Fullscreen HTML5Med Res (??MB)HTML4

LTspice Part 3: by Nicholas Vinen Modelling an NTC thermistor Last month, we designed a relay simulation and added it to our SoftStarter circuit. But to completely simulate the SoftStarter, we need an NTC Thermistor model and LTspice has no such model. Well, there's only one solution. . . make one! In the process, we'll learn a lot about designing simulation models and design some very handy building blocks that can be re-used later. A thermistor is a non-linear resistor which changes in value as the temperature changes. The resistance of an NTC Thermistor varies inversely to the temperature. In other words, its resistance drops as it heats up. High power NTC thermistors are useful for reducing inrush current, especially in mains-powered circuits, as they have a high enough initial re- sistance to limit the current drawn by capacitor-input power supplies and motors, but a low enough resistance (once they warm up) that they don’t interfere with the load’s operation and don't waste much power. We took this a step further in our SoftStarter, published in the April 2012 issue (www.siliconchip.com.au/ Article/705). By building a circuit which shorts out a current-limiting thermistor with a relay a few seconds after mains power is applied, we get the best of both worlds; once the relay activates, the power loss in the thermistor is zero. The circuit for that project is shown here, in Fig.1. Developing that circuit took some trial-and-error as we had to build it and assess its performance in order to tweak Fig.1: the original circuit from our SoftStarter, published in the April 2012 issue. This reduces inrush current to the connected device each time mains power is applied. This was revised to add load current sensing in the Soft Starter for Power Tools, in the July 2012 issue but this month we’re simulating the more basic circuit shown here. 78  Silicon Chip siliconchip.com.au the component values. If you look at the original article, we published some simulation curves showing how an NTC thermistor can be used to reduce inrush current. So why didn’t we simulate the circuit before building it? It was because SPICE does not have built-in support for any kind of variable resistance device, which would allow us to simulate the behaviour of an NTC thermistor. But it is possible to build a (fairly complex) sub-circuit to do the job instead and this article will show you how. The variable resistance is created using two high-voltage Mosfets in series, connected source-to-source, with their gates joined together. They are then shunted with a resistor, setting the maximum resistance of the device. The minimum resistance is determined by the properties of the Mosfets and how their gates are controlled. The reason for using two Mosfets is to prevent body diode conduction in one direction, as the body diodes are facing in opposite directions. Since their gates and sources are joined, they both must always have the same gate-source voltage, so they are simple to control and the on-resistance of the combination is simply twice the onresistance of a single Mosfet. Note that SPICE generally does not model the body diode conduction in a Mosfet. To simulate a realistic Mosfet, you may need to connect a zener diode across it, with the zener voltage equal to the avalanche breakdown voltage of the Mosfet you've chosen. But just in case SPICE decides to get clever and simulate avalanche breakdown for us, our back-to-back Mosfets will work just like they would in reality, preventing current from flowing unless they are both switched on. Before we proceed, please note that all the sub-circuits, symbols and test circuits shown in this article are available for download in a ZIP package from the Silicon Chip website (free for subscribers). So you may wish to download this and “play along” with the tutorial. You can easily experiment with the circuits, changing values and seeing the effects. depending on the simulated temperature of the NTC thermistor. We need a way to track dissipation and average/ accumulate the instantaneous power to determine the temperature, then use this to vary the resistance. The simulated temperature also needs to drop over time when dissipation is low, simulating the normal cooling process and that temperature needs to translate into an appropriate voltage to drive the Mosfets, to achieve the right resistance value for a given simulated temperature. Broadly, our solution is as follows. We charge a capacitor via a diode and resistor to simulate thermistor heating. The voltage across this capacitor will represent the temperature. A resistor across this capacitor will simulate cooling to ambient temperature. We will then amplify and level-shift this temperature-proxy voltage and apply it to the Mosfet gate, and adjust the amplification factor and RC time-delay constants until the result closely matches the behaviour of a real thermistor. To charge the capacitor representing temperature, we need a voltage that's proportional to the instantaneous dissipation in the thermistor and this can be calculated as the product of the voltage across and current through the thermistor. That sounds simple but it isn’t easy to arrange in SPICE. For a start, heating does not depend on the polarity of the voltage or the direction of the current so we need to compute their absolute values before multiplication. And unfortunately, there's no easy way to multiply two voltages in SPICE. So we have to build an analog multiplier circuit for this job. Measuring voltage and current The complete sub-circuit for our thermistor simulation is shown in Fig.2, with its corresponding symbol at top. In the lower left-hand corner, you can see our two back-to-back Mosfets, M1 and M2, with 10W resistor R1 across them. We have chosen 10W since this matches the nominal cold resistance of the SL32 10015 type NTC thermistor used in the SoftStarter. We are using IPB200N25N3 Mosfets because they have a high voltage rating along with a low RDS(on) of 20mW. Since they are in series, this gives a minimum thermistor resistance of 40mW. The SL32 10015 typically measures 48mW at the full rated current of 15A, with its body temperature at 228°C. It doesn't matter that the Mosfet resistance is slightly lower since the whole sub-circuit incorporates feedback and it will adjust the Mosfet gate voltage to achieve the required resistance, to keep the body temperature steady for a given current. The Mosfets just need to have a low enough RDS(on) to be able to give the required current. We have placed a voltage source, V1, in series with the simulated thermistor. It is set to 0V DC. It might seem weird to have a voltage source of zero volts but voltage sources also double as current meters in SPICE. So V1 is used to measure the current through Building the control circuitry So that's how we're going to provide a controlled resistance but that leaves a rather complex problem to solve, which is how to actually produce a Mosfet gate voltage to give a resistance which varies siliconchip.com.au Fig.2: our complete NTC thermistor simulation sub-circuit, along with its symbol at top. X1 and X2 are precision rectifiers while X3 is an analog multiplier that calculates the instantaneous dissipation of the simulated thermistor. This is accumulated in capacitor C1 and the voltage across it is ultimately applied to the gates of Mosfets M1 and M2 to control the transconductance appropriately. September 2017  79 the thermistor. Note that the points labelled "a" and "b" are the ports used for external connection to the thermistor. H1 is a current-controlled voltage source and you can see that its value field is set to "V1". As a result, the voltage across H1 will track the current through V1, ie, with 1A through V1, there will be 1V across H1; you can change the ratio but in this case, the default of 1A:1V is fine. We then feed the output of H1 to subcircuit X2, which produces an output that is the absolute value of the voltage at the input. Similarly, the voltage across the thermistor is fed to another absolute voltage sub-circuit, X1. Calculating absolute voltage The sub-circuit to calculate the absolute value of a voltage is shown in Fig.3. It's quite straightforward. In the real world, this is typically done with a "precision full-wave rectifier" comprising two op amps, two diodes plus some resistors. The op amps cancel out the forward voltage of the diodes. We could simulate such a circuit, however, it would slow the overall simulation down as it would have to simulate two op amp ICs plus a bunch of other components. So we came up with this much simpler circuit using just two voltagecontrolled switches (S1 & S2) and two voltage-controlled voltage sources (E1 & E2). Both E1 and E2 are set for a gain of unity ("1"), with the input voltage and ground connected to their + and – inputs respectively. So essentially they are just buffers. But because E1's output is floating, if we hook up its output terminals in reverse, it acts as a voltage inverter. Both switch models are set up so that the switch is on its input is positive (ie, positive input voltage higher than negative input voltage). The threshold for S2 is 1µV higher than S1, to prevent them both conducting if the input voltage is exactly 0V. So if the input voltage is positive, S1 connects the buffered signal from E2 directly to the output terminal. And if it's negative, the output of E1 is positive and this is instead connected to the output terminal. You can see the simple symbol we came up with for this sub-circuit at the top of Fig.3. The test circuit is shown in Fig.4, with the results of the simulation shown above. The input is a 3V peak80  Silicon Chip Fig.3: our precision rectifier sub-circuit is quite simple; it either applies the input voltage (buffered by E2) to the output, via voltage-controlled switch S1, or if the input is negative, it is inverted by voltage-controlled voltage source E1 and this positive voltage is applied to the output instead. Fig.4: test circuit for the precision rectifier, which shows a sinewave with a DC offset in green overlaid with the output of the rectifier, in blue. to-peak sinewave offset by 0.5V and shown in green. The output is shown in blue. As you can see, the output is a perfectly rectified version of the input. Tracking instantaneous power So, the outputs of X1 and X2 shown in Fig.2 are a rectified (always-positive) version of the voltage and current across the simulated resistor respectively. Both voltages are referenced to the bottom end of the thermistor (terminal "b"), which is effectively the ground for this circuit. As a thermistor is only a two-terminal device, it must "float". The outputs of X1 and X2 are fed to voltage-controlled voltage sources E2 and E3 which both have a gain of 0.05, ie, they attenuate the voltages by a factor of 20. This is to ensure the resulting voltages are quite low (just a few volts), so they can be fed to the analog multiplier block, X3. X3 has a "power supply" of 15V, so the inputs need to be in the range of 0-15V. We could use resistive dividers to reduce the voltages for X3 but then the source impedance seen by X3 would be non-zero and might affect its operation. SPICE components such as voltage-controlled voltages sources are “ideal” in that they have infinite input impedance and zero output impedance. The output voltage from multiplier block X3 is the product of its input voltages and so the output voltage corresponds to the instantaneous dissipation in the thermistor, scaled down by a factor of 400 (20 x 20). So 1V out corresponds to 400W dissipation in the simulated thermistor. siliconchip.com.au Fig.5: the analog multiplier is based on a real circuit and uses log/anti-log stages and summation to multiply the two input voltages, at Vin1 and Vin2. Vin2 is converted into a current which is sunk from the emitters of Q1 and Q2. The voltage at Vout is almost exactly equal to the product of the two input voltages. V1 exists to measure the current at the collector of Q1. F1 is set up to provide exactly the same current, as its “value” field is set to V1. F1 also has a gain value, not shown in the circuit, which we’ve set to 1. The output voltage which is the product of Vin1 and Vin2 appears at the collector of PNP transistor Q3. This is then fed to voltage-controlled voltage source E2, which acts as a buffer and gain stage. We’ve set its gain to 7.3 as we found that this provides an output of 1V when Vin1 = 1V and Vin2 = 1V. The test circuit for this sub-circuit is shown in Fig.6. Both input signals (green and blue) are sinewaves which vary between 0V and 1V but at different frequencies, so the peaks and troughs coincide at various points throughout the 10ms simulation time. The output of the multiplier is shown in red. Note that the red curve is very close to 0V when either input is at 0V and very close to 1V when both inputs are at 1V. So it is operating effectively as a multiplier. Ideal diode model Fig.6: our analog multiplier test circuit. Its inputs are sinewaves with 1V peak amplitude, shown in green and blue, with the resulting product shown in red. Analog multiplier operation The internals of X3 are shown in Fig.5, with its symbol at top. We got the basis of this circuit from the following URL: www.sayedsaad.com/montada/ showthread.php?t=22594 Essentially, the circuit computes the logarithm of the two input voltages, adds them, then exponentiates the result to produce the output voltage. The result will be proportional to the product of the input voltages, Vin1 and Vin2. Vin1 is fed to a voltage-controlled voltage source, E1, with a gain of unity. This acts as a voltage buffer so that the source impedance won’t affect the rest of the circuit. Voltage source V6 provides a -0.15V bias to this signal, which we experimentally determined was necessary in order to achieve a 0V siliconchip.com.au output when Vin1 = 0V (regardless of the magnitude of Vin2). Vin2 is fed to voltage-controlled current sink G1, with resistor R6 (10MW) in parallel. R6 is not in the original design but we found that this sped up the SPICE simulation, because in cases where Vin2 is very close to zero, the simulation of this circuit breaks down. As you can see, G1’s gain factor is one ten-thousandth, ie, 0.0001. This is so that for Vin2 of 1V, G1 sinks 100µA, to match fixed current source I1 and provide correct scaling of the output. I1 is connected to the positive rail (V+) to supply transistors Q4 and Q5 which are configured as diodes. The collectors of transistors Q1 and Q2 are fed by a current mirror formed by voltage source V1 and voltage-controlled current source F1. As shown in Fig.2, the output of X2 which represents the dissipation (labelled “pout” for “power output”) passes through diode X4 then 10GW resistor R2, before charging 5nF capacitor C1. R2 limits the rate of C1’s charging to represent the fact that the thermistor body doesn’t increase in temperature instantly when the dissipation increases; it has thermal inertia. Resistance values that high are rarely seen in real circuits because leakage currents can overwhelm them but that isn't an issue in a simulation; it’s the time constant that’s critical. The purpose of diode X4 is to model the fact that the rate of thermistor heating depends on dissipation but the rate of cooling depends on its temperature. In other words, a very high dissipation should heat the thermistor up fast but if dissipation falls to zero, it cannot cool down back to its original temperature in that same time; it might take much longer. So this diode only allows the “heat” to flow in one direction. But we don’t want to use a real diode model because its forward voltage would interfere with this process. It would not conduct until the dissipation rose above a certain level and would then reduce the maximum voltage applied to C1. We would prefer an “ideal” diode which essentially September 2017  81 acts as a switch, turning on as soon as the voltage at the anode is above the cathode and switching off as soon as that reverses. So that’s exactly how we’ve modelled it. The sub-circuit and corresponding symbol are shown in Fig.7. The voltage controlled switch’s control terminals are connected directly to the switch terminals. The threshold is set to 0.1mV and the hysteresis value is the same. That means the voltage across the ideal diode during forward conduction will be well under 1mV. Finishing the thermistor model Getting back to Fig.2, the time constant of R2/C1 determines how quickly the modelled thermistor heats up due to internal dissipation while R4/C1 set its cool-down characteristics. Placing resistor R4 across C1 accurately models cooling since, in the real world, the rate of cooling is proportional to the difference between an object’s temperature and the ambient temperature. In the simulation, current through R4 is proportional to the voltage across C1 (a proxy for the temperature) and so the rate that “heat” leaves the model is directly related to its temperature. So the simulated temperature, labelled “temp”, is applied to the inputs of another voltage-controlled voltage source, E1, with a gain value of 500. Besides applying gain, the other reason for E1 is that it stops the following circuitry from drawing current from C1 and affecting the thermal simulation. Voltage source V4 has a fixed value of 3.2V and this provides the Mosfet gate switch-on bias voltage for M1 and M2. Note that E1’s negative output terminal is connected to the sources of M1 and M2. This means that with a simulated temperature at ambient, the gates of M1 and M2 are 3.2V above their source terminals, just on the edge of conduction. For each 2mV across C1, the gate-source voltage increases by 1V. This gain figure was determined experimentally, by comparing the behaviour of the simulated thermistor to figures in the SL32 10015 data sheet. This figure was found to give a realistic time constant and ultimate resistance under sustained load. It’s important to realise that this model contains a negative feedback path. As the voltage across C1 increases, Mosfets M1 and M2 switch on harder, reducing the voltage across R1 and this, in turn, 82  Silicon Chip Fig.7: another type of precision rectifier, this time in the form of an ideal diode (ie, a half-wave rectifier). This is basically just a switch which allows current to flow from input to output only when the input voltage is higher than the output voltage. Fig.8: a simple test circuit for our now complete NTC thermistor model, utilised here as X1. The load is primarily capacitive so draws the most current around the mains peak. You can see how the capacitor voltage (green) rises relatively slowly, over around 50ms, while the thermistor dissipation (blue) starts very high but drops down to a low level after around 100ms. reduces the dissipation and thus the voltage at “pout”. That then allows the voltage across C1 to stabilise at a value that depends on the voltage and current flow between points “a” and “b”. 1W resistor R3 between E1/V4 and the gates of M1/M2 provides a tiny delay for this negative feedback which helps the simulation converge faster (see the side panel for more details on this phenomenon). The 100MW bleed resistor effectively between the gate and source terminals of M1/M2 was added for a similar reason. Testing the NTC thermistor Fig.8 shows the test circuit. We have a 325V peak sinewave representing the mains, with the thermistor in between it and the test load. There’s a simple half-wave rectifier feeding a 1000µF high-voltage capacitor with a 100W bleeder/load resistor. This is intended to crudely simulate a capacitor-input switchmode power supply with a load. Above it, you can see the result of the simulation, with the voltage across R2 in red, voltage across C1 in green and instantaneous dissipation in X1 in blue. (By the way, to plot dissipation of a component in Windows, hold down the ALT key while clicking on that component. Once you’ve done that, to display the average power, zoom over the relevant portion of the waveform and hold CTRL while clicking on the siliconchip.com.au run the simulations very slowly or halt altogether. This is due to a failure to converge – see the side panel explaining this problem. Putting it all together Fig.9: another test of the NTC thermistor model, this time with a primarily resistive load of around 15A. It takes around 100ms for the load voltage to rise close to the full 230VAC with thermistor dissipation initially averaging 600W, dropping down to 10W in the steady-state condition after around 200ms. Fig.10: we can now complete our simulation of the SoftStarter. It uses the relay and NTC thermistor sub-circuits we’ve developed plus a typical load comprising an EMI suppression capacitor, bridge rectifier, mains filter capacitor and 100W equivalent resistive load. We can probe the voltages and currents at various points more easily than with the real circuit, which floats at mains potential. formula at the top of the plot window.) As shown, the voltages rise quite gradually, over the first few mains cycles. If you remove X1 from the circuit, C1 charges almost instantly, in under 1ms, drawing a peak current of almost 1000A! A real capacitor would have too much parasitic resistance/inductance to draw quite so much current but the contrast is still educational. Note how the thermistor dissipation drops initially, then rises a little before finally dropping down to a stable level. That’s because after the thermistor heats up a little initially and its resistance drops, it allows more current to flow into C1 which briefly increases its dissipation before the voltage across X1 siliconchip.com.au drops, further reducing its dissipation. Fig.9 shows a variation on this test circuit, where we have replaced the capacitor input power supply with a resistive load shunted with an EMI suppression capacitor. With a load resistor of 16W, it will draw 14.4A RMS on a continuous basis (ie, 230VAC ÷ 16W). As you can see, in this case, the thermistor heats up a little more gradually and as the voltage across R2 approaches the full 230V RMS, dissipation in the thermistor drops from an initial average of 600W down to around 10W after about 200ms. Note that if you are experimenting with these circuits, you may find that certain changes will cause SPICE to Fig.10 shows our now complete SoftStarter circuit at bottom, based on what we finished with last month (ie, incorporating the relay model we developed then) but now also including our thermistor, X2, plus a test load circuit comprising EMI suppression capacitor C4, bridge rectifier D7-D10, filter capacitor C5 and resistive load R6. The simulation output at top shows the mains voltage at V1 (green), voltage across the load at C5/R6 (cyan), current through simulated thermistor X2 (blue), voltage across the relay coil (mauve) and thermistor dissipation (red). As you can see, the inrush current is limited to around 20A, which is pretty much the same peak current that the load draws during normal operation. You can see the thermistor dissipation is very high over the first few cycles but drops to below 10W after about 500ms, at which time the relay coil voltage rises and the thermistor is shorted out. Its dissipation then drops to almost zero; if the relay didn’t close then, its dissipation would continue to drop, to a steady-state value of around 4W. So in other words, the simulation is working correctly and showing how the real circuit behaves! Note that a small amount of current is still shown flowing through the thermistor even after the relay contacts close. This is as a result of the non-zero relay contact resistance we’ve programmed into our model. But because the product of current and voltage is so low, dissipation still appears as a flat line once the relay latches. Note also that Fig.10 shows the voltage across the relay coil of X1, even though that part of the circuit is not connected directly to ground. This can be achieved by right-clicking in the plot window and selecting “Add Trace”, then typing in the expression V(x)-V(y), where “x” and “y” are nodes in the circuit. This is one reason why it’s a good idea to label nodes in the circuit (as we have with VOUT) since the automatically generated node names like “n004” can change if you modify the circuit. You also need to figure them out (by September 2017  83 Simulation slowness, pausing or intermittent failure SPICE simulations have two distinct phases, the first of which is optional, but normally present. The first phase is where it determines the initial DC operating point. In other words, for every component which has state – primarily capacitors (charge) and inductors (magnetic field strength) – it needs to determine the steady-state condition* with which to start the simulation. If you have something like an oscillator in the circuit, it won’t have a steady state, but SPICE will still attempt to determine a reasonable starting point – a condition which a real circuit may find itself in at some point in time, prior to any AC signals being applied. Various circuit configurations can make this impossible. One thing that often throws SPICE off and prevents it from finding the initial DC operating point is nodes which have no DC current path to ground. For example, it’s perfectly valid to apply an AC signal to a pair of series-connected capacitors, with them operating as a capacitive voltage divider. But unless you have a way for current to flow from the junctions of these capacitors to ground, SPICE will often throw up its arms in disgust. The usual solution to this problem is to connect a high-value resistors from this junction to ground. It will have negligible effect on the operation of the circuit but may help SPICE to converge on an initial operating point solution. If you’ve drawn up a circuit and can’t figure out any way to get SPICE to get past this initial hurdle and start the simulation, your other option is to get it to skip this step entirely and either start with everything in a default state (capacitors and inductors discharged etc). Or alternatively, you can specify the initial state of the components yourself. In fact, you can even adopt a “mix-and-match” approach, providing initial states for some component and letting SPICE figures the other out. You may need to use trial and error to determine which components need their initial conditions defined before the software will reliably complete this step. To set the initial condition of a component, modify its value and add " ic=xx" to the end, where xx is the initial value. For example, a capacitor can have a value of "10uF ic=5V" and an inductor can have a value of "100uH ic=1A". If you also add " uic" to the end of the simulation command (labelled "skip initial operating point solution" in the LTspice configuration dialog), all components will start with a value of 0V/0A unless the initial condition is specified. Note that you can also abort the initial operating point solution, if it gets stuck, by pressing the ESC key on your keyboard. SPICE will then take whatever its last guess was as to the initial conditions and run the simulation. SPICE can also get stuck during the simulation, for similar reasons. This is often at the point where a transistor is moving into or out of conduction, a diode is becoming forward biased and so on. The rapid changes in circuit behaviour at these points can cause it to move forward in smaller and smaller time steps. It will normally eventually get past that point but it may take a long time, and it may get stuck again soon afterwards. There are various techniques you can use to avoid or mitigate this. First, it helps to understand why this happens. The following course notes contain some useful information on this aspect of SPICE: www3.imperial.ac.uk/pls/portallive/docs/1/7292571.PDF This document is from the Department of Electrical and Electronic Engineering, Imperial College London. On page 24, it states “There are convergence problems associated with very high conductance [… and] very high resistance”. On pages 23 and 24, it shows an example of attempting to iteratively solve a circuit involving a current source, resistor and diode and shows how, depending on the algorithm used, the software may not be able to converge on the solution. The following pages discuss the GMIN parameter, one of several you can adjust in LTspice which may help prevent it from getting stuck. This can be changed by going to the “Control Panel” menu option in the “Tools” menu and clicking on the SPICE tab. We experimented with some of these options and found that changing the “Default Integration Method” from “modified trap” to “trapezoidal” sometimes caused our simulations to run much more smoothly with a range of different component parameters. Changing the “Solver” from “Normal” to “Alternate” had an even bigger effect on the simulation’s performance. There were times where it would absolutely crawl with the Normal solver but ran very fast and reliably with the Alternate solver. So if you find your simulation getting stuck, it’s well worth trying to change these parameters before resorting to modifying your circuit. If you do need to modify the circuit, we suggest the following: add high-value resistors across capacitors, or from the ends of capacitors to ground. Add high-value resistors or low-value capacitors across diodes and/or transistor junctions. For generic components, try different component models, or try using models of similar parts. Many of these changes can have negligible impact on the accuracy of your simulation while potentially making SPICE run much faster and without getting “stuck” as often. For example, in our SoftStarter simulation (shown in Fig.10), we sometimes get an error message that the initial operating point solution failed, implicating diode D7. While changing the Default Integration Method helped, another solution we found was to put a low-value capacitor across D7. This has hardly any effect on the results but seemed to overcome that particular problem. So that’s one example of a way to modify your circuit when SPICE is “playing up”. * a circuit may have zero, one or many steady-state conditions. These are conditions where the series of simultaneous equations that represent the circuit's behaviour converge to a fixed set of values. This is important for transient simulations as without a steady-state condition, SPICE cannot model the behaviour of the circuit. hovering the mouse over a point in the circuit and looking at the bottom of the window) before you can enter the expression, whereas if the circuit nodes are labelled, the names are obvious. Conclusion So what is this simulation good for? First, it would allow us to more easily tweak the power supply component 84  Silicon Chip values, the time constant values which set the relay delay time and so on. It also allows us to examine the voltages and currents applied to each component to verify that they will not experience conditions outside their ratings. For example, we can examine the expected inrush current for various different types of load and whether the relay time delay is sufficient to allow the thermistor to finish its job of limiting that current before it’s shorted out. We could also see the effect of disconnecting the load and then re-connecting it some time later, before the thermistor has had a chance to fully cool down. That’s it for this month. In our next SPICE tutorial, we will look at simulating audio circuits, especially those which involve op amps. SC siliconchip.com.au