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
a voltage to bias the or i the previous example. If the user then tried to increase the output current above 10 A, SPICE would not be able to converge because the regulator will not allow such a large current. AC Analysis calculating the gain. 3 dB frequency input and output impedance, and noise of a circuit as a function of Numerical Method 1. A DC solution is performed to calculate the Q-point for the circuit. 2. A linearized circuit is constructed at the Q point. To do this, all nonlinear elements are replaced by their linearized equivalents. For example, a nonlinear current source I=avi+ bv would be replaced by a linear voltage controlled current source I= V(2av1a)+ V(3bv2d 3. All inductors and capacitors are replaced by complex impedances, and conductances evaluated at the quency of interest. 4. Nodal analysis is now used to reduce the circuit to a linear algebraic complex matrix. The AC node ly now be found by applying an excitation vector(which represents the independent voltage and current sources)and using Gaussian elimination(with complex arithmetic) to calculate the node voltages. AC analysis does have limitations and the following types of nonlinear or large signal problems cannot be modeled 1. Distortion due to nonlinearities such as clipping, etc. 2. Slew rate-limiting effects 3. Analog mixers 4. Oscillators Noise analysis is performed by including noise sources in the models. Typical noise sources include thermal oise in resistors I=4kTAf/R, and shot I=2qL, Af, and flicker noise in semiconductor devices. Here, T temperature in Kelvins, k is Boltzmann's constant, and Af is the bandwidth of the circuit. These noise sources are inserted as independent current sources, In; (f)into the AC model. The resulting current due to the noise ource is then calculated at a user-specified summation node(s) by multiplying by the gain function between the noise source and the summation node Ai (). This procedure is repeated for each noise source and the the contributions at the reference node are root mean squared(RMS) summed to give the total noise at the reference node. The equivalent input noise is then easily calculated from the transfer function between the ircuit input and the reference node Ais f). The equation describing the input noise is therefore: 1=AO0240mO Example 13.2. Cascode Amplifier with Macro Models: Here, we find the gain, bandwidth, input impedance, and output noise of a cascode amplifier. The circuit for the amplifier is shown in Fig. 13.5. The circuit is assumed to be fabricated in a monolithic IC process, so it will be necessary to consider some of the parasitics of the IC process. A cross-section of a typical IC bipolar transistor is shown in Fig. 13. 4 along with some of the parasitic elements. These parasitic elements are easily included in the amplifier by creating a"macro model"for each transistor. The macro model is then implemented in SPICE form using subcircuits. The input to the circuit is a voltage source(VIN), applied differentially to the amplifier. The output will be taken differentially across the collectors of the two upper transistors at nodes 2 and 3. The input impedance of the amplifier can be calculated as VIN/I(VIN) or because vin =1.0 just as 1/I(VIN). These quantities are shown plotted using PROBE in Fig. 13.6. It can be seen that the gain of the amplifier falls off at high frequency c 2000 by CRC Press LLC
© 2000 by CRC Press LLC a voltage to bias the output in the previous example. If the user then tried to increase the output current above 10 A, SPICE would not be able to converge because the regulator will not allow such a large current. AC Analysis Ac analysis uses phasor analysis to calculate the frequency response of a circuit. The analysis is useful for calculating the gain. 3 dB frequency input and output impedance, and noise of a circuit as a function of frequency, bias conditions, temperature, etc. Numerical Method 1. A DC solution is performed to calculate the Q-point for the circuit. 2. A linearized circuit is constructed at the Q point. To do this, all nonlinear elements are replaced by their linearized equivalents. For example, a nonlinear current source I = aV1 2 + bV2 3 would be replaced by a linear voltage controlled current source I = V1 (2aV1q ) + V2(3bV2q 2 ). 3. All inductors and capacitors are replaced by complex impedances, and conductances evaluated at the frequency of interest. 4. Nodal analysis is now used to reduce the circuit to a linear algebraic complex matrix. The AC node voltages may now be found by applying an excitation vector (which represents the independent voltage and current sources) and using Gaussian elimination (with complex arithmetic) to calculate the node voltages. AC analysis does have limitations and the following types of nonlinear or large signal problems cannot be modeled: 1. Distortion due to nonlinearities such as clipping, etc. 2. Slew rate-limiting effects 3. Analog mixers 4. Oscillators Noise analysis is performed by including noise sources in the models. Typical noise sources include thermal noise in resistors In 2 = 4kT Df /R, and shot In 2 = 2qId Df , and flicker noise in semiconductor devices. Here, T is temperature in Kelvins, k is Boltzmann’s constant, and Df is the bandwidth of the circuit. These noise sources are inserted as independent current sources, Inj(f ) into the AC model. The resulting current due to the noise source is then calculated at a user-specified summation node(s) by multiplying by the gain function between the noise source and the summation node Ajs(f ). This procedure is repeated for each noise source and then the contributions at the reference node are root mean squared (RMS) summed to give the total noise at the reference node. The equivalent input noise is then easily calculated from the transfer function between the circuit input and the reference node Ais(f ). The equation describing the input noise is therefore: Example 13.2. Cascode Amplifier with Macro Models: Here, we find the gain, bandwidth, input impedance, and output noise of a cascode amplifier. The circuit for the amplifier is shown in Fig. 13.5. The circuit is assumed to be fabricated in a monolithic IC process, so it will be necessary to consider some of the parasitics of the IC process. A cross-section of a typical IC bipolar transistor is shown in Fig. 13.4 along with some of the parasitic elements. These parasitic elements are easily included in the amplifier by creating a “macro model” for each transistor. The macro model is then implemented in SPICE form using subcircuits. The input to the circuit is a voltage source (VIN), applied differentially to the amplifier. The output will be taken differentially across the collectors of the two upper transistors at nodes 2 and 3. The input impedance of the amplifier can be calculated as VIN/I(VIN) or because VIN = 1.0 just as 1/I(VIN). These quantities are shown plotted using PROBE in Fig. 13.6. It can be seen that the gain of the amplifier falls off at high frequency I A f A f In f i is js j j = ( ) Â[ ] ( ) ( ) 1 2
c FIGURE 13.4 BT cross-section with macro model elements VCC 手6 3 8 10 FIGURE 13.5 Cascode amplifier for AC analysis, created using PSPICE 1,K1230V AGain Zin r requency FIGURE 13.6 Gain and input impedance of cascode amplifie c 2000 by CRC Press LLC
© 2000 by CRC Press LLC FIGURE 13.4 BJT cross-section with macro model elements. FIGURE 13.5 Cascode amplifier for AC analysis, created using PSPICE. FIGURE 13.6 Gain and input impedance of cascode amplifier
as expected. The input impedance also drops because parasitic capacitances shunt the input. This example took 1 min on an ibm pc Pitfalls. Many novice users will forget that AC analysis is a linear analysis. They will, for example, apply a 1-V signal to an amplifier with 5-V power supplies and a gain of 1000 and be surprised when SPICe tells them that the output voltage is 1000 V. Of course, the voltage generated in a simple amplifier must be less than the power supply voltage, but to examine such clipping effects, transient analysis must be used. Likewise, selection of a proper Q point is important. If the amplifier is biased in a saturated portion of its response and ac analysis is performed, the gain reported will be much smaller than the actual large signal gain. Transient Analysis Transient analysis is the most powerful analysis capability of a simulator because the transient response is so hard to calculate analytically. Transient analysis or many types of analysis, distortion, basic operation of certain circuits like switching power supplies. Transient analysis is also the most CPU intensive and can require 100 or 1000 times the CPU time as a dC or AC analysis Numerical Method In a transient analysis time is discretized into intervals called time steps. Typically the time steps are of unequal ength, with the smallest steps being taken during portions of the analysis when the circuit voltages and currents are changing most rapidly. The capacitors and inductors in the circuit are then replaced by voltage and current sources based on the following procedure. The current in a capacitor is given by I= Cav/dt. The time derivative can be approximated by a difference In this equation the superscript k represents the number of the time step. Here, k is the time step we are presently solving for and (k-1)is the previous time step. This equation can be solved to give the capacit current at the present time step. =V(2C△)-V-(2C△)-1 Here, At=tk-re-l, or the length of the time step. As time steps are advanced, V-1- V5: 15-l, I2. Note that the second two terms on the right hand side of the above equation are dependent only on the capacitor voltage and current from the previous time step, and are therefore fixed constants as far as the present step is concerned. The first term is effectively a conductance(g= 2C/An)multiplied by the capacitor voltage, and the econd two terms could be represented by an independent current source. The entire transient model for the capacitor therefore consists of a conductance in parallel with two current sources( the numerical values of these are, of course, different at each time step). Once the capacitors and inductors have been replaced as indicated, the normal method of DC analysis is used. One complete DC analysis must be performed for each time point. This is the reason that transient analysis is so CPU intensive. The method outlined here is the trapezoidal time integration method and is used as the default in SPICe. Example 133. Phase-Locked Loop Circuit: Figure 13.7 shows the phase-locked loop circuit. The phase detector and voltage-controlled oscillator are modeled in separate subcircuits. Examine the VCO subcircuit and note the PULSE-type current source ISTART connected across the capacitor. The source gives a current pulse 03. E-6 s wide at the start of the simulation to start the vco running. To start a transient simulation SPICE first computes a DC operating point(to find the initial voltages Ve- on the capacitors). As this dC point is a valid, although not necessarily stable, solution, an oscillator will remain at this point indefinitely unless some perturbation is applied to start the oscillations. Remember, this is an ideal mathematical model and no noise c 2000 by CRC Press LLC
© 2000 by CRC Press LLC as expected. The input impedance also drops because parasitic capacitances shunt the input. This example took <1 min on an IBM PC. Pitfalls. Many novice users will forget that AC analysis is a linear analysis. They will, for example, apply a 1-V signal to an amplifier with 5-V power supplies and a gain of 1000 and be surprised when SPICE tells them that the output voltage is 1000 V. Of course, the voltage generated in a simple amplifier must be less than the power supply voltage, but to examine such clipping effects, transient analysis must be used. Likewise, selection of a proper Q point is important. If the amplifier is biased in a saturated portion of its response and AC analysis is performed, the gain reported will be much smaller than the actual large signal gain. Transient Analysis Transient analysis is the most powerful analysis capability of a simulator because the transient response is so hard to calculate analytically. Transient analysis can be used for many types of analysis, such as switching speed, distortion, basic operation of certain circuits like switching power supplies. Transient analysis is also the most CPU intensive and can require 100 or 1000 times the CPU time as a DC or AC analysis. Numerical Method In a transient analysis time is discretized into intervals called time steps. Typically the time steps are of unequal length, with the smallest steps being taken during portions of the analysis when the circuit voltages and currents are changing most rapidly. The capacitors and inductors in the circuit are then replaced by voltage and current sources based on the following procedure. The current in a capacitor is given by Ic = CdVc /dt. The time derivative can be approximated by a difference equation: In this equation the superscript k represents the number of the time step. Here, k is the time step we are presently solving for and (k – 1) is the previous time step. This equation can be solved to give the capacitor current at the present time step. Here, Dt = t k – tk–1, or the length of the time step. As time steps are advanced, Vc k–1 Æ Vc k ; Ic k–1 Æ Ic k . Note that the second two terms on the right hand side of the above equation are dependent only on the capacitor voltage and current from the previous time step, and are therefore fixed constants as far as the present step is concerned. The first term is effectively a conductance (g = 2C/Dt) multiplied by the capacitor voltage, and the second two terms could be represented by an independent current source. The entire transient model for the capacitor therefore consists of a conductance in parallel with two current sources (the numerical values of these are, of course, different at each time step). Once the capacitors and inductors have been replaced as indicated, the normal method of DC analysis is used. One complete DC analysis must be performed for each time point. This is the reason that transient analysis is so CPU intensive. The method outlined here is the trapezoidal time integration method and is used as the default in SPICE. Example 13.3. Phase-Locked Loop Circuit: Figure 13.7 shows the phase-locked loop circuit. The phase detector and voltage-controlled oscillator are modeled in separate subcircuits. Examine the VCO subcircuit and note the PULSE-type current source ISTART connected across the capacitor. The source gives a current pulse 03.E-6 s wide at the start of the simulation to start the VCO running. To start a transient simulation SPICE first computes a DC operating point (to find the initial voltages Vc k–1 on the capacitors). As this DC point is a valid, although not necessarily stable, solution, an oscillator will remain at this point indefinitely unless some perturbation is applied to start the oscillations. Remember, this is an ideal mathematical model and no noise I I C V V t t c k c k c k c k k k + = - - - - - 1 1 1 2 I V C t V C t I c k c k c k c k = ( ) - ( ) - - - 2 2 1 1 D D
MULTIPLIER ut 女 800K “式“ 7 M10 vCO FIGURE 13. 7 Phase-locked loop circuit for transient analysis, created with PSPICE. sources or asymmetries exist that would start a real oscillator--it must be done manually. The capacitor CI would have to be placed off-chip, and bond pad capacitance(CPADI and CPAD2)have been included at the capacitor nodes. Including the pad capacitances is very important if a small capacitor Cl is used for high frequency operation In this example, the Pll is to be used as a FM detector circuit and the FM signal is applied to the input using a single frequency FM voltage source. The carrier frequency is 600 kHz and the modulation frequency is 60 kHz. Figure 13.8 shows the input voltage and the output voltage of the PlL at the vCo output and at the phase detector output. It can be seen that after a brief starting transient, the PLL locks onto the input signal Loop Filter output 3.0vr 工 nput signa 中与1 FIGURE 13.8 Transient analysis results of PLL circuit, created using PSPICE c 2000 by CRC Press LLC
© 2000 by CRC Press LLC sources or asymmetries exist that would start a real oscillator—it must be done manually. The capacitor C1 would have to be placed off-chip, and bond pad capacitance (CPAD1 and CPAD2) have been included at the capacitor nodes. Including the pad capacitances is very important if a small capacitor C1 is used for highfrequency operation. In this example, the PLL is to be used as a FM detector circuit and the FM signal is applied to the input using a single frequency FM voltage source. The carrier frequency is 600 kHz and the modulation frequency is 60 kHz. Figure 13.8 shows the input voltage and the output voltage of the PLL at the VCO output and at the phase detector output. It can be seen that after a brief starting transient, the PLL locks onto the input signal FIGURE 13.7 Phase-locked loop circuit for transient analysis, created with PSPICE. FIGURE 13.8 Transient analysis results of PLL circuit, created using PSPICE
Process Device Parameter Simulation Simulation Extraction Simulation Netlist Extraction Simulation FIGURE 13.9 Data flow for complete process-device- circuit modeling. and that the phase detector output has a strong 60-kHz component. This example took 251 s on a Sun SPARC-2 workstation(3046 time steps, with an average of 5 Newton iterations per time step) Pitfalls. Occasionally SPICE will fail and give the message Timestep too small in transient ana which means that the process of Newton iterations at certain time steps could not be made to converge. One of the most common causes of this is the specification of a capacitor with a value that is much too large, for example, specifying a 1-F capacitor instead of a I pF capacitor(an easy mistake to make by not adding the"p"in the value specification). Unfortunately, we usually have no way to tell which capacitor is at fault from the type of failure generated other than to manually search the input deck. Other transient failures are caused by MOSFET models. Some models contain discontinuous capacitan (with respect to voltage)and others do not conserve charge. These models can vary from version to version so it is best to check the users guide Process and device simulation Process and devices simulation are the steps that precede analog circuit simulation in the overall simulation flow(see Fig. 13.9). The simulators are also different in that they are not measurement driven as are analog circuit simulators. The input to a process simulator is the sequence of process steps performed(times, temper atures, gas concentrations)as well as the mask dimensions. The output from the process simulator is a detailed description of the solid-state device(doping profiles, oxide thickness, junction depths, etc. ) The input to the device simulator is the detailed description generated by the process simulator(or via measurement ). The output of the device simulator is the electrical characteristics of the device(Iv curves, capacitances, switching transient curves) rocess and device simulation are becoming increasingly important and widely used during the integrated circuit design process. A number of reasons exist for this As device dimensions shrink, second-order effects can become dominant. Modeling of these effects is Computers have greatly improved, allowing time-consuming calculations to be performed in a reasonable mulation allows access to impossible to measure physical characteristics Analytic models are not available for certain devices, for example, thyristors, heterojunction devices and GBTS Analytic models have not been developed for certain physical phenomena, for example, single event upset, hot electron aging effects, latchup, and snap-back Simulation runs can be used to replace split lot runs. As the cost to fabricate test devices increases, this dvantage becomes more important Simulation can be used to help device, process, and circuit designers understand how their devices and Clearly, process and device simulation is a topic which can be and has been the topic of entire texts. The following sections attempt to provide an introduction to this type of simulation, give several examples showing what the simulations can as h, and provide references to additional sources of information c 2000 by CRC Press LLC
© 2000 by CRC Press LLC and that the phase detector output has a strong 60-kHz component. This example took 251 s on a Sun SPARC-2 workstation (3046 time steps, with an average of 5 Newton iterations per time step). Pitfalls. Occasionally SPICE will fail and give the message “Timestep too small in transient analysis”, which means that the process of Newton iterations at certain time steps could not be made to converge. One of the most common causes of this is the specification of a capacitor with a value that is much too large, for example, specifying a 1-F capacitor instead of a 1 pF capacitor (an easy mistake to make by not adding the “p” in the value specification). Unfortunately, we usually have no way to tell which capacitor is at fault from the type of failure generated other than to manually search the input deck. Other transient failures are caused by MOSFET models. Some models contain discontinuous capacitances (with respect to voltage) and others do not conserve charge. These models can vary from version to version so it is best to check the user’s guide. Process and Device Simulation Process and devices simulation are the steps that precede analog circuit simulation in the overall simulation flow (see Fig. 13.9). The simulators are also different in that they are not measurement driven as are analog circuit simulators. The input to a process simulator is the sequence of process steps performed (times, temperatures, gas concentrations) as well as the mask dimensions. The output from the process simulator is a detailed description of the solid-state device (doping profiles, oxide thickness, junction depths, etc.). The input to the device simulator is the detailed description generated by the process simulator (or via measurement). The output of the device simulator is the electrical characteristics of the device (IV curves, capacitances, switching transient curves). Process and device simulation are becoming increasingly important and widely used during the integrated circuit design process. A number of reasons exist for this: • As device dimensions shrink, second-order effects can become dominant. Modeling of these effects is difficult using analytical models. • Computers have greatly improved, allowing time-consuming calculations to be performed in a reasonable amount of time. • Simulation allows access to impossible to measure physical characteristics. • Analytic models are not available for certain devices, for example, thyristors, heterojunction devices and IGBTS. • Analytic models have not been developed for certain physical phenomena, for example, single event upset, hot electron aging effects, latchup, and snap-back. • Simulation runs can be used to replace split lot runs. As the cost to fabricate test devices increases, this advantage becomes more important. • Simulation can be used to help device, process, and circuit designers understand how their devices and processes work. Clearly, process and device simulation is a topic which can be and has been the topic of entire texts. The following sections attempt to provide an introduction to this type of simulation, give several examples showing what the simulations can accomplish, and provide references to additional sources of information. FIGURE 13.9 Data flow for complete process-device-circuit modeling
