This chapter provides an overview of several Harmonic Balance (HB) analysis methods. The HB method is a powerful technique for the analysis of high-frequency nonlinear circuits such as mixers, power amplifiers, and oscillators. The method matured in the early 1990s and quickly became recognized as the simulator of choice for relatively small, high-frequency building blocks. With the adoption of new developments in the field of numerical mathematics, the range of applicability of HB has expanded to very large nonlinear circuits, and to circuits that process complicated signals composed of hundreds of spectral components. Cadence® AWR® Microwave Office® software incorporates the modern Cadence® AWR® APLAC® HB simulator, which is built on the latest developments in numerical mathematics and circuit simulation. This APLAC simulator is the default HB simulator in the AWR Microwave Office program, and should be used for all new designs. However, for assured backward compatibility with older design project simulations, the AWR Microwave Office program still includes its older, "legacy" HB simulator. The principle of operation, the most important features, and some common applications of HB simulation are summarized in the following section after a brief comparison of HB and transient simulators.
Transient simulations allow the simulation of switching behavior, while HB simulations yield steady state solutions. Transient simulations can handle circuits that are not ordinarily responsive to HB simulations such as frequency dividers, elements or circuits with hysteresis, highly nonlinear circuits, and digital circuits with memory. Both HB and transient simulators are available in the AWR Microwave Office program.
In cases where both HB and transient analysis are applicable, the better choice is dependent on the stimuli, circuit type, available element models, and the desired measurements. Harmonic balance is a frequency domain solver and transient analysis is in the time domain. For example, transient analysis is the better choice if the stimuli are not periodic and have short rising or falling edges, the circuit shapes pulses using a large number of transistors, and the measurement is rise or fall time. If the stimulus has a finite and discrete spectrum, the models are S-parameter files, and the desired measurement is power at a specific frequency, then HB is the better choice.
In most cases, you can use both simulators to solve the same problem and verify the results. The choice of which simulator to use is primarily a matter of efficiency. For example, during the design phase, microwave amplifier designers often use large capacitors and inductors (ideal bias tees) to block DC from the input and output, and to choke off the RF signal from the DC supplies. These capacitors and inductors have time constants that are significantly larger than the period of the input signal. To simulate the steady-state response of such an amplifier using transient analysis, you may need to simulate hundreds or thousands of periods for the transient effects to die out. Otherwise, to see the start up of an amplifier from when the input signal is first switched on, HB analysis requires two tones to represent the switched RF signal, one of which is a pulse with a very low frequency and hundreds of harmonics.
Unlike time domain simulators, HB simulators analyze circuits in the frequency domain. The development of frequency domain simulation technology was motivated by the following deficiencies of time domain methods in applications to high-frequency circuits:
Distributed circuit elements are almost exclusively modeled, measured and analyzed in the frequency domain, and their incorporation in SPICE-like simulators is notoriously unreliable and inefficient.
Multi-tone simulations (those that involve an application of two or more sinusoids that are harmonically unrelated) are very common in RF and microwave applications but, again, very difficult to handle in time domain simulators. Consider, for example, an amplifier that is to be tested by an application of two equal-amplitude sinusoids located at 9.999 GHz and 10.001 GHz. Such a test is frequently applied to determine the third-order intercept, a popular figure of merit of an amplifier's linearity.
The two-tone input may be viewed as a high-frequency carrier modulated by a comparatively very slow sinusoid where, in this case, f_{carrier} = 10 GHz and f_{modulation} = 1 MHz. So, there are 10,000 carrier cycles per one cycle of the modulation (envelope) signal and, in addition, the simulator must follow the slow envelope over several periods to determine the steady-state. More importantly, a time domain simulator takes many steps per carrier cycle in order to maintain accuracy. In all, each unknown circuit waveform (in a time domain simulator, "unknown circuit waveforms" are usually the node voltages and certain branch currents) is sampled at hundreds of thousands of instants to find the solution, and worse, the number of samples increases with the ratio of carrier/envelope bandwidth. The solution process is therefore slow, memory consuming, and often simply impractical.
Many high-frequency circuits are high-Q, implying that they exhibit transients that last over hundreds and even thousands of carrier cycles. RF and microwave designers are primarily interested in steady-state responses, and time is wasted in the process of simulating through the transients.
HB simulators overcome these problems in a rather elegant and efficient manner, by resorting to a frequency domain formulation of circuit equations (equations that arise from an application of Kirchoff's laws and the circuit elements' constitutive relations.) The frequency domain formulation is obtained by substituting the unknown waveforms with their phasor equivalents, and then matching the phasor coefficients that correspond to distinct frequencies.
The following figure illustrates the principle behind HB simulation.
As shown in this figure, the circuit is partitioned in two subnetworks -- one that contains all the linear elements and another that encompasses the nonlinear devices. The voltages at the interconnecting ports are considered as the unknowns, so the goal of HB analysis is to find the set of voltage phasors in such a way that Kirchoff's laws are satisfied to desired accuracy. One way to state this goal in formal terms is:
Find
V_{1}(ω_{k}),V_{2}(ω_{k}),...,V_{N}(ω_{k}) | (6.1) |
for all ω_{k} such that relation
|I_{L}(ω_{k})-I_{NL}(ω_{k})|<ε | (6.2) |
holds at each interconnecting port.
Here, ω_{k} is the set of significant frequencies in the port voltage spectra and ε specifies the desired accuracy.
The solution search, in most general terms, consists of the following steps:
Specify the set of significant frequencies, specify the desired accuracy, and determine an initial guess at the solution.
Calculate the currents that enter the linear subnetwork.
Calculate the currents through the nonlinear devices.
Calculate the difference between the two sets of currents.
Determine a new guess at the solution in a way that reduces the difference.
Repeat the process starting at Step 2 until Kirchoff's laws are satisfied.
The elegance of the HB approach, in reference to the problems seen by time domain simulators, lies in the following observations:
At each step of the iterative solution search, the currents entering the linear subnetwork are related to the interconnecting port voltages by the linear subnetwork's Y-parameters. Distributed components, therefore, are simulated in the most natural way, by means of frequency domain linear circuit techniques.
The frequency domain representation of two-tone signals, as will soon be apparent, usually consists of less than 100 terms. This is in contrast to the time domain representation that requires hundreds of thousands of samples.
HB simulators impose the steady-state conditions by virtue of phasor expansion of the unknown signals. Simulation times are, therefore, independent on the length of circuit transients.
Knowing the basic steps of HB analysis, a number of practical questions need to be answered. Some of these questions have a significant impact on the accuracy, speed and ultimate success of the simulation, as discussed in the following sections.
In general, phasor equivalents of nonlinear circuit waveforms consist of an infinite number of terms. If a circuit is driven by a sinusoidal waveform at a frequency ω_{0}, for example, these terms correspond to frequencies in the set nω_{0},n = 0,1,...,∞
as shown in the following figure.
For the purposes of simulation, you truncate this representation to a finite set of terms by discarding components beyond some point n=N. The act of spectrum truncation is a natural one, however, as high-frequency terms become less significant due to the band-limited nature of physical circuits.
Generally, the choice of N depends on the degree of nonlinearity. Power amplifiers operating deep in compression, for example, require more terms than low-noise amplifiers or amplifiers that behave almost linearly. The former may require N=8, for example, while the latter may need as little as N=3.
The idea of spectrum truncation is slightly more complicated in the case of "multi-tone" excitations. A multi-tone excitation involves two or more tones that are not integer-related, as in the previous example that involved ω_{1}=9.999 GHz and ω_{2}=10.001 GHz. In that case, it may be shown that circuit phasors correspond to frequencies in the set
Again, you truncate this set as shown in the following figure.
In general, the spectral components that are retained in the simulation are given by
|mω_{1}+nω_{2}| | (6.3) |
, where
In the previous figure, the truncation was performed using M=N=2. The terms nω_{1} are often referred to as tone-1 harmonics and, similarly, mω_{2} are called tone-2 harmonics. The multipliers m and n are referred to as harmonic indices. The quantity |m|+|n| is known as the order of an intermodulation (also, mixing or distortion) product.
The two-tone spectrum shown in the figure may be simplified further by discarding intermodulation products that are higher than some K=|m|+|n|. In a near-linear low-noise amplifier tested under two-tone excitation, for example, experience shows that the terms at 2ω_{2}-2ω_{1} and 2ω_{2}+2ω_{1} are negligibly small. These terms being of order 4, it may be reasonable to exclude them from consideration by setting K=3. Modern HB simulators, like the ones featured in the AWR Microwave Office program, are very efficient and, in terms of speed, far less sensitive to the number of frequencies than early HB simulators; the speed improvement gained by limiting K is therefore small, and setting it to a small number should be avoided.
The case of three-tone analysis is analogous to the two-tone situation described previously. Three-tone simulations are very useful for (but not limited to) linearity testing of mixers, where the circuit is subject to an LO excitation and two-closely spaced sinusoids as an IF (or RF) input. In this case, every waveform in the circuit has an equivalent phasor representation at frequencies in the set
and this set is truncated subject to
Typically, the circuit behavior with respect to the LO signal is highly nonlinear, while the input signal suffers relatively mild distortion. In applications, therefore, P should be set larger than M and N; typically, P is at least 5 (and often two to three times as high), versus 2 or 3 for the remaining limits.
Regardless of the type of simulation, you should verify that the frequency set used in the analysis provides accurate results by increasing the number of frequencies slightly, repeating the simulation, and verifying that the simulation results changed by a negligible amount.
For most users, it is intuitive that a pure sinusoidal input requires single-tone analysis, and that two closely spaced sinusoids require a two-tone analysis. Confusion arises in simulations that involve sources such as square-wave pulses, which consist of a large number of harmonics that are not closely-spaced.
To prevent confusion, you should keep in mind that a simulation is considered n-tone if n is the smallest number of frequencies whose integer linear combinations describe all the other frequencies in the source. A square wave signal, or any periodic signal, has frequency components that are integer multiples of one frequency -- namely, the fundamental; therefore, such a simulation is considered single-tone.
As previously presented, the calculation of currents entering the linear ports is rather straightforward as it involves the familiar theory of linear multi-ports in the frequency domain. It is, however, less obvious how an HB simulator calculates the nonlinear device currents.
Nonlinear devices are almost exclusively specified as time domain functions of the controlling voltage waveforms. In an HB simulator, however, the controlling voltages are represented in the frequency domain. To evaluate the nonlinear device functions, the simulator resorts to the following procedure: 1) it converts the voltage phasors to the time domain by application of Fourier transformations 2) it evaluates the nonlinear devices in the time domain, and 3) it applies another set of Fourier transformations to obtain the current phasors.
Because of this brief excursion to the time domain, HB simulators are sometimes referred to as mixed (frequency-time) domain techniques. This is mostly a matter of nomenclature, but the frequency domain label is preferred because of the phasor representation of the unknown signals.
Domain transformations introduce, to a varying degree, inaccuracies in the evaluation of nonlinear devices. These inaccuracies are caused primarily by the aliasing phenomenon, the degree of which depends on the level of nonlinearity and the number of frequency components taken into account in the simulation. In principle, aliasing effects may be reduced to negligible levels simply by performing the analysis with a very large number of frequencies. This, however, is undesirable since it leads to slow simulations. A simpler method for reducing the effects of aliasing is based on what is known in HB terminology as "oversampling".
The lower limit on the number of time domain samples used in the evaluation of nonlinear devices is 2H (the Nyquist limit,) where H is the number of significant frequencies. To reduce aliasing, you are given the option of increasing the number of time domain samples beyond the Nyquist limit; the resulting number of samples is some multiple of 2H, for example, 2rH. Once the nonlinear device currents are evaluated at the 2rH time samples, a Fourier transformation yields rH frequency components of the currents. Finally, the rH components are truncated back to the original H components that were selected for the simulation.
Oversampling is an effective means of reducing the effects of aliasing without paying a significant penalty in simulation time. The question arises as to when to use it and what the right oversampling sampling factor should be.
In the AWR Microwave Office program, the default oversampling factor is 1. This should be sufficient in a majority of simulations with the possible exception of intermodulation analysis of mixers. In mixer intermodulation analysis, the simulator must be able to capture intermodulation products that can be as much as 100 dB smaller than the largest signal in the circuit (normally, the LO). Since the LO is very large, otherwise minor aliasing effects could effectively "mask out" the crucial intermodulation products or, at least, cause errors in their calculation. You can prevent this by properly selecting the set of significant frequencies, and by selecting a larger oversampling factor. You should check the results by repeating the simulation with a larger set of significant frequencies and a larger oversampling factor.
HB simulation is an iterative process that terminates when Kirchoff's laws for the circuit are satisfied. Two criteria are used to determine whether these laws are satisfied: the maximum absolute tolerance and the maximum relative tolerance between the linear and nonlinear currents at each frequency and at each interconnecting port. The simulation ends when either of these two criteria are met:
The default values used in the AWR Microwave Office simulator are sufficient in a majority of situations, but you should be cautious when simulating circuits that feature very small, but nevertheless significant, signals.
The simulator makes a finite number of attempts at satisfying Kirchoff's laws, after which it either reports convergence failure or it resorts to source stepping.
Convergence failures, though rare, are usually a consequence of very strongly nonlinear circuit behavior. In such cases, one difficulty encountered by the simulator is a lack of a "good guess" at the solution. Normally, the DC solution or the linear approximation of the circuit constitute a good guess, but that may not be the case for strongly nonlinear circuits.
To find a better initial guess, the simulator reduces the specified excitation level (thereby lowering the level of circuit nonlinearity) and attempts to find the "reduced" solution. Upon success, it uses that solution as the initial guess when solving the original problem.
Sophisticated convergence control algorithms in the APLAC HB simulator, coupled with source stepping, result in successful convergence in most situations. Occasionally, however, the simulator fails to converge. The following are some of the common causes and solutions:
Circuit instabilities. If the circuit being analyzed is not conditionally stable (or, in the case of oscillator analysis, unconditionally unstable), harmonic balance is likely to have a difficult time converging. Often an instability is caused by S-parameter data that has been extrapolated to DC or the higher harmonics of the simulation frequency. With the default (linear) interpolation, this extrapolation often results in devices that generate power.
Too few frequency components. If the circuit being analyzed is strongly nonlinear, it is important, both for accuracy and convergence, to specify a sufficient number of frequencies in the simulation. Ensuring this is the first step in troubleshooting convergence problems.
Nonlinear device modeling. Discontinuities in nonlinear model equations and their derivatives are a common source of convergence difficulties. When utilizing user-defined models, it is imperative to model nonlinear functions and their derivatives smoothly. General-purpose models have been devised with continuity in mind, but problems can still occur if their parameters are entered or extracted incorrectly.
For additional information on addressing convergence failures, see “APLAC HB Simulator Convergence” and “HB Simulator Convergence”. Further options for speeding up or improving convergence are available on the Circuit Options dialog box APLAC Sim tab under Error and Convergence Settings and Harmonic Balance Analysis Options. See “Harmonic Balance Options” for more information.
There are global and local Harmonic Balance options in the AWR Microwave Office. These two options differ in scope but are otherwise identical.
Global options are, by default, applicable to all schematics in the circuit. Sometimes, individual schematics contain circuits for which a set of options other than the global options yield faster or more accurate results. In this case, you can use local options to override global defaults.
Choose Options > Default Circuit Options to display the Circuit Options dialog box for setting global defaults. You can set local options for a schematic by right-clicking the schematic in the Project Browser and choosing Options to display the Options dialog box.
The following sections describe the available options.
Tone 1, Tone 2, and Tone 3 Harmonics values correspond to the quantities M, N and P in “Choice of Significant Frequencies”. Tone 1, Tone 2, and Tone 3 Over Sample specify the oversampling factor "r" discussed in “Calculation of Nonlinear Device Currents”. The default value r=1 is typically adequate; a possible exception is intermodulation analysis of mixers.
Limit Harmonic Order enables spectral truncation of harmonic components an order higher than Max Order, which is analogous to the quantity K in “Choice of Significant Frequencies”. Apply 'Max Order' to Intermods Only truncates only the intermodulation products with orders higher than Max Order, while including all the harmonics specified for each tone under Tone X Harmonics.
For example: in a two-tone simulation, Tone 1 and Tone 2 are set to seven harmonics each, Max Order is set to five, and both Limit Harmonic Order and Apply 'Max Order' to Intermods Only are selected. The following table shows the harmonics included in the simulation:
AWR Microwave Office software allows you to specify a project-level frequency sweep, as defined on the Project Options dialog box Frequencies tab. You can also define frequency sweeps for individual schematics on the Frequencies tab of the Options dialog box. In addition, you can define multiple frequency sweeps inside a schematic using the SWPFRQ control available in the Simulation Control category of the Elements Browser.
When setting up a nonlinear measurement, you can use any of these frequency sweeps for the fundamental frequency of the first tone. In the Add/Modify Measurement dialog box, simply choose the appropriate sweep in Sweep Freq by clicking the arrow button next to the option. The menu title changes from Sweep Freq (FDOC) when you choose Document (using the frequencies in the schematic's Options dialog box) to Sweep Freq (FPRJ) when you choose Project (using the frequencies in the Project Options dialog box) to Sweep Freq (FSWP1) (using the frequencies from the first SWPFRQ control) and so on.
The fundamental frequency for tones 2, 3, ...8 are set directly on the source element in the schematic.
Single-tone simulations are performed on the set of frequencies defined by
nω_{0},n=0,1,...,N | (6.4) |
The fundamental frequency, ω_{0}, is defined by the Nonlinear Frequencies or Project Frequency controls.
You can specify a variety of excitations for single-tone analysis, including sinusoidal, square wave and arbitrary file-based.
Two-tone simulations are performed on the set of frequencies defined by
|mω_{1}+nω_{2}| | (6.5) |
The tone-1 fundamental, ω_{1}, is controlled (as always) by the Nonlinear Frequencies or Project Frequency controls. There are several methods to specify the tone-2 fundamental. Some sources allow direct specification of ω_{2}, and others allow a specification of ω_{2} as an offset Δω from the tone-1 fundamental. The fundamental frequency of the second tone may, in addition, be specified as a function of the fundamental frequency of the first tone. To specify tone-2 as a function of tone-1, you use the _FREQH1 reserved variable, which takes on the value of the tone-1 fundamental frequency in global project units. For example, if Δω=0.1 GHz, you can define ω_{2} by entering _FREQH1 + 0.1 for the tone-2 source frequency, assuming the project frequency units are in GHz.
The frequency of tone 2 and higher can be swept independently using a SWPVAR block, so that all combinations of tone 1 and tone 2 frequencies are simulated. For example, to independently sweep the Fdelt parameter of a PORT2 element, or the Freq parameter of a PORTFN or PORT_SRC element, right-click the parameter in the schematic and choose
.Three-tone simulations use the set
|mω_{1}+nω_{2}+pω_{3}| | (6.6) |
The fundamentals may be specified directly in the source (using the PORTFN element) or by a combination of single and two-tone elements. For example, tone-1 and tone-2 may be specified by the PORT2 element while PORTFN may be used to specify the third.
AWR Microwave Office software supports simulations with up to eight tones. Tone X Harmonics and Tone X Over Sample options for tones 4 through 8 are set directly on the port (or voltage or current source.) Double-click the element symbol in the schematic to display the Element Options dialog box, then click the Show Secondary button. The NHarm and NSamp parameters set the number harmonics and oversampling factor, respectively.
There are two types of sources in AWR Microwave Office software: port sources and discrete sources. Discrete sources, which are found under Sources in the Elements Browser, are ideal voltage or current sources. Port sources, which are found under Ports in the Elements Browser, are defined by their available power and termination impedance.
Port sources serve two purposes. First, they provide a convenient and intuitive definition of power sources; second, they define the inputs and outputs of a circuit, allowing its use as a subcircuit within another schematic.
There are several types of ports used to specify excitations. A port is added to a schematic by dragging it from the Elements Browser and dropping it on the schematic. You can also double-click an arbitrary Port element and change the Port Type on the Element Options dialog box Port tab. For example, consider the simple termination (passive port) element located on the main toolbar:
Nonlinear measurements allow you to measure voltage, current, power, and more. Although categorized as nonlinear measurements, you can use them in conjunction with linear circuits, as long as a large signal port or source is present. To select a nonlinear measurement in the Add/Modify Measurement dialog box, under Measurement Type, expand the Nonlinear node and select a type from the list. Each measurement type offers multiple measurements; for example, large signal S-parameters, power at a specific harmonic (Pcomp), voltage spectrum (Vharm), or current waveform (Itime) and others.
A brief description of the selected measurement is provided below the lists. For detailed information about the measurement, click the Meas Help button. Nonlinear measurements generally require knowledge of specific currents or voltages (or both), which are selected in Measurement Component. If the measurement is to be made at one of the ports in the top level schematic, you can select that port in Measurement Component.
When measurements need to be made internal to the circuit, there are ways of identifying the relevant currents and voltages, without the insertion of invasive elements that break the physical connections in the circuit.
A good way to identify internal circuit voltages and currents for measurements is the measurement probe (M_PROBE). When placed on an element pin, you can select this probe as a measurement component to identify the voltage on that pin, the current into that pin, or the power calculated from the voltage and current. If an M_PROBE is placed inside a subcircuit, then the list includes one entry for the M_PROBE per instance of the subcircuit. Note that M_PROBE must be placed on a pin; it does not identify a voltage if placed in the middle of a wire. After simulation you can move the M_PROBE to check its associated measurements at different pins, without simulating again.
Pins can also be identified for voltage and current measurements without an M_PROBE. When setting up the measurement, click the ellipsis button next to Measurement Component to display a view of the schematic that you can navigate.
Double-click any element pin, or select the element, and identify its pin from the list on the left. You can also select a 2-port element: voltage is measured at pin 1 (numbered or marked with a slash on the symbol) with pin 2 as the reference. Current is measured as flowing from pin 1 to pin 2 on all elements except sources, where the measurement direction is reversed.
You can measure power by selecting a Measurement Type of Nonlinear > Power in the Add/Modify Measurement dialog box. Measurements of this type also require a Measurement Component. If the selected measurement component is an M_PROBE or an element pin, the power is calculated as the product of the voltage at that pin, and the current into it. If an element is selected, then the power is measured as the sum of the powers at all pins of that element. This is equivalent to the power dissipated in that pin.
Whenever possible, power measurements have complex values; for example, power at a specific harmonic (Pcomp). In some cases power measurements must include the real part only, if they are to be useful and logical; for example, total power (PT).
Commonly, you want to measure power supplied by a source and power dissipated in a load (or voltages and currents associated with the source and the load.) You can do so by selecting the corresponding port or source as the Measurement Component. Currents, voltages, and powers are computed for ports, as shown in the following figure.
Note that only the ports in the top level schematic are available as measurement components. When measurements are made on a top level schematic, ports in the lower level only indicate connectivity, and do not present a load to those subcircuits.
Multi-Rate Harmonic Balance (MRHB) is available for the APLAC harmonic balance simulator only. MRHB is a technique of controlling what frequencies are simulated for each model in the circuit. For circuits with frequency conversion, this can significantly decrease the simulation time without losing accuracy. The main reasons to consider MRHB are:
Enable HB simulation for a circuit that wouldn't be possible otherwise due to time or memory limitations.
Turn a slow HB simulation to a quicker one.
MRHB should not be used if:
The circuit simulates in a few seconds already.
The circuit is a single-tone simulation.
Every element in the circuit truly shares the same frequencies.
The following example uses a simple up-converter circuit to demonstrate the basic concept of MRHB.
where f1 is the tone set at the input port and f2 is the tone set at the LO of the mixer. With HB analysis, there are many mixing products from f1 and f2 at the output of the mixer. See the following spectrum plot for a sample spectrum at the output of the mixer.
For this example the amplifier at the output of the mixer is narrow band. See the amplifier response trace on the graph that shows the amplifier is matched at the f1+f2 signal and quickly attenuates the other frequencies.
For traditional HB simulation, the amplifier at the output is solved for all the possible frequencies. For MRHB, the amplifier at the output is configured to only simulate at the dominate frequency. The following figure shows the spectrum at the output for the traditional HB analysis.
The following figure shows the spectrum with MRHB.
Finally, the following figure shows the voltage waveforms at the output of the circuit.
In this simple example, there may not be a lot of time and memory savings from having the last amplifier use a limited set of frequencies. On circuits with several frequency translations, however, the item and memory savings is significant. See examples in the Cadence® AWR Design Environment® platform to see circuits that are significantly faster without a loss of accuracy when using MRHB.
MRHB is configured by using MRHB blocks in a schematic, available from the Simulation Control category of the Elements Browser. Each model must be assigned to an MRHB block for the simulation to function, including ports and sources. You assign the block from the Model Options tab of the Element Options dialog box. See “Element Options Dialog Box: Model Options Tab” for details on this dialog box. Use the MRHB ID parameter name in the Multi-rate Harmonic Balance section of this dialog box.
You can visually inspect which models are in a specific group using the group highlighting feature. For more information about this feature see “Viewing Items for Extraction”.
Note that you can simplify the setup process by assigning blocks to subcircuits instead of all the individual models in the circuit.
Traditional harmonic balance configures the number of tones by the number of independent sources used in the design and the number of harmonics specified for each harmonic. In MRHB, the MRHB block configures these settings and applies them per model.
Determine the number of tones for the block you are configuring based on whether or not there is frequency conversion, and the type of input. For example, if your block is equivalent to a single-tone amplifier, then tones would be 1. If your block is equivalent to a two-tone amplifier, then tones would be 2. If your block is equivalent to a single-tone mixer, then tones would be 2. If your block is equivalent to a two-tone mixer, then tones would be 3.
Determine the new fundamental frequencies for each tone. These are set on the TONESPEC parameters and are set to the proper combinations of the unique tones in the original circuit. This might be as simple as typing "f1" which means tone 1. You can also type in combinations of tones, such as "2f2-f1" or "f1+f2"
Set up the tone truncation type and order. This is similar to setting the number of tones for each harmonic and the maximum order for intermodulation products.
For the tone truncation, the following figures help explain the meaning of the settings. For discussion purposes, this example uses a mixer with a 50 MHz IF frequency (tone 1) and a 1 GHz LO frequency (tone 2). For the Box TRUNC type you specify the maximum number for each tone, so the order of the tones is not limited. The order of the tones is the sum of the integers in front of the frequencies. For example "f1" is order 1, "f1 + f2" is order 2, "2f2-f1" is order 3. The following settings
will include the following harmonics. Note that there are two signals from the LO frequency (1 and 2 GHz) and then there are three sidebands for each of these frequencies.
For the Diamond TRUNC type you specify the maximum order for all the tones. The settings are as follows
will include the following harmonics. Note that there are two signals from the LO frequency (1 and 2 GHz) and then the number of sidebands for each LO frequencies decreases for each higher tone 1 signal.
For the Box and Diamond TRUNC type you specify the maximum number for each tone and the maximum order for all the tones.
AWR Microwave Office software is capable of analyzing noise in nonlinear circuits. Typical applications include:
Mixer noise figure simulation
Simulation of noise spectrum in amplifiers
Phase noise simulation is similar to noise analysis as described in “Phase Noise”. This section focuses on the background behind nonlinear noise analysis and its applications to mixer noise figure simulations.
Noise in electronic circuits exists in various forms, such as thermal, flicker, and shot noise. The following figure displays how a noise spectral density at an arbitrary node in a nonlinear circuit resting at DC may appear:
The low frequency portion represents low frequency noise, such as flicker noise, whereas the flat portion denotes the contribution of thermal and shot noise sources.
For the purpose of simulation, the noise spectrum is divided in a finite number of intervals over the frequency range of interest, as the following figure illustrates:
where each noise "sample" represents the noise power contained in a 1 Hz bandwidth.
If the circuit behaves linearly, a noise sample at some frequency ω_{n} contributes to output noise power at ω_{n} only, as follows:
Noise-related performance measures, such as noise figure and noise temperature, are computed by established correlation matrix techniques [1].
This is more complicated in the presence of a large signal drive, such as the LO pump in a mixer. If noise is assumed to be small by comparison to large-signal waveforms, the action of the LO is frequency translation of noise samples by the multiples of the LO frequency, as shown in the following figure.
Noise samples in a nonlinear circuit driven by a large-signal waveform are commonly referred to as noise sidebands. As the previous figure shows, the behavior of noise sidebands is analogous to the behavior of RF and IF signals in a mixer. In fact, the mathematical formulation that forms the basis for nonlinear noise simulation is very similar to the classical large-signal-small-signal [3], also known as conversion matrix, mixer analysis.
The circuit is first simulated with noise sources excluded, subject to large-signal excitation alone. Following large-signal analysis, noise sources are introduced at the ports connecting the nonlinear elements to the rest of the network, as shown in the following figure.
N_{L} and N_{NL} are random phasors of noise currents evaluated at each of the noise sidebands. N_{L} represents the Norton equivalents of all bias-independent noise sources, such as thermal noise sources, scattered within the linear subcircuit; N_{NL} represents bias-dependent noise sources contributed by the nonlinear components. Mean-square values of random noise phasors are their spectral densities. In the case of shot noise, for example,
q being electron charge, and I_{DC} being the bias current of the device contributing shot noise.
Conversion matrices relate the sideband phasors of small current excitations, such as N_{L} and N_{NL}, to the corresponding port voltage phasors. Formally, this relation may be expressed as V=T^{-1}N, ^{[1]}
where T is the conversion matrix and V, N are vectors of noise voltage (current) sidebands at interconnecting ports. A mean-square operation on the above relation yields the samples of noise voltage spectral densities in terms of samples of the known current spectral densities.
Noise analysis is best illustrated using a simple example.
The mixer shown in the schematic operates as an upper-sideband downconverter, with IF frequency in the range 0.5-0.6 GHz. The LO frequency is 3.5 GHz.
A noise analysis is executed if the noise control element NLNOISE (located in MeasDevice > Controls in the Elements Browser), is placed on the schematic. The following figure shows the schematic symbol of the NLNOISE element.
The following are NLNOISE parameters:
PortTo is the index of the output port. In the example, the output is the IF port and its index is 3.
PortFrom is the index of the input port. In the example, the input is port 1 (RF).
NFstart, NFend, and NFsteps define the range of noise frequencies to sweep over.
SwpType defines the type of noise frequency sweep (linear or log).
Noise Frequency Notes:
The following are comments on noise frequencies defined by NFstart, NFend, and NFsteps.
Recall that noise is analyzed about all the multiples of the LO, as shown in the following figure.
If you are interested in the noise figure of a downconverting mixer, for example, the most natural way to define noise frequencies is to specify the bounds of the upper-sideband noise range (N1,upper), which is 4.0 - 4.1 GHz in the example. However, any other frequency range is acceptable as well, as the simulator automatically sets up the remaining sidebands. Therefore, the "noise frequency range" should be interpreted as the width of any one of the sidebands shown in the figure.
Noise analysis can be carried out with one-tone or two-tone large signal excitation. The noise analysis with one large signal tone is much faster, as it has been optimized using an iterative solution of the linear systems and FFT-speed matrix vector multiplications with conversion matrix. The noise analysis with two large signal tones is significantly slower, therefore nonlinear noise analysis with one large signal tone is the default setting.
You can enable the nonlinear noise analysis with two-tone large signal tones using the secondary parameters of NLNOISE, LSTone, and SSTone, as shown in the following figure.
You can compute the noise figure, the noise temperature, and the output spectral density of a noisy circuit. The large-signal excitation may be swept in power and/or frequency, in addition to the noise frequency sweep.
Suppose that in the previous mixer example you want to compute the noise figure and the output spectral density. With the RF port terminated and the noise control element properly defined, the mixer example schematic displays as shown in the following schematic.
Noise analysis can be carried out with one-tone or two-tone large signal excitation. The noise analysis with one large signal tone is much faster, as it has been optimized using the iterative solution of the linear systems and fast and exact matrix-vector multiplications using special properties of the conversion matrix.
To compute the noise figure, you need to specify the appropriate noise frequencies at the output and the input. In a down-converting mixer, the appropriate sidebands are the IF for the output, and the upper-sideband RF for the input.
AWR Microwave Office software can perform the nonlinear noise analysis with one-tone or two-tone large signal analysis. The first type of nonlinear noise analysis is more common as it is significantly faster, and sufficiently accurate in most practical situations when the power of RF signal is much smaller than that of the LO.
One-tone noise analysis means that the large signal solution is obtained with one tone only, that of the local oscillator (LO) whose frequency is denoted f0. All other tones, including RF are treated as perturbations to the large signal solution driven by the LO. All noise sideband frequencies f are then expressed as:
h_{1}f_{0}+h_{2}Δf | (6.7) |
where h_{1}=-N.....N
with N being the number of tone 1 harmonics. The index h2 can only take two values, +1 for Upper sideband and -1 for Lower sideband. Δf is the offset frequency of the frequency sweep specified in the NLNOISE element.
This example addresses noise conversion from RF to IF.
For f_{IF}, h_{1}=0 h_{2}=1 (h_{2}=1 means Upper in the dialog box)
For f_{RF}, h_{1}=1 h_{2}=1 (h_{2}=1 means Upper in the dialog box)
The harmonic indices f_{IF} and f_{IF} are specified in the following dialog box.
The settings in this figure correspond to the index pairs for IF frequency (output) and for RF frequency (input).
The following figures show the noise figure and power spectral density (Nonlinear Noise NPo_NL measurement) at the output port.
You can calculate conversion gain in the standard manner, using two-tone large-signal S-parameter measurements. Alternatively, the conversion gain may be calculated with the Nonlinear Noise Conv_G_SP measurement. This measurement displays the conversion gain that is computed as a by-product of noise simulation. This is a "small-signal" version of conversion gain, accurate when the input power level is appreciably smaller (for example, 15 dB or more) than the LO power.
Conversion matrix analysis, which forms a basis for nonlinear noise simulation, requires an equal number of LO harmonics and noise sidebands. To perform an analysis that takes into account the noise sidebands shown in the noise analysis range figure, for example, the large-signal response needs to be computed at 7 LO harmonics (including DC).
For noise simulation, the number of tone-1 harmonics in Harmonic Balance options is essentially the number of tone-1 harmonics with noisy sidebands. The large-signal solution is transparently computed at a larger number of harmonics, as required by conversion noise analysis.
All other HB controls apply to the large-signal solution in the usual manner.
AWR Microwave Office software incorporates extensions of existing harmonic balance capabilities to oscillator analysis. Highlights of these features are:
Precise determination of the oscillation frequency under large-signal conditions
Rigorous computation of the large-signal spectrum, including spurious harmonic products
Phase noise analysis
This section provides an introduction to oscillator analysis in the AWR Microwave Office program, and includes several simulation examples.
In general, oscillators can be analyzed in the frequency domain (using the harmonic balance technique), or in the time domain using transient simulators such as SPICE, its derivatives, or Spectre™. If you are only interested in the steady state and not in the transient process (startup of the oscillator), the harmonic balance approach has the following advantages:
The steady-state is computed directly, avoiding costly and potentially inaccurate time-integration through transients.
Frequency domain analysis accommodates multi-port parameter descriptions of distributed elements in the most natural way, resulting in highly accurate simulations that are compatible with measured or EM-simulated S-parameter data.
While frequency domain analysis is the preferred method for the analysis of oscillators (those that operate at high frequencies in particular), oscillators have traditionally presented a serious challenge in the field of simulation technology. The difficulties stem from the mathematical implications, in high-Q circuits especially, of the lack of prior knowledge of the fundamental oscillation frequency.
To address these challenges, AWR Microwave Office software resorts to a special device called the "oscillator probe" [1], which eases these difficulties and allows for fast and robust oscillator simulations, even in cases of extremely high resonator Q.
Consider an oscillator in steady state operation as shown in the following highly simplified schematic.
Now, suppose that a sinusoidal voltage source of amplitude V and frequency ω_{p} is applied to the oscillator at the node denoted by X as shown in the following schematic.
The source impedance is given by:
that is, it presents a short circuit at the source frequency and an open circuit elsewhere. The combination of the source and the ideal impedance element is referred to as the oscillator probe.
Next, suppose that the probe voltage is equal to the steady state operating voltage at node X. Under those circumstances, no current flows through the probe at frequency ω_{p}. In addition, by the definition of the probe impedance, no current flows through the probe at any other harmonic of ω_{p}. The probe no longer disturbs the circuit, its frequency equals the oscillation frequency, and its amplitude equals the amplitude, at the node to which the oscillator is connected, of the original, probe-free oscillator.
This argument leads to the conclusion that the problem of solving for an oscillator's steady-state operation can be approached by:
Connecting the oscillator probe to a suitable node in the circuit
Finding the amplitude and frequency of the probe that results in zero current flow through the probe
In this manner, in effect, oscillator analysis is reduced to standard HB analysis running in the inner loop of a routine that attempts to locate probe parameters (amplitude and frequency) that result in zero current flow through its terminals. The outlined procedure is the basis for oscillator simulation in the AWR Microwave Office program.
APLAC oscillator analysis is based on using an oscillator probe element (OSCAPROBE) in harmonic balance analysis. The oscillation frequency is found using optimization. The search for the solution, the amplitude and frequency at the probe, is based on the frequency range specified by the Fstart and Fend parameters of the OSCAPROBE element. The voltage across OSCAPROBE should be between zero and the maximum voltage, VpMax, which should not be set unnecessarily large, because it may slow down the analysis.
If advanced harmonic balance options are available, you can use Transient Assisted Harmonic Balance simulation (TAHB) to aid convergence when simulating oscillators. Enabling TAHB for oscillators is the same as for normal TAHB on the Circuit Options dialog box APLAC Sim tab. For oscillator analysis TAHB performs additional steps beyond those for aiding normal HB analysis. Those steps aim to find good initial guesses for probe voltage and oscillation frequency.
Note that OSCAPROBE has a TranKick parameter which helps the oscillator start up in transient analysis. TranKick is set to "Yes" by default. To perform transient simulation of oscillator start-up from noise, set TranKick to "No".
Two conditions must be satisfied for an oscillator simulation to occur:
Recall that the AWR Microwave Office program invokes those simulators that are appropriate for the required measurements. Oscillator analysis is appropriate when any nonlinear or oscillator measurement is requested. Those measurements are located in the Nonlinear > Power, Nonlinear > Voltage, Nonlinear > Current and Oscillator categories.
The oscillator probe must be connected to the oscillator. The OSCAPROBE is located in the Elements Browser in the MeasDevice > Probes category.
For example, suppose that the power spectrum measurement (Nonlinear > Power Pharm measurement) is defined for the following schematic.
The OSCAPROBE element is next introduced between the resonator and the active device, which is the probe's recommended location. When the simulation is executed, AWR Microwave Office software automatically performs an oscillator analysis, carrying out the steps shown in the analysis flowchart.
To a varying degree, probe parameters influence the speed, and ultimately, the convergence of an oscillator analysis. Although most users find the oscillator analysis fast and simple to use, it is helpful to become familiar with probe parameters in the event that the analysis fails, either internally or due to user error.
The following shows the schematic symbol of the oscillator probe.
The most significant probe parameters are Fstart and Fend. These two parameters indicate the range to search for start-up frequency. Choosing roughly +- 25% of the resonator's center frequency is sufficient in most cases. Fsteps is the number of steps used in the search for start-up frequency, and it rarely needs to be changed from default. Exceptions may occur in extremely high-Q cases, where you may need to increase Fsteps or narrow the frequency range.
The probe has a number of secondary parameters that are used to aid convergence or to increase simulation speed, but are otherwise best left at default values. VpMax and Vsteps for example, control the probe voltage stepping as discussed in “Analysis Flow”. The simulator steps the probe voltage, from a small value to VpMax in steps of Vsteps, in an attempt to locate a suitable starting point for rigorous oscillator analysis. If the simulator occasionally returns a "Could not find a starting point for oscillator analysis" message, you are prompted to increase Vsteps and/or VpMax.
The value of ΔV=V_{pMax}/V_{steps} is used to limit the maximum Newton step in oscillator analysis, so specifying a very large Vsteps value could slow the simulation.
Parameters of lesser significance are Iter and Damp.
Iter is the total number of analysis iterations and Damp is a parameter for the so-called damped Newton iteration. Decreasing Damp or increasing Iter from default values may improve convergence in rare circumstances.
NOTE: In addition to the mentioned parameters, several of the probe's secondary parameters are designated as "not used". These parameters are manipulated internally by the simulator, and are likely to be removed in a future release.
Harmonic balance simulation runs in the inner loop of oscillator analysis, so harmonic balance parameters apply as usual, controlling the number of harmonics and simulation accuracy.
The location of the probe plays an important role in oscillator simulation. The recommended location is at a node connecting the resonator and the active device. In many cases an alternate probe location results in successful and even slightly faster simulations; however, you are encouraged to follow the recommended placement of the probe. Not doing so opens the possibility of failure to detect start-up in an otherwise well-built oscillator.
All nonlinear measurements apply to oscillator analysis in the usual way. You can view voltages, currents and power at any port or meter, in the time or the frequency domain. You can examine dynamic load lines and power efficiency in the same way as amplifiers.
One additional measurement is the Oscillator OSC_FREQ measurement, which you can use to display the oscillation frequency. In the event that a bias is swept, as in the case of a VCO, the x-axis automatically displays the value of the tuning voltage. If no swept voltage source is present in the circuit, the OSC_FREQ measurement displays the oscillation frequency on both axes.
AWR Microwave Office software is capable of single-tone analyses of free running (but possibly voltage-controlled) oscillators only; support for self-oscillating mixers and injection-locked oscillators is not included in the present version.
You must place the probe in a top-level schematic.
If a frequency component measurement, such as Vcomp or Pcomp, is defined prior to the execution of an oscillator simulation, the oscillation frequency is not known at the time of creation. For this reason, Harmonic Index in the Add/Modify Measurement dialog box displays a multiple of an arbitrarily chosen fundamental equal to 1 GHz. After the simulation is complete, the indices are reset to the correct oscillation frequency. Note that the arbitrarily chosen frequency affects the appearance of the Add/Modify Measurement dialog box, not the validity of displayed results.
A typical oscillator simulates between less than a second and five seconds on a modern computer, depending on the number of harmonics, the output power, the oscillator Q, the number of active devices in the circuit, and the level of complexity of linear models.
To improve the speed of the simulation, you should attempt to decrease the value of the VMax and Vsteps parameters. The number of harmonics has a significant impact on simulation speed, but reducing it below 5 is not recommended. The accuracy settings have a relatively small impact on analysis times, and should not be altered in an attempt to speed up simulations.
Oscillator noise analysis is closely related to the nonlinear noise analysis of the previous section. Noise in the form of noise currents perturbs the steady state of the oscillator, resulting in noisy voltages at the output. The relation between the sidebands of noise sources and the noise sidebands of the output signal is described by the circuit's conversion matrix, as previously discussed. In turn, the noisy voltage sidebands are related to phase noise [2].
Phase noise analysis is enabled by the presence of an OSCNOISE element (located in the Elements Browser MeasDevice > Controls category) in the schematic of the oscillator circuit. The following shows the OSCNOISE element.
OFstart, OFend and OFsteps define the noise sweep range, as an offset from the carrier. SwpType selects between linear and log sweep.
With the noise control in place, a phase noise analysis is performed automatically, following a large-signal oscillator simulation.
In nearly all cases, improvements in HB simulators render this analysis type obsolete. Please try the regular HB simulator first, and severely reduce all input signal amplitudes by the same factor to see the small signal response.
Linear harmonic balance (AC-HB) analysis is similar to AC analysis, except it allows non-sinusoidal inputs with arbitrary frequencies, and spectral and time-domain measurements. It is small signal analysis with arbitrary waveforms.
Again, an initial DC analysis calculates the operating point of all nonlinear elements, which determines their linear equivalent, and the circuit is treated as completely linear. Unlike AC analysis, however, AC-HB handles multiple input sources with arbitrary waveforms (for example, pulse, triangle, and sawtooth), at arbitrary frequencies. By superposition, the output is the sum of the linear responses to each frequency component in the input signal(s). The circuit is treated as linear, so the output only has spectral components at the same frequencies as the input(s). No new frequency components are created; there is no intermodulation. The default number of harmonics for each input tone are the same as for regular HB analysis. Choose Options > Default Circuit Options to display the Circuit Options dialog box for setting global defaults, or set local options for a schematic by right-clicking the schematic in the Project Browser and choosing Options to display the Options dialog box, then click theAWR Sim tab.
You can view AC-HB results using standard harmonic balance power, voltage, and current measurements (Pcomp, Vtime, Iharm, etc.) under the Nonlinear measurement type. To use AC-HB analysis, set up the desired harmonic balance measurement, but select AC-HB or Aplac AC-HB as the Simulator.