Analog Circuit Simulation:Types of Analysis

Types of Analysis

For analog circuits, there are three commonly used methods of analysis, these being DC, AC, and transient analysis. DC analysis is used to examine the steady-state operation of a circuit; that is, what the circuit voltages and currents would be if all inputs were held constant for an infinite time. AC analysis (or sinusoidal steady state) examines circuit performance in the frequency domain using phasor analysis. Transient analysis is performed in the time domain and is the most powerful and computationally intensive of the three. For special applications, other methods of analysis are available such as the Harminic-Balance method, which is useful for detailed analysis of non-linear effects in circuits excited by purely periodic signals (like mixers and RF amplifiers).

DC (Steady-State) Analysis

DC analysis calculates the steady-state response of a circuit (with all inductors shorted and capacitors removed). DC analysis is used to determine the operating point (Q-point) of a circuit, power consumption, regulation and output voltage of power supplies, transfer functions, noise margin and fanout in logic gates, and many other types of analysis. In addition, a DC solution must be calculated to find the starting point for AC and transient analysis.

To calculate the DC solution, we need to solve Kirchoff ’s equations formulated earlier. Unfortunately, since the circuit elements will be non-linear in most cases, a system of transcendental equations will normally result and it is impossible to solve this system analytically. The method which has met with the most success is Newton’s method or one of its derivatives.

Newton’s Method

Newton’s method is actually quite simple. We need is to solve the system of equations F(X) = 0 for X, where both F and X are vectors of dimension N. (F is the system of equations from modified nodal analysis, and X is the vector of voltages and current that we are solving for). Newton’s method states that given an initial guess for Xi, we can obtain a better guess Xi + 1 from the equation:

We assemble the Jacobian matrix for the circuit at the same time that we assemble the circuit equations. Analytic derivatives are used in most simulators.

The –1 in Eq. 13.10 indicates that we need to invert the Jacobian matrix before multiplying by the vector F. Of course, we do not need to actually invert J to solve the problem; we only need to solve the linear problem F = YJ for the vector Y and then calculate Xi + 1 = Xi – Y. A direct method such as the LU decomposition is usually employed to solve the linear system.

For the small circuit of Figure 13.3, analyzed in steady state (without the capacitor), the Jacobian entries are:

For a passive circuit (i.e., a circuit without gain), the Jacobian will be symmetric and for any row, the diagonal entry will be greater than the sum of all the other entries.

Newton’s method converges quadratically, provided that the initial guess Xi is sufficiently close to the true solution. Quadratically implies that if the distance between Xi and the true solution is d, then the distance between Xi + 1 and the true solution will be d2. Of course, we are assuming that d is small to start with. Still, programs like SPICE may require 50 or more iterations to achieve convergence. The reason for this is that, often times, the initial guess is poor and quadratic convergence is not obtained until the last few iterations. There are additional complications like the fact that the model equations can become invalid for certain voltages. For example, the BJT model will “explode” if a junction is forward-biased by more than 1 V or so since: exp(1/Vt) = 5e16. Special limiting or damping methods must be used to keep the voltages and currents to within reasonable limits.

Example Simulation

Most circuit simulators allow the user to ramp one or more voltage sources and plot the voltage at any node or the current in certain branches. Returning to the differential pair of Figure 13.1, we can perform a DC analysis by simply adding a .DC statement (see Figure 13.7). A plot of the differential output voltage (between the two collectors) and the voltage at the two emitters is shown in Figure 13.8. Observe that the output voltage is zero when the differential pair is “balanced” with 2.0 V on both inputs. The output saturates at both high and low values for V1, illustrating the non-linear nature of the analysis. This simulation was run using the PSPICE package from MicroSim Corporation. The simulation run is a few seconds on a 486 type PC.

AC Analysis

AC analysis is performed in the frequency domain under the assumption that all signals are represented as a DC component Vdc plus a small sinusoidal component Vac .

The series has an infinite number of terms; however, we assume that if Vac is sufficiently small, all terms above first order can be neglected. The first two terms on the right-hand side are the DC solution and, when taken together, yield zero. The third term Wac is the vector of independent AC current sources which drive the circuit. The partial derivative in the fourth term is the Jacobian element, and the derivative of Q in parentheses is the capacitance at the node. When we substitute the exponential into Eq. 13.14, each term will have an exponential term that can be canceled. The result of all these simplifications is the familiar result:

This equation contains only linear terms which are equal to the partial derivatives of the original problem evaluated at the Q point. Therefore, before we can solve the AC problem, we must calculate the DC bias point. Rearranging terms slightly, we obtain:

The solution at a given frequency can be obtained from a single matrix inversion. The matrix, however, is complex but normally the complex terms share a sparsity pattern similar to the real terms. It is normally possible (in FORTRAN and C++) to create a suitable linear solver by taking the linear solver which is used to calculate the DC solution and substituting “complex” variables for “real” variables. Since there is no non-linear iteration, there are no convergence problems and AC analysis is straightforward and fool-proof.

The same type of analysis can be applied to the equations for modified nodal analysis. The unknowns will of course be currents and the driving sources voltage sources.

The only things that must be remembered with AC analysis are:

1. The AC solution is sensitive to the Q point, so if an amplifier is biased near its saturated DC output level, the AC gain will be smaller than if the amplifier were biased near the center of its range.

2. This is a linear analysis and therefore “clipping” and slew rate effects are not modeled. For example, if a 1-V AC signal is applied to the input of a small signal amplifier with a gain of 100 and a power supply voltage of 5 V, AC analysis will predict an output voltage of 100 V. This is of course impossible since the output voltage cannot exceed the power supply voltage of 5 V. If you want to include these effects, use transient analysis.

AC Analysis Example

In the following example, we will analyze the differential pair using AC analysis to determine its frequency response. To perform this analysis in SPICE, we need only specify which sources are the AC driving sources (by adding the magnitude of the AC signal at the end) and specify the frequency range on the .AC statement (see Figure 13.9). SPICE lets the user specify the range as linear or “decade,” indicating that we desire a logarithmic frequency scale. The first number is the number of frequency points per decade. The second number is the starting frequency, and the third number is the ending frequency.

Figure 13.10 shows the results of the analysis. The gain begins to roll off at about 30 MHz due to the parasitic capacitances within the transistor models. The input impedance(which is plotted in kW) begins to roll off

at a much lower frequency. The reduction in input impedance is due to the increasing current that flows in the base-emitter capacitance as the current increases. SPICE does not have a method of calculating input impedance, so we have calculated it as Z = Vin/I(Vin), where Vin = 1.0, using the post-processing capability of PSPICE. This analysis took about 2 seconds on a 486 type PC.

Noise Analysis

Noise is a problem primarily in circuits that are designed for the amplification of small signals like the RF and IF amplifiers of a receiver. Noise is the result of random fluctuations in the currents which flow in the circuit and is generated in every circuit element. In circuit simulation, noise analysis, is an extension of AC analysis. During noise analysis, it is assumed that every circuit element contributes some small noise component either as a voltage Vn in series with the element or as a current In across the element. Since the noise sources are small in comparison to the DC signal levels, AC small signal analysis is an applicable analysis method.

Different models have been developed for the noise sources. In a resistor, thermal noise is the most important component. Thermal noise is due to the random motion of the electrons:

There are other types of noise that occur in diodes and transistors; examples are flicker and popcorn noise. Noise sources, in general, are frequency dependent.

Noise signals will be amplified or attenuated as they pass through different circuits. Normally, noise is referenced to some output point called the “summing node.” This would normally be the output of the amplifier where we would actually measure the noise. We can call the gain between the summing node and the current flowing in an element j in the circuit Aj(f ). Here, f is the analysis frequency since the gain will normally be frequency dependent.

It is also common to reference noise back to the amplifier input and this is easily calculated by dividing the above expression by the amplifier gain. Specifying noise analysis in SPICE is simple. All the user needs to do is add a statement specifying the summing node and the input source. Spice then calculates the noise at each as a function of frequency

See Figure 13.11 for example output. Many circuit simulators will also list the noise contributions of each element as part of the output. This is particularly helpful in locating the source of noise problems.

Transient Analysis

Transient analysis is the most powerful analysis capability because the transient response of a circuit is so difficult to calculate analytically. Transient analysis can be used for many types of analysis, such as switching speed, distortion, and checking the operation of circuits like logic gates, oscillators, phase- locked loops, or switching power supplies. Transient analysis is also the most CPU intensive and can require 100 or 1000 times the CPU time of DC or AC analysis.

Numerical Method

In transient analysis, time is discretized into intervals called time steps. Typically, the time steps are of unequal length, with the smallest steps being taken during intervals where the circuit voltages and currents are changing most rapidly. The following procedure is used to discretize the time-dependent terms in Eq. 13.1.

Time derivatives are replaced by difference operators, the simplest of which is the forward difference operator:

where h is the time step given by h = tk + 1 – tk. We can easily solve for the charge Q(tk + 1) at the next time point:

using only values from past time points. This means that it would be possible to solve the system simply by plugging in the updated values for V each time. This can be done without any matrix assembly or inversion and is very nice. (Note for simple linear capacitors, V = Q/C at each node, so it is easy to get V back from Q.) However, this approach is undesirable for circuit simulation for two reasons. (1) The charge Q, which is a “state variable” of the system, is not a convenient choice since some nodes may not have capacitors (or inductors) attached, in which case they will not have Q values. (2) It turns out that forward (or explicit) time discretization methods like this one are unstable for “stiff ” systems, and most circuit problems result in “stiff systems.” The term “stiff system” refers to a system that has greatly varying time constants.

To overcome the stiffness problem, we must use implicit time discretization methods which, in essence, means that the G and W terms in the above equations must be evaluated at tk + 1. Since G is non-linear, we will need to use Newton’s method once again.

The most popular implicit method is the trapezoidal method. The trapezoidal method has the advantage of only requiring information from one past time point and, furthermore, has the smallest error of any method requiring one past time point. The trapezoidal method states that if I is the current in a capacitor, then:

Therefore, we need only substitute the above equation into Eq. (13.1) to solve the transient problem. Observe that we are solving for the voltages V(tk + 1), and all terms involving tk are constant and will not be included in the Jacobian matrix. An equivalent electrical model for the capacitor is shown in Figure 13.12. Therefore, the solution of the transient problem is in effect a series of DC solutions where the values of some of the elements depend on voltages from the previous time points.

All modern circuit simulators feature automatic time step control. This feature selects small time steps during intervals where changes are occurring rapidly and large time steps in intervals where there is little change. The most commonly used method of time step selection is based on the local truncation error (LTE) for each time step. For the trapezoidal rule, the LTE is given by:

and represents the maximum error introduced by the trapezoidal method at each time step. If the error (e) is larger than some preset value, the step size is reduced. If the error is smaller, then the step size is increased. In addition, most simulators select time points so that they coincide with the edges of pulse-type waveforms.

Transient Analysis Examples

As a simple example, we return to the differential pair and apply a sine wave differentially to the input. The amplitude (2 V p-p) is selected to drive the amplifier into saturation. In addition, we make the frequency (50 MHz) high enough to see phase shift effects. The output signal is therefore clipped due to the non-linearities and shifted in phase due to the capacitive elements in the transistor models (see Figure 13.13). The first cycle shows extra distortion since it takes time for the “zero-state” response to die out. This simulation, using PSPICE, runs in about one second on a 486 type computer.