Chapter 5-SPICE for Power Electronics and Electric Power-Book, Lecture notes of Power Electronics

Download Chapter 5-SPICE for Power Electronics and Electric Power-Book and more Lecture notes Power Electronics in PDF only on Docsity! 96 SPICE for Power Electronics and Electric Power, Second Edition respectively. TYPE is the type name of the elements as shown in Table 5.1. An element must have the correct model type name. That is, a resistor must have the type name RES, not type IND or CAP. However, there can be more than one model of the same type in a circuit with different model names. (tolerance specification) is used with .MC analysis only, and it may be appended to each parameter with the format [ DEV/<distribution name> <value in % from 0 to 9> ] [ LOT/<distribution name> <value in % from 0 to 9> ] where <distribution name> is one of the following: UNIFORM Generates uniformly distributed deviations over the range of ± <value> GAUSS Generates deviations with Gaussian distribution over the range ±4, and <value> specifies the ±1 deviation In PSpice schematics, the user can assign a model name for the breakout specify the model parameters. PSpice can open the menu with the model name, Rbreak, as shown in Figure 5.1(b), and the model name can be changed. TABLE 5.1 Type Names of Elements Breakout Device Name Type Name Resistor Rbreak RES Resistor Cbreak CAP Capacitor Dcbreak D Diode Lbreak IND Inductor QbreakN NPN Bipolar junction transistor QbreakP PNP Bipolar junction transistor JbreakN NJF n-channel junction FET JbreakP PJF p-channel Junction FET MbreakN NMOS n-channel MOSFET MbreakP PMOS p-channel MOSFET Bbreak GASFET n-channel GaAs MOSFET Sbreak VSWITCH Voltage-controlled switch Wbreak ISWITCH Current-controlled switch XFRM_LINIEAR None Linear magnetic core (transformer) XFRM_NONLINIEAR CORE Nonlinear magnetic core (transformer) ZbreakN NIGBT n-channel IGBT devices in the library breakout.slb as shown in Figure 5.1(a). The user can also Passive Elements 97 5.2.1 SOME MODEL STATEMENTS FIGURE 5.1 Breakout library for models. (a) Breakout devices, (b) PSpice model editor. .MODEL RLOAD RES (R=1 TC1=0.02 TC2=0.005) .MODEL RLOAD RES (R=1 DEV/GAUSS 0.5% LOT/UNIFORM10%) .MODEL CPASS CAP (C=1 VC1=0.01 VC2=0.002 TC1=0.02 TC2=0.005) .MODEL LFILTER IND (L=1 IL1=0.1 IL2=0.002 TC1=0.02 TC2=0.005) (a) (b) 100 SPICE for Power Electronics and Electric Power, Second Edition FIGURE 5.4 Resistor schematics and parameters. (a) Symbol, (b) element menu, (c) resistor’s model parameters. TABLE 5.2 Model Parameters for Resistors Name Meaning Unit Default R Resistance multiplier 1 TC1 Linear temperature coefficient °C−1 0 TC2 Quadratic temperature coefficient °C−2 0 TCE Exponential temperature coefficient %/°C 0 R1 Rbreak 2 (a) (b) (c) Passive Elements 101 If RNAME is included and TCE is specified, the resistance as a function of temperature is calculated from TCE* (T − T0) RES = RVALUE * R * 1.01 where T and T0 are the operating temperature and room temperature, respectively, in degrees Celsius. 5.4.1.1 Some Resistor Statements R1 6 5 10K RLOAD 13 11 ARES 2MEG .MODEL ARES RES (R=1 TC1=0.02 TC2=0.005) RINPUT 15 14 RRES 5K .MODEL RRES RES (R=1 TCE=2.5) 5.4.2 CAPACITOR The symbol of a capacitor is C, and its name must start with C. The schematic of a capacitor with a breakout model is shown in Figure 5.5(a). Its value and initial condition can be changed as shown in Figure 5.5(b). The model parameters of capacitors are shown in Figure 5.5(c). The capacitor’s name and its nominal value can be changed. Its description takes the general form C<name> N+ N− CNAME CVALUE IC=V0 FIGURE 5.5 Capacitor schematics and parameters. (a) Breakout model, (b) initial con- dition, (c) capacitor’s model parameters. C2 Cbreak 10 uF (a) (b) C2 C2 H 1.5V Cbreak Normal (c) Lbreak* CAP .model Cbreak Cap C=1 VC1=0.01 VC2=0.002 102 SPICE for Power Electronics and Electric Power, Second Edition N+ is the positive node and N− is the negative node. The voltage of node N+ is assumed positive with respect to node N− and the current flows from node N+ through the capacitor to node N−. CNAME is the model name, and CVALUE is the nominal value of the capacitor. IC defines the initial (time-zero) voltage of the capacitor, V0. The model parameters are shown in Table 5.3. If CNAME is omitted, CVALUE is the capacitance in farads. The CVALUE can be positive or negative but must not be zero. If CNAME is included, the capacitance, which depends on the voltage and temperature, is calculated from CAP = CVALUE * C * (1 + VC1 * V + VC2 * V2) * [1 + TC1 * (T − T0) + TC2 * (T − T0)2] where T is the operating temperature and T0 is the room temperature in degrees celsius. 5.4.2.1 Some Capacitor Statements C1 6 5 10UF CLOAD 12 11 5PF IC=2.5V CINPUT 15 14 ACAP 10PF C2 20 19 ACAP 20NF IC=1.5V .MODEL ACAP CAP (C=1 VC1=0.01 VC2=0.002 TC1=0.02 TC2=0.005) Note: The initial conditions (if any) apply only if the UIC (use initial condi- tion) opinion is specified on the .TRAN command that is described in Section 6.9. 5.4.3 INDUCTOR The symbol of an inductor is L. Its name must start with L. The schematic of an TABLE 5.3 Model Parameters for Capacitors Name Meaning Unit Default C Capacitance multiplier 1 VC1 Linear voltage coefficient V−1 0 VC2 Quadratic voltage coefficient V−2 0 TC1 Linear temperature coefficient °C−1 0 TC2 Quadratic temperature coefficient °C−2 0 inductor with a breakout model is shown in Figure 5.6(a). Its value and initial Passive Elements 105 specified by a PWL source as shown in Figure 5.8(b). The breakout devices are used to specify the parameters of model RMD for R1 and R2 as shown in Figure 5.8(c), of model LMOD for L1 as shown in Figure 5.8(d) and of model CMOD for C1 as shown in Figure 5.8(e). The Transient Analysis is set at the Analysis Setup as shown Figure 2.6(d). The operating temperature is set from the simulations setting menu FIGURE 5.8 PSpice schematic for Example 5.1. (a) PSpice schematic, (b) PWL param- eters, (c) RMD parameters, (d) LMOD parameters, (e) CMOD parameters. 1 − 32 R2 RMD 20 V Vs+− CMOD C1 4 V 2.5 uF LMOD L1 3 A1.5 mH + R1 RMD 60 (a) (b) (c) (d) (e) in Figure 2.6(a), and its specifications are set at the transient menu as shown in as shown in Figure 5.2. 106 SPICE for Power Electronics and Electric Power, Second Edition The circuit file contains the following statements: The inductor has an initial current of 3 A, which is taken into consideration by UIC in the .TRAN command. 5.5 MAGNETIC ELEMENTS AND TRANSFORMERS The magnetic elements are mutual inductors (transformer). PSpice allows simu- lating two types of magnetic circuits: • Linear magnetic circuits • Nonlinear magnetic circuits Example 5.1 RLC circuit SOURCE
* Input step voltage represented as a PWL waveform: VS 1 0 PWL (0 0 10NS 10V 2MS 10V) CIRCUIT

* R1 has a value of 60 Ω with model RMOD: R1 1 2 RMOD 6 * Inductor of 1.5 mH with an initial current of 3 A and model name LMOD: L1 2 3 LMOD 1.5MH IC=3A * Capacitor of 2.5 µF with an initial voltage of 4 V and model name CMOD: C1 3 0 CMOD 2.5UF IC=4V R2 3 0 RMOD 2 * Model statements for resistor, inductor, and capacitor: .MODEL RMOD RES (R=1 TC1=0.02 TC2=0.005) .MODEL CMOD CAP (C=1 VC1=0.01 VC2=0.002 TC1=0.02 TC2=0.005) .MODEL LMOD IND (L=1 IL1=0.1 IL2=0.002 TC1=0.02 TC2=0.005) * The operating temperature in 50°C. .TEMP 50 ANALYSIS


* Transient analysis from 0 to 1 ms with a 5.µs time increment and using initial conditions (UIC). .TRAN 5US 1MS UIC * Plot the results of transient analysis with the voltage at nodes 3 and 1. .PLOT TRAN V(3) V(1) .PROBE V(3) V(1) .END The results of the simulation that are obtained by Probe are shown in Figure 5.9. Passive Elements 107 5.5.1 LINEAR MAGNETIC CIRCUITS The symbol of mutual coupling is K. The general form of coupled inductors is K<name> L<(first inductor) name> L<(second inductor) name> + <(coupling) value> For linear coupled inductors, K<name> couples two or more inductors. <(cou- pling) value> is the coefficient of coupling, k. The value of coefficient of coupling must be greater than 0 and less than or equal to 1: 0 < k ≤ 1. The inductors can be coupled in either order positively or negatively as shown in Figure 5.10(a) and Figure 5.10(b), respectively. In terms of the dot convention FIGURE 5.9 Transient response for Example 5.1. FIGURE 5.10 Coupled inductors. (a) Positively coupled, (b) negatively coupled, (c) single- phase transformer. Time 0 s 0.1 ms 0.2 ms 0.3 ms 0.4 ms 0.5 ms 0.6 ms 0.7 ms 0.8 ms 0.9 ms 1 ms V(3) V(1) 0 V 5 V 10 V 15 V Output voltage Step input voltage • • • • • • • • NP+ M NP− v1 L1 L2 L1 L1 L2 L3 L2 i1 i2 Mi1 i2 NS+ NS− 1 2 3 4 3 5 4 1 2 + − v2 + − v1 + − v2 + − v1 vs1 + + − vs2 + −− (a) Positively coupled (b) Oppositely coupled (c) Single-phase transformer 110 SPICE for Power Electronics and Electric Power, Second Edition from 60 to 120 Hz with a linear increment. The total number of points in the sweep is 2. The coefficient of coupling for the transformer is 0.999. SOLUTION It is important to note that the primary and the secondary have a common node. Without this common node, PSpice will give an error message because there is no DC path from the nodes of the secondary to the ground. The PSpice schematic is shown in Figure 5.12(a). K-linear couples L1 and L2 with a coupling of 0.9999. The voltage marker displays the output waveforms in Probe at the end of the simulation. The PSpice plot of the input and output voltages are b of the high-frequency value of 120 V. The circuit file contains the following statements: FIGURE 5.12 Example 5.2 Coupled linear inductors SOURCE
* Input voltage is 120 V peak and 0° phase for ac analysis: VIN 1 0 AC 120V CIRCUIT

R1 5 2 0.5 * A dummy voltage source of VY = 0 is added to measure the load current: VY 1 5 DC 0V * The dot convention is followed in inductors L1 and L2: L1 2 0 1mH L1 0 4 0.5mH * Magnetic coupling coefficient is 0.999. The order of L1 and L2 is • • • • • ••• • • 1 0 0 V 5 2 4 6 7 Vy = 120 sin ωt vovin iL RL 0 V 0.5 Ω 0.5 Ω 150 Ω 0.5 mH 0.5 mH R1 Vx R2 K 0.9999 L1 L2 + + − − shown in Figure 5.13(b). The break frequency is f = 79.81 Hz at 84.906 V (70.7%) Passive Elements 111 The transformer is considered to be linear and its inductances remain constant. The results of the simulation, which are stored in output file EX5.2.OUT, are Note: PSpice (that is, the net list using PSpice A/D) is better suited to printing the magnitudes and phases of voltages. Schematics is, however, better suited to drawing the schematics and plots of voltages and currents. 5.5.2 NONLINEAR MAGNETIC CIRCUITS For a nonlinear inductor, the general form is K<name> L<(inductor) name> <(coupling) value> + <(model) name> [(size) value] For an iron-core transformer, k is very high, greater than 0.999. The model type name for a nonlinear magnetic inductor is CORE, and the model parameters and defaults to 1. It represents the number of lamination layers, so that only one model statement can be used for a particular lamination type of core. * not significant. K12 L1 L2 0.999 R2 4 6 0.5 RL 6 7 150 * A dummy voltage source of VX = 0 is added to measure the load current: VX 7 0 DC 0V ANALYSIS


* Ac analysis where the frequency is varied linearly from 60 Hz to 120 Hz with two points: ACLIN260HZ120HZ * Print the magnitude and phase of output current. Some versions of * Pspice and SPICE do not permit reference to currents through resistors [e.g., IM(RL), IP(RL)]. .PRINT AC IM(VY)IP(VY)IM(RL)IP(RL) ; Prints to the output file .END FREQ IM(VY) IP(VY) IM(RL) IP(RL) V(4) V(2) 6.000E+01 1.915E+02 –3.699E+01 3.389E-01 –1.271E+02 5.100E+01 7.220E+01 1.200E+02 1.325E+02 –5.635E+01 4.689E-01 –1.465E+02 7.056E+01 9.989E+01 are shown in Table 5.5. [(size) value] scales the magnetic cross section 112 SPICE for Power Electronics and Electric Power, Second Edition If the <(model) name> is specified, the mutual coupling inductor becomes a nonlinear magnetic core and the inductor specifies the number of turns instead of the inductance. The list of the coupled inductors may be just one inductor. The magnetic core’s B − H characteristics are analyzed using the Jiles–Ather- ton model [2]. be as follows: * Inductor L1 of 100 turns: L1 1 2 100 * Inductor L2 of 10 turns: FIGURE 5.13 PSpice schematic for Example 5.2. (a) Schematic, (b) frequency responses. L2 0.5 mH Vy 0 V + − Vin ACMAG = 120 V ACPHASE = 0 +− RL 150 R2 0.5 6 V Vx 0 V + − 7 1 5 V R1 0.5 2 K K1 COUPLING = 0.999K_Linear L1 L2 L1 1 mH 4 (a) Frequency 1.0 Hz 10 Hz 100 Hz 1.0 KHz V(R1:2) V(L2:2) 0 V 40 V 80 V 120 V (79.811, 84.906) Input voltage Output voltage (b) If the inductors of Figure 5.10(a) use the nonlinear core, the statements would Passive Elements 115 L2 2 0 1000 R2 2 0 1000 ; Load resistance * Coupled inductors with k = 0.999 and model CMOD: K12 L1 L2 0.9999 CMOD * Model parameters for CMOD: .MODEL CMOD CORE (AREA=2.0 PATH=62.73 GAP=0.1 MS=1.6E+6 + A = 1E + 3C = 0.5K = 1500) ANALYSIS


* Transient analysis from 0 to 3 s in steps of 0.05 s: .TRAN 0.05S 3S .PROBE .END FIGURE 5.15 PSpice schematic for Example 5.3. (a) Schematic, (b) instantaneous input current and flux density. IN+− L2 400 L1 800 RL 1 k 21 K K12 COUPLING = 0.9999 K_CMOD L2L1 (a) 20 A 20 K 0 SEL» 0 A −20 A −20 K 0 S 1.0 S Time 2.0 S 3.0 S I (IN) B (K12) Input current Flux density versus time (b) 116 SPICE for Power Electronics and Electric Power, Second Edition The B−H characteristic obtained by Probe is shown in Figure 5.16. The plot of the flux density, B(K12), against the magnetic field, H(K12), is shown in Figure 5.16, which gives Bmax = 178.57 and Hmax = 18.61 k. Note that by using the Probe menu, the x axis has been changed to H(K12). EXAMPLE 5.4 FINDING THE OUTPUT VOLTAGE AND CURRENT OF A COUPLED- INDUCTOR WITH A NONLINEAR MAGNETIC CORE The coupled inductor in Example 5.2 is replaced by a nonlinear core with the B–H of the inductors are L1 = 200 turns, L2 = 100 turns, and k = 0.9999. The input voltage FIGURE 5.16 Typical B−H characteristic. FIGURE 5.17 Circuit with nonlinear coupled inductors. H(K12) −200 −100 0 100 200 B(K12) −20 K 0 20 K B–H characteristic (178.571, 18.610 K) • • • • • • ••• • • 1 5 2 4 6 7 Vy vs vo is iL RL 0 V 0 V 0.5 Ω 0.5 Ω 150 Ω 800 turns 400 turns R1 Vx R2 K 0.9999 L1 L2 + + + − − − characteristic shown in Figure 5.6. This is shown in Figure 5.17. The parameters Passive Elements 117 is vs = 170 sin(2π × 60t). Plot the instantaneous values of the secondary voltage and current from 0 to 35 msec with a 10-µsec increment. The results should be available for display and as hard copy by using Probe. The model parameters of the core are AREA = 6.0, PATH = 82.73, GAP = 0.1, MS = 1.6E + 6, ALPHA = 1E − 3, A = 1E + 3, C = 0.5, and K = 1500. SOLUTION The primary and the secondary have a common node. Without this common node, PSpice will give an error message because there is no DC path from the nodes of K-break couples L1 and L2 with a coupling of 0.9999 and its model parameters are specified in K_CMOD as shown in Figure 5.18(b). The voltage and current markers display the output waveforms in probe at the end of the simulation. The circuit file contains the following statements: Example 5.4 Nonlinear coupled inductors SOURCE
* Input sinusoidal voltage of 170 V peak and 0° phase: VS 1 0 SIN (0 170V 60HZ) CIRCUIT

* A dummy voltage source of VY = 0 is added to measure the load current: VY 1 5 DC 0V R1 5 2 0.5 * Inductors represent the number of turns: L1 2 0 800 L2 4 0 400 * Coupled inductors with k = 0.9999 and model CMOD: K12 L1 L2 0.9999 CMOD * Model parameters for CMOD: .MODEL CMOD CORE (AREA=2.0 PATH=62.73 GAP=0.1 MS=1.6E+6 + A=1E+3 C=0.5 K=1500) R2 4 6 0.5 RL 6 7 150 * A dummy voltage source of VX = 0 is added to measure the load current: VX 7 0 DC 0V ANALYSIS


* Transient analysis from 0 to 35 ms with a 100-µs increment: .TRAN 10US 35MS * Print the output voltage and current. .PRINT TRAN V(4) I(VX) ; Prints in the output file .PROBE ; Graphics post-processor .END 120 SPICE for Power Electronics and Electric Power, Second Edition • Voltage-controlled switches • Current-controlled switches • Time-dependent switches Note: The voltage- and current-controlled switches are not available in SPICE2. However, they are available in SPICE3. FIGURE 5.20 Transmission line. (a) Transmission line, (b) coaxial line. FIGURE 5.21 Switch with a variable resistance. (a) Switch, (b) on state, (c) off state. + − + − • • • • • • • • • 1 3 42 1 2 4 0 3 Z0 Z0I3 Delayed V3−V4 Delayed I1 Delayed V1−V2 Delayed (a) Transmission line (a) Coaxial line Inner shell, T1 Outer shell, T2 N+ N− N+ N− N+ N− S1 Ron Roff (a) Switch (b) On-state (b) Off-state Passive Elements 121 5.7.1 VOLTAGE-CONTROLLED SWITCH The symbol of a voltage-controlled switch is S. Its name must start with S, and it takes the general form S<name> N+ N− NC+ NC− SNAME N+ and N− are the two nodes of the switch. The current is assumed to flow from N+ through the switch to node N−. NC+ and NC− are the positive and SNAME is the model name. The resistance of the switch varies depending on the voltage across the switch. The type name for a voltage-controlled switch is VSWITCH, and the model parameters are shown in Table 5.6. The PSpice schematic is shown in Figure 5.22(b). The voltage-controlled switch statement is S1 6 5 4 0 SMOD .MODEL SMOD VSWITCH (RON=0.5 ROFF=10E+6 VON=0.7 VOFF=0.0) FIGURE 5.22 Voltage-controlled switch. (a) Positive and negative nodes, (b) PSpice schematic. TABLE 5.6 Model Parameters for Voltage-Controlled Switch Name Meaning Unit Default VON Control voltage for on-state V 1.0 VOFF Control voltage for off-state V 0 RON On resistance W 1.0 ROFF Off resistance W 106 NC+ N+ N−NC− Vg Rg S1 K1 + − • • (a) Equivalent circuit S1 Sbreak + − − + (b) 122 SPICE for Power Electronics and Electric Power, Second Edition Note the following 1. RON and ROFF must be greater than zero and less than 1/GMIN. The value of GMIN can be defined as an option as described in .OPTIONS command in Section 6.5. The default value of conductance, GMIN, is 1E − 12 Ω−1. 2. The ratio of ROFF to RON should be less than 1E + 12. 3. The difficulty due to the high gain of an ideal switch can be minimized by choosing the value of ROFF to be as high as permissible and that of RON to be as low as possible compared with other circuit elements, within the limits of allowable accuracy. EXAMPLE 5.5 STEP RESPONSE WITH A VOLTAGE-CONTROLLED SWITCH is vs = 200 sin(2000πt). Plot the instantaneous voltage at node 3 and the current through the load resistor RL for a duration of 0 to 1 msec with an increment of 5 µsec. The model parameters of the switch are RON = 5M, ROFF = 10E + 9, VON = 25M, and VOFF = 0.0. The results should be available for display by using Probe. SOLUTION voltage source E1 is set to 0.1. The voltage and current markers display the output waveform in probe at the end of the simulation. The input voltage is specified by a sinusoidal source. The breakout voltage controlled switch (S1) is used to specify the switch model SMOD as shown in Figure 5.24(b) and its model parameters are RON = 5M, ROFF = 10E+9, VON = 25M, and VOFF = 0. The voltage source VX = 0 V is inserted to monitor the output current. The listing of the circuit file is as follows: Passive Elements 125 of 1 µsec. The model parameters of the switch are RON = 1E + 6, ROFF = 0.001, ION = 1MA, and IOFF = 0. The results should be available for display by using Probe. SOLUTION display the output waveforms in Probe at the end of the simulation. The initial voltage on the capacitor C1 specifies the input source. The breakout current-controlled switch (W1) is used to specify the parameters of the switch model WMOD as shown in Figure 5.28(b) and its model parameters are ION = 1MA, IOFF = 0, RON = 1E + 6, and ROFF = 0.01. FIGURE 5.26 Current-controlled switch. (a) Equivalent circuit, (b) PSpice schematic. TABLE 5.7 Model Parameters for Current-Controlled Switch Name Meaning Unit Default ION Control current for on-state A 1E−3 IOFF Control current for off-state A 0 RON On resistance W 1.0 ROFF Off resistance W 106 FIGURE 5.27 Circuit with a current-controlled switch. NC+ N+ N−NC− VN W1 M2 (a) Equivalent circuit W1 Wbreak + − Vx C1 40 μF 1 2 200 V + – 0V 0 W1 3 L 50 μH • • • • • 126 SPICE for Power Electronics and Electric Power, Second Edition The voltage source VX = 0 V is inserted to monitor the controlling current. The listing of the circuit file is as follows: FIGURE 5.28 PSpice schematic for Example 5.6. (a) PSpice schematic, (b) specifications of ISWITCH. Example 5.6 Current-controlled switch SOURCE

* C1 of 40 µF with an initial voltage of 200 V: C1 1 0 4 0UF IC=200 * Dummy voltage source of VX = 0: VX 2 1 DC 0V * Current-controlled switch with model name SMOD: W1 2 3 VX SMOD * Model parameters: .MODEL SMOD ISWITCH (RON=1E+6 ROFF=0.001 ION=1MA IOFF=0) L1 3 0 50UF CIRCUIT


* Transient analysis with UIC (use initial condition) option: .TRAN 1US 160US UIC * Plot the voltage at node 1 and the current through VX. .PLOT TRAN V(1) I(VX) ; On the output file .PROBE ; Graphics post-processor .END L1 50 uH V 2 1 I −+ WMOD W1 3 Vx 0 V +− C1 40 uF 200 V (a) (b) Passive Elements 127 The results of the simulation that are obtained by using Probe are shown in Figure 5.29. Switch S1 acts as diode and allows only positive current flow. The initial voltage on the capacitor is the driving source. 5.7.3 TIME-DEPENDENT SWITCHES PSpice schematics support two types of time-dependent switches: • Time-dependent close switch • Time-dependent open switch The closing or the opening time and the transition time of the switch are specified by the switch parameters as shown in Table 5.8. FIGURE 5.29 Transient response for Example 5.6. TABLE 5.8 Model Parameters for Close/Open Switch Name Meaning Default Tclose/Topen Time at which switch begins to close/open 0 Ttran Time required to switch states from off state to on state (must be realistic, not 0) 1 µsec Rclosed Closed-state resistance 10 mΩ Ropen Open-state resistance (Ropen/Rclosed < 1E+10) 1 MΩ Time 0 s 40 us 80 us 120 us 160 us I(L1) V(Vx:−) −200 0 200 Switch current Capacitor voltage 130 SPICE for Power Electronics and Electric Power, Second Edition L Inductor L<name> N+ N− LNAME LVALUE IC=10 K Linear mutual inductors (transformer) K<name> L<(first inductor) name> L<(second inductor)name> <value>] K Nonlinear inductor K<name> L<(inductor) name> <(coupling value> + <(model) name> [(size) value] R Resistor R<name> N+ N− RNAME RVALUE S Voltage-controlled switch S<name> N+ N− NC+ NC− SNAME FIGURE 5.33 PSpice schematic for discharging an RC Circuit. (a) PSpice schematic, (b) output voltage at switch transition (off). Vin T3 = 1 s T2 = 1 ns T1 = 0 V1 = 0 V2 = 1 V V3 = 1 V +− R1 10 C1 2 uF V U1 TOPEN = 20 us TTRAN = 2 u 1 2 (a) Time 0 s 50 us 100 us 150 us V(R1:2) 0 V 0.5 V 1.0 V Discharging a capacitor (b) Passive Elements 131 T Lossless transmission lines T<name> NA+ NA− NB+ NB− Z0=<value> [TD=<value>] + [F=<value> NL=<value>] W Current-controlled switch W<name> N+ N− VN WNAME Suggested Reading 1. D.C. Jiles and D.L. Atherton, Theory of ferromagnetic hysteresis, Journal of Magnetism and Magnetic Material, Vol. 61, No. 48, 1986, pp. 48-60. 2. M.H. Rashid, Introduction to PSpice Using OrCAD for Circuits and Electronics, 3rd ed., Englewood Cliffs, NJ: Prentice-Hall, 2003 chap. 4. 3. M.H. Rashid, SPICE For Power Electronics and Electric Power. Englewood Cliffs, NJ: Prentice-Hall, 1993. 4. PSpice Manual, Irvine, CA: MicroSim Corporation, 1992. 5. J.F. Lindsay and M.H. Rashid, Electromechanics and Electrical Machinery. Engle- wood Cliffs, NJ: Prentice-Hall, 1986. PROBLEMS Write the PSpice statements for the following circuits. If applicable, the output should also be available for display and as hard copy by using Probe. 5.1 A resistor R1, which is connected between nodes 3 and 4, has a nominal value of R = 10 kΩ. The operating temperature is 55°C, and it has the form 5.2 A resistor R1, which is connected between nodes 3 and 4, has a nominal value of R = 10 kΩ. The operating temperature is 55°C, and it has the form 5.3 A capacitor C1, which is connected between nodes 5 and 6, has a value of 10 pF and an initial voltage of −20 V. R R T T T T 1 0 0 2 1 0 2 0 002 = + − + − [ . ( ) . ( ) ] R R T T1 4 51 01 0= × −. . ( ) 132 SPICE for Power Electronics and Electric Power, Second Edition 5.4 A capacitor C1, which is connected between nodes 5 and 6, has a nominal value of C = 10 pF. The operating temperature is T = 55°C. The capacitance, which is a function of its voltage and the operating temperature, is given by 5.5 An inductor L1, which is connected between nodes 5 and 6, has a value of 0.5 mH and carries an initial current of 0.04 mA. 5.6 An inductor L1, which is connected between nodes 3 and 4, has a nominal value of L = 1.5 mH. The operating temperature is T = 55°C. The inductance is a function of its current and the operating temperature, and it is given by 5.7 L1 = 1.2 mH and L2 = 0.5 mH. The coefficients of coupling are K12 = K21 = 0.999. 5.8 time increment of 25 µsec. The output voltage is taken across the capacitor. Use Probe for graphical output. 5.9 5.10 with a decade increment and 10 points per decade. The output voltage is taken across the capacitor. Print and plot the magnitude and phase angle of the output voltage. Assume a source voltage of 1 V peak. C C V V T T T 1 2 0 1 0 01 0 002 1 0 03 0 05 = + + × + − + − ( . . ) [ . ( ) . ( T0 2) ] L L I I T T T 1 2 0 1 0 01 0 002 1 0 03 0 05 = + + × + − + − ( . . ) [ . ( ) . ( T0 2) ] Passive Elements 135 5.17 currents for five cycles of the switching period with a time increment of 10 µsec. The model parameters of the voltage-controlled switches are RON = 0.025, ROFF = 1E + 8, VON = 0.05, and VOFF = 0. The output should also be available for display and as hard copy by using Probe. FIGURE P5.13 Three-phase transformer. • • • • • • • • • • • • R1 R2 L1 RL1 L3 L4 L6 L5 L2 vp vP 0.5 Ω 0.5 Ω 150 Ω RL2 150 Ω RL3 150 Ω R3 = 0.5 Ω + + − vs + − − (a) Primary (b) Secondary 136 SPICE for Power Electronics and Electric Power, Second Edition FIGURE P5.17 Switching circuit. Vs Vg1 S1 S2 + − 20 V 5 0 0.5 1 1.5 t(ms) Vg2 5 0 0.5 1 1.5 t(ms) 50 Ω 15 mH (a) Circuit (b) Controlling switch voltages • •