Lesson 9: Transformers
Learning ObjectivesIn this lesson you will learn how to place and use linear and non-linear transformer symbols to simulate magnetic circuits in PSpice A/D.
Linear TransformersLinear transformers are created in OrCAD Capture and PSpice A/D using multiple occurrences of the common inductor symbol L and the K_Linear symbol. Both symbols are located in the Analog symbol library.
1. Draw a schematic and assign reference designators to the inductors. (Reference designators may be automatically annotated as you place the inductors).
Reference designator values assigned to the coupled inductors Li fields are (i=1,2,…6). Be sure to specify the value for the Coupling property.
Linear transformers are based on the SPICE coupling device K and must couple two or more inductors. Values of the inductors are measured in Henrys.
Linear Transformer CircuitThe polarity of the current is determined by the order of the nodes in the inductors, not by the order of the inductors in the coupling statement.
The coupling value is the coefficient of mutual coupling and must have a value between 0 and 1. The equation for coupling is:
For transformers of normal geometry, the coupling is usually 1. Values less than one occur for air core transformers when the coils do not completely overlap.
Non-linear TransformersPSpice A/D supports the simulation of non-linear transformers. A transformer becomes non-linear if the coupling statement contains a reference to a core model. Other than a reference to a model, creating a non-linear transformer is no different than creating a linear one.
• The magnetic core’s B-H characteristics are analyzed using the Jiles-Atherton and Tibrizi core models.
Non-linear transformers are created using the Kbreak symbol to couple inductors in the design. The inductor is a winding whose value equals the number of turns. The non-linear transformer may couple a single inductor.
Coupling InductorsFor more information on the PSpice A/D format of the Jiles-Atherton model please see the PSpice Reference Guide.
For more information on the Jiles-Atherton model please see D.C. Jiles and D.L. Atherton, “Theory of ferromagnetic hysteresis,” Journal of Magnetism and Magnetic Materials, 61, 48 (1986).
Also see PSpice A/D application note PSPA021L: Using Coupled Inductors and Inductor Cores. This is available at http:\\www.pspice.com in the Help Online section.
Lab 9-1: Linear TransformerSpecify the inductors to be coupled by entering their reference designators into the L1 – L6 fields. L1 – L6 will contain the reference designators of the inductors to be coupled, not the values of the inductors. The inductor values will still be specified on each individual inductor, as normal.
3. Run the simulation and examine the results in the Probe window. The following figure shows the expected results.
From the cursor display you can see that the value on the center-tapped node is exactly half of that on the end.
Lab 9-2: Non-linear Transformers2. Configure the L1-L3 properties as they were for the K_Linear (L1=L3, L2=L4, L3=L5). You may need to flip the inductor symbols to have the correct orientation.
5. Run the simulation and examine the results in the Probe window. You should now see that the core model is saturating.
There are specific center-tapped symbols added to the 9.2 breakout library; Xfmr_Nonlin/Ct-Pri, Xfmr_Nonlin/Ct-Pri/Sec, and Xfmr_Nonlin/Ct-Sec.
Modify the above circuit using one or more predefined symbols. Edit the PSpice A/D model for predefined symbols. Examine the subcircuit definition.
EMA Design Automation