Why doesn't this RC circuit simulate as expected? (i.e. what am I doing wrong?)

Question

I am trying to learn about RC circuits. As I understand it, the indicated point in the basic RC circuit below should produce a current and voltage curve like this. However, when I attempt to simulate the circuit in the embedded CircuitLab and (other online simulators also) I get nothing. I also tried in Digikey's Partsim and got the same results. So it must be something I'm doing wrong...

I chose Time Domain simulation with the following parameters: (I assume the Time Constant for this circuit is about 1 second, so 2 sec should generate a nice curve...)

I'm measuring V and I at the point indicated.

Here's what I get. Notice the scale shows 9.000V top and bottom, and current 0.000A top and bottom.

It makes no sense! Please tell me where I went wrong! Thank you!

^{simulate this circuit – Schematic created using CircuitLab}

Answer 1

The default initial conditions for time domain simulations is almost always the "steady-state" condition assuming all sources were at their \$t=0\$ state since \$t=-\infty\$.

There are a few different fixes for this:

1. Switch to a time dependent source (like what Jim did with a square wave source)
2. Disable the "initial condition" solve step, which usually initializes all nodal voltages/branch currents to 0 (when applicable).

3. Manually specify the initial conditions. Unfortunately, CircuitLab doesn't appear to allow you to do this (other than disabling the "skip initial" step). However, for SPICE-like simulators you can add an .ic command to manually specify the value to use. For example, here I've set the initial conditions V(out)=4V in LTSPICE.

Answer 2

Before starting the transient simulation, the simulator performs a DC analysis which concludes that the capacitor is fully charged so once the transient analysis starts, since your source doesn't change, the output doesn't move either.

The small movement you see in your first simulation waveform are probably due to a small numerical computation error difference between the DC and transient solvers. Once the transient solver "sees" an error it tries to correct for it in the subsequent time steps. Try zooming out your axes on the voltage and current to see how much those waveforms are actually moving by. My bet is that they are pegged at 9V and 0A respectively.

Answer 3

Try running it with a square wave input with a 4 second period, running it for 4 seconds total to see the entire period.

^{simulate this circuit – Schematic created using CircuitLab}