Tutorials, news, snippets, and other various musings about the electrical engineering industry.

Quick Tutorial: Exposing Components Prone to Failure with Smoke Analysis in PSpice Advanced Analysis

Most SPICE simulators are really good at simulating circuits and showing you what the outputs will be but, on their own, they don’t do anything to bring attention to components that may be stressed or overloaded.


As the designer, it’s your job to ensure that the parts in your design are within their stress limitations; this is a laborious job so shortcuts are usually taken. These shortcuts can range from not doing anything to only measuring certain components in your design that you feel are particularly stressed. Shortcuts can sometimes lead to oversights which can manifest themselves as component failures in the lab or the field hurting your reputation and your pocketbook.


With Smoke Analysis in PSpice Advanced Analysis and a bit of preparation on your components, this laborious task becomes trivial, quickly yielding results that are meaningful.




There will be a video at the end of this entry covering all the topics in this post.  We’ll be using the RF_amp circuit that is available in your C:\Cadence\SPB_16.6\tools\pspice\capture_samples\advanls\rfamp directory if you would like to follow along.


Component Preparation

Each component in the design that you’d like to include in the Smoke Analysis needs to have its limitations defined so they can be tested against measurements. The limitations are entered differently for passive components compared to active ones so we’ll outline them below separately.



For passive components, the recommended parts to use are the RESISTOR, CAPACITOR, INDUCTOR, and VARIABLES parts from the PSPICE_ELEM library (located at C:\Cadence\SPB_16.6\tools\capture\library\pspice\advanls\pspice_elem.olb).





The properties in these parts are nicely linked to each other so nothing much needs to be set up.  You only need to set your maximums in the VARIABLES block and all the passive devices that you have placed will reflect the limits that you have entered there.


For active components, you need to edit the PSpice model (RMB > Edit PSpice Model or Edit > PSpice Model) and in the resulting PSpice Model Editor, on the Smoke tab, fill in the specific component limitations that you would typically be able to get from the datasheet.




In this example, we’ll track the VCE (Maximum Collector Emitter Voltage) property of this component (Q1) which has a limit of 12V valid for the PEAK of the measurement.  You can see what type of measurement this maximum is valid for by hovering anywhere over the line; the available valid options are PEAK, AVG and RMS.




Note that if you have a model that is not showing the Smoke Tab, you can add the tab by selecting Model > Add Smoke… in the PSpice Model Editor.



Checking Limitations in Probe

If you don’t have Smoke Analysis and you want to check your components against their limits, you’ll need to become very familiar with Measurements and even then, tracking all of them can become difficult.  We’ll take a look at tracking just one of the Smoke Limits, Q1’s VCE of 12 V PEAK.


In Capture, run the simulation and take a look at the results in PSpice.  To aid in understanding, we’ll take a look at the differential voltage waveform, VCE of Q1 below:




From this, we can see that the waveform is a sinusoid centered on ~8.125V with a small peak to peak amplitude of ~30mV.  We can eyeball the Peak at ~8.142V but if we want something more specific, we can set up a measurement (View > Measurement Results) and get it exactly.


Choose Click here to evaluate a new measurement… and click in or type: Max(V(Q1:C)-V(Q1:E))




This will show you the more detailed result of 8.142237520V; note that this is under the Smoke limit of 12V that was set up in the model.




To replicate what’s available with Smoke, measurements would need to be set up for every component for a variety of different measurements and the actual limit will need to be remembered and checked against the measurement.  This is better than looking at waveforms but is itself, a very time consuming and error-prone task.



Smoke Analysis

Now that we have got our components all set up with their Smoke limits, and we’ve run a sample transient simulation we can run Smoke Analysis in Capture by going to PSpice > Advanced Analysis > Smoke




This opens up the PSpice Advanced Analysis window on the Smoke tab and runs the analysis which just takes a second.  The very top items we can see 3 lines representing component the VCE of Q1 which has measurements for Average, Peak and RMS but as we noted previously in the Model Editor, only the Peak is valid for this measurement.




You can see the Average and RMS measurements are greyed out in the % Max column automatically because of this and if you’d like to, you can remove them (RMB > Hide Invalid Values or Analysis > Smoke > Hide Invalid Rows) so that they don’t show up.





Design in Some Safety Margin with Derating

If you want to design in some margin to stay off the maximum limitations that your parts have, it’s easy to do with Derating.  Click on Analysis > Smoke > Derating > Standard Derating or RMB > Derating > Standard Derating and rerun the simulation to get updated results.


Notice that the VCE for Q1 is still rated for Peak at 12V and is still being measured at 8.1422V. Now, however, it’s being derated 50% which means that we’re creating an artificial limit of 6V to give ourselves a safety margin. Our measurement exceeds this derated limit so we get a red bar graph in the % Max column letting us know that we’re driving this 36% harder than we should.




Note: that this uses the default derating values that come with the tool but if you’d like to customize these derating percentages you can do that.




With a little bit of component setup, Smoke Analysis will tell you what components in your design are going to have issues performing their duties and for what specific reason they will fail. If you make changes in your design and need to re-check your results, it’s just a simple Smoke simulation run away. It allows you to proceed with confidence knowing that the components in your design are going to be able to stand up to whatever harshness they encounter, with a bit of room to spare.



Please watch the video below if you’d like to dig into this a bit more and leave comments if you have any additional questions. Thanks for taking time to read about Smoke Analysis within PSpice Advanced Analysis.