Virtual Workshop: Design for Reliability, Component Stress

August 10, 2020

Duration: 15 minutes| Version Required: 17.4

The smoke analysis tools in PSpice makes it easy to find stressed components, so you can design a more reliable circuit. Smoke analysis looks at your entire circuit and models expected current, voltage, power and temperature conditions for every component in your circuit. The tool then compares those simulation results to your components' limitations, helping you to quickly determine what is being pushed too far and are likely to fail. With the advanced analysis tools in PSpice, you can be confident your designs are reliable and won't fail in the field.

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

  1. Open OrCAD PSpice Designer.

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

  1. Select RF Amplifier and Open.

  1. 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

 

 

  1. Under Simulation Profile in the project hierarchy, right click on SCHEMATIC1-Tran and select Make Active.

Note: If you want to create a new simulation profile instead of using the one provided, see the Bonus portion of this workshop.

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

  1. View the Transient Simulation.

  1. Back in the schematic, select PSpice > Advanced Analysis > Smoke.

Note: Smoke Analysis calculates safe operating limits using component parameter maximum operation conditions and derating factors.

  1. View the Smoke Analysis Simulation.

Note: Mouse over the flags in the left column for more information. View the bar graph for easy identification of potential problem components:

  • Red bars show values that exceed safe operating limits.
  • Yellow bars show values getting close to the safe operating limits (between 90 and 100%).
  • Green bars show values well within the safe operating limits (less that 90 percent).
  • Grey bars indicate thar limits are not valid for the parameters.

  1. Right click and select Hide Invalid Values.

Note: This will remove the values that are not typically defined from the simulation.

  1. Right Click and select Derating > Standard Derating.

Note: Simulations can be run with no derating, standard derating, or custom derating.

  1. Select Run > Start Smoke from the menu (CTRL-R).

  1. Right click on Component: Q1, Parameter: VCE and select Find in Design.

Note: This will bring you to the schematic and highlight the corresponding component.

  1. Select Place > PSpice Component > Search from the menu.

  1. In the Search Window, type 30V NPN Transistor and select the Search icon.

  1. In the schematic, select Q1 and press Delete on the keyboard.

  1. In the Search Results, double click on 2N2219.

  1. Click to place the part where Q1 was located.

  1. Right click and select End Mode (ESC).

Note: If the component is placed as “Q?”, double click the “Q?” and name the component Q3.

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

  1. In the Transient Simulation Window, select Plot > Add Plot to Window from the menu.

  1. Right click on an existing plot and select Delete Plot.

  1. Right click on the remaining existing plot and select Delete Plot.

  1. Select Trace > Add Trace from the menu (Insert).

  1. In the Trace Expression Window, select from the Simulation Output Variables to create the equation, V(Q3:C, Q3:E).

  1. In Simulation Output Variables, select V(Q3:C).

  1. In the Trace Expression box, use the keyboard to complete the equation by adding “, Q3:E”.

  1. Click OK. The trace has been added to the plot.

  1. Select Trace > Evaluate Measurement from the menu.

  1. In the Trace Expression Window, select from the Functions and Simulation Output Variables to create the equation, Max(V(Q3:C)-V(Q3:E)).

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

  1. In Simulation Output Variables, select V(Q3:C).

  1. In the Trace Expression box, use the keyboard to enter a minus sign after V(Q3:C).

  1. In Simulation Output Variables, select V(Q3:E).

  1. Click OK. The measurement has been added to the simulation window.

  1. In the Smoke Analysis Simulation Window, select Run > Start Smoke from the menu (CTRL-R).

  1. View the effects of the new component on the simulation.

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

 

Bonus: Creating a New Transient Simulation Profile

  1. In the schematic, select PSpice > New Simulation Profile.

  1. For the Name, add Transient.
  2. Leave Inherit From set to none and select Create.

  1. Set Run to Time to 10us.

  1. Set Maximum Step Size to 1ns.

  1. Click Ok. The simulation profile has been added to the project hierarchy and automatically selected as the active profile.

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

  1. Open the transient simulation results.

  1. Select Trace > Add Trace from the menu.

  1. From the Simulation Output Variables, select V(In).

Note: Type the desired Simulation Output Variable after the asterisk (*) to filter the variables.

  1. Click OK. The trace has been added to the plot.

  1. Select Trace > Add Trace from the menu.

  1. From the Simulation Output Variables, select V(Load).

  1. Click OK. The trace has been added to the plot.

  1. Select Plot > Add Plot to Window from the menu.

  1. With the new plot selected, select Trace > Add Trace from the menu.

  1. In the Functions or Macros drop-down, select Analog Operators and Functions. Select ABS().

  1. In Simulation Output Variables, select V(In).

  1. Click OK. The trace has been added to the plot.

  1. Select Trace > Add Trace from the menu.

  1. In the Functions or Macros drop-down, select Analog Operators and Functions. Select ABS().

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

  1. Click OK. The trace has been added to the plot.

Ensuring the design of a reliable circuit through the identification of potentially stressed components is essential to product success. With the smoke analysis tool in PSpice, you can look at your entire circuit and models expected outputs for each circuit component and compare them to your component’s limitations. This will help you to quickly determine what components are likely to fail and adjust during the design phase.

 

 

 

No Previous Articles

Next Video
Extracting S-Parameter Models with Sigrity Power SI
Extracting S-Parameter Models with Sigrity Power SI

S-Parameter models are a critical way to verify your design interconnect and parasitics will operate within...