Advanced Tutorial Lesson 13: Exploring Digital Filters
Contents
 1 What You Will Learn
 2 A Note on RF.Spice's Generic Digital Filter Block
 3 Testing a Basic Delay Element
 4 Building an FIR Filter: The Moving Average Filter
 5 Filtering Noisy Signals Using Moving Average Digital Filters
 6 Building & Testing a Recursive Digital Filter
 7 Examining the Transient Response of an IIR Digital Filter
What You Will Learn
In this tutorial you will learn how to use RF.Spice's Generic Digital Filter Block to define finite impulse response (FIR) and infinite impulse response (IIR) filters. You will also use RF.Spice's Signal Sampler Block to create discretetime versions of continuoustime signals and will learn how to generate noisy waveforms using RF.Spice's Random Pulse Generator.
A Note on RF.Spice's Generic Digital Filter Block
In RF.Spice A/D the generic digital filter block is defined by its Zdomain transfer function, which is a rational function of the Ztransform variable:
[math] H(z) = \frac{N(z)}{D(z)} = \frac{ \sum_{m=0}^{M} b_m z^m }{ \sum_{n=0}^{N} a_n z^n } [/math]
with the assumption that N ≥ M.
You need to specify the highest polynomial degree (N) and enter arrays of polynomial coefficients for the numerator and denominator of the transfer function in the property dialog of the generic digital filter block. This part can be accessed from Menu > Parts > Digital Signal Processing Blocks > Generic Digital Filter Block. To open the property dialog of this device, doubleclick on its symbol and then click the Edit Model... button.
Error creating thumbnail: Unable to save thumbnail to destination 
Error creating thumbnail: Unable to save thumbnail to destination 
For a regular digital filter, you need to insert zero padding among the numerator and denominator polynomial coefficients. 
For example, the coefficient array for a polynomial P(z) = z^{2} + z + 1 must be entered as "1 0 1 0 1". If the degree of the polynomial is N, then you need to enter a total of 2N+1 entries that include N padded zeros. The reason for this is RF.Spice A/D in fact constructs a polynomial in (z^{1/2}) behind the scene. So in reality, you enter the coefficients for the successive powers of (z^{1/2}):
[math] P(z) = z^2 + z + 1 = \sum_{n=0}^{N} a_n z^n = \sum_{k=0}^{2N} a^{\prime}_k (z^{1/2})^k = 1(z^{1/2})^4 + 0(z^{1/2})^3 + 1(z^{1/2})^2 + 0(z^{1/2}) + 1 [/math]
Note that the term z^{1/2} corresponds to a delay equal to half the sampling period.
Testing a Basic Delay Element
The following is a list of parts needed for this part of the tutorial lesson:
Part Name  Part Type  Part Value 

V1  Finite Sequence Pulse Generator  Waveform TBD 
R1  Resistor  100 
X1  Generic Digital Filter Block  Defaults, deg = 1, Numer = "1", Denom = "1 0 0", freq = 1Hz 
Place and connect the part as shown in the figure below:
Error creating thumbnail: Unable to save thumbnail to destination 
In the first part of this tutorial lesson, you will define a digital filter as a basic delay element. The Zdomain transfer function of this filter is given by:
[math]H(z) = z^{1/2} = \frac{1}{z} = \frac {0(z^{1/2})^2 + 0(z^{1/2}) + 1}{1(z^{1/2})^2 + 0(z^{1/2}) + 0} [/math]
This means that N= 1, M = 0, the coefficients of the denominator must be "1 0 0" and the numerator has only one coefficient "1". You don't have to enter the leading zero coefficients in the numerator.
As the source of your circuit, you are going to define five pulse of period 1s with a duty cycle of 20%. For this purpose, you can use a Finite Sequence Pulse Generator, which can be accessed from Parts > Waveform Generation Blocks > Basic Waveforms >. Set the pulse period to 1s, pulse width to 0.2s, n = 5, and set the rise and fall times both to 5ms.
Using pulse waveforms with zero rise or fall times in digital signal processing blocks may cause output overshoots or undershoots. 
Error creating thumbnail: Unable to save thumbnail to destination 
Run a Transient Test of this circuit with the parameters specified below:
Start Time  0 

Stop Time  8s 
Linearize Step  10ms 
Step Ceiling  1ms 
Preset Graph Plots  v(1), v(2) 
The simulation results are shown in the figure below using the graph window's Separate Plots with Vertical Tiling. You can see that the output waveform is simply the same as the delayed version of the input waveform by one clock cycle (T = 1s).
Building an FIR Filter: The Moving Average Filter
The following is a list of parts needed for this part of the tutorial lesson:
Part Name  Part Type  Part Value 

V1  Random Pulse Generator  Waveform TBD 
R1  Resistor  100 
X1  Generic Digital Filter Block  Defaults, deg = 2, Numer = "1 0 1 0 1", Denom = "3 0 0 0 0", freq = 1Hz 
One of the simplest finite impulse response (FIR) digital filters is a moving average filter. A threepoint moving average filter is defined by the following transfer function:
[math]H(z) = \frac{1}{3} \left[ 1 + z^{1} + z^{2} \right] = \frac {z^2 + z + 1}{3z^2} [/math]
This filter sums each data sample with delayed versions of the signal by one and two clock cycles, and divides the sum by 3 to get the average. In other words, the relationship between the output and input signal can be expressed as:
[math] v_o(t) = \frac{1}{3} \left[ v_i(t) + v_i(tT) +v_i(t2T) \right] [/math]
where T = 1/f_{c} is the sampling period and f_{c} is the clock frequency. Therefore, M = N = 2 in the case, and the numerator and denominator coefficient arrays are "1 0 1 0 1" and "3 0 0 0 0", respectively.
Place and connect the part as shown in the above figure from the last part. For the input, this time you are going to use a random pulse generator with the parameters specified in the table below. By default, a random pulse generator create pulses with random amplitudes and random widths. The parameter n_rand determines how many possible values of amplitude or pulse width will be considered. In this project, the pulse width will be fixed at w = 0.2s, and only the pulse amplitude will be randomized. That's why you need to set the value of random_amp to 1 and set the value of random_wid to 0.
period  1s 

duty cycle  0.2 
random_amp  1 
random_wid  0 
n_rand  10 
rise_time  5m 
fall_time  5m 
max_val  1V 
Error creating thumbnail: Unable to save thumbnail to destination 
Run a Transient Test of this circuit with the parameters specified below:
Start Time  0 

Stop Time  100s 
Linearize Step  10m 
Step Ceiling  1m 
Preset Graph Plots  v(1), v(2) 
The simulation results are shown in the figure below for the random pulse input and the filtered output signal:
When working with randomized signals, you should expect your results to look different than the graphs shown in these tutorial lessons. 
Filtering Noisy Signals Using Moving Average Digital Filters
The following is a list of parts needed for this part of the tutorial lesson:
Part Name  Part Type  Part Value 

V1  Sinusoidal Voltage Source  Waveform TBD 
V2  V3  Random Pulse Generator  Waveform TBD 
R1  Resistor  100 
A1  Summer Block  Defaults 
A2  Summer Block  Defaults, in_gain = [1 1], out_gain = 0.15 
X1  Signal Sampler Block  Defaults, T = 1s, duty_cycle = 0.2, rise_time = 5ms, fall_time = 5ms 
X2  Generic Digital Filter Block  Defaults, deg = 4, Numer = "1 0 1 0 1 0 1 0 1", Denom = "5 0 0 0 0 0 0 0 0", freq = 1Hz 
In this part of the tutorial lesson, you will build a noisy digital signal. To do so, you will take a sinusoidal signal, sample it at a clock rate of 1s using RF.Spice's Signal Sampler Block and add a random pulse waveforms with a peaktopeak variation of 0.4V. The figure below shows the property dialog of the signal sampler block:
Error creating thumbnail: Unable to save thumbnail to destination 
In order to generate a noisy signal, you can superpose a scaleddown random pulse with your sampled discretetime signal. However, keep in mind that the output of RF.Spice's random pulse generator fluctutate between 0 and its "max_value". In order to create a noise component fluctuating between positive and negative values, you will use two statistically uncorrelated random pulse generators and sum up their outputs with opposite signs, and scale down (attenuate) the output of the summer. RF.Spice's Summer Block allows you to create a linear combination of the two input signals and also define an output gain as shown in the figure below.
In this circuit you have two different summer blocks A1 and A2 with different properties. For basic summer A2, you will accept all the default parameter values. Since the Summer Block is a native XSPICE process device, by default all of its instances share the same model unless you force a certain part to have a "Unique Model".
For this part of the tutorial lesson, you will define a 5point moving average filter with the following Zdomain transfer function:
[math]H(z) = \frac{1}{5} \left[ 1 + z^{1} + z^{2} + z^{3} + z^{4} \right] = \frac {z^4 + z^3 + z^2 + z + 1}{5z^4} [/math]
In this case, M = N = 4, and the numerator and denominator coefficient arrays are "1 0 1 0 1 0 1 0 1" and "5 0 0 0 0 0 0 0 0", respectively.
Place and connect the part as shown in the above figure from the last part. Define the waveforms of the sinusoidal source V1 and the two random pulse generators V2 and V3 according to the table below:



Place and connect all the parts as shown in the figure below:
Run a Transient Test of this circuit with the parameters specified below:
Start Time  0 

Stop Time  100s 
Linearize Step  10m 
Step Ceiling  1m 
Preset Graph Plots  v(1), v(2), v(3), v(7) 
The simulation results are shown in the figure below. v(7) is the random noise signal with a maximum peaktopeak amplitude of 0.3V before being superposed with the sampled sinusoid. v(1) is the noisy discretetime sinusoidal signal. From the plot of the output signal v(2) in the figure, you can see that the digital filter cleans up and smoothes out the noisy input signal.
Next, open the property dialog of the two random pulse generators V2 and V3 and set their number of random amplitude levels to n_rand = 20. Also, in the property dialog of the summer block A1, set the value of out_gain equal to 0.4. This will increase the peaktopeark noise amplitude to 0.8V superimposed on a sinusoid with a peaktopeak amplitude of 2V. Run another transient test of your system an plots the signal graphs as shown in the figure below. You can clearly see that the input signal to the digital filter has now become much noisier, and the filter is still doing a quite decent job of removing the noise.
Building & Testing a Recursive Digital Filter
The following is a list of parts needed for this part of the tutorial lesson:
Part Name  Part Type  Part Value 

V1  AC Voltage Source  1V 
R1  Resistor  100 
X1  Generic Digital Filter Block  Defaults, deg = 1, Numer = "1", Denom = "1 0 0", freq = 1Hz 
Recursive digital filters, also know as Infinite Impulse Response (IIR) filters, have many applications including the digital or discretetime counterparts of classic continuoustime filters. The Zdomain transfer function of a fifthorder elliptic lowpass digital filter is given by:
[math]H(z) = \frac{ 0.01943z^5 + 0.02111z^4 + 0.03771z^3 + 0.03771z^2 + 0.02111z + 0.01943 }{ z^5  2.7580z^4 + 4.0110z^3  3.3711z^2 + 1.6542z  0.3796 } [/math]
In this case, M = N = 5, and the eleven numerator and denominator array coefficients are given by:
N(z): 0.01943 0 0.02111 0 0.03771 0 0.03771 0 0.02111 0 0.01943
D(z): 1 0 2.7580 0 4.0110 0 3.3711 0 1.6542 0 0.3796
Place and connect the part as shown in the figure below:
Error creating thumbnail: Unable to save thumbnail to destination 
You are primarily interested in the frequency response of this digital filter. Therefore, run an AC frequency sweep of your filter with the following parameters:
Start Frequency  1mHz 

Stop Frequency  2Hz 
Steps/Interval  0.5mHz 
Interval Type  Linear 
Preset Graph Plots  VDB(2) 
The frequency response of the digital filter is shown in the figure below, where you can see a lowpass behavior. Note that the frequency response of digital filters is periodic with a period equal to the sampling period, which is 1Hz in this case.
Examining the Transient Response of an IIR Digital Filter
For the last part of this tutorial lesson, you are going to use the circuit of the previous part. But you will replace the AC voltage source with a Finite Sequence Pulse Generator identical to the one you used in the first part of the lesson. The following are the source's specifications:
pulse period  1s 

pulse width  0.2s 
n  5 
rise_time  5m 
fall_time  5m 
max_val  1V 
Run a Transient Test of this circuit with the parameters specified below:
Start Time  0 

Stop Time  20s 
Linearize Step  10ms 
Step Ceiling  1ms 
Preset Graph Plots  v(1), v(2) 
The simulation results are shown in the figure below. As you can see from the figure, even though your input pulse sequence has a finite duration or 5s, its output has an infinite duration. But is decays very fast.