PSpice for TI: Transient Analysis
In this video, you will learn to perform transient analysis and understand the value of check point restart. You will need a time domain stimulus to explore this capability. A more precise output will be given if you know when your application will achieve steady state. To make it easier, the simulator will store states at user defined intervals and will allow you to use any specific interval as your start point. Waveforms within PSpice for TI can be configured to be displayed according to desired checkpoints. Understanding this feature you can quickly validate steady state response with different component values.
In addition to this content, more tutorials and a complete training course can be found from Cadence.
Resources
In this video, an example of a buck converter circuit is used so you can learn how to perform transient analysis and understand the capability of CheckPoint Restart, which is unique to PSpice. To run a transient analysis, it's necessary for a time domain stimulus to be present in the circuit. In the example circuit, it will be in the form of a pulse source driving the gate of the MOSFET.
Access the modeling apps to place any type of source, including the pulse source, that's necessary in an example circuit. Select independent sources from the sources list and enter values for the pulse-voltage source. Place the gate pulse source on the schematic. Now create a new simulation profile and name it "transient analysis."
Within the simulation settings GUI under Analysis Type, transient analysis is selected by default. Enter four milliseconds as a total runtime of the simulation. Then enter a time for when you want to save the data after.
This field is useful if you know the time after which your circuit achieves steady state. It helps generate a more precise simulation result, which is beneficial for efficient waveform analysis. For this example, as we're not sure of when the circuit achieves steady state, simply enter a "0" to save the data from the start of the simulation.
Here you can provide the maximum internal step size. If you wish to keep this variable empty, PSpice varies and reduces it as needed to find circuit solutions. To use the CheckPoint Restart feature, you need to first enable the Save Checkpoint option. Enter the location of where you want to save the checkpoints during the simulation and enter the simulation interval as well.
The simulator will store states with these intervals. And you can use any one of these later as your simulation start point. Click OK to save the simulation settings.
Place the voltage markers on the schematic to measure input voltage, voltage across the MOSFET's drain and source, and output voltage. Run the PSpice simulation. The voltage waveforms are displayed for the buck regulator circuit.
Now, to plot current waveforms, go to Plot in the menu and select "add plot to window." This avoids plotting voltage and current waveforms on the same y-axis. Add the current markers on the schematic to measure inductor current and diode current.
In addition to the voltage waveforms, the current waveforms are now displayed. Waveforms within PSpice can be configured to be displayed exactly according to the latest display configuration. To accomplish this, from the probe window settings, select "last plot."
To restart the simulation from a specific checkpoint, deselect Save Checkpoints and select Restart Simulation. PSpice has already saved all the checkpoints. Select a simulation time of three milliseconds from the dropdown menu. Select OK. Run the simulation again. Notice that the simulation now runs much faster compared to the previous one, and it begins from three milliseconds.
There is another advantage to using the CheckPoint Restart feature in PSpice. You can even reuse the same checkpoints with modified component value changes. For example, let's change the load resistance value to eight ohms. Run the simulation again. This way you can quickly validate steady state response with different component values. Now you have successfully perform transient analysis and learned the unique CheckPoint Restart capability in PSpice.
This video is part of a series
-
Explore PSpice® for TI design and simulation tool
video-playlist (12 videos)