LTspice simulating varying capacitance in cap-to-voltage simulation [closed]

Question

I am interested in simulating the increasing output voltage and the end of this circuit when the parameter C1, changes according to a list of increasing capacitance values. So far I have managed to perform a simulation with varying caps how ever what I obtain is the capacitance value changing overtime, what I would like to have is a capacitances vs. voltages graph/tab.

---

Hi i did as you suggested however as soon as i try to insert the .meas command my programm crashes. Do you know why? Thank you 1: https://i.sstatic.net/Fy703e0V.png [2]: https://i.sstatic.net/ykZJKft0.png

Ok I have managed but the option Plot .step and .meas data is disabled

Answer 1

1 V for the sine input is too "large" ... I used 10 mV.
The opamp used is LT1037. Don't have ADA4610 in my database.
The opamp shows some "instability" with square wave input.
That is why I used sinusoidal excitation input.

Function v(vo) vs C1 seems linear (from 1 nF to ~ 1 uF)

Made with microcap v12

Answer 2

With LTspice, this is probably easier in an AC analysis as shown in the example below. You can do this in a Transient analysis if clipping is of interest.

Use the .step command to change the value of C1. This produces a family of curves for each value of C1.

Use the .measure command to measure the value at the desired frequency, 105 kHz in this example.

To plot the different values at 105 kHz: View -> SPICE Error Log, or Ctrl+L.
This will bring up a text window where the measurement data is shown.
Right-click in this window and select Plot step'ed .meas data.
You should now see the, in PSpice parlance, performance data plot.

Below is the error log from the simulation. The results of the measure statement is highlighted (highlighting done my me) in yellow. If there is a syntax error in the .measure statement, LTspice will not give any indication of an issue except that there will be no information from the .measure statement.

Some notes about the setup of the graphs.
The upper graph is the plotted stepped measured data.
The lower graph is the probed data at node out.

You stated that you were interested in the output in volts. To get the graph to show volts instead of dBV, right-click on the left y-axis and select Cartesian. Next, modify the trace name from V(out) to abs(V(out) to show the magnitude results (instead of the real portion of the complex number). Right-click on the right y-axis and select Don't plot imaginary component. These steps are performed since the Cartesian data is shown in complex (real+imaginary) form.

For the plotted measured data, do the same steps as above. Changed the x-axis to linear (right-click on the x-axis) if so desired.

The opamp is the universal opamp model which is a behavioral model. It doesn't need a power supply and can give unrealistic output voltages as seen in the above graph (not many opamps can output 50 volts).