Table of Contents Previous Next


Lesson 9: Transformers

Learning Objectives

In this lesson you will learn how to place and use linear and non-linear transformer symbols to simulate magnetic circuits in PSpice A/D.
When you finish this lesson you will:
• Create a linear transformer
• Create a non-linear transformer using the core models from the magnetics library

Linear Transformers

Linear 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.
To create a linear transformer:
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.
2. Place a copy of the K_Linear symbol anywhere on the schematic and edit its properties.


Below is an example of a PSpice A/D netlist for a simple linear transformer circuit.
I1 1 0 AC 1mA
L1 1 0 10uH
L2 2 0 10uH
R2 2 0 .1
K12 L1 L2 1

Linear Transformer Circuit




The above graphic shows a linear transformer implemented in a schematic.
To complete the circuit using the “dot” convention, place a “dot” on the pin 1 of each inductor.
The 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:
Coupling = Mij/(Li*Lj)1/2
where:
Li and Lj are a coupled-pair of inductors
Mij is the mutual inductance between Li and Lj
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.
The linear branch relation for transient analysis is:
Vi = Li * dIi/dt + Mij * dIj/dt +Mik *dIk/dt + …

Non-linear Transformers

PSpice 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.
There are four behavioral differences between a linear and non-linear transformer:
• The magnetic core’s B-H characteristics are analyzed using the Jiles-Atherton and Tibrizi core models.
• The inductors become windings, so the value on the inductor symbol is the number of turns.
• The list of coupled inductors may number only one.
• A model statement is required to define the referenced core model.
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.
Below is a netlist example of a non-linear transformer:
L1 5 9 20;inductor with 20 turns
K1 L1 1 K528T500_3C8;Ferroxcube torroid core
L2 3 8 15;Primary winding with 15 turns
L3 4 6 45;secondary winding with 45 turns
K2 L2 L3 1 K528T500_3C8;another core (not the same as K1)
Core models can be found in the magnetic library.

Coupling Inductors




The above circuit shows the settings for a non-linear transformer.
For 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 Transformer

Lab Objectives
In this lab you will create a center-tapped linear transformer.



Constructing the Circuit
1. Draw the circuit shown above using the R, L, 0, VSIN, and K_Linear symbols.
2. Wire the circuit together as shown in the above figure.
3. Configure the VSIN to have an offset of 0, Vampl = 100 and Freq = 60.
Configuring the Coupling Symbol
1. Double-click on the K_Linear symbol to edit its properties.
Specify 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.
2. Type L3 in the L1 property, L4 in the L2 property, and L5 in the L3 property.



3. If desired, make L1-L3 visible.
You may do this through either the Property Editor or the Display Properties dialog box.
4. Close the Property Editor and return to the schematic view.
Configuring the Simulation



1. Configure a transient analysis with a Run to time of 50mS and a Maximum step size of .1mS.
2. Click OK to close the Simulation Settings dialog.
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 Transformers

Lab Objectives
In this lab you will create and simulate a nonlinear transformer.
Create a Non-linear Transformer



1. Using the same circuit as in the last lab, replace the K_Linear symbol with Kbreak.
2. 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.
3. For Coupling type .99.
4. Change the values of R1, R2, and R3 to .125.
5. Run the simulation and examine the results in the Probe window. You should now see that the core model is saturating.
Additional Exercise
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
http://www.EMA-EDA.com
http://www.TimingDesigner.com
Voice: (585) 334-6001
Fax: (585) 334-6693
techsupport@EMA-EDA.com

Table of Contents Previous Next