Designer’s Guide Community

New member

Guest

Noise figure simulation of a differential LNA???
Aug 02^nd, 2004, 12:11pm

Hi,

Could anybody please help me with how to simulate a differential RF lna circuit using Cadence spectre tool? The spectre manual has the procedure for a single ended lna. I need to find the gain, S-parameters and noise figure of the circuit.
I have couple of questions:

1. I tried using the differential circuit testbench given in this site but I am getting incorrect noise figure. I did the noise chart to see the contributors, and it shows the ouput port as causing 96% of the noise! Anybody familier with this, please help!!!

2. Where should the load be connected? Right now I have it across the output port(vsin).

Could anybody please guide me?!

Back to top

IP Logged

Andrew Beckett

Senior Fellow

Offline

Life, don't talk to
me about Life...

Posts: 1742
Bracknell, UK

Re: Noise figure simulation of a differential LNA?
Reply #1 - Aug 3^rd, 2004, 9:58pm

When you measure noise figure, you really need to specify the output of the noise analysis as a "probe" rather than as a pair of voltages.

When you do this, the noise analysis knows where the load is, and can therefore remove the noise from the load from the noise figure calculation (normally it would not be included).

You could of course make your output port have a noise temperature of -273.152 degrees C, and keep the output as a pair of voltages, but the right way to do it is really to just specify "probe" as the output type on the noise analysis form (or pnoise, or qpnoise, or whatever you're doing).

With sp analysis this isn't an issue, because you always specify the output as a port. However, if you are looking at contributors, you must be doing a conventional "noise" analysis rather than "sp".

Note, in all of this I'm assuming your load is a "port" component (you mentioned "vsin" at one point, which confused me a bit).

Regards,

Andrew.

Back to top

IP Logged

Student

New Member

Offline

Posts: 2

Re: Noise figure simulation of a differential LNA?
Reply #2 - Aug 4^th, 2004, 8:17am

Thanks for the reply Andrew. It still isnt working though. I tried doing the noise analysis only when, doing it with S-parameters did not work.

I am using ideal baluns(from analogLib) at the input and output. I am giving input to differential pin of input balun and am grounding the common-mode pin, and on the output side, I am connecting the output port to the differential pin and grounding the common-mode pin again.

I am using a psin port, I mentioned "vsin" by mistake.

Right now, the simulation is still not converging. I think there is something wrong with the balun connection. I am not sure though.

Back to top

IP Logged

Andrew Beckett Senior Fellow Offline Life, don't talk to me about Life... Posts: 1742 Bracknell, UK	Re: Noise figure simulation of a differential LNA? Reply #3 - Aug 4^th, 2004, 3:31pm OK, you hadn't previously said that it wasn't converging. "doesn't work" is a little non-specific... When you say it isn't converging, do you mean DC convergence, or PSS convergence (or even timestep convergence)? Regards, Andrew.
Back to top	IP Logged

Student

New Member

Offline

Posts: 2

Re: Noise figure simulation of a differential LNA?
Reply #4 - Aug 4^th, 2004, 4:56pm

Hi,

The error I am getting is:

Matrix is singular(detected at 'L1:1' and 'I30.K1:t1'), no DC solution found(no convergance).

To get rid of it, I tried connecting both the input and output baluns common mode pins to psin port with a dc source value of 1V. It is still giving a very high value of noise figure(18dB). I am not sure if I am giving the right values at the baluns. What should be given for a rf differential circuit?

Thanks a lot for looking into this. I really appreciate it. I have not designed the circuit and am actually interested in doing its fault analysis. But I need to know how to simulate it first.

Back to top

IP Logged

Ken Kundert

Global Moderator

Offline

Posts: 2384
Silicon Valley

Re: Noise figure simulation of a differential LNA?
Reply #5 - Aug 4^th, 2004, 8:04pm

Student,
You have created a loop of short circuits. Connecting the common-mode point of the balun to either ground or to a voltage source connected to ground basically shorts any common mode signals across the input of your circuit. If in addition you have an inductor across the input, you have created a loop of shorts. The loop includes L1 and the balun, which presumably is I30. The easiest way to avoid the problem is to determine what common-mode impedance your circuit would expect to see at its input and output, and then put a resistor of that value in series with the common-mode input of the balun.

It is a common mistake to focus completely on the differential path in a differential circuit. But the common mode path must also be considered and tested. Otherwise you set yourself up for nasty surprises. Fortunately, this surprise occurred during simulation where it did not cost you anything except some delay.

-Ken

Back to top

IP Logged