Create Spice Amplifier Models Using Second-Order Approximations

Spice Netlist

A basic Spice model that simulates an amplifier’s bandwidth, magnitude, phase, and transient response can be up and running in as little as three lines of code. The first line determines the input and output pins, and the second is a second-order transfer function representing the main characteristics of the amplifier. The third contains the .END statement.

Designers can add common circuit blocks such as common-mode rejection ratio (CMRR), power-supply rejection ratio (PSRR), output limiting, and spectral noise to provide as much simulation detail desired. This article offers two examples for developing transfer functions of amplifiers with fixed gains of 10 and 2. The general procedure is:

1. Measure the amplifier pulse response in the lab.
2. Determine the overshoot and settling time from the pulse response.
3. Perform the calculations.
4. Simulate the netlist to verify simulation.
5. Adjust the bandwidth if necessary.

In its standard form, the transfer function represents an amplifier’s frequency and transient response:

where ωn is the natural undamped frequency, ξ is the damping ratio, and S is σ + jω.

Figure 1 shows the pulse response of an amplifier with a gain of 10. No peaking is evident in the pulse response, so we can choose a default value of 1 mV (that is, an overshoot of M = 0.025%). Since:

The damping ratio, ξ, is:

In this example:

Depending on whether the settling time, ts, was measured to within ±2% or ±5% of final value, either of two equations can be used to calculate ωn:

(±5%)

The initial estimate of settling time to within ±2% of the final value was approximately 11 µs. But this estimate fell short on bandwidth, so the estimate was modified to 7 µs to give the correct simulated –3-dB point. A spreadsheet calculator such as the one shown in Table 1 simplifies any adjustments that may be needed. Then:

These values can be plugged into Equation 1, which is multiplied by 10/S for a gain-of-10 amplifier.

So, the final transfer function for the Spice netlist is:

Table 2 presents the resulting Spice netlist for the gain-of-10 amplifier. Figure 2 shows the simulated frequency response.

The second example involves a gain-of-2 amplifier with the pulse response shown in Figure 3. The procedure described in the first example is used to obtain the initial transfer function for simulation. However, a graphical technique offers a better approach for estimating the settling time.

Using the transfer function, run three simulations to obtain three pairs of data for settling time versus bandwidth. Plot the data in Excel and extract a formula. The settling times chosen for simulation were 500 ns, 1 µs, and 2 µs. A power trend-line in Excel displayed the following formula:

Since the desired –3-dB point for this amplifier is approximately 1.44 MHz, ts is approximately 340 ns. This value should be used in the Excel calculation.

Again, insert the resulting values into Equation 1, the transfer function, and multiply the function by 2/S for a gain of 2:

So, the final transfer function for the Spice netlist is:

Table 4 shows the Spice netlist. Figure 4 shows the amplifier’s simulated frequency response. To speed up time domain simulations, replace the variable S with 2π. For example:

E2 4 0 Laplace \{V(1)\} = \{3.165e14/(S^2 + 2.353e7*S + 1.583e14)\}

becomes:

E2 4 0 Laplace \{V(1)\} = \{3.165e14/(6.283^2 + 2.353e7*6.283 + 1.583e14)\}

The third example involves an amplifier with a typical –3-dB bandwidth of 900 kHz that is configured for a gain of five. Using the amplifier’s pulse response (Fig. 5), the designer can determine the peak overshoot and settling time, which can be within either ±2% or ±5% of the final value. In this case, the overshoot, Mp, is approximately 22%, and the settling time, ts, to ±2% of the final value is 2.2 µs.

As before, the next step is to calculate the transfer function. For an overshoot of 22%, the damping ratio is:

Next, determine the natural undamped frequency using the two settling time equations (for ts within ±2% or ±5% of final value) and use the value that provides the best model. A spreadsheet calculator makes it easy to do this. Using the settling time of 2.2 µs provides an ωn of 4.18 × 106 radians per second.

Now, obtain the second-order transfer function from the parameters. The numerator and s0 term equal ωn2, and the s1 term equals 2ξωn = 2 × 0.434 × 4.18 × 106 = 3.636 × 106. Initially, this gives the unity-gain transfer function:

For a gain-of-five amplifier, multiply the transfer function by the step function 5/S to get the final transfer function:

The final transfer function for the Spice netlist is:

Table 5 shows the Spice netlist for the gain-of-five amplifier. Figure 6 shows the amplifier’s simulated frequency response. Peaking, gain, and the –3-dB point were accurate compared to measured responses in the lab.

Existing circuits commonly used for CMRR, PSRR, offset voltage, supply current, spectral noise, input/output limiting, and other parameters can be combined with the second-order model. Figure 7 shows a proposed general template using two cascaded amplifiers.

If no Spice model exists for a specific part, a second-order approximation can produce a model that simulates bandwidth, magnitude, phase, and transient response in as little as three lines of code. For further troubleshooting and analysis such as pole location, step response, and bode plots, the transfer function can be easily examined with math software. Additional circuit blocks can be added to provide as much simulation detail as desired.