your input section:



I can build a simplified model of this:




The OP-AMP has been replaced with a voltage controlled voltage source E1. I have given the amplifier a gain of 10 million to represent an op-amp with a 140 dB of gain. This is essentially a model of a perfect op-amp.

I have set the input to 0 by not having an input. 

I have placed an AC source in series with the power supply so that I can measure the gain from the power supply to the output. The measured gain is shown here:




It  is -6dB.

Way too much gain from the power supply to the output.

If modify the model so that I have power supply ripple at 100kHz 0.1V pk and an input 1 MHz 0.2V pk (0.1V peak after 50 Ohm loading) and I measure the output FFT. I see two signals the Power Supply ripple and the amplified input signal. The desired signal has a gain of +6dB from input to output. There is a gain of -6dB from the power supply to the output.








Regards,

Jay_Diddy_B

[awallin]

Thanks Jay, nice simulations!

The improved version of the biasing voltage divider looks like this:


Here the idea is to shunt resistor-noise from the divider R2/R3 to ground via C5.
So as not to short-circuit the signal also to ground we need a 'T' shape with new resistor R9 (50R here).
If you have time and interest, could you run your simulations for this biasing circuit also?

Having said that, my v3 design uses split supplies and is inspired by the Symmetricom 6502B teardown. I am now working on the linear regulators and powersupply input filtering. The idea is to use TPS7A47 and TPS7A33 LDOs, BNX025 filters, and maybe a discrete LC-filter and/or common-mode choke as well. Ideas welcome.
The plan is to use something like a Traco Power TMT for +/- 12V and feed that to the LDOs
http://assets.tracopower.com/TMT/documents/tmt-datasheet.pdf

Stay tuned, v3 boards, assembly, and measurement results hopefully within 2-3 weeks...

Anders

[Jay_Diddy_B]

Hi Anders and the group,

I have modified my model to this:



When I run the simulation I get:



The PSRR is improved at higher frequencies. At low frequencies the circuit can be simplified to the Thevenin equivalent of the two 1K resistors and the 10uF capacitor, giving a 20dB/decade slope from 31.8Hz.


The input impedance, for the main input is 25 Ohms with the values shown. This can be corrected like this:



The 50 Ohm resistors are changed to 100 Ohm:



The low frequency PSRR is not changed:


The circuit has about 11 dB PSRR at 50 Hz and 16.4 dB at 100 Hz.


Regards,

Jay_Diddy_B