10.1.1 Output Variable

You need to specify a node voltage or an independent current or voltage source. In this example, the output variable is V(out).

10.1.2 Number of Runs

This is the number of times the AC, DC or transient analysis is run. The maximum number of waveforms that can be displayed in Probe is 400. However, for printed results, the maximum number of runs has now been increased from 2000 to 10,000. The first run is the nominal run where no tolerances are applied.

10.1.3 Use Distribution

The model parameter deviations from the nominal values up to the tolerance limits are determined by a probability distribution curve. By default, the distribution curve is uniform; that is, each value has an equal chance of being used. The other option is the Gaussian distribution, which is the familiar bell-shaped curve commonly used in manufacturing. Component values are more likely to take on values found near the center of the distribution compared to the outer edges of the tolerance limits.

You can also define your own probability distribution curves using coordinate pairs specifying the deviation and associated probability, where the deviation is in the range − 1 to + 1 and the probability is in the range from 0 to 1. More information can be found in the PSpice A/D Reference Guide in < install dir > docpspcrefpspcref.pdf.

10.1.4 Random Number Seed

As with most random number generators, an initial seed value is required to generate a set of random numbers. This value must be an odd integer number from 1 to 32,767. If no seed number is specified, the default value of 17,533 is used.

10.1.5 Save Data From

This allows you to save data from selected runs. For example, if you just want to see the circuit response from the nominal run, select none. If you want to save all the runs, select All. If you want to select every third run from the nominal run, i.e. the fourth, seventh, tenth, etc., select Every, then enter 3 in the runs box. If you want to save data from the first three runs, select First and then enter 3 in the runs box. If you want to save data from the third, fifth, seventh and tenth run, select Runs (list) and enter 3, 5, 7, 10 in the runs box. Saved runs will be displayed in Probe.

10.1.6 MC Load/Save

PSpice now has history support which allows you to save randomly generated model parameters or component values from a Monte Carlo run in a file, which can be used for subsequent analysis.

10.1.7 More Settings

This option allows you to specify Collating Functions which are applied to the output waveforms returning a single resulting value. For example, the MAX function searches for and returns the maximum value of a waveform. The YMAX function returns the value corresponding to the greatest difference between the nominal run waveform and the current waveform. The RISE and FALL functions search for the first occurrence of a waveform crossing above or below a set threshold value. For each function, you can specify the range over which you want to apply these functions. Fig. 10.3 shows the available collating functions.

The collating functions are summarized as:

YMAX: Find the greatest difference from the nominal run

MAX: Find the maximum value

MIN: Find the minimum value

RISE_EDGE: Find the first rising threshold crossing

FALL_EDGE: Find the first falling threshold crossing

Fig. 10.4 shows a Sallen and Key 1500 Hz band pass filter circuit. Tolerances will be added to the resistors and capacitors and a Monte Carlo analysis will be performed to predict the statistical variation of the band pass frequency.

1. Draw the circuit in Fig. 10.4. If you are using the demo CD, use the ua741 opamps, which can be found in the eval library; otherwise, the LF411 opamp can be found in the opamp library. Performing a Part Search will result in the LF411 opamp being sourced from different manufacturers. It does not matter which one you use. V1 is a V_AC source from the source library, used for an AC analysis, and the power symbols are VCC_CIRCLE symbols from Place > Power, renamed + 12 V and − 12 V, respectively.

2. You need to add a 5% tolerance to all the resistors. Hold down the control key and select the resistors R1, R2 and R3, then rmb > Edit Properties. In the Property Editor highlight the entire Tolerance Row (or column) as shown in Fig. 10.5 and rmb > Edit. In the Edit Property Values box (Fig. 10.6), type in 5% and click on OK.

3. To display the component tolerances on the schematic, select the entire TOLERANCE row as in Fig. 10.5, rmb > Display and in Display Properties (Fig. 10.7), select Value Only and click on OK.

4. Repeat Step 2 by assigning a 10% tolerance to capacitors C1 and C2.

5. Create a PSpice simulation profile called AC Sweep for an AC logarithmic sweep from 100 to 10 kHz with 50 points per decade (Fig. 10.8). Select Monte Carlo/Worst Case in the Options box.
The output variable is V(out) and the number of runs is 50. The distribution used will be uniform and you will use the default random seed setting by leaving the Random number seed box empty. Your Monte Carlo simulation settings should be as shown in Fig. 10.9.

6. Place a dB voltage marker on node out (PSpice > Markers > Advanced > dB Magnitude of Voltage) and run the simulation.

7. When PSpice launches, a list of available runs is shown (Fig. 10.10). Select All and click on OK.

8. Fig. 10.11 shows the band pass filter response showing a spread in the center frequency. Open the output file, View > Output File{ XE “Output File” } and scroll down to see the results for each Monte Carlo run. At the bottom of the file, you will see a summary of the statistical results and the deviation from the nominal for each run.

However, to get a better picture of the spread of the center frequency, you can use a Performance Analysis to display histograms representing the statistically generated data. Performance analysis will be covered in more detail in Chapter 12, but for now, the steps required for a performance analysis for the bandpass filter are introduced in Exercise 2.

Exercise 2

1. In Probe, from the top toolbar, select Trace > Performance Analysis. At the bottom of the Performance Analysis window, click on Wizard, then in the next window click on Next. You will be presented with a list of measurements as shown in Fig. 10.12.

2. Select the CenterFrequency measurement and click on Next.

3. In the Measurement Expression window (Fig. 10.13), enter the name of the trace to search as V(out). Alternatively, you can click on the Name of trace to search icon and search for the trace name, V(out).

Enter a value of 3 for the db level down for measurement as shown. The center frequency of the filter will be measured 3 dB down either side of the maximum value for the Monte Carlo nominal run (no component tolerances applied). Click on Next in the Performance Analysis Wizard.

4. The nominal trace waveform of the band pass circuit will be displayed (Fig. 10.14). This is the simulation response using the component nominal values. The trace shows two points where the measurements from the waveform will be taken. In this case, the center frequency is defined at 3 dB down from the maximum value. This is shown so that you can confirm whether you are seeing the correct circuit response and that the measurements are taken at the correct points on the waveform.

5. Click on Next in the Performance Analysis Wizard.

6. Histograms will now be displayed (Fig. 10.15) representing the generated statistical data together with a summary of statistical data.

7. Change the resistor tolerances to 1% and the capacitor tolerances to 5% and re-run the simulation. Run a performance analysis as before using the center frequency measurement as above. The results are shown in Fig. 10.16.

8. Run another Performance analysis but this time, use the bandwidth measurement.

Filter Specifications

The gain of the filter is given by:

$\begin{array}{l}\mid G\mid =\frac{\mathrm{R}3}{2\mathrm{R}1}\hfill \\ \mid G\mid =\frac{150\times {10}^3}{2\times 1.5\times {10}^3}=50\hfill \end{array}$

or in dB:

${\left|G\right|}_{\mathrm{dB}}=20{log}_{10}50=34\mathrm{dB}$

The band pass center frequency is given by:

$f=\frac{1}{2\pi \mathrm{C}\sqrt{\left(\frac{\mathrm{R}1\mathrm{R}2}{\mathrm{R}1+\mathrm{R}2}\right)}\mathrm{R}3}$

where C1 = C2 = C

$\begin{array}{l}f=\frac{1}{2\pi \times 10\times {10}^{-9}\sqrt{\left(\frac{1.5\times {10}^3\times 1.5\times {10}^3}{1.5\times {10}^3+1.5\times {10}^3}\right)\times 150\times {10}^3}}\hfill \\ f=1501\mathrm{Hz}\hfill \end{array}$

The − 3 dB bandwidth is given by:

$\begin{array}{l}f=\frac{1}{\pi \mathrm{CR}3}\hfill \\ f=\frac{1}{\pi \times 10\times {10}^{-9}\times 150\times {10}^3}=212.2\mathrm{Hz}\hfill \end{array}$