PCB Design Blogs

I came across a question on a social media site about how to know when the absolute maximum ratings for a component have been exceeded? In other words, how do you identify components that are stressed due to power dissipation, increase in junction temperature, secondary breakdowns, or violations of voltage/current limits? The question also mentions a phrase that tells us exactly what we are looking for “when will a component break or burn out.” You can know using Smoke analysis of PSpice A/D and PSpice Advanced Analysis. Use Smoke analysis to identify stressed components in your design and then fix the issue. It is very important to identify and fix probable stresses because over time, stressed components can cause circuit failure and your product might malfunction or stop working.

Smoke analysis uses the Maximum Operating Conditions (MOC) provided by manufacturers and the derating factors you supply to calculate the Safe Operating Limits of a component. Circuit simulation results are then compared to the component’s safe operating limits. If the circuit simulation exceeds the safe operating limits, Smoke identifies the problem parameters.

Smoke analysis includes average, RMS, or peak values from simulation results and can be used to compare these values against corresponding safe operating limits. Use Smoke to identify:

• Components exceeding manufacturers’ limits
• Breakdown voltage across device terminals
• Maximum current limits
• Power dissipation for each component
• Secondary breakdown limits
• Junction temperatures

A component will fail and consequently, the design will malfunction if the MOC is exceeded. Use the derating factor to add a safety factor or adjust what is specified by manufacturers. Derating factor is a percentage of the MOC applied to ensure components are operating at a safe level. Safe operating limit is the maximum safe operating values for component parameters in a working circuit with derating or safety factors applied.

So, let’s run Smoke analysis on a design and see how it works. 

Running Smoke Analysis

To run Smoke analysis, the components of interest must have the Smoke parameter defined and transient analysis results must be available with relevant information. Ensure the transient analysis result is per your requirement and use components that are ready for Advanced Analysis.

In the following example, you will use the RF amplifier demo design.

1. Open the RF amplifier demo design by choosing File – Open – Demo Designs and then selecting RF amplifier.

The design is Advanced-analysis-ready as indicated by the Y under the PSpiceAA column. 

A simulation profile for transient analysis is already present but it is not the active profile.

2. Select SCHEMATIC1-Tran to make the existing transient simulation profile active.

You can also right-click SCHEMATIC1-Tran under Simulation Profiles of PSpice Resources, and choose Make Active from the pop-up menu.

You can double-click the profile or, once the profile is active, choose PSpice – Edit Simulation Profile to view the settings.

3. Run transient analysis by clicking Run PSpice ( ).

The simulation results are displayed in PSpice and you are ready to perform Smoke analysis.

4. Choose PSpice – Advanced Analysis – Smoke.

The PSpice Advanced Analysis window appears with the results.

The length of the bars indicates the stress level of a component. A green bar is a good news because the component is less than 90% of the MOC. A yellow bar represents a stress level of 90% to 100% and means the component might need your attention. A red bar showing more than 100% stress definitely needs action.

Gray bars can be ignored as they are for parameters not suitable for the component type. Right-click and choose Hide Invalid Values to hide the gray bars.

The results show that no action is required, and the design is good to go as far as stress is concerned. But observe that the title of the display specifies that there is no derating applied and the asterisk for Component Filter value indicates that the results are out of sync with the derating definition and needs to be rerun. The result might change if you introduce derating. Check that out in the next activity.
 

Adding Derating to Smoke Analysis

Smoke analysis, by default, uses 0% derating or no safety margin, which means 100% component rating is considered while running analysis. You can, however, add the default derating values or your own derating values. For example, if you are designing space flight hardware, you will use the recommended derating guideline MIL-STD 975M by NASA for, say, the resistors in your design. Similarly, you will use recommendations based on SD-18 for packages.

In all cases, you will try to keep the operating parameters of a component below its derating curve. For example, the MIL-STD 975M derating guideline for the power of a resistor is 60% till 70 C and 0 at 110 C as shown in the following image. The shaded area of the graph then defines the safe operating area for any resistor in your design for MIL-STD 975M.

In this activity, you will add the standard derating value, which is a predefined derate specification covering all devices and specifications such as rated power, junction temp, and currents.

1. Right-click in the PSpice Advanced Analysis window and choose Derating.

The No Derating option is selected by default. You can add your own derating files by choosing Custom Derating Files. For now, you will use the preinstalled derating table that comes with PSpice Advanced Analysis.

2. Choose Standard Derating.
 
3. Click Start/Resume ( ) in the PSpice Advanced Analysis window to run the analysis again.

After you added deration, a red bar appears showing that component Q1 is stressed for the peak value of VCE where it is operating at 136%. You can find out the component in the design and try to eliminate the stress.

Finding a Component in the Design

The design you used is a small sample design. In real life, the circuit will have thousands of components, and locating a component immediately might take time, or you might end up updating the wrong component. PSpice Advanced Analysis takes care of that by highlighting the exact component for you.

1. Right-click the red bar and choose Find in Design.

The schematic is in focus and the part is highlighted.

You can now make changes to ensure the component is not stressed. For example, by modifying the resistance R8. Another way to manage stress is to improve case-to-ambient thermal resistance (RCA) by introducing a heatsink.

2. Save the changed design and run transient analysis again.

3. Click Start/Resume ( ) in the PSpice Advanced Analysis window to run Smoke analysis again.

The results will be updated in the PSpice Advanced Analysis window. You can keep on adjusting and changing the design till you reach the expected results.

Conclusion

Reliability is the cornerstone of our products. Smoke analysis helps you address potential reliability issues in your design. Starting from an intuitive interface that quickly informs you of the status of components using color and length, it also provides you with all the information you might want to know. You can then adjust and manage your design to ensure your product is reliable and robust.

Another advantage with Smoke analysis and derating is that both are post-processing analyses requiring minimal time to run no matter how complex your design is. You can always try different deratings without worrying about time to find out what suits you best.

If you want to know more about the other advanced analyses types including Monte Carlo, Sensitivity, Optimizer, or Parametric Plotter, look out for our next posts.

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.