This is only a preview of the May 2018 issue of Silicon Chip.
You can view 35 of the 104 pages in the full issue, including the advertisments.
Items relevant to "800W (+) Uninterruptible Power Supply (UPS)":
Items relevant to "Multi-use Frequency Switch":
Items relevant to "LTspice Simulation: Analysing/Optimising Audio Circuits":
Items relevant to "USB Port Protector – just in case!":
Items relevant to "12V Battery Balancer":
Items relevant to "El Cheapo Modules 16: 35-4400MHz frequency generator":
Purchase a printed copy of this issue for $10.00.
Y Using Analysing and optimising audio circuits by Simulation Part IV by Nicholas Vinen We concluded our last tutorial (September 2017) saying that our next LTSpice tutorial would cover simulating op amps and audio circuits. It has been a while coming . . . but here it is! S imulating audio circuits can be useful for a number of reasons, including: • optimising filter component values for the desired roll-off point and minimal passband ripple • characterising complex and/or cascaded filter responses – corner frequency, roll-off rates, out-of-band attenuation, bandwidth limitations, etc • optimising amplifier circuits for stability, bandwidth, etc • measuring frequency response and headroom • checking expected circuit operation • verify DC operating conditions • checking that component voltages, currents, dissipation and heating are within safe operating limits This article will cover most of the above tasks and the circuits and techniques presented here can be applied to the remainder (and others we haven’t mentioned). Filter optimisation There are dozens of different kinds of filters that you might use in an audio circuit, including low-pass, high-pass, band-pass and notch types from simple passive (RC, LC) filters to complex multi-pole active filters or resonant passive filters. The characteristics of the most simple RC filters can be calculated quite easily, using well-known formulas such as f (-3dB) = √(2π x R x C) to determine the corner frequency for an RC high-pass or low-pass filter. But as soon as you start working with multi-pole filters or multiple cascaded RC filters, the calculations become much more difficult. Luckily, simulating such circuits is simple and will quickly give you gain and phase plots. For example, let’s say that we have two cascaded RC low-pass filters with a buffer stage between them. And say they use identical components, so they have the same -3dB corner frequencies and 6dB/octave roll-off. We can use 1kΩ resistors and 1nF capacitors to keep it simple. So we expect the resulting combination to have a 12dB/octave roll-off but the -3dB frequency of a single filter (159kHz) is now the -6dB point of Fig.1: a simple secondorder RC low-pass filter drawn up in LTspice, using ideal buffer E1 to isolate the stages. We can then compare its performance to more typical second-order filter circuits to see their pros and cons. siliconchip.com.au Celebrating 30 Years the combined filter. So what is the new -3dB point? Simulating it Rather than using an op amp model as the buffer stage between the two filters, we’ll use a unity-gain voltagecontrolled voltage source. This has the benefit of being simpler to use (no need to wire up supply rails etc), infinite bandwidth, no distortion and no noise. To set up this simulation, we create a new schematic sheet in LTspice and add and wire up the components as shown in Fig.1. Refer to the earlier articles in this series for details on how to do this. See www.siliconchip.com. au/Article/10677 We already introduced the voltagecontrolled voltage source, in this case, component E1. You need to right-click on it and set the “Value” field to 1 so that it operates at unity gain. For the voltage source, right-click on it and click on the “Advanced” button to show all the fields, then set the “AC Amplitude” field to 1V (under “Small signal AC analysis”). We label the input and output nets using the “Label Net” button in the toolbar, for easier analysis later. Finally, select the Simulate -> Run menu option and then switch to the AC Analysis tab and set the type of sweep to Octave, the number of points per octave to 10, start frequency to 10Hz and stop frequency to 10MegHz (other options would be valid but let’s stick with these for now). Do not set the stop frequency to May 2018 43 Fig.2: Bode plots showing the frequency and phase response for the intermediate and output notes of the Fig.1 circuit. We can then use cursors to determine their -3dB points and calculate the roll-off rates. 10MHz, since this will be interpreted as 10mHz! Having run the simulation, click on the output node and a plot similar to that shown in Fig.2 should appear (we’ve also clicked on the junction of C1 and R1 to compare the response of a single stage). The output response is shown in green and the green dotted line is the output phase. The intermediate response is shown in blue. As you would expect, the combined response has a steeper roll-off. Now, to determine the -3dB point, click on the “V(output)” label at top and cursors appear, along with the box shown at lower right, which contains additional information. Drag the horizontal cursor to the right until the Mag: reading in the box is very close to -3dB and then you will see the corner frequency at left, which is just above 100kHz. Phase and group delay readings are also shown. Comparing other multi-pole filter arrangements The problem with cascading two RC filters with a buffer in between to produce a two-pole filter, is that the resulting output impedance pf the cascaded filter is relatively high. But it is possible to build a two-pole filter around a single buffer/gain stage and obtain a very low output impedance. Two common approaches to this are Sallen-Key and Multiple-Feedback filters. An excellent website for designing such a filter is at: siliconchip.com.au/ link/aajq One of the biggest problems with designing this type of filter to achieve a specific response is that you inevitably need components with unrealistic values, such as 4.39kΩ or 1.42nF. With some tweaking, you may arrive 44 Silicon Chip at component values which are close to what’s actually available. But that leaves us with two questions: how much does the deviation from ideal values affect the filter response, and which of the two filters topologies is best? LTspice can help us answer both these questions. For this exercise, let’s aim to build a realistic filter with the same -3dB point and roll-off as we determined above with our naive attempt, ie, 102.375kHz and 12dB/octave respectively. At the website above, we set the filter order to 2, cutoff frequency to 102.38kHz and experimented with the “Desired Rx” value until we got realistic looking values below. This was with a “Desired Rx” value of 2.4kΩ. We then drew up both resulting filter circuits in LTspice, as shown in Fig.3. There are several important points to note about this circuit we’ve drawn up. Firstly, we have chosen to use LT1464 op amps as these have 1MHz bandwidth and this will provide a good demonstration of how op amp bandwidth effects filter behaviour. Also, we have used the Net Label tool to label the supply rails of each op amp V+ and V- and we then added two extra stacked voltage sources, V2 and V3, both set to 5V DC with the junction connected to ground. By labelling the top and bottom V+ and Vas well, we’re providing ±5V supply rails for each op amp without cluttering up the schematic. The output of the “naive” filter has been re-labelled out1 so that we can label the two new filter outputs out2 and out3, for easy comparison. (In case you can’t immediately see out2 and out3, they are just above U2 and U3). U2 is used for the Sallen-Key second-order filter which uses two resistors and two capacitors, all with different values, while the MultipleFeedback second-order filter is based around U3 and it uses three equal-value resistors plus two capacitors. The Multiple-Feedback filter is an inverting type while the Sallen-Key is non-inverting; this may be imortant in some applications. While we were able to use equal-value resistors in the Multiple-Feedback filter, that isn’t guaranteed to always be the case. Note that the output of the two new filters is taken from the output pin of an op amp, so the impedance is low and can be fed into another filter network. You would need an extra op amp buffer for the naive filter to achieve the same result. Now since these are all second-order low-pass filters with the same corner Fig.3: here we’re simulating three low-pass filter circuits drawn using op amp models, all with a -3dB point of 100kHz. Celebrating 30 Years siliconchip.com.au if we needed to). So it ends up attenuating the signal even further. Another couple of things to note: both of the new filters give less attenuation of the signal below the -3dB point, ie, they roll-off more quickly which is good if you’re going for a “brick wall” type response. And the use of a real op amp has actually pushed the naive filter -3dB point slightly higher, to around 110kHz, which is why the curves don’t all meet at one point. Higher bandwidth op amps Fig.4: the resulting frequency response plots of the three filter circuits shown in Fig.3 (green=out1, blue=out2, red=out3). While the graphed lines may seem light here, they are quite visible on-screen. frequency, you would expect the results to be very similar but you might be surprised. Comparing filter responses We now run the same AC analysis as before but this time, after clicking on the out1, out2 and out3 nets to plot the response, we right-click on the phase axis at right and click the “Don’t plot phase” button to de-clutter the resulting Bode plot. We’ve expanded the plot to fill the window for increased clarity and the result is shown in Fig.4. The naive filter response is shown in green, Sallen-Key in blue and Multiple-Feedback in red. The most surprising aspect to this plot is that while both the additional filters have a much faster roll-off above the ~100kHz -3dB point, above 1MHz (the -3dB bandwidth of the op amps), the naive filter actually provides superior attenuation. And as shown the Sallen-Key filter does a particularly poor job at higher frequencies, with a peak at around -15dB attenuation at 1.8MHz and it’s not much better at higher frequencies either. This is because capacitor C4 couples some of the signal from the input straight to the op amp’s output and its limited bandwidth means that it isn’t able to prevent that coupled signal from feeding through. (To explain, there is no extra open-loop gain at higher frequencies and that means that negative feedback cannot act to provide a low output impedance). The Multiple-Feedback filter does a better job because capacitor C5 is siliconchip.com.au a smaller value and there are two resistors, R5 and R7, in series before it, plus C6 will shunt much of the feedthrough signal to ground. Even so, you can see that the slope of the red trace changes slightly around 1MHz to be more flat, allowing the blue trace of the naive filter to “catch up” to it at 1MHz. That’s because the naive filter starts with a completely passive RC filter which rejects at least some portion of the signal regardless of the op amp bandwidth. And the op amp’s limited bandwidth actually helps us here, since there’s no path for the signal to “feed through” it (ignoring parasitic PCB capacitance, which we aren’t simulating here although we could add it So how does this change if we use a higher bandwidth op amp? That’s easy to test; simply delete U1-U3 and replace them with LT1357s which have a gain-bandwidth product of 25MHz. Then re-run the simulation. The result is shown in Fig.5. All three curves now meet at the design -3dB point of 102.375kHz and it’s clear that the Multiple-Feedback filter now gives the best performance, with much less effect on frequencies below 100kHz than the naive filter, a much quicker roll-off above this point and very little change in its rate of attenuation up to 10MHz; just a slight change in the rate of attenuation, which reaches -75dB at 10MHz. By comparison, the Sallen-Key filter gives virtually identical performance up to 1.4MHz but it reaches a maximum attenuation of -50dB at 2.2MHz, above which is attenuation factor actually falls, giving -40dB at 10MHz. Its Fig.5: the same frequency response plots as shown in Fig.4 but this time, with 25MHz op amps, giving better results. You can see that the Sallen-Key filter is still less than ideal but its rebound has been pushed to a higher frequency. Fig.6: a similar plot to Fig.5 but this time up to 100MHz, so we can see how the filters behave between 10MHz and 100MHz. Celebrating 30 Years May 2018 45 Fig.7: a simplified hifi audio amplifier circuit simulated using components available in the libraries supplied with LTspice. curve crosses the naive filter for a second time at 2.73MHz, with the naive filter continuing to provide attenuation, reaching -72dB at 10MHz. If we go back to the schematic, right-click on the simulation command (which starts with “.ac”) and change the finish frequency to 100MHz (“100MegHz”), we get the plot shown in Fig.6. This shows that the Sallen-Key bode plot has a peak of -31dB at 35MHz, above which it again begins to slowly roll off. By comparison, the MultipleFeedback filter does continue to increase its attenuation at higher frequencies although at a reduced rate. The naive filter overtakes it at 15MHz, where both reach -78.5dB. The Multiple-Feedback filter reaches -100dB at 100MHz while the Naive filter is at -132dB by 100MHz. Simulating an amplifier with discrete components Our article on Amplifier Stability and Compensation in the July 2011 issue gave fairly detailed information on using SPICE to simulate an amplifier and test it for stability under difficult conditions, for example, when it is driven into clipping. Rather than go back over that, we will instead build a simple amplifier circuit in the simulator to analyse the amplifier efficiency, determine the dissipation in the major components and examine how power flows from the transformer through to the loudspeaker load. We’ve drawn up a minimalistic hifi Fig.8: the voltage across load resistor RL is shown in mauve while the dissipation in that resistor (ie, load power) is in green. 46 Silicon Chip power amplifier circuit in LTspice and this is shown in Fig.7. We’ve used only components from the built-in libraries. The test input signal, a 2.1V peak sinewave is from V1. This is fed into the base of PNP transistor Q1, which forms a differential input pair with Q2. Q2 is connected to the output via a 12kΩ/510Ω divider, setting the amplifier gain to 24.5 times. NPN transistors Q3 and Q4 are the current mirror load for the input pair while PNP transistor Q5 is the constant current source for their emitters. The differential stage output current flows from the collector of Q1 to the base of Q8, the VAS (voltage amplification stage) transistor which has a 100pF compensation capacitor, to stabilise the amplifier. Fig.9: this shows how the amplifier output voltage plus the AC and DC supply voltages behave when power is first applied. Celebrating 30 Years siliconchip.com.au Fig.10: this demonstrates how current is drawn in brief bursts from the simulated transformer secondaries at their voltage peaks. Q10 and its two base resistors form the Vbe multiplier that sets the bias voltage for the output stage and thus the quiescent current. The bias resistor values were determined experimentally and set the output stage quiescent current to 120mA per transistor pair. PNP transistor Q9 is the constant current source for the VAS while Q6 controls the base bias for both Q5 and Q9. The output stage consists of driver transistors Q11 and Q14 and power transistors Q12, Q13, Q15 and Q16 (in Darlington emitter follower configuration). These have 0.1Ω emitter resistors and there is an RLC filter at the output to isolate the load (at high frequencies) and ensure stability. The test load is an 8-ohm resistance, RL. The power supply consists of sinewave voltage sources V2 and V3 which represent the two halves of a centretapped transformer secondary (45-045VAC). This is rectified by bridge rectifier DP1-DP4 and the supply is filtered by a pair of 10,000F capacitors. Examining power supply behaviour Fig.8 shows the output voltage in mauve. This is a zoomed-in portion of the simulation output since the waveform is clipped initially as the power supply filter capacitors charge up. But if we’re interested in looking at the output power, that muddies the water. As expected, the output is a sinewave. The 2.1V peak input has been amplified by the 24.5 times gain to yield peak voltages of just over ±50V. The green plot is the instantaneous dissipation in the load resistor. This is plotted by holding down the ALT key in Windows and then clicking on the load resistor, RL. Control-clicking the green text at the top (“V(output)*I(RL)”) then yields the integral box shown at lower right. This reveals that the amplifier is delivering siliconchip.com.au around 165W average to the load in this condition. The instantaneous dissipation in RL is 0W when the applied voltage passes through 0V and rises to a peak of around 330W at both the positive and negative sinewave maxima. Note that this is a sine-squared waveform which is why there is a 2:1 ratio between peak and RMS power, not the sqrt(2) ratio you would expect for a normal sinewave. Fig.9 shows a “zoomed out” version of the simulation plot where you can see the V+ (green) and V- (blue) power rails initially charging up. This is unrealistically fast as we have simulated a transformer with a zero ohm output impedance; you could add a small series resistance and/or inductance if you wanted a more realistic simulation of amplifier switch-on. The mauve waveform once again shows the amplifier output and you can see that it is initially clipped by the low supply rail voltages, especially on negative excursions due to R25 and C11, which form an RC low-pass filter for the negative rail at the front end of the amplifier. These components are important to prevent supply rail ripple due to the load current from affecting the input pair and VAS but they do slow down the amplifier’s start-up somewhat. And as shown, they also make the waveform initially clip asymmetrically. Normally, this would not be a problem as there would typically be a relay between the amplifier and the output terminals with a delayed switch-on to prevent a thump from the speakers at power-up. The red and cyan traces in Fig.9 are the simulated transformer secondary waveforms and they show how the supply rails are pumped up when the transformer secondary voltages peak and the rails slowly decay, as the load current is drawn during the subsequent mains half-cycles. You can also see how the two halves of the centretapped secondary alternately charge up the supply rails. This is shown in more detail in Fig.10. This time the supply rails are plotted in blue (V+) and cyan (V-) while the simulated secondary voltages are in red and green. Current from voltage sources V2 and V3, representing the transformer secondaries, is shown in grey and mauve. Ignoring the initial very high current on the first mains half-cycle, the remaining current pulses are semirealistic and you may be surprised to see that zero current is drawn from the transformer most of the time, with brief peaks to nearly 40A being drawn over a ~1ms period every 10ms. Calculating amplifier efficiency If we zoom into the plot so that we remove the initial surge current and then CTRL-click the I(V2) text at the top of the window, this gives us an RMS current of 8.3A. If we assume a Class-AB amplifier efficiency of 70%, for 165W output we need an input power of 235W and with two 60VAC secondaries, you would expect 2A [235W ÷ 60V ÷ 2] = drawn from each supply rail. Fig.11: averaging the power drawn from the transformer to calculate the amplifier input power, so we can calculate its efficiency. The circuit is shown larger in Fig.7. Celebrating 30 Years May 2018 47 Fig.12: the instantaneous dissipation in the output and driver transistors. These can be averaged to estimate how hot they will get. The reason for the discrepancy is the fact that current is only drawn for such a short period during the secondary voltage peaks. This means that I^2R losses in the transformer, wiring, rectifier etc will all be a lot higher than you would get with a resistive load on the transformer. If you think about it, though, it’s very rare for a transformer to have a resistive load. Transformers are mostly used to drive rectifiers in similar configurations to this. Hence, transformer ratings tend to be quite conservative as they have to deal with supplying such high peak currents with a low duty cycle. So does this mean that a huge amount of power is being wasted in the transformer? Not really. It just means the power factor is poor. We can determine the real power drawn from the “transformer” by labelling the output (top) of V2 as V2V and the bottom of V3 as V3V, then re-running the simulation, and plotting the product of current and voltage. To do this, we right-click on the resulting plot and selecting “Delete Traces”, then right-click again and select “Add Trace” and type in the formula: “I(V2)*V(V2V)”. Add another trace with the formula “I(V3)*V(V3V)”. We can then zoom into a single mains cycle and controlclick the formula at the top of the window to get an average reading. The result is shown in Fig.11. You need to be careful when zooming that you get exactly 20ms (or a multiple thereof) on the horizontal axis or the averaged values will not be correct. We get a figure of very close to 123W for both V2 and V3. Thus the total power draw of the circuit is 246W. That means the actual amplifier efficiency is 67% [165W ÷ 246W], pretty close to the 70% that we estimated earlier. 48 Silicon Chip Determining device dissipation We can measure the dissipation in the output transistors, driver transistors and rectifier diodes by alt-clicking them and then control-clicking the formula that appears at the top of the window. Fig.12 shows the dissipation of one pair of output transistors in green and blue and one of the drivers in red. As you can see, we get a reading of around 17.5W for each of the four main output devices. Repeating the same exercise gives a dissipation figure of 2W total for the two drivers plus 2W in each of the rectifier diodes, for a total (including the load) of 245W [165W + 17.5W x 4 + 2W x 5], leaving just one watt unaccounted for, most of which turns out to be due to the 0.1Ω emitter resistors. So this shows how the simulation can help you determine efficiency, calculate device dissipation and so on. It’s a good idea to check dissipation for the smaller transistors too. Depending on the current through each stage, they could potentially be buys close to their specified limit as they would normally be in much smaller packages than the output transistors. You could also easily measure the peak and average current in the output devices to check that they are within with each device’s capabilities. Conclusion While this article has covered a lot of ground, there are still many other audio circuits that we have not discussed and which can benefit from a SPICE simulation but we don’t have the space to cover them all. However, the above should give you an idea of how to “probe” and measure the simulated circuits. It’s especially helpful for tweaking component types and values to achieve an optimal result. For example, you could increase the amplitude of the input sinewave to the amplifier and investigate what happens when the amplifier is driven into clipping. You could build a simulated loudspeaker load based on resistors and inductors and possibly even include a crossover network, to better explore how the load’s reactance affects amplifier operation, stability and efficiency. All the circuits shown in this article are available for download from the SILICON CHIP website (in a ZIP package) so feel free to experiment, probe, tweak and find out for yourself just how they work and what effect your changes will have. After all, you can’t blow anything up! In fact, why not over-drive things to destruction just to see what happens? It’s a simulation: you won’t have to buy any new components! SC Linear Technology More than a year ago, Analog Devices completed the acquisition of Linear Technology (the owners of LTspice). LTspice is still available as a free download but you can now access it via siliconchip. com.au/link/aajo You may find that if you have an older installation of LTspice, the automatic update feature no longer works because the URL it fetches is no longer valid. We suggest you download and install the latest version from the above link, which should then be able to keep itself up-to-date. One major advantage of the new version is that there are now many Analog Devices (ADxxxx) parts available to simulate, along with the existing set of Linear Technology (LTxxxx) parts. However! We have found the latest version of LTspice (version XVII) to be considerably less stable than the older version that we used (version IV). Hence, you may wish to keep your old version of the software in case these bugs have not yet been fixed. You may notice that some of our screen captures are from the earlier version, for this reason. Celebrating 30 Years siliconchip.com.au