Hi,

I am trying to figure out how the circuit simulators (ADS or Cadence and so forth..) actually measure the S-parameters of a 2-port network.
The classical definition of S-parameters is to use the incident (Vi) and reflected (Vr) voltage waves. For example in order to measure S11 we will calculate S11=Vr/Vi. This is actually the way a network analyzer works. It drives the port with an incident wave and using a directional coupler it separates the reflected wave and thus can measure it.

What I find hard to understand is, suppose that my 2-port network includes a series resistor and a shunt capacitor (both lumped) with 50 ohm ports.How does the simulator measure the reflected wave (Vr). there is no directional coupler used...

Is it possible to reproduce the S-parameters simulation results using an AC simulation?

Thanks in advance....

Frank, Thank you for the link.
In this document it actually plots the S11 over frequency. Do you know how it calculated the S11 from the simulation?
One way I can think of is that it finds the input impedance by dividing the voltage by the current on the input node. and then it uses the relationship gamma=(Zin-50)/(Zin+50) to find S11. so effectively there is no reflected wave measurements here like in a real network analyzer...

Hi Rfmagic,

The measurement setup is as follows:
1. The AC source has a magnitude of 2 V
2. The source resistor is the port impedance (50 ohms)
3. S11 is the AC voltage at the input of the DUT minus 1.

S11=20*log10(Vin-1)

In Wes' simulation he performs the subtraction by using a 1 Vac source from the input node to the node labeled S11.

You can understand the relation by thinking of limiting cases.

1. If Zin=50 ohms then Vin=1 (i.e. it is matched) and S11=1 or -inf dB
2. If Zin=inf then Vin=+2V and S11=+1 or 0dB
3. If Zin=0 then Vin=0 and S11=-1 or 0dB

Have fun.

Frank and RFICDUDE thanks for your answers.

so if we use the wave terminology, (Vin-1) is the reflected wave and 1V is the incident wave?

thanks a lot, Now it is well understood.