Chapter 11

 

Filters and Tuned Amplifiers

 

 

 

In this chapter we shall use Spice and PSpice to investigate the frequency response of various types of active-RC filter circuits and an LC tuned amplifier. We shall also demonstrate how Spice (PSpice) can be used in the process of fine-tuning a design. This process is known as computer-aided design.

 

11.1 The Butterworth And Chebyshev Transfer Functions

 

Two filter functions commonly used to approximate low-pass transmission characteristics are the Butterworth and Chebyshev transfer functions.  In Chapter 7 of this text we demonstrated how PSpice can be used to compute the frequency response of an arbitrary transfer function by specifying the gain of a dependent source as a Laplace Transform function.  Adopting a similar approach, in the following we shall verify that the two filter functions calculated in Examples 11.1 and 11.2 of Sedra and Smith, 3^rd Edition, do indeed meet the required specifications.

 

The following 9th-order Butterworth transfer function,

 

 

was calculated by Sedra and Smith in Example 11.1 so that it's magnitude response would satisfy the following filter specifications:  f_p=10 kHz, A_max=1 dB, f_s=15 kHz, A_min=25 dB and dc gain = 1.  An important constraint imposed by PSpice when specifying the gain of a dependent source as a Laplace transform expression, as demonstrated in section 7.1, is that the expression must fit on a single line in the PSpice input file (i.e., limited to 131 characters).  The transfer function specified in Eqn. (11.1} is very long and it could not be specified on a single line.

 

 

 

 

To get around this problem, we simply break-up the transfer function into several first and second-order transfer functions and assign each one as the gain of a separate VCVS. The resulting set of VCVSs are then connected in cascade as shown in Fig. 11.1.  The input file describing this circuit arrangement to PSpice is listed in Fig. 11.2. Here we are requesting that the transfer function be evaluated linearly over the frequency interval beginning at 1 Hz and ending at 20 kHz with 100 points collected.

 

On completion of Spice, the magnitude response of the 9th-order Butterworth transfer function is shown in Fig. 11.3.  The top graph displays an expanded view of the passband region and the bottom graph displays a view of both the passband and stopband regions. On review of these results we see that at f=f_p=10 kHz the gain is 1 dB below the dc value (and is monotonically decreasing). At f=f_s=15 kHz we find that the gain is about 25 dB below the dc value (more precisely, using Probe we find at this frequency the gain is -25.8 dB). Thus, we can conclude that the transfer function of Eqn. 11.1) meets the required specifications.

 

Repeating the above analysis for the following 5th-order Chebyshev transfer function given in Example 11.2 of Sedra and Smith,

 

 

we would like to verify that the magnitude of this transfer function meets the same specifications as did the above 9th-order Butterworth transfer function.

 

Adopting the same approach as for the above Butterworth transfer function, we can describe Chebyshev transfer function to PSpice with the input file shown listed in Fig. 11.4. Submitting this to PSpice results in the plot of the magnitude response shown in Fig. 11.5. Both an expanded view of the passband and a broader view of both the passband and stopband regions are shown. On inspection of these results, we see that the gain in the passband region (0 Hz to 10 kHz) oscillates between 0 and -1 dB. For frequencies above 10 kHz, we see that the gain rolls off monotonically with increasing frequency. At the stopband edge of f=f_s=15 kHz, we see from the lower graph in Fig. 11.4 that the gain is -40 dB. Therefore, we can conclude that the lower-order Chebyshev filter function given by Eqn. (11.2) satisfies the same specifications as the higher-order Butterworth filter function described by Eqn. 11.1).

 

 

 

11.2 Second-Order Active Filters Based on Inductor Replacement

 

In Fig. 11.6 we display a circuit consisting of a cascade of two second order simulated-LCR resonator circuits and a single first-order op amp RC circuit. The components of this circuit were selected such that it realizes the 5th-order Chebyshev function given in Eqn. (11.2). Using Spice we would like to verify this by comparing the magnitude response of this circuit with that computed directly from its transfer function as calculated above and shown in Fig. 11.5. We shall assume that the op amps are quasi-ideal and modeled after a VCVS with a gain of 10⁶ V/V as shown in part (b) of Fig. 11.6. This step would normally be the first step after the circuit has been designed and one wants to verify that the synthesis procedure was correct.

 

 

 

 

 

 

The Spice input file describing this circuit is shown listed in Fig. 11.7. Since the same type of op amp is repeated many times in this circuit, we have chosen to represent this quasi-ideal op amp with a single subcircuit named ideal_opamp. A detailed discussion of subcircuits was presented in Chapter 2 and will not be repeated here.  An AC analysis is requested over the linear frequency interval beginning at 1 Hz and ending at 20 kHz. One-hundred points are to be computed. The input to the filter is driven by a 1 V AC signal.

 

Submitting the Spice input file listed in Fig. 11.7 to Spice, results in the magnitude response shown plotted in Fig. 11.8. Both an expanded view of the passband and a view of the passband and stopband regions are shown. When one compares these results with those computed directly from the transfer function given in Eqn. (11.2) above in Fig. 11.5 we see that they are, for all practical purposes, identical. Thus, we can conclude that we carried out the synthesis procedure correctly.  The next step would be to investigate how the filter magnitude response is affected by the frequency characteristics of a real op amp. This we shall do in the next section on a Tow-Thomas biquad circuit.

 

 

 

11.3 Second-Order Active Filters Based on the Two-Integrator-Loop Topology

 

Another important class of biquadratic active-RC filter circuits are those that are formed by cascading two integrators in an overall feedback loop. In Fig. 11.9 we show the Tow-Thomas biquad based on this idea.  The components were selected such that this circuit realized a second-order bandpass filter with f_o=10 kHz, Q=20 and unity center-frequency gain. Using Spice we would like to investigate the frequency response of this filter circuit assuming that each op amp is of the 741-type and compare it to its ideal frequency response (i.e., one with ideal op amps).

 

One possible approach for evaluating the nonideal frequency response behavior of the bandpass filter shown in Fig. 11.9 is to describe the entire circuit to Spice including a detailed description of the 741 op amp at the transistor level. This would certainly lead to the most accurate representation of the bandpass filter circuit; however, it would require large amounts of computer time and storage to compute the frequency response.  A more reasonable approach, and the one we will undertake here, is to utilize a macromodel of the 741 op amp.

 

To be more specific, we shall model the terminal behavior of the 741 op amp with the single-time constant linear network shown in Fig. 11.10. Other time-constants can also be included in this model by simple extension of the middle stage. One may also be tempted to add nonlinearities into this model; however, Spice linearizes a circuit about its operating point prior to the start of the AC analysis. Hence, the inclusion of any op amp nonlinearity in AC analysis serves no purpose and is ignored by Spice. Nonlinearities can, of course, be included in the model when performing transient analysis.  It is a simple matter to derive the open-circuit transfer function of the equivalent op amp circuit shown in Fig. 11.10 and determine that it has a one-pole response given

(11.3)

The 741 op amp is an internally-compensated op amp which has a frequency response characterized by a one-pole frequency roll-off,

      (11.4)

 

where A_o denotes the DC gain and w_b is the 3-dB frequency. Nominally, the 741 op amp has a DC gain of 2.52 x 10⁵ V/V and a 3 dB frequency of 4 Hz. Comparing the above two equations, we can write two equations in three unknowns. That is, A_o=G_mR₁ and w_b = 1/R₁C₁. Assigning C₁=30 pF, we can solve for G_m=0.19 mA/V and R₁=1.323 x 10⁹. We can also add some input and output resistances to account for the effects of loading. Here we shall choose R_id=2 MOhm, R_icm=500 MOhm and R_o=75 Ohm.

 

The Spice input file describing the Tow-Thomas biquad circuit of Fig. 11.9 is shown listed in Fig. 11.11. The op amp macromodel shown in Fig. 11.10 representing the small-signal nominal frequency response behavior of the 741 op amp is described by the subcircuit nonideal_opamp also included in this Spice listing. A 1 V AC signal is applied to the input of the filter; thus, the output voltage of the filter will also represent the filter transfer function.  The frequency response of the filter is computed between 8 kHz and 12 kHz using 100 points linearly separated from one another. We shall also concatenate another Spice deck on the end of this one with the nonideal subcircuit replaced with one containing a model of an ideal op amp, such as the one used in the previous example shown listed in Fig.  11.7, thus generating the ``ideal’’ frequency response.

 

The results of the two circuit simulations, one assuming ideal op amps and another with op amps modeled after the 741-type, are shown collectively in Fig. 11.12. On comparison of their magnitude responses, we see that there are significant differences between them. In fact, we see that the center frequency of the circuit using the 741 op amp has shifted to the left by about 100 Hz and it's 3 dB bandwidth has decreased from 500 Hz to approximately 110 Hz. This, in effect, is an increase in the intended filter Q of 20 up to 90.  In addition, the center frequency gain has also increased from 0 dB to 14 dB.

 

The above results serve to illustrate the adverse effects that actual op amps such as the 741-type have on the frequency response of a Tow-Thomas filter circuit. One possible approach for minimizing these effects is to add into the circuit what is known as a compensation capacitor. There are several ways in which to include the compensation capacitor in the circuit. Here we shall consider adding the compensation capacitor across resistor R₂ in the circuit of Fig. 11.9.  The actual value of the capacitor is not known at this time, so instead we shall search for the value of capacitance that improves the filter overall response. That is, we shall determine the value of capacitance that will make the magnitude response of the filter approach most closely to the desired or ideal response.  To do this, we shall begin with a capacitance value of 20 pF and simulate the magnitude response of the filter. We shall compare this result to the ideal magnitude response and determine whether the added capacitance improves the filter response. If it does, we shall continue increasing the value of this capacitance until we no longer improve the filter response.  Here we are utilizing Spice in the process of computer-aided design and not just analysis.

 

To demonstrate this design process, we have plotted in Fig. 11.13 the magnitude response that results from varying the value of the compensation capacitor from 0 pF to 80 pF in 20 pF increments. We see from these results that as the compensation capacitance increases from 0 pF, both the filter Q and the resonant peak of the filter response tend more closely towards the desired response. However, once the value of the compensation capacitor exceeds 60 pF, we begin to deviate away from the desired response. This suggests that the best result lies between 60 pF and 80 pF. More refinement of the same approach between these two values identifies that the best results occur when the compensation capacitor is set at 64 pF.

 

In Fig. 11.14 we compare the filter magnitude response with a compensation capacitor of 64 pF against the ideal response.  As is evident, the actual filter magnitude response has about the same filter $Q$ and similar center frequency gain as the ideal response but have slightly different center frequencies. We can conclude from this computer-aided design process that much of the nonideal effects caused by the limited bandwidth of the 741 op amp has been eliminated by the addition of this single compensation capacitor.  Finally, we should note that a closed form expression [Sedra and Brackett, 1978] exits for determining the required value of the compensation capacitor. This expression, however, relies on knowledge of the value of the op amp f_t. In practical situations, one would not know the exact value of f_t and the appropriate value of the compensation capacitance could be found by using a variable capacitor, in much the same way as done above with Spice.

 

 

 

 

 

 

 

11.4 Single-Amplifier Biquadratic Active Filters

 

Another important class of second-order filter circuits are the single-amplifier biquads or SABs. In Fig. 11.15 we display a filter circuit of the Sallen-and-Key type intended to realize a highpass filter function with f_o=10 kHz and Q=4. The op amp will be assumed to be of the 741 type - identical to the situation created in the previous problem. Using Spice we would like to calculate the magnitude response of this circuit over a frequency interval beginning at 1 kHz and ending at 10 MHz and compare it to the response of the same circuit when implemented with an ideal op amp.  A logarithmic frequency sweep of ten points per decade will be chosen to be calculated.

 

The Spice input file describing the Sallen-and-Key filter circuit shown in Fig. 11.15 implemented with a 741 op amp is shown listed in Fig. 11.16. An identical Spice listing is also appended at the end of this file with the nonideal op amp subcircuit replaced by an ideal op amp subcircuit. This will enable us to compare the frequency response of a real circuit implementation with the ideal response.

 

The results of the two simulations are shown plotted in Fig. 11.17. For frequencies less than 100 kHz, the two curves shown are very similar. Above this frequency, the magnitude response of the circuit implemented with a 741 op amp is beginning to deviate significantly from the ideal response. One might also be tempted to add that it appears more like a bandpass filter function than a highpass, with the exception that the magnitude response appears to be leveling off at about -11 dB. These results serve to illustrate the difficulty of realizing a highpass filter function using op amps that have an inherent lowpass frequency characteristic.

 

 

 

11.6 Tuned Amplifiers

 

In Fig. 11.18 we show a special kind of frequency selective network called the LC-tuned amplifier.  Loading the drain of a typical resistor-biased transistor circuit with an LC tank circuit results in an amplifier with a highly selective amplitude response. This class of circuit finds extensive application in high-frequency communications systems such as radio. The tuned circuit portion of this amplifier was designed in Example 11.4 of Sedra and Smith such that this amplifier has a center-frequency of 1 MHz, a 3-dB frequency of 10 kHz and a center-frequency gain of -10 V/V.

 

The resistor biasing network was added to bias transistor M₁ at g_m=5 mA/V and r_o=10 k-Ohm, much like that assumed by Sedra and Smith in their example. MOSFET M₁ is assumed to be 10 um long and 1250 um wide. It also has the following device parameters:  u_nC_ox=100 uA/V², V_T=+2 V and lambda=0.1 V^-1.  Using Spice, we would like to calculate the magnitude response of this circuit and compare it to what we are expecting.

 

The Spice input file describing this circuit is seen listed in Fig. 11.19. The input is driven by a 1 V AC signal and two types of analysis are requested. The first is simply an operating point calculation (.OP) which we shall use to compute the bias point of the MOSFET. These results will be used to determine whether the MOSFET has been biased correctly. Secondly, an AC command is specified to compute the frequency response of this amplifier in a frequency range beginning at 0.99 MHz and ending at 1.01 MHz with 100 points computed in a linear fashion between the two frequency end points.

 

Submitting the Spice input deck shown listed in Fig. 11.19 and collecting the results, we obtained the magnitude response of the tuned amplifier as shown in Fig. 11.20. Here we see that the center frequency of the magnitude response is almost exactly at the intended design value of 1 MHz. However, both the gain of the amplifier at its center frequency of 15.86 V/V and its 3-dB bandwidth of 9.01 kHz do not agree with their design values. To account for these differences, one only has to review the small-signal model for the MOSFET calculated by Spice through the .OP command, seen listed below:

 

 

Here we see that both the g_m and r_o (or 1/GDS) of the transistor has deviated from our initial design of 1 mA/V and 10 k-Ohm, respectively.  Since, both the center frequency gain and 3 dB bandwidth of the tuned amplifier shown in Fig. 11.18 are functions of these two parameters (see Sedra and Smith) we would also expect them to deviate from the intended design values. To obtain better estimates of the center frequency gain and the 3-dB bandwidth, we can use the actual bias data generated by Spice. For instance, the equivalent resistance seen at the drain of M₁ is R = r_o||R_L = (1/5.27 x 10^-5)||(2.5 x 10³) = 2.208 k-Ohm. Thus, the magnitude of the center frequency gain is g_m R = 7.18 m x 2.208 k = 15.85 V/V. Likewise, the 3 dB bandwidth is B=1/RC= 1/(2.208 k x 7.958 n) or 9.057 kHz. Both these values are now much closer to what we obtained through simulation.

 

To demonstrate another example of a computer-aided design, let us consider adjusting the value of the load resistor R_L in the tuned amplifier shown in Fig, 11.18 such that the required 10 kHz bandwidth is achieved.

 

To make matters more realistic, we shall account for the MOSFET parasitic capacitances by including the following model statement for the device:

    

 

The dc parameters of this MOSFET are identical to those used previously. The 1 k-Ohm source resistance will also be included in order to properly account for the effect of these capacitances on the overall circuit behavior. The Spice deck for this example is quite similar to that seen in Fig. 11.19 and is therefore not shown here.

 

To begin this computer-aided design process, we shall first determine the 3-dB bandwidth of this tuned amplifier with the MOSFET parasitic capacitances present and the load resistance set at its nominal value of 2.5 k-Ohm. This requires that we re-submit the revised Spice job for analysis and plot the magnitude response of this circuit. On doing so, we find that the 3-dB bandwidth is 9.06 kHz. In order to increase the bandwidth of this tuned amplifier to 10 kHz, we must decrease the value of the load resistance.  How much we should decrease R_L is not known at this time; instead we shall perform a search using Spice. Beginning with R_L equal to 2.45 k-Ohm, we shall compute the 3-dB bandwidth and then repeat the same process while incrementally decreasing the value of R_L by, say, 50 Ohm until we reach, say, 2.0 k-Ohm. Hopefully, we shall find that the amplifier 3 dB bandwidth has increased to 10 kHz, or more, with the range of load resistance that we selected above. If not, then we must continue the search process with values of R_L less than 2 k-Ohm.

 

In Fig. 11.21 we present an expanded view of the magnitude response of the tuned amplifier for the various load resistances. Although it is not directly evident, with the cursor facility of Probe, we were able to determine the 3-dB bandwidth in each case. We found that for a load resistance of 2.20 k-Ohm the 3-dB bandwidth was slightly greater than 10 kHz (actually, 10.1 kHz). For a load resistance of 2.25 k-Ohm, we found that the 3-dB bandwidth is 9.966 kHz. We can therefore conclude that a 10 kHz bandwidth for this amplifier will occur with a load resistance somewhere between 2.20 k-Ohm and 2.25 k-Ohm. Using a more refined increment for the load resistance, we can repeat the same process stated above with the load resistance varied between 2.20 k-Ohm and 2.25 k-Ohm with a 10 Ohm increment. On doing so, we find that the tuned amplifier will have a 10 kHz bandwidth when the load resistance is 2.24 k-Ohm.  Any more refinement would probably not be worth the extra effort given that the resistor cannot be specified any more accurately.

 

11.7 Spice Tips

 

·      The element statement of a dependent source having a gain expressed in terms of a Laplace transform function cannot be longer than 131 characters in length.

 

·      The small-signal frequency response behavior of the 741 op amp can be modeled in Spice with a very simple macromodel. This macromodel consists of a single-time-constant linear network that represents the dominant pole behavior of the op amp.

 

·      Spice is not only useful for analyzing a design, it is also useful for fine tuning a design.

 

11.8 Bibliography

 

A. S. Sedra and P. O. Brackett, Filter Theory and Design: Active and Passive, Portland, Ore.: Matrix, 1978.

 

11.9 Problems

 

11.1.      A third order lowpass filter has transmission zeros at w = 2 rad/s and w = ¥. Its natural modes are at s=-1 and s=-0.5 ± j 0.8. The dc gain is unity. With the aid of PSpice, plot the magnitude and phase of the transfer function for this filter.

 

11.2.      With the aid of PSpice, prepare a plot of both the magnitude and phase of the following filter transfer functions capturing the most important frequency information:

 

(a)  

 

(b)   

 

(c).  

 

(d)   

 

(e)   

 

   

11.3.      Analyze the RLC network of Fig. P11.3 using Spice to determine the nature of its transfer function over the frequency range between 0.001 Hz and 10 Hz. Shunt the 2 H inductor with a 0.1 F capacitor.  Observe the modified frequency response.

Fig. P11.3

 

11.4.      Design a Butterworth filter that meets the following lowpass specifications: f_p=10 kHz, A_max=2 dB, f_s=15 kHz, and A_min=15 dB. Use PSpice to confirm your design by plotting the magnitude of your transfer function.

 

11.5.      Contrast the attenuation provided by a fifth-order Chebyshev filter at w_s=2w_p to that provided by a Butterworth filter of equal order. For both, A_max=1 dB. Plot |T(s)| for both filters on the same axes using PSpice.

Fig. P11.6

 

11.6.      Design the above lowpass op amp circuit in Fig. P11.6 to have a 3-dB frequency of 10 kHz, a dc gain of magnitude 10 and an input resistance of 10 k-Ohm. Verify your design using Spice. Assume a high-gain VCVS representation for the ideal op amp.

 

11.7.      For the lowpass op amp circuit designed in the above problem, consider applying a 1 kHz sinewave of 1 V amplitude to its input and observe its output steady-state time-response using Spice. Repeat for an input signal of the same amplitude but of a much higher frequency of 100 kHz. Now, combine these two sine-wave signals by connecting two voltage sources in series and apply it to the input of the filter. Compare the voltage signal appearing at the input to the filter with that appearing at the output. Comment on your results.

 

11.8.      For the lowpass op amp circuit designed in Problem 11.7 above, consider applying a 1 V step to its input and observe its output step response using Spice.

Fig. P11.9

 

11.9.      Design the highpass op amp circuit shown in Fig. P11.9 to have a 3-dB frequency of 100 kHz, a high-frequency input resistance of 100 k-Ohm and a high-frequency gain magnitude of unity. Verify your design using Spice by plotting the magnitude response of the filter as a function of frequency.  Assume a high-gain VCVS representation for the ideal op amp.

 

11.10.   For the highpass op-amp circuit designed in the above problem, consider applying a 1 MHz sinewave of 1 V amplitude to its input and observe its output steady-state time-response using Spice. Repeat for an input signal of the same amplitude but of much lower frequency at 10 kHz. Now, combine these two sine-wave signals by connecting two voltage sources in series and apply it to the input of the filter. Compare the voltage signal appearing at the input to the filter with that appearing at the output. Comment on your results.

 

11.11.   For the highpass op amp circuit designed in Problem 11.10 above, consider applying a 1 V step to its input and observe its output step response using Spice.

 

11.12.   For the first-order op amp circuit shown in Fig. P11.12, select the value of its components such that a transmission zero is formed at a frequency of 1 kHz, a pole at a frequency of 100 kHz, and has a dc gain magnitude of unity. The low-frequency input resistance is to be 1 k-Ohm. Plot the magnitude of the transfer function of the circuit that results using Spice.

 

11.13.   By cascading a first-order op amp-RC lowpass circuit with a first-order op amp-RC highpass circuit one can design a wideband bandpass filter. Provide such a design for the case the midband gain is 12 dB and the 3-dB bandwidth extends from 100 Hz to 10 kHz. Select appropriate component values under the constraint that no resistors higher than 100 k-Ohm are to be used, and the input resistance is to be as high as possible.  Verify your design by simulating the magnitude response of your circuit as a function of frequency.

Fig. P11.12

 

11.14.   Use two first-order op amp-RC all-pass circuits in cascade to design a circuit that provides a set of three-phase 60 Hz voltages, each separated by 120° and equal in magnitude. Use 1 uF capacitors. Verify your design by simulating the steady-state time-response of your circuit subject to a 1 Vrms 60 Hz sine-wave signal apply to its input. Plot your results using Spice.

 

11.15.   Verify using Spice the design of a lowpass LCR resonator circuit that has natural modes with w_o=10⁴ rad/sec and Q=1/Ö2. Utilize C=1 uF.

Fig. P11.16

 

11.16.   The circuit of Fig. P11.16 has been designed to realize an allpass transfer function that provides a phase shift of 180° at 1 kHz and to have a Q=1. Verify using Spice that this is indeed the case.

 

11.17.   It is required to design a fifth-order Butterworth filter having a 3-dB bandwidth of 10⁴ rad/s and a unity dc gain. Use a cascade of two second-order simulated-LCR resonator circuits and a single first-order op amp RC circuit. Verify your design using Spice.

Fig. P11.18

 

11.18.   The KHN circuit shown in Fig. P11.18 is used to realize a pair of complex poles located at w=10⁴ rad/s and Q=2. With the aid of Spice, analyze the circuit to determine the transfer functions V₁/V_i, V₂/V_i and V₃/V_i. Classify each as either lowpass, bandpass, bandstop, etc.

 

11.19.   For the KHN circuit shown in Fig. P11.18, compare the magnitude response |V₂/V_i(jw)| between 1 Hz and 10 MHz for op amp dc gain A_o of 10⁶, 10⁴ and 10².

Fig. P11.20

 

11.20.   The filter circuit shown in Fig. P11.20 is a generalization of the Tow-Thomas biquad and commonly referred to as the ``universal filter.’’ The components of this filter circuit were chosen to realize a pair of complex poles described by w_o=10 kHz and Q=5, and a pair of transmission zeros, forming either a lowpass notch or highpass notch filter transfer function depending on which switch is closed. Using Spice, plot the magnitude of the output voltage for different switch positions. At what frequencies are the transmission zeros located at?  Apply a 1 V AC signal to the input of the filter so that the output voltage represents the transfer function of the filter circuit.  Also, assume that the op amps are almost ideal with a dc gain of 10⁶.

Fig. P11.21

 

11.21.   The circuit of Fig. P11.21 has been designed to realize a lowpass notch filter with w_o=10³ rad/s, Q=10, dc gain = 1, and w_n=1.2 x 10⁴. Verify that this is indeed the case with Spice assuming that the op amps are almost ideal with a frequency independent voltage gain of 10⁶ V/V.

 

11.22.   Repeat Problem 11.21 above, but this time model each op amp after the small-signal frequency characteristics of the 741 op amp. Compare your results to those found previously in Problem 11.21.

 

11.23.   Consider applying an input signal consisting of two 1 V peak sinewaves of 100 and 1909.86 Hz to the input of the notch filter shown in Fig. P11.21. Compare the voltage waveform appearing at the input of the filter with the voltage waveform appearing at its output.

 

11.24.   Using Spice, plot the magnitude response |V₂/V_i| of the KHN filter circuit shown in Fig. P11.18 assuming that each op amp has a unity-gain bandwidth of 10 MHz and a dc gain of 10⁶ V/V. Compare these results to the ideal response (i.e., ideal op amp case).

 

11.25.   With the aid of Spice, compare the ideal or desired magnitude response of the 5th-order Chebyshev filter circuit shown in Fig. 11.6 with the magnitude response obtained when each op amp has a unity-gain bandwidth of 10⁶ Hz.

 

11.26.   Assuming that the resistors and capacitors used to realize the bandpass filter circuit in Fig. 11.9 have ±5% tolerances associated with them, select an arbitrary set of resistors and capacitors that lie within this tolerance, but are not the nominal value shown in the circuit schematic. Subsequently, with the aid of Spice, calculate the magnitude response |V_o/V_i| of the modified filter circuit as a function of frequency.  How does this frequency response compare to the nominal frequency response?  Assume a high-gain VCVS representation for each op amp.  (Some versions of Spice, such as PSpice, have a special analysis command called the Monte Carlo Analysis which allow the user to repeat this process of randomly selecting sets of component values according to a predefined distribution.  Different analysis can then be compared and provide a useful sense of operation under normal manufacturing conditions).

 

11.27.   In the example of section 11.3, the Tow-Thomas bandpass filter circuit shown in Fig. 11.9 was analyzed using Spice assuming that the op amps had a single-pole frequency response with unity-gain bandwidth of 1 MHz and found to deviate significantly from the ideal case. Consider compensating for the effect of op amp finite bandwidth by adding a capacitor of value 4C(w_o/w_t) = 63.6 pF across resistor R₂ and re-analyzing the frequency response of the filter. How does the magnitude response compare with the ideal behavior? Is it better?

 

11.28.   The magnitude response of the filter circuit shown in Fig. 11.9 deviates significantly from the desired or ideal frequency response, as demonstrated in section 11.3. One method used to decrease the deviation from the ideal response is to re-connect the noninverting input terminal of the op amp A₃ from ground to the inverting input terminal of op amp A₂. Using Spice, simulate this situation and compare the bandpass magnitude response of this modified filter circuit with its ideal response assuming that the op amps have a unity-gain bandwidth of 1 MHz.

 

11.29.   For the highpass SAB circuit shown in Fig. 11.15, consider changing the resistors into capacitors and multiplying their value by a factor of 10¹². Likewise, change the capacitors into resistors and multiply their value by 1/10¹². Plot the magnitude of the filter transfer function.  What type of filter function results?

 

11.30.   Design a fifth-order Butterworth lowpass filter with a 3-dB bandwidth of 5 kHz and a dc gain of unity using the cascade connection of two Sallen-and-Key circuits and a first-order section. Use a 10 k-Ohm value for all resistors. Verify your design using Spice.

 

11.31.   To estimate the sensitivities of the bandpass SAB circuit shown in Fig.  P11.31, consider varying, separately, each component of the circuit by +1% of its nominal value, and with the aid of Spice, compute the modified magnitude response of the filter transfer function. Then, using these results, together with the nominal magnitude response of the filter, calculate an estimate of the filter sensitivity as a function of frequency according to the formula:

 

11.32.   Simulate the operation of the switched-capacitor integrator circuit shown in Fig. P11.32 and observe the voltage appearing at the output of the op amp for at least 10 us. Initialize the feedback capacitor to 0 V.  Model the op amp to have a unity-gain bandwidth of 10⁶ Hz.

Fig. P11.31

 

Fig. P11.32

 

11.33.   A bandpass amplifier is shown in Fig. 11.18. Design the amplifier to produce a center frequency of 5 MHz with a 3-dB bandwidth of 50 kHz. What is the center frequency gain?  Verify your design using Spice. Assume that the MOSFET has Spice parameters: V_to=1 V, k_p=50 uA/V² and lambda=0.05 V^-1.

Fig. P11.34

 

11.34.   A bandpass amplifier is shown in Fig. P11.34 whose output is coupled to the load resistor of 10 k-Ohm through a transformer. The transformer consists of a primary and secondary inductor, L_p=100 uH and L_s=10 uH, respectively, which have a coupling coefficient of 0.8. To specify this coupling, the following Spice statement is included in the Spice input file together with the two inductor statements: K1 Lp Ls 0.8.  Using Spice determine the frequency response of this amplifier. What is the center frequency and bandwidth of this amplifier?  Assume that the BJTs have model parameters I_S=10^-16 A, b_F=100 and V_A=75 V.