Mor M. Peretz Power Electronics Laboratory Department of Electrical and Computer Engineering Ben-Gurion University of the Negev, ISRAEL

Transcription

1 Mor M. Peretz Power Electronics Laboratory Department of Electrical and Computer Engineering Ben-Gurion University of the Negev, ISRAEL [1]

2 PSpice A/D simulation program allows to analyze electrical circuits containing combinations of analog and digital devices. Along with Orcad Schematics for design entry, PSpice becomes a software-based circuit board that you can test your design before approaching hardware Aac Adc I2 1 2 L1 {Lr} 1 C1 {Cr} V 2 1 R1 {R} 2-4 1Hz 1. KHz 1KHz 1KHz 1. MHz 1MHz DB(V(1)) Fr equency [2]

3 : Outline 1. File Types a. Files generated by OrCAD Capture. b. Files generated by PSpice. c. Directory structure of analog/mix signal projects. 2. Devices a. Passive components. b. Active and non-linear components Device modeling. c. Analog Behavioral Modeling. 3. Basic simulation types a. DC sweep and bias point. b. AC sweep c. Transient Analysis and Fourier components. d. Parametric sweep and performance analysis. [3]

4 File types In order to simulate a design, you need to provide PSpice information about the circuit components and connections, analysis type and parts models. This data comes in a file package called Project. Some files are generated by Capture, others by PSpice and some are defined by the user. Starting an analog design, the first file created is the project file (.OPJ) which contain data of the package structure. The circuit schematics is drawn using Capture and is saved in a design file (.DSN). [4]

5 Files generated by OrCAD Capture Netlist file (.NET) Contains a list of device names, values and their connections. 1 IOFF = IAMPL = {max} FREQ = {f} I1 1Aac Adc I2 1 V 2 L1 {Lr} 1 C1 {Cr} R1 {R} PARAMETERS: max = 1 f = 1k Cr = 1u Lr = 1u R = 1 VOFF = VAMPL = {max} FREQ = {f} 1Vac Vdc 2 V1 V2 3 V L2 1 2 {Lr} V 4 C2 1 2 {Cr} V 5 V R2 {R} V Demo1.zip [5]

6 Circuit file (.CIR) Files generated by OrCAD Capture Contains simulation type commands, all the netlists (links) and model information. [6]

7 Data file (.DAT) Files generated by PSpice Contains simulation results which can be displayed by PSpice plot. After PSpice displays the initial set of results, you can add waveforms and obtain post-simulation analyses Hz 1. KHz 1KHz 1KHz 1. MHz 1MHz DB(V(1)) Fr equency [7]

8 Output file (.OUT) Files generated by PSpice ASCII text file that contains: complete netlist, simulation commands, simulation results, warnings and errors. The output file is divided into section, each section is seperated by a banner displaying the date and time and the SPICE version used. First section: copy of input netlist and circuit files. Second section: initial solution. Check out demo1.zip \\tran.out or \\ac.out [8]

9 User-defined files Additional files that used for simulation are user defined, provide information about settings, probe etc. Markers file (.MRK) Contains information of the nodes assigned in schematics for measurments. Probe file (.PRB) Contains information of the waveformes viewed in the PSpice plot and other user defined measurements (Display control), axis, grid line properties etc. Model file/library (.LIB) Contains electrical definition of parts. PSpice uses this data to determine the part response to various inputs (static, dynamic). [9]

10 Directory structure of analog/mix signal projects Project directory <Project_Name> Capture 1 (and up) introduces a new directory structure. Design level, schematics level and the profile level are organized in their respective directories. In order to simulate projects created by older versions you need to convert your project when starting Capture..OPJ.DSN Design level <Project_Name>-PSpiceFiles.LIB SCHEMATIC1 Schematic level.sim.net Profile level <Simulation_name>.CIR.DAT.OUT.MRK.PRB [1]

11 Devices Passive components L uH C1 1n R1 1k V I R = = = L C V I di dt dv dt Components which are represented by their (know) relations. No model used for PSpice modeling. Selecting those devices from Breakout library will allow to use of parametric modeling such as tolerances. [11]

12 Active components Device modeling Devices that include gain and probably nonlinearities. Modeling of such devices is complicated and requires great effort (knowledge in math and physics is a must). Fortunately, the basic components are already modeled and the user only needs to define (or vary) the model parameters to fit the specific design. Q1 QbreakN D1 Dbreak Many manufacturers frequently provide data about the PSpice models of their devices in datasheets or supply a complete, ready-to-use models (.CIR or.lib files). Lets take a look at some basics in the basic models the p-n diode and BJT transistor. [12]

13 Diode Model (demo2.zip dc.sim) R S I C j I VD N V I e T = S,VD D VD + BV V IS e T,VD Current source definition > > V1 D1 Dbreak Is Saturation current N Emission coefficient VT = k T/q - thermal voltage K - Boltzmann s constant q - electron charge T Temperature ( K) 4. A 2. A A V. 2V. 4V. 6V. 8V 1. V I(D1) V_ V1 Diode I-V curves, varying N [13]

14 D1 Diode Model V1 Dbreak Diode model parameters used OrCAD Schematics circuit 5A A Reverse breakdown -5A -15V - 1V -5V V 5V I(D1) V_ V1 Diode I-V curves, full range [14]

15 Bipolar Junction Transistor model The model used in PSpice for the BJT is a modified version of the basic EM model. The complete model (of course) includes: Parasitic elements (resistances and capacitances), emission coefficients and many more!!! I E N α I I C I EO P P I B (demo2.zip dc_q.sim) α N I E I CO Basic Ebers-Moll model N I C 5Vdc V2 R1 {Rb} Q1 Qbreakn R2.1 R3.1 Vdc V3 2. A 1. A OrCAD Schematics circuit A BJT output curves, varying Rb Model parameters - check out demo2.lib -1.A V 1. V 2. V 3. V 4. V I(Q1:c) V_ V3 [15]

16 Bipolar Junction Transistor model Model example Q2N2222 discrete BJT (demo2.zip dc_q.sim) [16]

17 ABMs expression driven ( V(%IN1) +V(%IN2) +V(%IN3) ) / 3. Voltage source V + V 3 + V in1 in in 2 3 V out = (V(%IN1) +V(%IN2) +V(%IN3)) / 3. Current source V + V 3 + V in1 in in 2 3 I out = expression rows s Frequency dependent - VS V out = Vin s + 1 ABM3 In Schematics double click object to edit properties [17]

18 Expression Dependent sources E/GVALUE Allow to make flexible description of circuit components. Mathematical expressions are used to describe operation of a circuit segment. Example: Describe the operation of a bridge rectifier using EVALUE. E1 IN+ OUT+ IN- OUT- EVALUE V(%IN+, %IN-) G1 IN+ OUT+ IN- OUT- GVALUE V(%IN+, %IN-) D1 Dbreak D2 Dbreak V1 FREQ = {f} VAMPL = {ampl} VOFF = D3 Dbreak D4 Dbreak out_brg Bridge rectifier R1 1k e abs({ampl}*sin(6.28*{f}*time)) E1 out_abm IN+ OUT+ IN- OUT- EVALUE Using ABM R2 1k 1. V 5. V SEL>> V V( out _br g) 1V 5V Bridge rectifier ABM V 8. ms 8. 5ms 9. ms 9. 5ms 1. ms V( o u t _ a b m) Ti me [18]

19 Data driven dependent sources Example: use of ETABLE as an ideal OPamp. with power supply limitations R3 E2 G2 IN+ OUT+ IN- OUT- GTABLE V(%IN+, %IN-) TABLE = (-15,-15) (15,15) IN+ OUT+ IN- OUT- ETABLE V(%IN+, %IN-) TABLE = (-15,-15) (15,15) 1k 1Vac Vdc VOFF = VAMPL = 5 FREQ = {f} R4 V2 1k in_amp V5 E2 out_amp IN+ OUT+ IN- OUT- ETABLE V(%IN+, %IN-)*1k 2V V out = Expr. Table 16V SEL>> -2V 5. V V( out _amp) large-signal 12V V 8V small-signal 4V 1. Hz 1Hz 1Hz 1. KHz 1KHz 1KHz V( o u t _ a mp ) Fr equency -5.V s 2ms 4ms 6ms 8ms 1ms V( i n_amp) Ti me [19]

20 Frequency dependent sources Example: use of ELAPLACE to create a low-pass filter. E3 IN+ OUT+ IN- OUT- ELAPLACE V(%IN+, %IN-) XFORM = 1/s 1Vac Vdc V4 R5 1k out_rc C1.1u -5 SEL>> -1 DB( V( out _RC) ) 1Vac Vdc V3 E3 out_laplace IN+ OUT+ IN- OUT- ELAPLACE V(%IN+, %IN-) 1/(s+1) R6 1k Hz 1Hz 1Hz 1. KHz 1KHz 1KHz DB( V( out _l apl ace) ) Fr equency [2]

21 Frequency domain dependent sources Example: use of GFREQ to emulate high order resonant network (simplified piezoelectric model) 1Vac Vdc V2 1 R2 {r} L2 {L} C5 {Cin} -5 E4 IN+ OUT+ IN- OUT- GFREQ V(%IN+, %IN-) TABLE = (,,) (1Meg,-1,9) IN+ OUT+ IN- OUT- EFREQ V(%IN+, %IN-) TABLE = (,,) (1Meg,-1,9) G C2 {C} -1 1d DB(I(in)) DB(I(V2)) 1Vac Vdc in V V G1 V IN+ OUT+ IN- OUT- GFREQ V(%IN+, %IN-) d SEL>> - 1d 15Hz p(-i(in)) p(-i(v2)) Fr equency 25Hz [21]

22 DC Sweep Perform a DC sweep analysis on the circuit. DC sources, global parameters of model parameters can be used as the sweep source. To calculate the DC response of a given circuit, PSpice removes time from the design. This is accomplished by considering capacitors as open circuit and inductors as short circuit, and using only the DC values of sources. The simulator also uses the DC sweep algorithm to perform the bias point calculations in some cases such as small-signal analysis. How to setup a DC sweep: 1. Create new simulation Profile in Capture (for first time setup, one should enter profile name). 2. Select DC sweep as the analysis type. 3. Enter parameters and sweep range. [22]

23 DC Sweep Lets take a look at the example of the diode I-V characteristics: (demo2.zip dc.sim) Edit prof. Simulation profile name Create prof. Sweep source Range [23]

24 AC Analysis Performs a frequency response analysis by calculating the small-signal of the circuit to a combination of inputs using local linearization around the bias point. 1. Non-linear components such as dependent sources are converted into a combination of linear sources with respect to their bias point, then the simulator performs a linear small-signal analysis. 2. Since AC sweep is a linear analysis, PSpice calculates nodes values in terms of gain and phase. How local linearization of non-linear devices works: 1. Calculate bias point. 2. Compute the partial derivatives. 3. Each derivative is considered as a linear source. [24]

25 AC Analysis Example Analog Behavioral Model (demo4.zip) Dependent voltage source (EVALUE) feeds a passive RC network. The source output emulates a multiplication between the input and a constant. R R V 1 V 2 C - + V1b V 2 C 1Vac Vdc V1 E1 IN+ OUT+ IN- OUT- EVALUE 1*V(%IN+, %IN-) R1 1k out C1 1u + - V2b V 1 Linearized circuit Hz 1Hz 1KHz 1. MHz DB(V(out)) Fr equency Original circuit Small-signal response [25]

26 AC Analysis In this example we can see that this constant acts as an amplifier of the AC input. Small-signal response input with gain (K=1) 4 Small-signal response no gain (K=1) Hz 1Hz 1 KHz 1. MHz DB(V(out)) Fr equency Hz 1Hz 1 KHz 1. MHz DB(V(out)) Fr equency Note that once the circuit is linerized, the simulator shuts DC sources and perform a linear AC sweep. [26]

27 Simulation setup: AC Analysis 1. Create new simulation Profile. 2. Select AC sweep as the analysis type. 3. Enter parameters and sweep range. [27]

28 Transient Analysis Calculates the response of the circuit starting at TIME= up to a specified time. To start the transient simulation, PSpice calculates the bias point (as described for the DC sweep). Data of the bias point calculation is written into the output file. PSpice uses an adaptive time step to maintain accuracy. The time step increases or decreases according to the activity in a specific region. The maximal time step can be defined in the simulation profile, the default is 2% of the total run time specified. [28]

29 Example: Full bridge rectifier (demo3) Transient Analysis 1V out_brg D1 Dbreak D3 Dbreak V1 FREQ = {f} VAMPL = {ampl} VOFF = R1 1k V D2 Dbreak D4 Dbreak Schematic design - 1V 8. ms 8. 5ms 9. ms 9. 5ms 1. ms V( D1 : 1, D4 : 2 ) V( out _br g) Ti me Transient results [29]

30 Fourier components Calculates the DC and AC components of a waveform which results from the transient analysis. To ways to facilitate Fourier analysis: 1. Usint the Probe window, a FFT operation of the complete waveform (all the time span) is done. Its spectral content displayed. 2. Through the output file options in the simulation profile. The DC and AC components up to the n-th harmonic is calculated. The results (including Total Harmonic Distortion) can be viewed thru the output file. Note that this function uses only a portion of the waveform. Sampling interval = time step [3]

31 Transient Analysis - FFT Example: Full bridge rectifier (demo3) method 1: FFT button Input signal pure sine Output signal AC components [31]

32 Fourier components Example: Full bridge rectifier (demo3) method 2: D1 Dbreak D3 Dbreak out_brg V1 FREQ = {f} VAMPL = {ampl} VOFF = R1 1k D2 Dbreak D4 Dbreak [32]

33 Parametric Sweep Performs multiple runs of a standard analysis where in each run a global/model parameter or a component value is varied. This is the equivalent of simulating the same circuit several times for a swept parameter. When the simulation is complete. A list of all runs apear. Using Performance Analysis, you can specify measurements as a function of the sweep parameter. Example: Performing AC sweep on a series and parallel RLC circuits fed by a sinusoidal voltage/current source, by considering the frequency as a global paraneter. IOFF = IAMPL = {max} FREQ = {f} I1 1Aac Adc I2 1 2 L1 {Lr} 1 1 C1 {Cr} 2 1 R1 {R} 2 VOFF = VAMPL = {max} FREQ = {f} 1Vac Vdc 2 V1 V2 3 L2 1 2 {Lr} C {Cr} (demo1) R2 {R} [33]

34 Example, cont. Parametric Sweep Results for parallel circuit 1-1 4K 8K 12K Max_XRange( V( 1),. 5m, 1m) f 1V 5V Performance analysis SEL>> V s. 5ms 1. ms... Max(V(1)) Ti me [34]

35 Parametric Sweep Goal functions Example: express the 3-dB bandwidth of a parallel RLC circuit as a function of the circuit resistance. Using AC sweep and considering {R} as the global parameter, we use the 3-dB bandwidth goal function which defined in PSpice. 8 2K 4 AC response multiple sweeps Performance Analysis 1K -4 1Hz 1. KHz 1 KHz 1KHz 1. MHz 1MHz... DB(V(1)) Fr equency. 2K. 4K. 6K. 8K 1. K 1. 2K Bandwi dt h_bandpass_3db( V( 1) ) R [35]