Harmonic Balance Basics

This is a description of Harmonic Balance (HB) simulation, including when to use it, how to set it up, and the data it generates. Examples are provided to show how to use this simulation. Detailed information describes the parameters, theory of operation, and troubleshooting information.

Overview

Harmonic balance is a frequency-domain analysis technique for simulating distortion in nonlinear circuits and systems. It is usually the method of choice for simulating analog RF and microwave problems, since these are most naturally handled in the frequency domain. Within the context of high-frequency circuit and system simulation, harmonic balance offers several benefits over conventional time-domain transient analysis. Harmonic balance simulation obtains frequency-domain voltages and currents, directly calculating the steady-state spectral content of voltages or currents in the circuit. The frequency integration required for transient analysis is prohibitive in many practical cases. Many linear models are best represented in the frequency domain at high frequencies. Use the HB simulation to:

• Determine the spectral content of voltages or currents.
• Compute quantities such as third-order intercept (TOI) points, total harmonic distortion (THD), and intermodulation distortion components.
• Perform power amplifier load-pull contour analyses.
• Perform nonlinear noise analysis.

Refer to the following topics for details on Harmonic Balance simulation:

• Using Harmonic Balance Simulation explains when to use Harmonic Balance simulation, describes the minimum setup requirements, and gives a brief explanation of the Harmonic Balance simulation process.
• Examples of Harmonic Balance Simulation describes in detail how to set up a basic single-point and a swept harmonic balance simulation, using a power amplifier.
• Reference Equations
• Limitations describes the harmonic balance simulator's limitations.
• HB Simulation Parameters provides details about the parameters available in the HB Simulation controller in ADS.
• Theory of Operation is a brief description of the harmonic balance simulator.
• Troubleshooting a Simulation offers suggestions on how to improve a simulation.
• Harmonic Balance for Nonlinear Noise Simulation describes how to use the simulator for calculating noise.
• Harmonic Balance for Oscillator Simulation describes how to use the simulator with oscillator designs.
• Harmonic Balance for Mixers describes how to use the simulator with mixer designs.
• Transient Assisted Harmonic Balance describes how to use the automated TAHB to generate the transient initial guess for the Harmonic Balance simulation.
• Harmonic Balance Assisted Harmonic Balance describes how to use HBAHB when performing a multi-tone harmonic balance simulation so the simulator automatically selects which tones to use in generating the final HB solution.
• For the most detailed description about setting up, running, and converging a harmonic balance simulation, see Guide to Harmonic Balance Simulation in ADS.

Using Harmonic Balance Simulation

This section describes when to use Harmonic Balance simulation, how to set it up, and the basic simulation process used to collect data.

License Requirements

The Harmonic Balance simulation uses the Harmonic Balance Simulator license (sim_harmonic) which is included with all Circuit Design suites except RF Designer. You must have this license to run Harmonic Balance simulations. You can work with examples described here and installed with the software without the license, but you will not be able to simulate them.

When to Use Harmonic Balance Simulation

Start by creating your design, then add current probes and identify the nodes from which you want to collect data.

How to Use Harmonic Balance Simulation

For a successful analysis:

• Add the HarmonicBalance simulation component to the schematic and double-click to edit it. Fill in the fields under the Freq tab:
  • Enter at least one fundamental frequency and the number (order) of harmonics to be considered in the simulation.
    Make sure that frequency definitions are established for all of the fundamentals of interest in a design. For example, mixers should include definitions for RF and LO frequencies.
  • If more than one fundamental is entered, set the maximum mixing order. This limits the number of mixing products to be considered in the simulation. For more information on this parameter, see Harmonics and Maximum Mixing Order.
• Choose Auto Select option for Matrix Solver under the Solver tab in the Harmonic Balance controller. For tips on using this option, see Selecting a Solver.
• You can use previous simulation solutions to speed the simulation process. For more information, see Reusing Simulation Solutions.
• You can perform budget calculations as part of the simulation. For information on budget analysis, see the chapter "Using Circuit Simulators for RF System Analysis" in the Using Circuit Simulators documentation.
• You can perform small-signal analysis. Enable the Small-signal option and fill in the fields under the Small-Sig tab. For details, see Harmonic Balance for Mixers.
• You can perform nonlinear noise analysis. Select the Noise tab, enable the Nonlinear noise option, and fill in the fields in the Noise(1) and Noise(2) dialog boxes. For details, see Harmonic Balance for Nonlinear Noise Simulation.
• If your design includes NoiseCon components, select the Noise tab, enable the NoiseCons option and fill in the fields. For more information, see Harmonic Balance for Nonlinear Noise Simulation.
• If your design includes an OscPort component, enable Oscillator and fill in the fields under the Osc tab. Harmonic Balance for Oscillator Simulation focuses specifically on simulating oscillator designs.

For details about each field, click Help from the dialog box.

What Happens During Harmonic Balance Simulation

To perform a harmonic balance simulation, you only need to specify one or more fundamental frequencies and the order for each fundamental frequency. Agilent EEsof EDA recommends that all other parameters remain set to their default values. The simulator will set up the simulation in a proper way so that near optimal performance can be achieved without any additional parameter tweaking. For example, with Auto Select as the default choice for selecting matrix solvers, the simulator will determine whether the Direct Solver or the Krylov Solver is more effective for a particular circuit. For multi-tone HB simulations, the simulator will automatically determine whether to use Harmonic Balance Assisted Harmonic Balance (HBAHB) and how to set it up to achieve the optimal simulation speed.

Examples of Harmonic Balance Simulation

This section gives detailed setups to perform these simulations on a power amplifier:

• Single Tone Harmonic Balance Simulation applies a single tone to the power amplifier. This tone and 7 harmonics are analyzed.
• Swept Harmonic Balance Simulation sweeps the input from 500 to 1500 MHz and analyzes the performance of the amplifier at points along the sweep.

Single Tone Harmonic Balance Simulation

The following figure illustrates the setup for simulating a power amplifier circuit.

Example setup for a basic harmonic balance simulation

Note This design, HB1.dsn, is in the Examples directory under Tutorial/SimModels_prj. The results are in HB1.dds.

1. From the Sources-Freq Domain palette, select and place a V_1Tone source on the schematic. Edit the component to set these values:
   • V = 0.01 V
   • Freq = 20 MHz. This is the first and only fundamental.
2. Ensure that the inputs and outputs of nodes at which you want data to be reported are appropriately labeled. In this example, the output node has been labeled Vout.
3. From the Simulation-HB palette, select and place the HB component on the schematic, then double-click to edit it. Select the Freq tab and edit these parameters:
   • Frequency = 20 MHz
   • Order = 7
     Click Add. If this line appears as the second fundamental frequency in the list, select the one above it and click Cut. Make sure that 1 20 MHz 7 is the only line that appears in the list of fundamental frequencies.

     Note With only a single frequency defined, the parameter Maximum mixing order is not available.

4. Simulate. When the simulation is finished, a Data Display window opens. The following plot illustrates the results of the simulation, showing the fundamental and seven harmonics, declining in voltage (Vout) with increasing frequency.
   

Swept Harmonic Balance Simulation

In this example, the fundamental is swept from 500 MHz to 1500 MHz in 25 MHz steps. At 41 points along the sweep, data is collected for the value of the fundamental and 8 harmonics.

The following figure illustrates the setup for a swept harmonic-balance simulation of a power amplifier circuit.

Setup for a swept harmonic balance simulation

Note This design, HB2.dsn, is in the Examples directory under Tutorial/SimModels_prj. The results are in HB2.dds.

To perform a swept harmonic balance simulation:

1. From Sources-Freq Domain palette, select and place a P_1Tone component on the schematic and edit it to set these values:
   • Num = 1
   • P = dbmtow(-10). The function dbmtow() is used to convert power in dBm to watts for the purpose of simulation.
   • Freq = freq_swp. This sets the frequency to a variable which will be defined later.
2. Label the nodes at which you want data to be reported, in this example, label the output node as Vout.
3. From the Simulation-HB palette, select and place an HB simulation component on the schematic and edit it to select the Freq tab. Set the following parameters:
   • Frequency = freq_swp MHz. This is the only fundamental, or Freq[1].
   • Order = 8
     Click Add. If any other fundamentals appear in the list, select each line and click Cut. Make sure that 1 freq_swp MHz 8 is the only line that appears in the list of fundamental frequencies.

     Note Ensure that frequencies are established for all of the frequencies of interest in a design under test (for example, RF, LO, and IF frequencies). You may want to display them on the schematic to facilitate editing.

4. Select the Sweep tab. Ensure that Start/Stop is selected and set the following:
   • Parameter to sweep = freq_swp
   • Sweep Type = Linear
   • Start = 500*
   • Stop = 1500
   • Step = 25
5. Click OK to accept changes and close the dialog box.
6. From Data Items palette, select and place a VAR (variables and equations) component on the schematic and edit it:
   • Under Variable or Equation Entry Mode, select Name=Value.
   • Under Select Parameter, select the default equation X=1.0 and in the field to the right, change it to freq_swp=1. This assigns freq_swp to the fundamental.
7. Click OK to accept changes and close the dialog box.
8. Simulate. When the simulation is finished, a Data Display window opens. One way to plot Vout is against the harmonic index. By setting the Trace Type to a spectral display, it shows the strength of each of the eight harmonics as the fundamental changes from 500 MHz to 1500 MHz.
   

The harmonic index (harmindex) is a sequential index of frequencies, starting with zero. It is generated either during a frequency sweep, or during oscillator analysis (since the oscillation frequency as an unknown variable is swept during the analysis). The harmindex is always the innermost variable, which makes it the independent variable. Each harmindex value corresponds to an actual simulated frequency (harmonic or intermod product) for each frequency value of the frequency sweep. The following illustration shows the relationship between the LO, the RF frequency, and the harmonics generating the harmindex in a table of results. Assuming a downconverting mixer design, the

• LO freq = 16 GHz
• RFfreq (swept) = 12 GHz to 14 GHz in 2 GHz steps
• The Harmonic Balance controller is set to:
  • Freq [1] = LO (Order = 1)
  • Freq [2] = RF (Order = 1)
  • MaxOrder = 2

Here are the reported values for the simulation frequency freq relative to the harmindex value that would appear in the data display:

Reference Equations

For equations on which the harmonic balance simulation is based, please see Harmonic Balance Background in the Guide to Harmonic Balance Simulation in ADS.

Limitations

Harmonic balance is limited in that the signal must be quasi-periodic and representable as a superposition of a number M of discrete tones. As M becomes large, the amount of required internal memory becomes excessive since the internal matrix size grows as M ². Using Krylov linear solvers instead of direct methods reduces the memory growth from quadratic to linear (proportional to M). Therefore, the Krylov solvers enable harmonic balance to be used on very large circuits, and circuits with a large number of tones.

HB Simulation Parameters

ADS provides access to harmonic balance simulation parameters enabling you to define aspects of the simulation listed in the following table:

Important For details about backward compatibility of default values for selected parameters, see Backward Compatibility Exceptions.

Tab Name	Description	For details, see...
Freq	Frequencies of fundamentals.	Setting Fundamental Frequencies
Sweep	Sweep type and associated characteristics.	Setting Up a Sweep
Initial Guess	Sets parameters related to initial guess, including automated transient assisted harmonic balance (TAHB), harmonic balance assisted harmonic balance (HBAHB), initial guess from a data file, and initial guess for parameter sweep. It also allows the user to save the final solution in a data file.	Setting Up the Initial Guess
Oscillator	Enabling and setting up parameters for oscillator analysis.	Enabling Oscillator Analysis
Noise	Parameters related to noise simulation, including sweeps, input and output ports, and the nonlinear noise controllers to be simulated.	Selecting Nonlinear Noise Analysis
Small-Sig	Parameters related to small-signal/large-signal simulation.	Setting Up Small-Signal Simulations
Params	Parameters related to status level for summary information and device operating-point levels, as well as parameters related to FFT oversampling and convergence.	Defining Simulation Parameters
Solver	Parameters enabling you to choose between a Direct or Krylov solver or an automatic selection. The automatic selection is the default and recommended choice, since it allows the simulator to choose the most effective solver for each particular circuit. Additional parameters manage memory usage.	Selecting a Harmonic Balance Solver Technique
Output	Selectively save simulation data to a dataset.	Selectively Saving and Controlling Simulation Data
Display	Control the visibility of simulation parameters on the Schematic.	Displaying Simulation Parameters on the Schematic

For additional information on setting up a harmonic balance simulation, refer to these topics:

• Harmonic Balance for Nonlinear Noise Simulation describes how to use the simulator for calculating noise.
• Harmonic Balance for Oscillator Simulation describes how to use the simulator with oscillator designs.
• Harmonic Balance for Mixers describes how to use the simulator with mixer designs.
• For a thorough description about setting up, running, and converging a harmonic balance simulation, see Guide to Harmonic Balance Simulation in ADS.

Setting Fundamental Frequencies

On the Freq tab, you can specify the frequency portion of the simulation. The following table describes the parameter details. Names listed in the Parameter Name column are used in netlists and on schematics.

Setting Up a Sweep

On the Sweep tab, setting up the sweep portion of the simulation consists of two basic parts:

• Selecting the sweep type and setting the associated characteristics
• Optionally, specifying a sweep plan

To shorten simulation time in any parameter sweep, select a start point as close as possible to the convergence point and vary the parameter gradually. This yields better estimates for the next simulation, and achieves convergence more rapidly than if the parameter were changed abruptly. The following table describes the parameter details. Names listed in the Parameter Name column are used in netlists and on schematics.

Setting Up the Initial Guess

On the Initial Guess tab, setting up the initial guess for a harmonic balance simulation consists of:

• Setting Transient Assisted Harmonic Balance (TAHB).
• Setting Harmonic Balance Assisted Harmonic Balance (HBAHB).
• Setting Initial Guess and Final Solution parameters.

To set up a TAHB analysis:

• On the Initial Guess tab in the Harmonic Balance controller, select Auto, On, or Off for Transient Assisted Harmonic Balance.

It is recommended to use the TAHB Auto mode, which is the default setting. The simulator will turn on TAHB automatically if the circuit involves a divider. The TAHB On and Off choices are for you to manually turn on or off TAHB, which should be done only when you would like to override the simulator's automatic setting.

To set up a HBAHB analysis:

• Under the Initial Guess tab, in the HBAHB section, select either Auto, On, or Off.

The Auto mode is the default and is recommended, which allows the simulator to determine whether to use HBAHB and to optimize the HBAHB setup if it is used. Selecting the On mode forces HBAHB to be turned on and the default sequencing (1-tone, 2-tone, ...) will be used. Selecting the Off mode forces HBAHB to be turned off.

By using HBAHB, the simulator will generate its own initial guess for multi-tone Harmonic Balance from another harmonic balance analysis with fewer fundamental frequencies than the original multi-tone problem. You do not need to supply an initial guess. If you do provide an initial guess by enabling Use Initial Guess and entering a name for File (parameters UseInFile and InFile ), then that will take precedence over HBAHB so long as the file exists.

The following table shows the parameters available to set the Initial Guess. Names listed in the Parameter Name column are used in netlists and on schematics.

Enabling Oscillator Analysis

On the Oscillator tab, setting up an oscillator analysis consists of:

• Enabling Oscillator Analysis.
• Setting the simulation method to use OscPort or nodes (OscProbe).
• If specifying nodes, enter the node parameter values.

The following table describes the parameter details. Names listed in the Parameter Name column are used in netlists and on schematics.

Selecting Nonlinear Noise Analysis

The NoiseCon is used to select which NoiseCon nonlinear noise controllers should be simulated with the current harmonic balance analysis. These noise simulations will be performed in addition to any noise simulation that may be set up with Noise(1) and Noise(2) dialog boxes. The following table describes the parameter details. Names listed in the Parameter Name column are used in netlists and on schematics.

Setting Up Parameters for Noise(1)

Choose Noise (1) to set up and run a small-signal/Harmonic Balance noise analysis following the final time point of the simulation. The following table describes the parameter details. Names listed in the Parameter Name column are used in netlists and on schematics.

Setting Up Parameters for Noise(2)

Defining the Noise2 parameters consists of the following basic parts:

• Enable noise calculation.
• Specifying the nodes to use for noise parameter calculation.
• Specifying the noise contributors and the threshold for noise contribution.
• Optionally, specifying the bandwidth over which the noise simulation is performed

The following table describes the parameter details. Names listed in the Parameter Name column are used in netlists and on schematics.

Setting Up Small-Signal Simulations

The Small-Sig tab enables you to use a large-signal/small-signal method to achieve faster simulations when some signal sources are much smaller than others, and are assumed not to exercise circuit nonlinearities. For example, in a mixer the LO tone can be considered the large-signal source and the RF the small-signal source. The following table describes the parameter details. Names listed in the Parameter Name column are used in netlists and on schematics.

Defining Simulation Parameters

The Params tab enables you to define these basic simulation parameters:

• Enabling the Budget simulation.
• Specifying the amount of device operating-point information to save.
• Specifying the FFT oversampling ratio.

The following table describes the parameter details. Names listed in the Parameter Name column are used in netlists and on schematics.

Selecting a Harmonic Balance Solver Technique

The Solver tab enables you to select a Direct or Krylov solver, or to allow the simulator to assign one automatically. The automatic selection is the default and recommended choice, since it allows the simulator to choose the most effective solver for each particular circuit. Newton's method needs to solve a sequence of linear problems. If Newton's method doesn't converge or the convergence rate is too slow the Direct method will use arc-length continuation, while the Krylov method will use source stepping. The following table describes the parameter details. Names listed in the Parameter Name column are used in netlists and on schematics.

Advanced Continuation Parameters

These parameters are for arc-length continuation. The arc-length continuation is an extremely robust algorithm. If it fails, try all other convergence remedies first before adjusting these arc-length parameters. The following table describes the parameter details. Names listed in the Parameter Name column are used in netlists and on schematics.

Advanced Krylov Parameters

These parameters allow detailed configuration for the Krylov solver. Default values are recommended for optimal performance. The following table describes the parameter details. Names listed in the Parameter Name column are used in netlists and on schematics.

Backward Compatibility Exceptions

Beginning with ADS 2006A, the default value for the following parameter does not maintain backwards compatibility with ADS 2004A as shown in the following table. When a project created in 2004A is opened in 2005A or 2006A, this parameter will use the default value specified in 2006A regardless of the value specified in 2004A either by default or by the user.

Theory of Operation

Harmonic balance is a frequency-domain analysis technique for simulating distortion in nonlinear circuits and systems. It is well-suited for simulating analog RF and microwave problems, since these are most naturally handled in the frequency domain. You can analyze power amplifiers, frequency multipliers, mixers, and modulators, under large-signal sinusoidal drive.

Harmonic balance simulation enables the multitone simulation of circuits that exhibit intermodulation frequency conversion. This includes frequency conversion between harmonics. Not only can the circuit itself produce harmonics, but each signal source (stimulus) can also produce harmonics or small-signal sidebands. The stimulus can consist of up to twelve nonharmonically related sources. The total number of frequencies in the system is limited only by such practical considerations as memory, swap space, and simulation speed.

The Simulation Process

The harmonic balance method is iterative. It is based on the assumption that for a given sinusoidal excitation there exists a steady-state solution that can be approximated to satisfactory accuracy by means of a finite Fourier series. Consequently, the circuit node voltages take on a set of amplitudes and phases for all frequency components. The currents flowing from nodes into linear elements, including all distributed elements, are calculated by means of a straightforward frequency-domain linear analysis. Currents from nodes into nonlinear elements are calculated in the time-domain. Generalized Fourier analysis is used to transform from the time-domain to the frequency-domain.

The Harmonic Balance solution is approximated by truncated Fourier series and this method is inherently incapable of representing transient behavior. The time-derivative can be computed exactly with boundary conditions, v(0)=v(t), automatically satisfied for all iterates.

The truncated Fourier approximation + N circuit equations results in a residual function that is minimized.

N x M nonlinear algebraic equations are solved for the Fourier coefficients using Newton's method and the inner linear problem is solved by:

• Direct method (Gaussian elimination) for small problems.
• Krylov-subspace method (e.g. GMRES) for larger problems.

Nonlinear devices (transistors, diodes, etc.) in Harmonic Balance are evaluated (sampled) in the time-domain and converted to frequency-domain via the FFT.

A frequency-domain representation of all currents flowing away from all nodes is available. According to Kirchoff's Current Law (KCL), these currents should sum to zero at all nodes. The probability of obtaining this result on the first iteration is extremely small.

Therefore, an error function is formulated by calculating the sum of currents at all nodes. This error function is a measure of the amount by which KCL is violated and is used to adjust the voltage amplitudes and phases. If the method converges (that is, if the error function is driven to a given small value), then the resulting voltage amplitudes and phases approximate the steady-state solution. The following flow chart presents a visual representation of the process:

Comparing Harmonic Balance and Time Domain Simulators

In the context of high-frequency circuit and system simulation, harmonic balance has a number of advantages over conventional time-domain transient analysis:

• Designers are usually most interested in a system's steady-state behavior. Many high-frequency circuits contain long time constants that require conventional transient methods to integrate over many periods of the lowest-frequency sinusoid to reach steady state. Harmonic balance, on the other hand, captures the steady-state spectral response directly.
• Harmonic balance is faster at solving typical high-frequency problems that transient analysis can't solve accurately or can only do so at prohibitive costs.The applied voltage sources are typically multitone sinusoids that may have very narrowly or very widely spaced frequencies. It is not uncommon for the highest frequency present in the response to be many orders of magnitude greater than the lowest frequency. Transient analysis would require an integration over an enormous number of periods of the highest-frequency sinusoid. The time involved in carrying out the integration is prohibitive in many practical cases.
• At high frequencies, many linear models are best represented in the frequency domain. Simulating such elements in the time domain by means of convolution can result in problems related to accuracy, causality, or stability.

Harmonics and Maximum Mixing Order

With multiple sources in a circuit, mixing products will occur. The parameter Maximum mixing order (on the Freq tab) determines how many mixing products are to be included in the simulation. Consider an example with two sources and three harmonics:

Source	Frequency	Order
Fund 1	5 MHz	3
Fund 2	7 MHz	3

If Maximum mixing order is 0 or 1, no mixing products are simulated. The frequency list consists of the fundamental (Fund) frequency and the first, second, and third harmonics of each source, as follows:

Frequency	Combination
0 Hz	DC term
5 MHz	Fund 1
7 MHz	Fund 2
10 MHz	Second harmonic of Fund 1
14 MHz	Second harmonic of Fund 2
15 MHz	Third harmonic of Fund 1
21 MHz	Third harmonic of Fund 2

If Maximum mixing order is 2, the sum and difference frequencies of the two fundamentals are added to the list:

Frequency	Combination
2 MHz	Fund 2 − Fund 1
12 MHz	Fund 2 + Fund 1

If Maximum mixing order is 3, the second harmonic of one source can mix with the fundamental of the other. These frequencies are also added to the list:

Frequency	Combination
3 MHz	Second harmonic of Fund 1 - Fund 2
9 MHz	Second harmonic of Fund 2 - Fund 1
17 MHz	Second harmonic of Fund 1 + Fund 2
19 MHz	Second harmonic of Fund 2 + Fund 1

This pattern is also used when there are three sources. The combined order is the sum of the individual signal orders that are added or subtracted to make up the frequency list.

Consider an example with the following three sources, where Maximum mixing order = 5:

Source	Frequency	Order
Fund 1	10.00 GHz	5
Fund 2	10.95 GHz	2
Fund 3	11.05 GHz	2

The frequencies that are used in the simulation and the combinations that produce them are listed in the following table.

Frequency List (Maximum mixing order = 5)

Frequency	Combination	Order
0.000 Hz	DC term	always present
100.0 MHz	Fund 3 - Fund 2	2
200.0 MHz	Second harmonic of Fund 3 - Second harmonic of Fund 2	4
850.0 MHz	Second harmonic of Fund 2 - Fund 1 - Fund 3	4
950.0 MHz	Fund 2 - Fund 1	2
1.050 GHz	Fund 3 - Fund 1	2
1.150 GHz	Second harmonic of Fund 3 - Fund 1 - Fund 2	4
1.900 GHz	Second harmonic of Fund 2 - Second harmonic of Fund 1	4
2.000 GHz	Fund 2 + Fund 3 - Second harmonic of Fund 1	4
2.100 GHz	Second harmonic of Fund 3 - Second harmonic of Fund 1	4
7.900 GHz	Third harmonic of Fund 1 - Second harmonic of Fund 3	5
8.000 GHz	Third harmonic of Fund 1 - Fund 2 - Fund 3	5
8.100 GHz	Third harmonic of Fund 1 - Second harmonic of Fund 2	5
8.850 GHz	Second harmonic of Fund 1 + Fund 2 - Second harmonic of Fund 3	5
8.950 GHz	Second harmonic of Fund 3 - Second harmonic of Fund 1	4
9.050 GHz	Second harmonic of Fund 2 - Second harmonic of Fund 1	4
9.150 GHz	Second harmonic of Fund 1 + Fund 3 - Second harmonic of Fund 2	5
9.800 GHz	Fund 1 + Second harmonic of Fund 3 - Second harmonic of Fund 2	5
9.900 GHz	Fund 1 + Fund 2 - Fund 3	3
10.00 GHz	Fundamental 1
10.10 GHz	Fund 1 + Fund 3 - Fund 2	3
10.20 GHz	Fund 1 + Second harmonic of Fund 3 - Second harmonic of Fund 2	5
10.85 GHz	Second harmonic of Fund 2 - Fund 3	3
10.95 GHz	Fundamental 2
11.05 GHz	Fundamental 3
11.15 GHz	Second harmonic of Fund 3 - Fund 2	3
11.90 GHz	Second harmonic of Fund 2 - Fund 1	3
12.00 GHz	Fund 2 + Fund 3 - Fund 1	3
12.10 GHz	Second harmonic of Fund 3 - Fund 1	3
12.95 GHz	Second harmonic of Fund 2 + Fund 3 - Fund 1	4
13.05 GHz	Fund 2 + Second harmonic of Fund 3 - Second harmonic of Fund 1	5
18.95 GHz	Third harmonic of Fund 1 - Fund 3	4
19.05 GHz	Third harmonic of Fund 1 - Fund 2	4
19.90 GHz	Second harmonic of Fund 1 + Fund 2 - Fund 3	4
20.00 GHz	Second harmonic of Fund 1
20.10 GHz	Second harmonic of Fund 1 + Fund 3 - Fund 2	4
20.85 GHz	Fund 1 + Second harmonic of Fund 2 - Fund 3	4
20.95 GHz	Fund 2 + Fund 1 - 2nd order
21.05 GHz	Fund 3 + Fund 1 - 2nd order
21.15 GHz	Fund 1 + Second harmonic of Fund 3 - Fund 2	4
21.90 GHz	Second harmonic of Fund 2
22.00 GHz	Fund 2 + Fund 3 - 2nd order
22.10 GHz	Second harmonic of Fund 3
22.95 GHz	Fund 3 + Second harmonic of Fund 2 - Fund 1	4
23.05 GHz	Fund 2 + Second harmonic of Fund 3 - Fund 1	4
28.95 GHz	Fourth harmonic of Fund 1 - Fund 3	5
29.05 GHz	Fourth harmonic of Fund 1 - Fund 2	5
29.90 GHz	Third harmonic of Fund 1 + Fund 2 - Fund 3	5
30.00 GHz	Third harmonic of Fund 1
30.10 GHz	Third harmonic of Fund 1 + Fund 3 - Fund 2	5
30.85 GHz	Second harmonic of Fund 1 + Second harmonic of Fund 2 - Fund 3	5
30.95 GHz	Second harmonic of Fund 1 + Fund 2	3
31.05 GHz	Second harmonic of Fund 1 + Fund 3	3
31.15 GHz	Second harmonic of Fund 1 + Second harmonic of Fund 3 - Fund 2	5
31.90 GHz	Fund 1 + Second harmonic of Fund 2	3
32.00 GHz	Fund 1 + Fund 2 + Fund 3	3
32.10 GHz	Fund 1 + Second harmonic of Fund 3	3
32.95 GHz	Fund 3 + Second harmonic of Fund 2	3
33.05 GHz	Fund 2 + Second harmonic of Fund 3	3
34.00 GHz	Second harmonic of Fund 2 + Second harmonic of Fund 3 - Fund 1	5
40.00 GHz	Fourth harmonic of Fund 1
40.95 GHz	Third harmonic of Fund 1 + Fund 2	4
41.05 GHz	Third harmonic of Fund 1 + Fund 3	4
41.90 GHz	Second harmonic of Fund 1 + Second harmonic of Fund 2	4
42.00 GHz	Second harmonic of Fund 1 + Fund 2 + Fund 3	4
42.10 GHz	Second harmonic of Fund 1 + Second harmonic of Fund 3	4
42.95 GHz	Fund 1 + Second harmonic of Fund 2 + Fund 3	4
43.05 GHz	Fund 1 + Fund 2 + Second harmonic of Fund 3	4
44.00 GHz	Second harmonic of Fund 2 + Second harmonic of Fund 3	4
50.00 GHz	Fifth harmonic of Fund 1
50.95 GHz	Fourth harmonic of Fund 1 + Fund 2	5
51.05 GHz	Fourth harmonic of Fund 1 + Fund 3	5
51.90 GHz	Third harmonic of Fund 1 + Second harmonic of Fund 2	5
52.00 GHz	Third harmonic of Fund 1 + Fund 2 + Fund 3	5
52.10 GHz	Third harmonic of Fund 1 + Second harmonic of Fund 3	5
52.95 GHz	Second harmonic of Fund 1 + Second harmonic of Fund 2 + Fund 3	5
53.05 GHz	Second harmonic of Fund 1 + Fund 2 + Second harmonic of Fund 3	5
54.00 GHz	Fund 1 + Second harmonic of Fund 2 + Second harmonic of Fund 3	5

Selecting a Solver

Many harmonic balance simulators rely on the Newton-Raphson technique to solve the nonlinear systems of algebraic equations that arise in large-signal frequency-domain circuit simulation problems. Each iteration of Newton-Raphson requires an inversion of the Jacobian matrix associated with the nonlinear system of equations. When the matrix is factored by direct methods, memory requirements climb as O(H ²), where H is the number of harmonics. Thus, the factorization of a Jacobian at H=500 will require 2500 times as much RAM as one at H=10.

An alternate approach to solving the linear system of equations associated with the Jacobian is to use a Krylov subspace iterative method such as GMRES (generalized minimum residual). This method does not require the explicit storage of the Jacobian matrix J, but rather only the ability to carry out matrix-vector products of the form J • V, where V is an arbitrary vector. But the information needed to carry out such an operation can be stored in O(H) memory, not in O(H ²), in the context of harmonic balance. Thus, Krylov subspace solvers offer substantial savings in memory requirements for large harmonic-balance problems. Similar arguments show that even larger increases in computational speed can be obtained.

Note For circuits involving large numbers of frequencies, consider using the Circuit Envelope simulator.

Use the following guidelines when selecting a solver:

• Auto Select
  This option allows the simulator to choose the linear solver, which is recommended because the optimal choice can be made automatically for most circuits by this option. The simulator analyzes factors such as circuit or spectral complexity and compares memory requirements for each solver against the available computer memory. Based on this analysis it selects either direct solver or Krylov solver. Furthermore, when a solver is chosen by the simulator, parameters for that solver are also automatically optimized.
• Direct Solver
  The Direct Solver option is only recommended when the problem is small, and the simulator chooses the Krylov Solver yet convergence difficulty is encountered. A small problem can be roughly described as one where the circuit contains relatively few nonlinear components, there are one or two fundamental frequencies, relatively few harmonics, etc. In general, in such cases the Direct Solver is not only faster, but also exhibits superior convergence. The simulator will usually choose the Direct Solver for small problems automatically with the Auto Select option selected.
• Krylov Solver
  The Krylov Solver option is only recommended when the simulator chooses the Direct Solver and runs out of memory or convergence difficulty is encountered, especially when solving large problems. A large problem can roughly be described as one where memory usage exceeds 400 MB or the memory capacity of the computer (whichever occurs first). A problem may be large because of a large number of nonlinear components, a large number of harmonics required for simulation, or both. The simulator will usually choose the Krylov Solver for large problems automatically with the Auto Select option selected. Krylov is less robust than the Direct Solver method because it uses iterative algorithms to solve the matrix equations. However, it is much faster and requires much less memory than the Direct Solver for large problems.

In most cases, Auto Select will choose the most effective solver automatically. Choose Direct Solver or Krylov Solver only when the Auto Select option cannot deliver satisfactory performance for a certain circuit.

Simulation time may not be a good indicator for the choice. Some problems are small, but still take a long time to simulate because parameters are being swept over many steps; such a problem should really be viewed as a sequence of small problems, and thus Krylov is not necessarily applicable. When a parameter is swept, if it takes X seconds to compute a single solution using the Krylov solver, it will probably take approximately 10X seconds to compute 10 solutions. On the other hand, if it takes Y seconds to compute a single solution using the direct solver, it will probably take far less than 10Y seconds to compute 10 swept steps of the analysis.

For system-level applications (behavioral mixers, amplifiers, etc.), the Krylov solver should be the preferred method of solution, as it is very robust in this area. For some transistor-level circuits, the Krylov solver may experience convergence difficulties at high input power levels. If this occurs, an analysis using the direct solver or the Envelope simulator should be attempted.

To select a specific solver:

1. Select the Solver tab in the Harmonic Balance setup dialog box.
2. Select the desired solver option. In general, we recommend that you accept the defaults and click OK to close the dialog box (or select another tab to set additional simulation specifications, as needed).

For descriptions of the options and parameters associated with the solvers, click Help from the dialog box.

Reusing Simulation Solutions

Harmonic balance simulation solutions can be saved and used later as an initial guess for another simulation, including harmonic balance, large-signal S-parameter, gain compression, or circuit envelope. Reusing solutions can save a considerable amount of simulation time. For example, you can save a harmonic balance solution and perform a nonlinear noise simulation, using this saved solution as the initial guess. Doing so removes the time required to re-compute the nonlinear HB solution. Another instance would be to solve for an initial harmonic balance solution and then sweep a parameter to see the changes.

To save a simulation for reuse:

1. Add the desired simulation component to your schematic-harmonic balance, large-signal S-parameter, gain compression, or envelope. Double-click to edit it.
2. Select the Params tab. If using the Envelope controller, select the HB Params tab.
3. Enable Write Final Solution. Enter a filename and any extension, or use the default which is <project_name>.hbs. The file will be saved in the networks folder of the project.
4. Click OK. When you run the next simulation, the solution will be saved.

To select a solution file to be used as the initial guess:

1. Place the simulation component of interest on the schematic if one is not present, then double-click to edit it.
2. Select the Params tab.
3. Enable Use Initial Guess. Enter the filename and extension.
4. To view any messages regarding how the initial guess affects the simulation, add an Options component and set the Annotate parameter. For more information on how to do this, refer to the topic Reusing Simulation Solutions.

Note Since harmonic balance simulations also use the DC solution, for optimum speed improvement, both the DC solution and the HB solution should be saved and re-used as initial guesses.

The initial guess file does not need to contain all of the harmonic balance frequencies. For example, you could perform a one-tone simulation with a very nonlinear LO, save the solution, and then use it as an initial guess in a two-tone simulation.

The exact frequencies do not have to match between the present analysis and the initial guess solution. However, the fundamental indexes should match. For example, a solution saved from a two-tone analysis with Freq[1] = 1GHz and Freq[2] = 1kHz would not be a good match for a simulation with Freq[1] = 1kHz and Freq[2] = 1 GHz.

Troubleshooting a Simulation

This section presents suggestions to help achieve a successful simulation that is fast and accurate. It includes the following topics:

• Selecting the Number of Harmonics describes how to select an optimum number of harmonics in a simulation to ensure accuracy and minimize simulation time.
• Reducing Simulation Time describes other methods to help reduce simulation time.
• Solving Convergence Problems offers a variety of methods to try if your simulation is failing because it cannot converge.
• Oversampling to Prevent Aliasing describes how the Oversampling parameter can be set to prevent aliasing during a simulation.
• Linearizing Nonlinear Devices describes how making a circuit more linear can improve the chances of a successful simulation.

Also, refer to the troubleshooting sections in DC Simulation and AC Simulation.

Selecting the Number of Harmonics

The number of harmonics needed to simulate a circuit accurately depends on nonlinearities in the circuit, the accuracy desired, and the acceptable simulation time.

Consider the following in choosing or changing the number of harmonics:

• If the simulation has been run with fewer than the minimum number of harmonics that are required for convergence, no solution is found. The simulation may not converge.
• If the simulation has been run with the minimum number of harmonics that are required for convergence, the simulation converges but the results are inaccurate.
• If the simulation has been run with the optimum number of harmonics that are required for convergence, the simulation converges and the results are accurate.
• If the simulation has been run with the more than the optimum number of harmonics that are required for convergence, the simulation converges and the results are accurate, but the simulation takes longer than necessary.

To verify that the simulation is accurate, choose a certain number of harmonics and perform the simulation. Then double the number of harmonics and simulate the circuit again.

If the results are the same, the first choice used enough harmonics for an accurate simulation. If the results differ, double the second choice and run the simulation again. Continue this procedure until there is no change (or there is an acceptable change) in the simulation after the number of harmonics is doubled.

Reducing Simulation Time

To reduce simulation time while still maintaining an accurate simulation, consider the following factors in your simulation and make the appropriate trade-offs:

• Simulation frequencies – The number of harmonically unrelated frequencies applied to a network increases the required memory and simulation time considerably.
• Power levels – Power levels that increase the degree of nonlinearity will increase simulation time.
• Harmonics – The more harmonics to be considered, the greater the memory and simulation time required.
• Sample points – Increasing the amount of oversampling may result in a modest increase in simulation time, unless the Krylov option is selected. (Refer to Oversampling to Prevent Aliasing).
• Error tolerances – The smaller the error tolerances, the greater the simulation time.
• Device models – The number of nonlinear elements in a device model and the number of devices used in the circuit will affect both the memory and simulation time required.

Solving Convergence Problems

Nonconvergence is a numerical problem encountered by the harmonic balance simulator when it cannot reach a solution, within a given tolerance, after a given number of numerical iterations. There is no one specific solution for solving convergence problems. However, consider the following guidelines:

• Increase the value of Order (or other harmonic controls); this is the most basic technique for solving convergence problems. However, if the time penalty for doing so becomes severe, other methods should be attempted.
• Use the Status server window as the main tool in solving convergence problems (set StatusLevel=4). For each Newton iteration the L-1 norm of the residuals throughout the circuit is printed: a "*" indicates a full Newton step (vs. a Samanskii step).
• Convergence criteria are controlled by Voltage relative tolerance, and Current relative tolerance. In general, convergence speed is improved by increasing these values, but at the expense of accuracy. Similarly, the smaller these values are, the more accurate the results but the slower the convergence. To set these values, use the Convergence tab on the Options component.
• Newton convergence issues with Krylov methods (because linear problem solutions can only approximate) can be improved by using better preconditioners.
• For non-convergence due to tight tolerances, monitor the residuals in the Status Server window:
  • Increase I_AbsTol if the circuit is converging to within a few pA but not quite to I_AbsTol=1pA.
  • Increase I_RelTol if the problem is with nodes associated with large currents.
  • Increase I_AbsTol if the small current nodes are the issue.
  • Relax voltage tolerances for failure in the Newton update criterion.
• Set the Oversample parameter to a value greater than 1.0, such as 2.0 or 4.0. However, remember that although this can often solve convergence problems, it does so at the cost of computer memory and simulation time. For multiple-tone harmonic balance simulations, make sure that the largest signal in the circuit is assigned to Freq[1]. The simulator's FFT algorithm is set up so that aliasing errors are much less likely to affect Freq[1] than any other tone. For instance, assign the LO signal in a receiver chain to Freq[1] and the RF signal Freq[2]. For more information, refer to Oversampling to Prevent Aliasing.
• Circuits that contain MOSFETS may fail to converge as a result of inherent limitations in the SPICE MOSFET model (Level 1, 2 and 3). This problem can often be circumvented by using the device's Xqc parameter. Setting Xqc to a nonzero value allows the simulator to use a charge-based model (based upon the work of Ward and Dutton) for the gate capacitance. This often enables the simulator to converge, but at the cost of extracting an extra SPICE model parameter. Also, time-domain simulations usually handle MOSFETs with no difficulty.

  Note There are many references in the literature to SPICE MOSFET models. One is Antognetti and Mossobrio, Semiconductor Device Modeling with SPICE, Second Edition, McGraw-Hill, 1993.

• Harmonic balance simulation uses the parameters Current relative tolerance, Voltage relative tolerance, Current absolute tolerance, and Voltage absolute tolerance in the same way as DC simulation does. For more information, see Setting Convergence Options.
• Do not use more harmonics than you really need. Too many harmonics can introduce so many unknowns to the solution that the simulator cannot find an answer (because the Jacobian becomes ill-conditioned). Removing harmonics can make the circuit easier (and faster) to solve, but if too many harmonics are removed, Fourier series truncation errors will become important. The simulator will converge on an answer, but it will not be accurate. Refer to Selecting the Number of Harmonics for instructions on how to minimize the number of harmonics.
• If the simulator cannot find a solution, it will attempt to do source stepping. This sets all large-signal AC sources to zero (leaving DC sources alone) and attempts to achieve convergence at a lower level. Starting from this solution point, the simulator will try to converge at the original level by repeatedly solving the circuit at incrementally increasing source levels, using the results of each simulation as the initial guess for the next. Very rarely, circuits can exhibit a bizarre behavior that can cause this technique to fail.
• If the harmonic balance simulation cannot converge on a solution within a given number of iterations, try increasing the limit in the Max. Iterations field, under the Params tab.
• The internal circuit simulator engine in ADS (ADSsim) runs from a netlist. ADS writes a netlist file (netlist.log) before invoking ADSsim. The order of the components and model definitions in the netlist determine the initial Jacobian matrix ordering. This matrix ordering can affect the efficiency of the Jacobian factorization and cause either a simulation slow down or non-convergence.
• For convergence problems due to errors in the component model equations (incorrect derivatives, etc.) make sure ancient Berkeley MOSFET Level 1, 2, 3 are not the culprit and that the latest model version is used (especially BSIM3 models). Model problems can cause the Newton residual to hit a threshold (greater than the convergence criteria tolerances) and stale the convergence process or even exhibit random jumps (sudden increase in value). Set the device's Xqc parameter to a nonzero value to allow the simulator to use a charge-based model for the gate capacitance. This often enables convergence, but at the cost of extracting an extra SPICE model parameter.

Sweeps as Convergence Tools

Continuation methods provide a sequence of initial guesses that are sufficiently close to the solution to assure Newton's method convergence in Harmonic Balance. Sweeps can be used to formulate a specialized continuation method geared towards the particular circuit problem.

Try sweeping a parameter to correct a convergence problem. Find a circuit element that, when set to some different value, makes the circuit more linear. For instance, in an amplifier circuit there may be a resistor that can be used to lower the amplifier's gain. The simulator may be able to find a solution to the circuit under a low-gain condition. Then, if the component's value is swept toward the desired value, the simulator may be able to find a final solution. Start with a value that works, and stop with the desired value. Also, select Restart, on the Initial Guess tab. Usually, a better initial guess at each step helps the simulator to converge.

The two main ways to perform sweeps are:

• HB sweep within the HB controller. This is preferred for most sweeps, except frequency.
• Parameter sweep using a separate sweep controller.

Convergence and the Samanskii Steps

The Samanskii constant is a real non-negative number that is used to determine whether the simulator can skip the Jacobian evaluation in some iterations, and just reuse an approximate Jacobian instead (Samanskii steps). The Samanskii steps can significantly speed up the solution process. However, using an approximate Jacobian, particularly for a larger number of iterations, may result in poor or even no convergence. The constant is used in two ways. First, it becomes a more absolute measure when it is smaller. It then approaches the requirement that each iteration reduces the relevant norm by one-third.

Decreasing the Samanskii constant beyond a certain point (which in turn depends on the quality of the most recent Newton step) will make no difference. However, setting the Samanskii constant to zero will effectively disable any Samanskii steps altogether.

Increasing the Samanskii constant relaxes this requirements in general, but the condition becomes more dependent on the quality of the standard most recent Newton iteration. In other words, a more rapid convergence of the Newton step would also require better convergence of the Samanskii steps.

The default Samanskii constant of 2.0 corresponds to the quality of the Newton step such that the norm is reduced by 50% (decreasing the Samanskii constant will not make any difference if this is the case). Such a cut-off value gets larger with a more significant norm reduction of the Newton step. For example, an 83% norm reduction would result in a cut-off value of 10.

Note To edit this parameter, select the Display tab in the Harmonic Balance Simulation component and set SamanskiiConstant to display on the schematic page. You can then edit the parameter directly on the schematic.

Convergence and Arc-Length Continuation

Arc-length continuation is an extremely robust algorithm. If it fails, try all other convergence remedies first before adjusting arc-length parameters:

• MaxStepRatio controls the maximum number of continuation steps (default 100).
• MaxShrinkage controls the minimum size of the arc-length step (default 1e-5).
• ArcMaxStep limits the maximum size of the arc-length step (default is 0, i.e. no limiting).
• ArcMinValue & ArcMaxValue define the allowed range for the variation of the continuation parameter.

Oversampling to Prevent Aliasing

Oversampling increases the accuracy of the solution by reducing the FFT aliasing error, and improves convergence for circuits with many nonlinear devices.

Aliasing error is introduced during the evaluation of nonlinear devices when a time waveform is converted into a spectrum. Aliasing is caused by using too few time-points to represent the time waveform. The Nyquist criterion states that to avoid aliasing errors, the sampling frequency should be at least twice the highest frequency present in the time waveform. If not, error is introduced into the high-frequency Fourier coefficients. The only way to eliminate aliasing error is to increase the sampling rate (that is, to increase the number of data points). This can be done by oversampling the time waveform (select Fundamental Oversample, on the Params tab). The relationship between Order, Fundamental Oversample, and the number of samples for a single tone simulation is given by:

Number of Samples = 2*(Order[1] +1)*Oversample, rounded up to the nearest power of two.

For the same value of Order, different values of Fundamental Oversample can yield the same number of samples. Also, oversampling can occur even with a Fundamental Oversample value of 1, because the system rounds the FFT size up to the next power of two. This can be seen from the following two tables:

Order	Fundamental Oversample	Number of Samples
7	1	16
7	2	32
7	3	32
7	4	64
7	5	128
7	6	128

Order	Fundamental Oversample	Number of Samples
8	1	32
8	2	64
8	3	64
8	4	128
8	5	128
8	6	128

In a multitone HB simulation, it is possible to set the oversample for each tone. To do this, click More next to the Fundamental Oversample parameter. The Oversample Options dialog box appears enabling you to enter the Oversample values for each fundamental in the multitone simulation. For a multitone simulation, the number of samples is determined in two parts. First, the same method used for the single tone case applies to the first tone; that is, 2*(Order[1]+1)*Oversample, rounded up to the nearest power of two. Second, for all successive tones (Order[i], i > 1), the number of samples is (2*Order[i]+1)*Oversample, rounded up to the nearest power of two. The final resultant number of samples is the product of the number of samples from each part.

In the case of having different sample values, the same rules apply for determining the total number of samples. The value for Oversample[1] applies only to Order[1], and Oversample[2] applies only to Order[2]. If a value is given for Fundamental Oversample and for Oversample[1], the value of Oversample[1] will be used.

Order[1]	Order[2]	Oversample[1]	Oversample[2]	Number of Samples
5	3	1	4	512
5	3	2	3	1024
7	4	3	2	2048
7	4	4	1	1024

While oversampling does not increase the number of harmonics, it does increase the size of the FFT used in HB. This means that the HB simulation run time using the direct solver (which is determined by the Order and the circuit size) is not largely affected when the Fundamental Oversample is increased. However, an HB simulation run time using the Krylov solver will be slower since this solver's computational complexity depends on the size of the FFT.

Note that MaxOrder does not enter any of the calculations for the number of samples.

Linearizing Nonlinear Devices

The number of nonlinear devices in a network has a dramatic effect on the speed of harmonic balance simulation. For circuits with a large number of nonlinear devices, such as those found in RFICs and high-speed digital applications, a standard harmonic balance simulation may become extremely slow, especially for a multitone simulation or where large numbers of harmonics are involved. However, usually only a few devices in such circuits are driven into nonlinearity. Depending upon the application, many devices in the circuit may be operating in their linear region.

A significant increase in the speed of a harmonic balance simulation can be achieved without loss of accuracy if the devices that are operating in the linear region can be identified and linearized about their DC operating point. When these devices are simulated, they are treated as other linear elements and are evaluated in the frequency domain instead of the time domain. The increase in simulation speed is generally proportional to the number of valid device linearizations.