Programming mathematical software with complex numbers, where each numeric value has a real component and an imaginary component, can be complicated. As requested by our users, CircuitLab’s circuit simulator engine now tracks a *third* component for each complex-valued circuit variable (i.e. voltage or current in a frequency domain simulation).

The third component is the **integer wrap count**: the number of times that this variable has wrapped around a full circle, from a polar representation perspective. By adding wrap count to our internal complex number representation, we now return more human-friendly phase graphs in cases where a circuit’s phase response extends beyond the $\pm 180^\circ$ range.

Phase wrapping happens because we can’t distinguish between $f(t) = cos(2\pi f t)$ and $f’(t) = cos(2\pi f t + 2 \pi n)$ for any integer $n$. The two signals $f(t)$ and $f’(t)$ are identical.

When we use complex numbers to handle the frequency domain (i.e. the Fourier transform, or more generally the Laplace transform), we’re left with only a real component and an imaginary component to our solution. In most programming languages, a function called `atan2(imaginary_part, real_part)`

(2-argument arctangent) is used to compute the phase angle of a point on the complex plane. The range of this function is $(-\pi, +\pi]$ radians, or $\pm 180^\circ$. The `atan2`

function can never return phase angles outside that range.

Phase wrapping is therefore a **numerical ambiguity** that arises in many kinds of signal processing systems when we are trying to recover the phase. Earlier in my career, I encountered it while doing image processing with intentional Moiré interference patterns, as well as phase-shift laser rangefinders.

(*Side note:* most of today’s LIDAR systems being deployed in smartphones and autonomous vehicle systems use time-of-flight, not phase-shift, to measure distance. Each ranging concept has different strengths and vulnerabilities. These are mostly analogous to the issues found in radar, and I recommend comparing the Continuous-wave radar to Pulse-Doppler Radar Wikipedia pages for a brief primer.)

When a circuit simulator like CircuitLab computes the frequency response of a circuit, it:

- Iteratively solves the nonlinear equations to find the operating point of the circuit.
- Turns the circuit network, linearized about the operating point, into a system of equations. These are real-valued differential equations in the time domain.
- Applies the Laplace transform to turn the real-valued differential equations (with time derivatives) into a system of complex-valued equations in the Laplace domain (with no derivatives).
- Solves the complex-valued matrix equation at a desired frequency.

This lets us provide a sinusoidal steady-state stimulus at a particular voltage or current and then see how the rest of the linearized circuit model responds. Specifically, if stimulated at node (or edge current) X, what happens at some other node (or edge current) Y?

- Does the circuit amplify or attenuate?
- Does the phase lead or lag relative to the input?

Both of these questions, magnitude and phase, are answered by the complex number that comes out of our solution.

At a single frequency, our solution is a single complex number (for each voltage or current in the circuit).

But when we sweep over a range of frequencies, we can watch and follow along as this output point moves clockwise, counterclockwise, inward, and outward on the polar complex plane as frequency changes.

Each state variable (current or voltage) is represented by a complex number. By following each value around and watching closely to see if it moves across the $\pm \pi$ crossover line, we can appropriately increment or decrement the wrap count to provide continuity, so that:

$$\phi(z) = atan2( Im(z), Re(z) ) + 2 \pi \cdot Wrapcount(z)$$

This new formula for phase angle allows the simulator to represent complex numbers with phase angles like $-185^\circ$, which was impossible previously.

If you’re new to CircuitLab, we have a 1.5-minute video showing how to draw a circuit and run the Bode plot (magnitude and phase frequency response):

Next, let’s look at a few circuits where phase wrapping comes into play.

We can chain three one-pole low-pass filters in series, each providing $-90^\circ$ of phase lag past its respective cutoff frequency.

In this example, each LPF is implemented with a Laplace Block. For example, a transfer function of `1/(1 + s/(2*PI*100))`

creates a one-pole low pass filter with a -3dB frequency of 100 Hz. We’ve chained together 100Hz, 10kHz, and 1MHz LPFs:

*Click the circuit above and run the frequency domain simulation for yourself. Feel free to change the transfer functions and see how the plot changes.*

The frequency response of amplifiers, filters, and other linear circuits is usually analyzed as a **Bode plot**. The top subchart is a log10-y-scale magnitude plot. The bottom subchart is a degrees-scale phase plot. Both subcharts share a single log10-scale frequency x-axis. If you run the CircuitLab example above, or if you watch the video above, you’ll see that CircuitLab makes it very easy to go from a schematic to a Bode plot.

In both old and new versions of CircuitLab, the magnitude plot is the same:

There is a flat region from DC, followed by a -20 dB/decade region, then a -40 dB/decade region, and finally a -60 dB/decade region.

The phase plot is where things get interesting. In the old version of CircuitLab, the phase plot looked like this:

Notice that at around the 100 kHz point, the phase jumps from $-180^\circ$ to $+180^\circ$. This is a consequence of phase wrapping, rather than anything actually happening in the circuit above. The point on the complex plane has simply wrapped around.

In the new version of CircuitLab with phase unwrapping, the phase plot looks like this:

The unwrapped phase makes it more clear that each LPF adds $-90^\circ$ of phase lag. This is easier to understand, even if there’s no real difference between $-270^\circ$ and $+90^\circ$ of phase offset for a continuous sine wave.

Instead of using artificial (but convenient) Laplace Blocks, let’s build a real circuit, for example an AC-coupled analog amplifier using a NPN BJT:

*Click the circuit above and run the frequency domain simulation for yourself. Feel free to change the circuit and see how the plot changes. For example, make C1 10x bigger or 10x smaller than it is now and re-run the simulation.*

Again, the magnitude plot looks the same in both old and new versions of CircuitLab:

This amplifier gives about 10x voltage gain (+20 dB; see Orders of Magnitude, Logarithmic Scales, and Decibels) over a range of about 500 Hz to 50 kHz. The gain declines on either side of this range.

The phase plot is interesting too. In the old version of CircuitLab, the phase wrapped around and looked like this:

Note that the phase in the passband is right around $-180^\circ$. That’s because this is an inverting amplifier configuration. A small step *up* in the input causes a step *down* in the output.

In the new version of CircuitLab with phase unwrapping, the phase plot looks like this:

With phase unwrapping, it’s much easier to see that phase is relatively flat in the passband.

Eventually, at very high frequencies, the gain drops to 1 (+0 dB) and the phase drops to $-360^\circ$ (equivalent to zero). Basically, at very high frequencies, the capacitances in the circuit (specifically C1 and the base-collector capacitance $C_\mu$ of Q1) increasingly act like short circuits, and a small step up in the input causes an equally-sized step up in the output.

While there is no physical difference between a phase of $-185^\circ$ and $+175^\circ$, the discontinuity in the wrapped phase graphs made CircuitLab hard to use for frequency domain analysis.

This is especially true because there is often special interest in what’s happening from a **feedback and circuit stability standpoint** around the $\pm 180^\circ$ transition, or when analyzing circuits that naturally have inverting behavior in the frequency range of interest.

By modifying our complex number representation to have an integer wrap count, CircuitLab now unwraps the phase for the convenience of our users. In addition to adding new unit tests to our `ComplexNumber`

class around this new behavior, the example circuits above are also part of our extensive integration test suite which we run whenever we modify the simulation engine to ensure we don’t inadvertently cause any behavior regressions as we continue to extend the software.

We’ve just made it much easier to simulate a step response in CircuitLab. Finding a circuit’s unit step response in the time domain is one of the most common operations for anyone learning about or designing analog filters and amplifiers.

It’s always been possible to simulate step responses in CircuitLab using a combination of a voltage source and a switch, but we’ve now bundled this behavior into a signal component: the **Voltage Step Source** and the corresponding **Current Step Source**.

Here’s a simple example comparing voltage step responses between a series RC circuit and a parallel RL circuit:

Click to open and simulate the circuit above. Can you predict the shape of V(RC) and V(RL) before you run the simulation?

Here’s a more advanced example showing how an op-amp non-inverting amplifier can exhibit stability problems, including ringing and overshoot, even with small amounts of parasitic (undesired) capacitance at the feedback node:

Click to open and simulate the circuit above. How long does it take for the output to settle down after the input step? Is there a capacitance level beyond which this amplifier is basically useless?

**Note that the step only happens in a transient simulation.** A DC simulation (or DC Sweep) always happens *before* the step. This lets the simulator find the *old, pre-step* steady-state operating point first, before it models the transient change to a new post-step steady-state.

These new step source components are both available in the “Voltage Signal Sources” and “Current Signal Sources” sections of the CircuitLab toolbox, right between the configurable function generator source and the CSV input source:

After inserting a step source, you can double-click it to configure its amplitude and provide a delay. Conveniently, by default, a step source provides a unit step at t=0.

We’re introducing a new component to the CircuitLab toolbox: the **ideal diode**.

We’ve had semiconductor PN junction diodes since we’ve launched, which show the exponential current-voltage relationship and accurately model real-world diodes.

In contrast, the ideal diode is more like a simulated on-off switch: the I-V curve would be piecewise linear. It acts like it’s open-circuit when reverse biased, and short-circuit when forward biased. You can simply drag the ideal diode from the toolbox into your circuit, and optionally double-click to configure its parameters.

Here’s an example using four ideal diodes to build a full-wave rectifier:

Click to open and simulate the circuit above. Observe how the 4 diodes turn on and off at different times in the AC cycle.

Here’s an simulation comparing the regular PN Junction Diode with the ideal diode:

Click to open and simulate the circuit above.

Note that D2 (a PN junction diode) gives us a gentle knee as it transitions from off to on, as real diodes do. D2’s curve is smooth in the calculus sense: its derivative is continuous.

In contrast, ideal diodes D1 and D3 show an abrupt (piecewise-linear) knee when they change from off to on. These are not smooth in the calculus sense: their derivatives are discontinuous.

- Intending to accurately simulate real-world devices
- Simulation runtime is not a constraint

- Learning about signal rectification (where PN junction complexity is unnecessary)
- Simulating signal clamping behaviors (where hard clamping is acceptable)
- Simulating switching power supplies: buck, boost converters, etc. (where simulation performance is a constraint)
- Other cases where much faster-running simulations are preferred to accurate diode modeling

Both diode models, as well as Zener Diodes, photodiodes, and LEDs, are nows available in the CircuitLab toolbox:

CircuitLab is an in-browser schematic capture and circuit simulation software tool to help you rapidly design and analyze analog and digital electronics systems.