Finding variation in input impedance by varying a resistance using LTspice

Question

I am trying to find the input impedance \$R_{in}\$ for the circuit given below using a 1 kHz sinusoidal source.

I want to plot the input impedance on the y-axis and the parameter \$R_{2}\$ on the x-axis.

However, when I run the simulation I get a set of graphs corresponding to different values of \$R_{2}\$ with time on the x-axis.

How can I get the graph for variation of input impedance with respect to \$R_{2}\$?

Answer 1

Let's start by clarifying some things:

• Impedance is a frequency-dependent quantity. Therefore, as well as other transfer functions, it is characterized by phase and magnitude.
• LTspice perform a small signal ac analysis. This means that the result of this simulation only makes sense if the AC perturbation is small respect to DC operating point, so take care of this.

However, I assume you are interested only in impedance magnitude at the fixed frequency of 1KHz in function of parameter {r}. It's not a common thing in LT spice analysis but I got what you are looking for.
Follow these steps:

1. Remove your .tran directive
2. Right click on voltage source / small signal AC analysis / set the ac amplitude
3. Simulate/Edit Simulation Command/AC Analysis:
   Type of Sweep: Decade Number of points per decade: 1 Start Frequency: 1k Stop Frequency:1k In this way the simulation will evaluate the response of the circuit only for the frequency of 1kHz at the different values of stepped parameter {r}.
4. Run simulation, plot V/I
5. Right click on the left vertical axis (magnitude axis), click on linear Representation.
6. Right click on the right vertical axis (phase axis), click on "don't show phase"
7. Right click on time axis. In the quantity plotted tab, check if the content of the tab is the parameter you are interested in (in this case, r). Uncheck the Logarithmic box.

In the pic you can see an example of this analysis with a part of your circuit.

At this link you can read more about parametric plots in LT spice.

Answer 2

I want to plot the input impedance on the y-axis and the parameter R2 on the x-axis.

In Edit Simulation Cmd select AC Analysis, 1 point, start frequency 1k and stop frequency 1k. Run AC analysis, then plot V(Iin)/I(C2) which is the impedance at Iin. Change the left Y axis from Decibel to Linear to get resistance in Ω. You should get a graph like this:-

If the simulation is slow then increase the step size to eg. 0.5k. This will produce the same curve but not quite as smooth at the low end.