PCB Design Blogs

We all want to be sure, or as sure as we can be, that our products will work as expected in the real world under circumstances that may not always be under our control or per our specifications. We want to be adequately aware of how the output of the circuit may vary based on different parameters and their possible values; and how to identify the components with parameters critical to the measurement goals of the circuit design. That’s where Sensitivity Analysis comes to your aid.

Sensitivity Analysis can be used in different domains including finance and medicine to enhance the predictability of a system and deal with its uncertainties along with quite a few other applications, such as, decision making, feasibility testing, risk assessment, estimating requirements for input and output variables, or to understand how an output relates to an input. Sensitivity or what-if analysis saves money and effort because it can be safely conducted in a virtual environment without setting up tedious and complex prototyping and measurements.

As a designer, you will use PSpice® A/D Sensitivity Analysis along with Optimizer to enhance performance and by itself to identify components that have maximum effect on yield. Once you have identified the sensitive components, you can maximize productivity and reduce cost by tightening the tolerances of sensitive components and loosening the tolerances of the non-sensitive components. You can also use this analysis to progressively refine and develop your experimental circuits to market-worthy designs and products.

Sensitivity Analysis can provide you with either absolute or relative sensitivity of a component. The absolute sensitivity is a ratio measuring the change in output or measured value for a unit change in a parameter. Whereas, relative sensitivity is a percentage value measuring the change in output or measured value for one percent positive change in a parameter. You can get an in-depth understanding of the calculations used for both the sensitivity types from the PSpice product documentation. But, for now, it is useful to know that absolute sensitivity is good if tolerance limits are relaxed or bandwidth is high.

Let’s get into quick action then. First, what do you need to run a sensitivity analysis? Just verify the following and you are ready:

1. Circuit components have tolerance values
2. The circuit is simulated in PSpice
3. Measurements are available

You will start by adding measurements and then move on to running Sensitivity Analysis. If you want to work along, just open the RF Amplifier demo design (File – Open – Demo Designs) in OrCAD® Capture.

Creating Measurements

Before creating the measurements, you need to run any one of the basic PSpice simulations. In this example, you will run AC Sweep/Noise simulation.

1. Create a simulation profile of type AC Sweep. In this example, you create a profile defining a 1KHz to 1GHz frequency sweep.

2. Run the simulation by first selecting the AC profile and then clicking the Run PSpice icon.

PSpice A/D will appear with the results.

In this example, let’s see the noise.

3. Add two traces, for output noise and noise figure using the Trace – Add Trace menu in the PSpice A/D window.

You will add expressions to measure the following:

• Gain in dB
• Bandwidth in Hertz
• Noise figure in dB
• Output noise in volts

You will then run Sensitivity Analysis for these measurements.

To add measurements, follow these steps:

1. In PSpice A/D, choose Trace – Evaluate Measurement to open the Evaluate Measurement window

Under Functions and Macros, Measurements is selected. You can also choose from Analog Operators and Functions, Macros, or Plot Templates.

You can explore the various available options.

For now, create the expression to measure the gain in dB.

2. Select Max(1) from the Measurements list.

The measurement is listed in the Trace Expression field.

3. Choose Analog Operators and Functions and then click DB().

4. From Simulation Output Variables, select V(Load) to get the following expression. Scroll down if needed.

5. Click OK.

The measurement is added and selected.

Similarly, create and add the measurements for bandwidth, noise figure, and output noise, as shown in the following figure.

Running Sensitivity Analysis

To run sensitivity analysis, do the following steps:

1. In OrCAD Capture, choose PSpice – Advanced Analysis – Sensitivity.

PSpice Advanced Analysis opens.

Only resistors and capacitors are listed because only these have tolerances assigned. You can use the PSpice – Advanced Analysis – Add Tolerance option in OrCAD Capture to add global tolerances to the components of your circuit. You can also assign instance-specific tolerances as well.

2. Click in the Specifications section to import the measurements.

The Import Measurement(s) window opens.

The four measurements created for the AC profile are listed.

You can run sensitivity analysis for multiple simulation profiles in one go and easily get the overall view, that is, identify the most critical components of your circuits considering all possible operating conditions. And, you can also add new measurements here if needed.

3. Select the four measurements and click OK.

The measurements are selected. The analysis will be run for each of the selected measurements.

4. Choose Edit – Profile Settings.

The Profile Settings dialog opens with the Sensitivity tab active.

By default, the sensitivity variation is set at 40%. The sensitivity variation value determines the percentage of the tolerance range for the component values. For example, for a sensitivity variation of 40% and a tolerance of 10%, the component value stays within 4% of the nominal value.

5. Click OK to close Profile Settings.

6. Click the Start/Resume ( ) icon to run the analysis.

By default, the first row in the Specifications section with the gain measurement max(db(v(load))) is selected. Clicking another row will show the results for the measurement in that row.

You can see that gain, which is the function selected under specifications, is most sensitive to the value of the capacitor C6. However, this is in terms of absolute sensitivity. Let's check the value for relative sensitivity.

7. Right-click in any of the rows and choose Display – Relative Sensitivity to display relative sensitivity.

Now you can see that gain is most sensitive to the resistor R9.

8. Select the measurement for output noise, that is, max(v(onoise).

Notice that the sensitivity is maximum for R9 again.

Similarly, explore the other measurements. The results are already there for you, and you do not need to run separate analyses for each measurement or goal.

You can then use the Find in Design option of the popup menu to highlight the critical components in the design and optimize the design.

Conclusion

Running Sensitivity Analysis and identifying the components that are critical for the measurements of interest, and thereby the functioning of your design, helps you optimize the design. The next major step is to run PSpice Optimizer and achieve the ideal measurement per your requirement. You will do just that in the next post in this series.

Do SUBSCRIBE to be updated about upcoming blogs. If you have any topic you want us to cover or any feedback for us, you can write to us at pcbbloggers@cadence.com.