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

Size: px

Start display at page:

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

Egbert Marshall
6 years ago
Views:

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

2 Models and Devices A model defines the electrical behavior of a part. Models can be defined either as parameters set or by subcircuit netlist. Parameters sets are usually used to describe the behavior of builtin models by setting the model parameters (all or partial set) to new values using the PSpice.MODEL syntax. Example:.MODEL <name> type [parameters] For non built-in models, the parts description is done by implementing macro-models as subcircuits. Example:.SUBCKT <name> <pinout> <parameters> [2]

3 : Outline 1. Models a. How models are organized (libraries). b. Global and local models c. How to create and edit models (Model editor). d. Symbols. 2. Analog Devices a. Independent sources. b. Passive components. c. Dependent sources. d. Diode. e. Bipolar Junction Transistor BJT. [3]

4 How models are organized Device model and subcircuit definitions are saved in.lib files libraries. Model libraries are text files that contain information of the model parameters and/or the model connections. Most libraries contain parts of similar type. For instance, bipolar.lib --- BJT s models [4]

5 Global and local models Local models: Apply to current design. Created either manually and configured or by Capture, whenever a built-in model is modified. Global models: Apply to all the designs. To view the library list configured for simulation: Simulation settings>configuration files global local [5]

6 How to create and edit models Ways to create/edit models: Model parts from datasheet: Template-based modeling. Use manufacturer data to fit the model parameters. 2.PSpice command syntax: Define model parameters and subcircuit connections using the text editor. 3.Setup equivalent symbols. Describe part s behavior using subcircuit netlist, determine hierarchical levels in the design. [6]

Here you select the part type you want to model. 3.

7 Model parts using manufacturers data 1. Open the model editor start new model. 2. Enter model s name and select template. Here you select the part type you want to model. 3. Extract model parameters fit your desired model. Insert data For full details of how to fit the model refer PSpice user s guide. \\doc\pspug.pdf Model parameters [7]

Create Netlist Command 1. Sketch your design, assign names for nodes. 2. From Tools manu, select Create Subcircuit>open the PSpice dialog box. 3. Create your netlist. View example: Creating.

8 Create Netlist Command 1. Sketch your design, assign names for nodes. 2. From Tools manu, select Create Subcircuit>open the PSpice dialog box. 3. Create your netlist. View example: Creating.SUBCKT to a simplified OPAMP demo5, view clip: wav1.avi draw, wav1b.avi create.subckt in+ E2 IN+ OUT+ IN- OUT- EVALUE V(%IN+, %IN-) in- R1 1k C1 1u E1 IN+ OUT+ IN- OUT- EVALUE V(%IN+, %IN-)*1k out Simplified OPAMP Subcircuit created [8]

9 Symbols A symbol that is used for simulation: Links to the simulation model. Translates the netlist and pins connection. To create a symbol you need to: Start new parts library (.OLB). Select new>part. Attach implementation type in case you want the symbol to run is PSpice you need to select: PSpice model. Draw the desired shape, assign external pins (names and numbers). Define the PSpiceTemplate. View clip: wav2.avi - Creating symbol to the simplified OPAMP. Run the modeled device on demo6. (wav3a.avi) [9]

10 PSpiceTemplate Defines the PSpice syntax for the netlist entery. During netlist operation, Capture replace the actual pins with values from the PSpiceTemplate, then writes the translated statement to the netlist. PSpiceTemplate syntax: %<pin_name> R2 1k U1 1Vac Vdc V1 1 R1 in+ 3 2 out in- 1k MY_OPAMP PSpiceTemplate = X^@REFDES %in+ %in- For full details view PSpice user s guide. \\doc\pspug.pdf [1]

11 Analog Devices PSpice supports many types of analog devices, including sources and subcircuit designs. Devices are categorized into device types which include one or more model descriptions (e. g. the BJT model). The component description include: 1. Device declaration. 2. Model statement and parameters. 3. Electrical model in terms of schematic form and mathematical description. In the following, we will describe the basics in PSpice modeling for some popular components. For the full component description refer to PSpice reference manual. [11]

12 Independent Sources Description: A voltage/current source. Positive current flows from (+) to (-). Several types of sources are represented by this device just by specifying in the general form. General form: I/V<name> <(+) node> <(-) node> [ (DC) <value>] [ AC <mag> (phase)] [transient spec.] Examples: DC Voltage (5V): VDC AC (small-sig.): VAC 7 55 AC 1 Pulse V source: VPULSE 1 2 PULSE(V1 V2 TD TR TF PW PER) Sin V source: V SIN(OFF AMPL FREQ) V1 = V2 = TD = TR = TF = PW = PER = VPULSE V7 V4 Vdc VDC Adc IDC I1 1Vac Vdc VAC V5 1Aac Adc IAC I2 VOFF = VAMPL = FREQ = VSIN V6 IOFF = IAMPL = FREQ = ISIN I4 I1 = I2 = TD = TR = TF = PW = PER = I5 IPULSE [12]

13 General form: Passive Components - Resistor R<name> <(+) node> <(-) node> [model name] <value> [TC = <TC1> (,<TC2>)] Examples: Model form: R K Rf RMOD 1K Rtpm meg TC= 1m, -5m.MODEL <model name> RES [parameters] For Capture R part, the value is determined by the VALUE property. In case you need to assign tolerance use RBREAK Breakout parts: Designed for customizing model parameters. Useful for setting up tolerances (DEV or LOT). [13]

14 Passive Components - Resistor Parameters Description R Resistance multiplier TC1 Linear temp. coefficient TC2 Quadratic temp. coefficient TCE Exponential temp. coefficient T_ABS Absolute temp. T_MEASURED Measured temp. T_REL_GLOBAL Relative to current temp. Units C -1 C -2 %/ C C C C Defau lt 1 Equations: TEC specified: <Value> R 1.1 TCE(T-Tnom) TEC not specified:<value> R (1+TC1 (T-Tnom)+TC2 (T-Tnom) 2 ) Noise spectral power density per unit BW: i 2 = 4 k T/R [14]

15 Passive Components - Capacitor General form: C<name> <(+) node> <(-) node> [model name] <value> [IC = <initial voltage>] Examples: Model form: C u(F) Cf CMOD 1n C e-8 IC= 5(V).MODEL <model name> CAP [parameters] [15]

16 Passive Components - Capacitor Parameters Description Units TC1 Linear temp. coefficient TC2 Quadratic temp. coefficient T_ABS Absolute temp. T_REL_GLOBAL Relative to current temp. VC1 Linear voltage coefficient VC2 Quadratic voltage coefficient C -1 C -2 C C V -1 V -2 Defau lt Equations: If a model is specified, the capacitance value will thus be: <Value> C (1+VC1 V+VC2 V 2 )(1+TC1 (T-Tnom)+TC2 (T-Tnom) 2 ) Noise: Capacitor does not have a noise model. [16]

17 Passive Components - Inductor General form: L<name> <(+) node> <(-) node> [model name] <value> [IC = <initial current>] Examples: Model form: L u(H) Lin 1 7 LMOD.1m L e-6 IC=.25(A).MODEL <model name> IND [parameters] Inductor as winding: General form: L<name> <(+) node> <(-) node> <TURNS> [RESIS = value] [IC=value] Combining with a coupling element/ core model, the model defines an inductor which its value depends on the number of turns. [17]

18 Passive Components - Inductor Parameters Description L Inductance multiplier IL1 Linear current coefficient IL2 Quadratic current coefficient TC1 Linear temp. coefficient TC2 Quadratic temp. coefficient T_ABS Absolute temp. T_MEASURED Measured temp. T_REL_GLOBAL Relative to current temp. Units A -1 A -2 C -1 C -2 C C C Defau lt 1 Equations: If a model is specified, the inductance value will thus be: <Value> L (1+IL1 I+IL2 I 2 )(1+TC1 (T-Tnom)+TC2 (T-Tnom) 2 ) No noise model. [18]

19 Dependent Sources General form: E/G<name> node1 node2 cont1 cont2 gain E/G<name> <+node> <-node> <+cont> <-cont> <gain> E/G<name> <+node> <-node> POLY (<value>) <+cont> <-cont> <polynomial coefficient value> E/G<name> <+node> <-node> VALUE = (<Expr.>) E/G<name> <+node> <-node> TABLE {<Expr.>} < <in_val>,<out_val> > Examples: E Enon 1 2 POLY(2) Erect 3 9 VALUE = {abs(2*sin(6.28*1k*time))} [19]

20 Dependent Sources - POLY Basic SPICE polynomial expressions. PSpice allows controlled sources to be defined with a polynomial TF. For a VC-VS with the voltages V1, V2,, Vn, the output voltage is defined by the following: Vout = P + P1 V1 + P2 V2 + + Pn Vn + Pn+1 V1 V1 + Pn+2 V1 V2 + Pn+n V1 Vn + POLY syntax: <controlled source> <connection nodes> POLY(<dim>) <controlling in> <coefficients> [2]

21 Diode General form: D<name> <(+) node> <(-) node> <model name> [area value] Examples: Model form: D Dcut 4 8 DMOD D Dbreak.MODEL <model name> D [parameters] Anode Diode is modeled as an ohmic resistance is series with current source. The model defined by a set of equations which describe the diode behavior for several aspects: DC, (parasitic) Capacitance, Temperature and noise. Lets view the reference manual for details. RS I C Cathode [21]

22 General form: Bipolar Junction Transistor BJT Q<name> <collector> <base> <emitter> <model name> [area value] Examples: Model form: Q NPN_mot.MODEL <model name> NPN [parameters].model <model name> PNP [parameters] Collector BJT model is based on the Ebers-Moll model. The model defined by a set of equations for: DC, (parasitic) Capacitance, Temperature and noise. Many model parameters are used to define the model based on its equations. Base Rb 1k Cje Ibc2 Ibe2 Ibc1/BR Ibe1/BF RC Iepi (Ibe-Ibc)/Kqb RE Emitter [22]

23 Some model parameters: Bipolar Junction Transistor BJT Parameters Description Units Default BF Forward Beta 1 BR Reverse Beta 1 CJC Base-collector zero bias capacitance F IS Transport saturation current 1e-16 A N-C/E/F/R/S Emission coefficients R-B/C/E Base/Collector/Emitter ohmic resistance Lets view the reference manual for full details. [23]

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

Mor M. Peretz Power Electronics Laboratory Department of Electrical and Computer Engineering Ben-Gurion University of the Negev, ISRAEL [1] PSpice A/D simulation program allows to analyze electrical circuits