Fullscreen HTML5Med Res (??MB)HTML4

Circuit Surgery Regular clinic by Ian Bell LTspice 17.1 and Frequency Response Analysis – Part 1 R egular readers will know that Circuit Surgery regularly uses LTspice simulations to illustrate circuit operation and behaviour. LTspice was developed by Linear Technology and was originally also referred to as ‘SwitcherCAD’ because of its optimisations for simulating switching regulators and related circuits, which were a key Linear Technology product line. In 2017, Linear Technology became part of Analog Devices, who took over LTspice. The LTspice download is provided with a library of models of real components. Initially, these were for LT devices, but of course Analog Devices’ components were added after the merger. Another merger of Maxim Integrated into Analog Devices means their devices have been added too. Models for devices from other manufacturers (mainly passive components and transistors) are also included. LTspice updates it model library regularly and there are also minor software updates, such as bug fixes, but there have not been major software updates for some time. Version 17.0 (written as ‘LTspice XVII’) dates from 2016. In 2023, Analog Devices released LTspice 17.1, which it described as a significant upgrade to LTspice XVII. The key addition was a new frequency response analyser component and an associated .fra spice directive, which we will discuss in detail later. However, there are a few other changes that we will mention first. Download and install LTspice 17.1 can be downloaded for free from the Analog Devices website: https://bit.ly/pe-jan24-ltspice It is available for Windows 10 64-bit and forward, and MacOS 10.15 and forward. The older version is still available too. LTspice 17.1 can be installed alongside LTspice XVII since both the executables and models for the two versions are stored in different locations. You can run both apps at the same time but must not open the same file in both versions at the same time. Visually, the user interfaces look very similar, although user interface improvements and bug fixes are listed as enhancements. The new version is named simply ‘LTspice’, not ‘LTspice XVII’ in the 52 application title bar and desktop icons. If you want to use both and would like a more obvious visual indication, you could try changing the background image which appears in the background behind schematic and waveform windows (Control Panel> Operation > Background Image). Downloading and installing LTspice 17.1 is straightforward. During the install it asks if the installation is just for the current user or for everyone – this changes the default install location. On Windows, installed examples and libraries are always stored in the current user’s local application data folder (C:\users\[User]\AppData\Local\ LTspice\) rather than in the documents folder (C:\Users\[User]\Documents\ LTspiceXVII) that was used by the previous version. If you have custom libraries or symbols in the old location then you could copy them to the new location or use the control panel (Tools > Control Panel > Sym. & Lib. Search Paths) to add the location of your custom folders to the search path used by LTspice. Other enhancements The new version has improved the drawing speed of the waveform viewer when plotting large amounts of data. This was definitely a problem with the previous version, where, for example, just resizing the waveform viewer window could result in a lengthy redraw period (this is just drawing the waveform, not running the simulation). This can be observed with some of the simulations in the recent superhet receivers Circuit Surgery articles where the data sets were large because relatively long simulations were used to obtain enough data for LTspice to accurately plot the signal spectra. As a quick test I resized the full results (all key waveforms shown in separate plot panes) and the speed-up was obvious, with one example taking around 20 to 30 seconds to redraw in the old version, but only 2 to 3 seconds in LTspice 17.1. Another enhancement is that keyboard shortcuts can now be saved to and loaded from text files. Previous LTspice allowed changes to keyboard shortcuts, but there was no easy way to export these settings so that they could be used in another instance of LTspice (eg, to use on another computer or share with another user). This is now straightforward to do via the Control Panel, with the shortcuts stored in a humanreadable text file. Finally, Analogue Devices also lists some improvements to the simulator operation, specifically: fixed convergence problems, updated initial conditions behaviour and reduced multi-threaded CPU loading. Frequency response analysis LTspice’s frequency response analysis (FRA) is aimed at determining the behaviour of negative-feedback loops. All feedback systems have the potential to become unstable and oscillate, which is often disastrous (unless you are building an oscillator!). The FRA is aimed at determining the stability of negative-feedback circuits; that is, finding out how much margin of error you have between stable and unstable operation. If the margin is too low the circuit may become unstable in use due to changes in conditions (temperature, supply voltage, component tolerance, aging and so on). The LTspice FRA is (currently) optimised for use with switch mode-powers supplies (SMPS), but it can be used with other feedback circuits – however, the set-up and analysis provided may not be so convenient for non-SMPS scenarios. A comment on Analog Devices’ forum indicates that a new version may improve this situation soon. To introduce the basic ideas behind and the use of the FRA, we will look at simple op amp circuits rather than dealing with the complexities of a SMPS – the FRA can certainly be used in this context because an op-amp-based example is provided as part of the LTspice 17.1 download. To appreciate the use of the FRA it is necessary to understand the principles of negative feedback and stability. Therefore, before looking at the LTspice FRA in detail we will introduce the basics of negative feedback and stability in the context of standard, well-known op amp amplifier circuits. Op amp basics The output (V O ) of an op amp (see Fig.1) without any additional external components is given by: VO = AO(V1 – V2). Practical Electronics | March | 2024 manner determined by the Amplifier input signal Amplifier output signal Input network feedback, while keeping the AO Vout voltage across the op amp’s Sinp Sinp Sai So So – V2 Ao 1 inputs zero. + − As can be seem from the Feedback network Feedback Circuit Circuit examples in Fig.2, the gain Here, V1 is the voltage on the nonMixing signal output input network equations for the amplifier inverting input, V2 is the voltage on the signal signal So Sf β as a whole only depend on inverting input and AO is the open-loop the resistor values. Strictly voltage gain, which is specified on a device’s speaking these formulae are datasheet and is typically in the range 70 to Fig.3. Example structure of an amplifier with negative approximations, but if the 150dB (approximately 3000 to 30 million). feedback. Note: this is specifically the non-inverting op op amp’s open-loop gain is For an ‘ideal’ amplifier, open-loop gain amp amplifier. much larger than the overall tends to infinity. An op amp amplifies the circuit gain the approximation is very good. voltage difference between its two inputs We have three different gain values which The gain of the op amp itself does not change (V1 – V2), not the voltage with respect to can be used when discussing the amplifier when we apply feedback – it is the gain with feedback. These relate to the three ground at a single point. of the whole circuit which is determined paths in the circuit depicted in Fig.4. First, Op amps are usually used with negative by the feedback. In fact, the input-output the amplifier on its own has an open-loop feedback – a fraction of the output signal relationship of the op amp remains exactly gain of AO = SO/Sai. Second, the whole circuit is fed back and subtracted from the input as given in the equation above when the – it is applied at the inverting input to (amplifier with feedback) has a closed-loop feedback is in place. This implies the input achieve the subtraction. This creates a gain of AC = SO/Sinp. Finally, the value voltage difference is actually Vout / AO, loop from the output back to the input and −bAO is known as the ‘loop gain’, which is then to the output again – hence the term not zero as in the preceding discussion. the gain around the closed feedback loop. ‘feedback loop’ and why the gain of the However, as with the representation of op amp device on its own is referred to as circuit gain with the resistor formula, the Gain calculations ‘open-loop gain’ (gain when the feedback approximation to zero input difference Referring to Fig.3 we can calculate the loop is open, or not connected). The gain is very good for op amps with very high closed-loop gain in terms of the open-loop of the whole circuit with feedback is called open-loop gain. gain and feedback factor. The feedback the ‘closed-loop gain’ (AC). signal is the output multiplied by the feedback fraction (bSO). Subtracting the The most basic and commonly used op Feedback structure amp amplifier circuits in which negative feedback signal from the circuit input gives An abstract diagram of the structure of an feedback is applied are the inverting or the amplifier input as: amplifier with feedback is shown in Fig.3. non-inverting amplifier configurations, as This a system structure diagram, not a circuit shown in Fig.2. In both cases the negative Sai = Sinp − bSO schematic. Such diagrams are widely used feedback is applied via a pair of resistors by control engineers when developing which act as a potential divider feeding a systems (eg, in industrial control) that are The amplifier (and circuit) output is the fraction of the output voltage back to the a lot more complex than an op amp circuit. amplifier input multiplied by the amplifier inverting input. The gain of these circuits is In the context of an amplifier, the signals open-loop gain: therefore related to the ratio of the resistor (labelled S) could be either voltages or values, which sets the proportion of the currents. In general, the input signal (Sinp) SO = AOSai output fed back by the potential divider. may pass through an input network, as The amplifier as a whole is either inverting shown, which in the simplest case just Substituting for Sai: (negative gain) or non-inverting (positive multiplies the input by one – for example, gain) depending on whether the input in the non-inverting op amp amplifier SO = AOSinp − bAOSO signal is routed to the inverting or nonthe input goes straight to the op amp. inverting input. For the inverting op amp amplifier, the Collecting the output terms together gives: In an op amp amplifier, the negative resistors form a potential divider for the feedback is regulating/controlling the input signal, LTspice so the input network is not Response SO + bA OSO = A– OS inp 1 17.1 and Frequency Analysis Part differential input voltage to the op amp to simply unity gain. be zero. The differential input to the op amp The input signal then passes to the mixing And rearranging to find the closed-loop is a function of the circuit input minus the network, which subtracts the feedback (Sf) gain, we get: 17.1is and Frequency Analysis – Part 1 feedback. If the input voltage to the circuit from the LTspice input. This performed byResponse the 𝑆𝑆" 𝐴𝐴& changes the op amp output changes until 𝐴𝐴! = = op amp, and in the case of the inverting 𝑆𝑆#$% (1 + 𝛽𝛽𝐴𝐴& ) the subtraction of the feedback reduces amplifier, the ‘summing junction’ combines the voltage across the op amp’s inputs to signals at the inverting input. The amplifier In a typical op amp amplifier AO is very 𝑆𝑆" and b is 𝐴𝐴&a moderate fraction so bA zero. Thus, the output voltage will track block in Fig.3 represents the open-loop𝐴𝐴 =large O = ! (1much ) + 𝛽𝛽𝐴𝐴&larger changes in the circuit’s input voltage in a gain of the op amp. is𝑆𝑆usually than 1 and we can #$% 𝐴𝐴&(1 + 1 The feedback is obtained approximate bAO) to bAO. This means 𝐴𝐴! = = Vin R2 𝛽𝛽𝐴𝐴 𝛽𝛽of AO cancel in the AC from the output of the that the instances + & Vout amplifier by passing it equation to give: R1 – Vin through the feedback network 𝐴𝐴& 1 – Vout R2 𝐴𝐴! = = (resistor potential divider in 𝛽𝛽𝐴𝐴& 𝛽𝛽 the op amp amplifiers) which + multiplies it by a factor of b, This leads to the situation discussed above, R1 so Sf = bAOSai. (b is known where the op amp amplifier's gain is set by AC = –R2 / R1 AC = 1 + R2 / R1 the feedback resistors (which determine b), as the feedback factor and is independent of the op amp open-loop gain typically less than or equal Fig.2. Op amp amplifiers. (as long as bAO is much large than one). to one.) V1 + Fig.1. Open-loop op amp. Practical Electronics | March | 2024 53 inductor has an extremely high impedance and effectively breaks the loop, allowing a Sinp Sinp Sai So simulation in which a test So Ao 1 + signal is injected to show the − Loop gain AC characteristics of the loop Sf –βAo = S' f / Sf (ie, the frequency response of the loop gain). Unfortunately, Break in loop to this method does not give very define loop gain accurate results. S' f β Another approach was So published by R. David Middlebrook, ‘Measurement Fig.4. Structure of an amplifier with negative feedback of Loop Gain in Feedback showing the open-loop (red), closed-loop (green) and Systems’, in the International loop-gain (blue) relationships. Journal of Electronics in 1975. This uses test signals injected into the Loop gain closed-loop system (in a simulation, voltage The loop gain is an important parameter and current sources can be inserted in the when considering the stability of feedback loop). This allows (through the theory systems.. By definition, the start and the end developed by Middlebrook) to find the of a loop are the same point, so if we write voltage and current gains of the loop and the loop gain simplistically this way, say, combine these to find the loop gain. If the SO/SO, we just get 1. We can define loop gain feedback loop includes a low impedance by breaking the loop, as shown in Fig.4. This driving a high impedance at some point, allows us to obtain two different signals Sf then the current gain has minimal impact so and S'f which are really at the same point just the Middlebrook voltage gain is equal in the loop giving a gain for the complete to the loop gain. This ‘voltage only’ version open-loop path as S'f/Sf, which does not of the Middlebrook method is used by the cancel to 1. We trace the entire path of the new LTspice frequency response analysis. loop in the system diagram from, and back to, the break, so it does not matter where the break is – we get the same expression Phase shift for loop gain. For the circuit in Fig.4, the The output of a circuit does not respond loop contains three elements: the amplifier infinitely quickly to changes at its input, (gain AO), the feedback section (gain b) and so any signal fed back from the output to the input will be offset in time with the negative summation (gain −1), so the respect to the original input. Phase shift loop gain for this system is these multiplied represents the delay of a sinewave signal together, which is −bAO. through a circuit at a given frequency. If We broke the feedback loop to help the delay is constant then phase shift will define loop gain, and in theory it may be increase linearly with frequency, but often possible to break the loop of a feedback this is not the case, particularly over wide circuit for the purposes of simulation or frequency ranges. measurement to find loop gain (we cannot Consider a simple case in which there measure loop gain directly from the original is a fixed delay from input to output of circuit voltages). However, breaking the the circuit whatever the input signal does loop and retaining enough ‘normal’ circuit (things are usually more complicated than behaviour to make a valid measurement this). Say, for example, this delay was 0.1μs. is not straightforward – for example, the If the input frequency was 100Hz this time output driving the break may have to be would be 0.001% of the signal’s cycle loaded with the same impedance it sees in time and could probably be considered the normal circuit, and the DC conditions insignificant. However, at 2.5MHz the 0.1μs need careful attention so that the bias levels delay is a quarter of the signal’s cycle time in the ‘broken’ circuit match those in normal of 0.4μs (1/2.5×106 = 4.0×10–7). This would operation. Often, it isn't possible to obtain meaningful results using a broken loop. usually be expressed by saying that the circuit had a phase shift of 90° at 2.5MHz (one complete cycle of the waveform is Measuring loop gain 360°). At 5MHz 0.1μs is half the cycle time There are a number of approaches to of the signal. This is a significant point overcome this. For example, in simulation because a phase shift of 180° is equivalent the correct DC levels can be achieved to multiplying the signal by −1. by inserting an extremely high-valued inductor instead of a pure open circuit. This effectively keeps the loop closed Instability for DC (for which the inductor is a short Consider the total phase shift through the circuit), preventing any small DC levels amplifier and feedback network (in Fig.3) being open-loop amplified to cause the as we increase the input signal frequency amplifier output to saturate at the supply – in line with the above argument, phase levels. For AC signals this super-sized shift will tend to increase. Once the shift Circuit closed-loop gain AC = So / Sinp 54 Amplifier open-loop gain AC = So / Sai reaches 180° we have effectively inverted our feedback signal – what was negative feedback has become positive feedback. Returning to the closed-loop gain equation from above: AC = AO / (1 + bAO). If the value of the term (1 + bAO) approaches zero then the value of AC will tend towards infinity. That is infinite closed-loop gain – this results in instability, specifically the circuit oscillates. The condition for which (1 + bAO) = 0 is bAO = −1. This condition for instability specifically concerns the loop gain, not the closed-loop or open-loop gains. Phase margin and gain margin Looking at this in more detail, since A and b are phasor quantities (they have magnitude and phase shift), we get oscillation when the magnitude of bA (loop gain) is at least one (written |bA| ≥ 1 ) and the phase shift due to bAO is ±180°. Generally, the gain of an amplifier will decrease, and the phase shift will increase, as frequency increases. The question is – will the above conditions for instability occur as frequency increases? We can measure how close a circuit is to being unstable using the concept of gain margin and phase margin. As the loop gain magnitude approaches 1 the phase shift must be less than 180°. The difference between the phase shift at this point and 180° is the phase margin. Second, as the phase shift around the loop approaches ±180° the magnitude of the gain must be less than 1 to prevent oscillation. This difference between the loop gain when its phase shift reaches 180° and 1 (which is 0dB) is the gain margin (usually expressed in dB). Fig.5 shows a frequency response plot for an amplifier loop gain with the gain and phase margins indicated. The gain margin and phase margin are a pair of values for a feedback amplifier which indicate its stability. These values are fixed for a given circuit and do not change with frequency (unlike phase shift and gain). If we can obtain a plot of loop gain and phase shift against frequency then it can be used to assess circuit stability. This is what LTspice’s new frequency response analysis provides. LTspice FRA example Fig.6 shows an LTspice schematic of an op amp inverting amplifier configured for use with the new frequency response analysis (.fra directive). We will show a quick Introduction to LTspice Want to learn the basics of LTspice? Ian Bell wrote an excellent series of Circuit Surgery articles to get you up and running, see PE October 2018 to January 2019, and July/August 2020. All issues are available in print and PDF from the PE website: https://bit.ly/pe-backissues Practical Electronics | March | 2024 Gain (dB) Phase shift 0 0 Gain margin Log frequency Fig.5. (left) Example variation of gain and phase shift around a feedback loop (loop gain) with signal frequency, illustrating gain margin and phase margin. Fig.6. (above) Example circuit for LTspice frequency response analysis. –90 Phase margin –180 example here and discuss LTspice frequency response analysis in more detail next month. The schematic in Fig.6 is based on an example provided by LTspice in the download. The circuit has an input voltage source added to provide a source for a standard AC analysis (.ac directive) to show closed-loop gain for comparison. Fig.7. AC analysis results for the circuit in Fig.6 – this shows variation of closed-loop gain magnitude (solid) and phase (dotted) with frequency. To switch between the FRA and AC analysis swap the text on the schematic between comments and SPICE directives. Frequency response analysis requires the addition of an FRA component to the schematic at a suitable point in the feedback loop, in series with the loop. In Fig.6 it is inserted between the op amp output and feedback resistors (between nodes A and B). The FRA component has initial letter <at> in the same way that resistor names start with an ‘R’, capacitors with a ‘C’ etc. In order to run a frequency response analysis the .fra directive is used, as seen on the schematic. The operation of the frequency response analysis can be configured by right-clicking the FRA component. This example used the settings provided in the download example. Before looking at the FRA results, Fig.7 shows a standard LTspice AC analysis for the circuit output at node A. The FRA component was disabled for this analysis. AC analysis requires an input source with an AC amplitude defined, which is V3 in Fig.6. V3 is a 0V DC source so it has no effect on the circuit other than for AC analysis. The results in Fig.7 show the variation of closed-loop gain with frequency. The FRA results are shown in Fig.8 – this shows the variation of loop gain with frequency and can be used for stability analysis. LTspice prints the gain and phase margin values on the response plot. The results look similar – they are both frequency responses, but they are calculated in very different ways. The AC analysis used a linearised model of the circuit and requires a source with AC configured, whereas the FRA used transient simulation with waveforms at various frequencies and requires an FRA component – more on this next month. Simulation files Fig.8. FRA results for the circuit in Fig.6 – this shows variation of loop gain magnitude (solid) and phase (dotted) with frequency. Practical Electronics | March | 2024 Most, but not every month, LTSpice is used to support descriptions and analysis in Circuit Surgery. The examples and files are available for download from the PE website: https://bit.ly/pe-downloads 55