Rollins, J.G., Bendix, P. " Computer Software for Circuit Analysis and Design The Electrical Engineering Handbook Ed. Richard C. Dorf Boca raton crc Press llc. 2000
Rollins, J.G., Bendix, P. “Computer Software for Circuit Analysis and Design” The Electrical Engineering Handbook Ed. Richard C. Dorf Boca Raton: CRC Press LLC, 2000
13 Computer Software for Circuit analysis and Design gregory rollins uction. DC(Steady-State) Analysis. AC Analysis. Transient Process and device simulation Process simulation associates. Inc. Peter Bendix 13.2 Parameter Extraction for Analog Circuit Simulation Introduction. MOS DC Models. BSIM Extraction Strategy in LSI Logic Corp 13.1 Analog circuit Simulation . Gregory rollins ntroduction Computer-aided simulation is a powerful aid during the design or analysis of electronic circuits and semicon ductor devices. The first part of this chapter focuses on analog circuit simulation. The second part covers simulations of semiconductor processing and devices. While the main emphasis is on analog circuits, the same simulation techniques may, of course, be applied to digital circuits(which are, after all, composed of analog circuits). The main limitation will be the size of these circuits because the techniques presented here provide a very detailed analysis of the circuit in question and, therefore, would be too costly in terms of computer resources to analyze a large digital system The most widely known and used circuit simulation program is SPICE(simulation program with integrated circuit emphasis). This program was first written at the University of California at Berkeley by Laurence Nagel in 1975. Research in the area of circuit simulation is ongoing at many universities and industrial sites. Com- small personal computers to large mainframes. a list of some commercial simulator vendors can be foud 3 mercial versions of SPICE or related programs are available on a wide variety of computing platforms, fre the Appendix. It is possible to simulate virtually any type of circuit using a program like SPICE. The programs have built- in elements for resistors, capacitors, inductors, dependent and independent voltage and current sources, diodes, MOSFETS, JFETS, BJTs, transmission lines, transformers, and even transformers with saturating cores in some versions. Found in commercial versions are libraries of standard components which have all necessary The material in this chapter was published by CRC Press in The Circuits and Filters Handbook, Wai-Kai Chen Ed,1995. c 2000 by CRC Press LLC
© 2000 by CRC Press LLC 113 Computer Software for Circuit Analysis and Design 13.1 Analog Circuit Simulation Introduction • DC (Steady-State) Analysis • AC Analysis • Transient Analysis • Process and Device Simulation • Process Simulation • Device Simulation • Appendix 13.2 Parameter Extraction for Analog Circuit Simulation Introduction • MOS DC Models • BSIM Extraction Strategy in Detail 13.1 Analog Circuit Simulation J. Gregory Rollins Introduction Computer-aided simulation is a powerful aid during the design or analysis of electronic circuits and semiconductor devices. The first part of this chapter focuses on analog circuit simulation. The second part covers simulations of semiconductor processing and devices. While the main emphasis is on analog circuits, the same simulation techniques may, of course, be applied to digital circuits (which are, after all, composed of analog circuits). The main limitation will be the size of these circuits because the techniques presented here provide a very detailed analysis of the circuit in question and, therefore, would be too costly in terms of computer resources to analyze a large digital system. The most widely known and used circuit simulation program is SPICE (simulation program with integrated circuit emphasis). This program was first written at the University of California at Berkeley by Laurence Nagel in 1975. Research in the area of circuit simulation is ongoing at many universities and industrial sites. Commercial versions of SPICE or related programs are available on a wide variety of computing platforms, from small personal computers to large mainframes. A list of some commercial simulator vendors can be found in the Appendix. It is possible to simulate virtually any type of circuit using a program like SPICE. The programs have builtin elements for resistors, capacitors, inductors, dependent and independent voltage and current sources, diodes, MOSFETs, JFETs, BJTs, transmission lines, transformers, and even transformers with saturating cores in some versions. Found in commercial versions are libraries of standard components which have all necessary 1The material in this chapter was previously published by CRC Press in The Circuits and Filters Handbook, Wai-Kai Chen, Ed., 1995. J. Gregory Rollins Technology Modeling Associates, Inc. Peter Bendix LSI Logic Corp. 1
parameters prefitted to typical specifications. These libraries include items such as discrete transistors, op amps, phase-locked loops, voltage regulators, logic integrated circuits(ICs) and saturating transformer cores. Computer-aided circuit simulation is now considered an essential step in the design of integrated circuits, because without simulation the number of trial runs"necessary to produce a working IC would greatly increase the cost of the IC. Simulation provides other advantages, however: The ability to measure "inaccessible"voltages and currents. Because a mathematical model is used all voltages and currents are available. No loading problems are associated with placing a voltmeter or scilloscope in the middle of the circuit, with measuring difficult one-shot wave forms, or probing a microscopic die. Mathematically ideal elements are available. Creating an ideal voltage or current source is trivial with a simulator, but impossible in the laboratory. In addition, all component values are exact and no parasitic It is easy to change the values of components or the configuration of the circuit Unsoldering leads or designing IC masks are unnecessary. Unfortunately, computer-aided simulation has its own problems Real circuits are distributed systems, not the "lumped element models"which are assumed by simulators eal circuits, therefore, have resistive, capacitive, and inductive parasitic elements present besides the intended components. In high-speed circuits these parasitic elements are often the dominant perfor mance-limiting elements in the circuit, and must be painstakingly modeled. Suitable predefined numerical models have not yet been developed for certain types of devices or electrical phenomena. The software user may be required, therefore, to create his or her own models out of other models which are available in the simulator (An example is the solid-state thyristor which may be created from a NPN and PNP bipolar transistor. The numerical methods used may place constraints on the form of the model equations used The following sections consider the three primary simulation modes: DC, AC, and transient analysis. In each section an overview is given of the numerical techniques used. Some examples are then given, followed by brief discussion of DC (Steady-State) Analysis DC analysis calculates the state of a circuit with fixed (non-time varying) inputs after an infinite period of time. DC analysis is useful to determine the operating point(Q-point)of a circuit, power consumption, regulation and output voltage of power supplies, transfer functions, noise margin and fanout in logic gates, and many other types of analysis. In addition DC analysis is used to find the starting point for AC and transient analysis To perform the analysis the simulator performs the following steps: 1. All capacitors are removed from the circuit(replaced with opens) 2. All inductors are replaced with shorts 3. Modified nodal analysis is used to construct the nonlinear circuit equations. This results in one equation for each circuit node plus one equation for each voltage source. Modified nodal analysis is used rather than standard nodal analysis because an ideal voltage source or inductance cannot be represented using normal nodal analysis. To represent the voltage sources, loop equations(one for each voltage source or inductor), are included as well as the standard node equations. The node voltages and voltage source currents,then, represent the quantities which are solved for. These form a vector x. The circuit equations can also be represented as a vector F(x)=0 4. Because the equations are nonlinear, Newtons method (or a variant thereof) is then used to solve the Example 13.1. Simulation Voltage Regulator: We shall now consider simulation of the type 723 voltage regulator IC, shown in Fig. 13. 1. We wish to simulate the IC and calculate the sensitivity of the output IV c 2000 by CRC Press LLC
© 2000 by CRC Press LLC parameters prefitted to typical specifications. These libraries include items such as discrete transistors, op amps, phase-locked loops, voltage regulators, logic integrated circuits (ICs) and saturating transformer cores. Computer-aided circuit simulation is now considered an essential step in the design of integrated circuits, because without simulation the number of “trial runs” necessary to produce a working IC would greatly increase the cost of the IC. Simulation provides other advantages, however: • The ability to measure “inaccessible” voltages and currents. Because a mathematical model is used all voltages and currents are available. No loading problems are associated with placing a voltmeter or oscilloscope in the middle of the circuit, with measuring difficult one-shot wave forms, or probing a microscopic die. • Mathematically ideal elements are available. Creating an ideal voltage or current source is trivial with a simulator, but impossible in the laboratory. In addition, all component values are exact and no parasitic elements exist. • It is easy to change the values of components or the configuration of the circuit. Unsoldering leads or redesigning IC masks are unnecessary. Unfortunately, computer-aided simulation has its own problems: • Real circuits are distributed systems, not the “lumped element models” which are assumed by simulators. Real circuits, therefore, have resistive, capacitive, and inductive parasitic elements present besides the intended components. In high-speed circuits these parasitic elements are often the dominant performance-limiting elements in the circuit, and must be painstakingly modeled. • Suitable predefined numerical models have not yet been developed for certain types of devices or electrical phenomena. The software user may be required, therefore, to create his or her own models out of other models which are available in the simulator. (An example is the solid-state thyristor which may be created from a NPN and PNP bipolar transistor.) • The numerical methods used may place constraints on the form of the model equations used. The following sections consider the three primary simulation modes: DC, AC, and transient analysis. In each section an overview is given of the numerical techniques used. Some examples are then given, followed by a brief discussion of common pitfalls. DC (Steady-State) Analysis DC analysis calculates the state of a circuit with fixed (non-time varying) inputs after an infinite period of time. DC analysis is useful to determine the operating point (Q-point) of a circuit, power consumption, regulation and output voltage of power supplies, transfer functions, noise margin and fanout in logic gates, and many other types of analysis. In addition DC analysis is used to find the starting point for AC and transient analysis. To perform the analysis the simulator performs the following steps: 1. All capacitors are removed from the circuit (replaced with opens). 2. All inductors are replaced with shorts. 3. Modified nodal analysis is used to construct the nonlinear circuit equations. This results in one equation for each circuit node plus one equation for each voltage source. Modified nodal analysis is used rather than standard nodal analysis because an ideal voltage source or inductance cannot be represented using normal nodal analysis. To represent the voltage sources, loop equations (one for each voltage source or inductor), are included as well as the standard node equations. The node voltages and voltage source currents, then, represent the quantities which are solved for. These form a vector x. The circuit equations can also be represented as a vector F(x) = 0. 4. Because the equations are nonlinear, Newton’s method (or a variant thereof) is then used to solve the equations. Example 13.1. Simulation Voltage Regulator: We shall now consider simulation of the type 723 voltage regulator IC, shown in Fig. 13.1. We wish to simulate the IC and calculate the sensitivity of the output IV
C723 1 OPAMP ↓ 8 FIGURE 13.1 Regulator circuit to be used for DC analysis, created using PSPICE. characteristic and verify that the output current follows a"fold-back type characteristic under overload conditions The IC itself contains a voltage reference source and operational amplifier. Simple models for these elements are used here rather than representing them in their full form, using transistors, to illustrate model development. The use of simplified models can also greatly reduce the simulation effort. For example, the simple op amp used here requires only eight nodes and ten components, yet realizes many advanced features. Note in Fig. 13. 1 that the numbers next to the wires represent the circuit nodes. These numbers are used to describe the circuit to the simulator. In most SPICE-type simulators the nodes are represented by numbers, with the ground node being node zero. Referring to Fig. 13. 2, the 723 regulator and its internal op amp are represented by subcircuits. Each subcircuit has its own set of nodes and components. Subcircuits are useful for encapsulating sections of a circuit or when a certain section needs to be used repeatedly (see next section The following properties are modeled in the op amp 1. Common mode gain 2. Differential mode gain 4. Output impedan 5. Dominant pole 6. Output voltage clipping The input terminals of the op amp connect to a"T" resistance network, which sets the common and differential mode input resistance. Therefore, the common mode resistance is RCM RDIF 1 1E6 and the differential mode resistance is rdifl+ rDiF2= 2.0E5 Dependent current sources are used to create the main gain elements. Because these sources force current into a 1-02 resistor, the voltage gain is gm*R at low frequency. In the differential mode this gives (gDif"RI 00). In the common mode this gives(GCM'RI"(RCM/(RDIFI RCM=0.0909). The two diodes DI and D2 implement clipping by preventing the voltage at node 6 from exceeding VCC or going below VEE. The nodes are made "ideal"by reducing the ideality factor n. Note that the diode current is I,=I, lexp(v/(nv) 1], where V, is the thermal voltage(0.026 V). Thus, reducing n makes the diode turn on at a lower voltage a single pole is created by placing a capacitor( C1)in parallel with resistor RI. The pole frequency is therefore iven by 1.0/(2*I'RI'C1). Finally, the output is driven by the voltage-controlled voltage source El (which has a voltage gain of unity), through the output resistor R4. The output resistance of the op amp is therefore equal to R4 To observe the output voltage as a function of resistance, the regulator is loaded with a voltage source(vOUT) and the voltage source is swept from 0.05 to 6.0 V A plot of output voltage vs. resistance can then be obtained c 2000 by CRC Press LLC
© 2000 by CRC Press LLC characteristic and verify that the output current follows a “fold-back” type characteristic under overload conditions. The IC itself contains a voltage reference source and operational amplifier. Simple models for these elements are used here rather than representing them in their full form, using transistors, to illustrate model development. The use of simplified models can also greatly reduce the simulation effort. (For example, the simple op amp used here requires only eight nodes and ten components, yet realizes many advanced features.) Note in Fig. 13.1 that the numbers next to the wires represent the circuit nodes. These numbers are used to describe the circuit to the simulator. In most SPICE-type simulators the nodes are represented by numbers, with the ground node being node zero. Referring to Fig. 13.2, the 723 regulator and its internal op amp are represented by subcircuits. Each subcircuit has its own set of nodes and components. Subcircuits are useful for encapsulating sections of a circuit or when a certain section needs to be used repeatedly (see next section). The following properties are modeled in the op amp: 1. Common mode gain 2. Differential mode gain 3. Input impedance 4. Output impedance 5. Dominant pole 6. Output voltage clipping The input terminals of the op amp connect to a “T” resistance network, which sets the common and differential mode input resistance. Therefore, the common mode resistance is RCM + RDIF = 1.1E6 and the differential mode resistance is RDIF1 + RDIF2 = 2.0E5. Dependent current sources are used to create the main gain elements. Because these sources force current into a 1-W resistor, the voltage gain is Gm*R at low frequency. In the differential mode this gives (GDIF*R1 = 100). In the common mode this gives (GCM*R1*(RCM/(RDIF1 + RCM = 0.0909). The two diodes D1 and D2 implement clipping by preventing the voltage at node 6 from exceeding VCC or going below VEE. The diodes are made “ideal” by reducing the ideality factor n. Note that the diode current is Id = Is[exp(Vd /(nVt)) – 1], where Vt is the thermal voltage (0.026 V). Thus, reducing n makes the diode turn on at a lower voltage. A single pole is created by placing a capacitor (C1) in parallel with resistor R1. The pole frequency is therefore given by 1.0/(2*p*R1*C1). Finally, the output is driven by the voltage-controlled voltage source E1 (which has a voltage gain of unity), through the output resistor R4. The output resistance of the op amp is therefore equal to R4. To observe the output voltage as a function of resistance, the regulator is loaded with a voltage source (VOUT) and the voltage source is swept from 0.05 to 6.0 V. A plot of output voltage vs. resistance can then be obtained FIGURE 13.1 Regulator circuit to be used for DC analysis, created using PSPICE
Regulator circuit. subckt ic7231245678910 Complete circuit Type 723 voltage regula Load source x1121087。pam Internal voltage referenc s Power input v922.5 VpP 1374mm x11045678910ic723 927 56 mm Series Pass transistors model mm npn(is=le-12 bf=100 q31411mg3 q41112mq4 r14112.2k Ideal opamp with limiting subckt opamp 1 2 3 45 350 vcc vee +in -in out r4260.075 rd1381e5 r568510 rdi]2 48 le5 r68051 r7910270 Common mode gain Control cards gcm6080 le of del mq3 npn(is=le-9bf30 Differential mode gain gdi6043100 br5 ik 50m) r1601 model mq4 npn(is=le- 6 bf=30 cI60.01 dc vout 1.5.o1 d1 6 1 ideal plot dc i(vout) model ideal d (is=le-6 n,o1) ends opamp FIGURE 13.2 SPICE input listing of regulator circuit shown in Fig. 13.1 by plotting VOUT vS. VOUT/I(VOUT)(using PROBE in this case; see Fig. 13.3). Note that for this circuit, eventhough a current source would seem a more natural choice, a voltage source must be used as a load rather than a current source because the output characteristic curve is multivalued in current. If a current source were used it would not be possible to easily simulate the entire curve. Of course, many other interesting quantities can be plotted; for example, the power dissipated in the pass transistor can be approximated by plotting IC(Q3)*VC(Q3) For these simulations PSPICE was used running on an IBM PC. The simulation took 1 min of CPU time Pitfalls. Convergence problems are sometimes experienced if "difficult" bias conditions are created. An exam- ple of such a condition is if a diode is placed in the circuit backwards, resulting in a large forward bias voltage SPICe will have trouble resolving the current. Another difficult case is if a current source were used instead of ⊥(vout》 vaut/⊥(vout FIGURE 13.3 Output characteristics of regulator circuit using PSPICE. c 2000 by CRC Press LLC
© 2000 by CRC Press LLC by plotting VOUT vs. VOUT/I(VOUT) (using PROBE in this case; see Fig. 13.3). Note that for this circuit, eventhough a current source would seem a more natural choice, a voltage source must be used as a load rather than a current source because the output characteristic curve is multivalued in current. If a current source were used it would not be possible to easily simulate the entire curve. Of course, many other interesting quantities can be plotted; for example, the power dissipated in the pass transistor can be approximated by plotting IC(Q3)*VC(Q3). For these simulations PSPICE was used running on an IBM PC. The simulation took < 1 min of CPU time. Pitfalls. Convergence problems are sometimes experienced if “difficult” bias conditions are created. An example of such a condition is if a diode is placed in the circuit backwards, resulting in a large forward bias voltage, SPICE will have trouble resolving the current. Another difficult case is if a current source were used instead of FIGURE 13.2 SPICE input listing of regulator circuit shown in Fig. 13.1. FIGURE 13.3 Output characteristics of regulator circuit using PSPICE