Virtual Workshop: Design for Reliability, Component Tolerance

Duration: 15 minutes| Version Required: 17.4

Design reliability is an essential part of a successful project. Being able to produce the design at a reasonable cost is an added bonus, however identifying critical components hasn't always been the easiest task. With one click in OrCAD PSpice Designer Plus, you can easily simulate your circuit and ensure it is behaving as expected. The tools make it easy by providing you with an ordered list of critical components within your design so you can intelligently assign tighter/loser tolerances where needed. This helps you to optimize your design's overall performance and cost.

This document is intended to provide step by step instructions on performing sensitivity analysis using OrCAD PSpice Designer Plus. For this workshop, use the RF Amplifier Demo Design included in the OrCAD software.

1. Open OrCAD PSpice Designer Plus.

2. Select File > Open> Demo Designs from the menu.

3. Select RF Amplifier and Open.
4. Ensure the following values are set in the Tolerance and Smoke Limit variables:

Tolerance	Value
CTOL	10
RTOL	10
LTOL	0
VTOL	0
ITOL	0

 

Smoke Limit	Value
RMAX	0.25
RSMAX	0.005
RTMAX	200
VMAX	12
CMAX	50
CBMAX	125
CSMAX	0.005
CTMAX	125
CIMAX	1
LMAX	5
DSMAX	300
IMAX	1

 

5. In the project hierarchy, under Simulation Profile, ensure SCHEMATIC1-AC is the active simulation profile.

Note: If the SCHEMATIC1-AC simulation profile is not active, right click and select Make Active.

6. Select PSpice > Run from the menu (F11).

7. View the AC Simulation Results.

8. Select View > Measurement Results from the menu.

9. Check the box in the Evaluate column to view the corresponding measurements.

Note: If no measurements are listed or you would like more information on measurements, view the Bonus portion of this workshop.

10. Back in the schematic, select PSpice > Advanced Analysis > Sensitivity from the menu.

Note: Sensitivity Analysis examines how much each component affects circuit behavior by itself and in comparison to other components. It also varies all tolerances to create worst case minimum and maximum measurement values. You can use sensitivity analysis to determine sensitive components, identify which components affect the yield the most, adjust the tolerances of components and evaluate yield versus cost trade-offs.

11. In the Sensitivity Window, select Run > Start Sensitivity from the menu (CTRL-R).

12. Right click and select Display > Relative Sensitivity.

Note: Relative sensitivity is the percentage of change in a measurement based on a one percent positive of a component’s parameter value. Relative Sensitivity should be used when the tolerance limits are tight enough or have less bandwidth.

13. View the simulation results.

Note: Click on different specifications to view the results for the corresponding measurements. Results are displayed in the parameters table and specifications table. The parameter table includes:

• Parameter values at minimum and maximum measurement values
• Absolute or relative sensitivity per parameter
• Linear/Log bar graphs per parameter

The specifications table includes:

• Worst case minimum and maximum measurement values

14. Back in the schematic, under the Tolerance variables, double click on RTOL.

15. Change the Value to 4 and click OK.

16. Select PSpice > Run from the menu to run the AC Simulation with the new resistor tolerance.

17. When the simulation is complete, return to the Sensitivity Window and select Run > Start Sensitivity from the menu.

18. View the effect of the change in tolerance on the simulation results.

 

Bonus: Adding a Measurement to a PSpice Simulation Plot

1. In the Simulation Window, select Trace > Evaluate Measurement.
2. In the Trace Expression Window, select from the Functions and Simulation Output Variables to create the equation, MAX(DB(V(Load))), used in this workshop.

3. From the Functions and Macros drop-down, select Measurements and choose MAX(1).             

4. From the Functions and Macros drop-down, select Analog Operators and Functions and select DB().

5. In Simulation Output Variables, select V(Load).

6. Select OK. The measurement has been added to the simulation plot.

7. Select Trace > Evaluate Measurement from the menu.

8. In the Trace Expression Window, select from the Functions and Simulation Output Variables to create the equation, Bandwidth(V(Load),3), used in this workshop.

9. From the Functions and Macros drop-down, select Measurements and choose Bandwidth(1,db_level).

10. In Simulation Output Variables, select V(Load).

11. Enter 3 on the keyboard for the db_level.

12. Click OK. The measurement has been added to the simulation plot.

13. Select Trace > Evaluate Measurement from the menu.

14. In the Trace Expression Window, create the equation, Min(10*log10(v(inoise)*v(inoise)/8.28e-19)), used in this workshop.
15. Copy the following equation: Min(10*log10(v(inoise)*v(inoise)/8.28e-19))

16. In the Trace Expression box, paste the equation.

17. Click OK. The measurement has been added to the simulation plot.

18. Select Trace > Evaluate Measurement from the menu.

19. In the Trace Expression Window, create the equation, Max(v(onoise)), used in this workshop.

20. In the Trace Expression box, enter the following equation using the keyboard: Max(v(onoise)).

21. Click OK. The measurement has been added to the simulation plot.

Optimizing your design's overall performance and cost is essential in to creating a competitive product in today's market. Identifying critical components no longer needs to be a complicated task. With OrCAD PSpice Advanced Analysis, you can easily simulate your circuit, ensure it is behaving correctly, and have a complete, ordered list of critical components with just one click.

If you would like more tutorials, visit our walk-through page to view additional OrCAD and PSpice video tutorials and download design files.

Don't have OrCAD 17.4? Download the Trial Now