Creating a center tapped transformer to simulate in PSpice


PROBLEM:
How do I create a center tapped transformer for PSpice?

SOLUTION:
The purpose of this application note is to demonstrate the functions of MicroSim's circuitsimulator PSpice. The following circuit has been created on the DesignLab Evaluation copy release 8. Before attempting this application note, it is recommended to read Chapter 2 of the PSpice A/D User's Guide. If you do not have this guide, it is located on the CD in theOnline Documentation directory and on OrCAD's web site.

Before you begin
Transformers are widely used in the electrical industry and come in different configurations. On the Evaluation CD, there are only two transformers. Both are two port devices. This application note will demonstrate how to build and simulate a center-tapped transformer.

Creating the schematic
  1. Build a simple RL circuit energized by a VSIN. The resistor will represent the parisetic resistance and the inductor will represent the primary windings.
  2. Place two more inductors in series seperate from the first circuit. The two inductors will represent the secondary windings.
  3. Connect two resistors to ground, one from the first secondary winding and the second resistor on the next secondary winding.
  4. To complete the secondary side, ground the center tap port.
  5. To finish the transformer, couple the windings. Get the part "K_linear" and place it any where on the schematic.
  6. Double click on the K to edit the attributes. Set L1=L1, L2=L2, L3=L3 and Coupling=1.
  7. Double click on the VSIN to edit its attributes. Set VOFF=0, VAMPL=100V and FREQ=60.
  8. Set the resistor and inductor values where R1=1, R2=1k, R3=1k, L1=100, L2=50, and L3=50.
  9. To view the output and input waveforms in Probe, place voltage markers on the output and input nodes.
Simulating the design
To view the output and input waveforms as a function of time, use transient analysis.
  1. From the Analysis menu, choose Setup. Click on the Transient button to set up the parameters.
  2. Set Print Step=.1ms, Final Time=50ms and Step Ceiling to .1ms to simulate the circuit for 3 cycles. Once the data is entered, exit by clicking OK.
  3. At this point, there should be two boxes checked, Transient and Bias Point Detail. Exit the setup by clicking on Close.
  4. Next, simulate by choosing Simulate from the Analysis menu or press F11.
Viewing results in Probe
When PSpice is finished simulating, Probe will automatically open with the input and output waveforms plotted. This is due to the voltage markers placed on the schematic. Footnote: Symbols are now included in the breakout.olb file

Document number: PSP02130
Applies to: PSpice ver. All
Created on: 24-JUL-1998
Last modified: 9-JAN-2002

Copyright © 2005, Cadence Design Systems, Inc.
All rights reserved.