Solving Convergence Problems
This section discusses the different types of convergence problems that can occur when using the Harmonic Balance simulator. It also includes the remedies for these possible convergence problems. The parameters used for convergence are mentioned in this section, and are thoroughly described in Additional Parameters.
Prior to fixing a convergence problem, you should have some familiarity with the Convergence mode and Solver type parameters. Realize that the nonlinear outer solver, Newton solver, and Convergence mode parameter are one in the same. Similarly, the linear solver, inner solver, and solver type are one in the same. By default, these parameters are automatically adjusted by the simulator to achieve both speed and robustness. Convergence mode and Solver type are found on the Solver tab of the HB controller. Although it is not recommended to modify the Convergence mode or Solver type, you have the option to do so.
Convergence Mode
There are three choices for the nonlinear (outer) solver that can be selected by setting the Convergence mode (ConvMode on schematic). The maximum number of iterations for the nonlinear solver is controlled by the parameter Max. Iterations (MaxIters on schematic). Max Iterations can be set to Fast, Robust, or a Custom value. The Convergence mode parameter options are described below.
- Auto This is the default mode setting. It is both fast and robust. This mode will automatically activate advanced features to achieve convergence. The auto mode also allows for convergence at looser tolerances if the simulation does not meet the default tolerances. A warning message appears in the status window when this occurs, and it includes the tolerance level up to which convergence was achieved.
- Robust This option enables an advanced Newton solver. This mode is extremely robust, and ensures maximal KCL residual reduction at each iteration. The Robust convergence mode usually simulates slightly slower, yet works well for very nonlinear circuits (i.e., those with very high power levels). It is recommended that the maximum number of iterations (MaxIters) be set to Robust when this mode is selected. Another option is to select Custom and enter a value of 50 or higher.
- Fast This option enables the basic Newton solver. It is fast and performs well for most circuits. For highly nonlinear circuits, this mode may have difficulties converging. It is then recommended to switch to the Robust convergence mode.
Solver Type
When using harmonic balance, you can allow the simulator to choose a solver automatically, or select one of two linear (inner) solver techniques: Direct or Krylov. The linear solver is used to solve the matrix problem generated at each iteration of the Newton (outer) solver. The matrix size will be determined by both the size of the circuit and the total number of frequencies (fundamentals, their harmonics, and mixing products).
Auto Select Solver
This option allows the simulator to choose which solver to use. The Auto select solver is enabled by default. 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 the Direct or Krylov solver in a manner transparent to you. The selection choice heavily depends upon the amount of available RAM. The simulator will determine roughly how much RAM is available. Alternately, you can specify the amount of RAM to allocate; however, if this is not enough for the simulator, then it will either allocate more RAM or report an error. Furthermore, if the Krylov solver is chosen by the simulator, several options for that solver also are set automatically.
It is possible to override the choice of solver given by the Auto select solver option. This can be done simply by selecting Direct or Krylov from the Solver tab on the HB controller. When simulating large circuits, that is, those with many devices and harmonics, it is recommended to use the Krylov solver.
Direct Solver
The Direct solver uses direct matrix factoring methods (such as Gaussian elimination) to invert the Jacobian matrix. This solver is recommended for small circuits with relatively few devices, non-linear components, and number of harmonics. For large circuits, the direct solver will be slow and inefficient. This is because the computation time of the direct solver grows with the cube of the matrix size. For example, in a single-tone HB simulation, doubling the circuit size or doubling the number of harmonics (the Order) will slow the simulation run time by a factor of 8. Also, since the direct solver requires an explicit storage of the Jacobian, its memory requirements grow with the square of the matrix size. For example, the factorization of a Jacobian with a size 500 will require 2500 times as much RAM as one with a size of 10.
Krylov Solver
An alternate approach to solving the matrix problem is to use a Krylov subspace iterative method such as GMRES. The Krylov method is intended for solving large circuits with many devices, non-linear components, and number of harmonics. (A large circuit can be roughly described as one in which a simulation using the direct solver exceeds 100 MB of memory usage or the memory capacity of the computer, whichever occurs first.) The Krylov solver does not require the explicit storage of the Jacobian matrix, but rather only the ability to carry out matrix-vector products. As a result, Krylov solver's memory requirements grow linearly with the matrix size, rather than quadratically as in the direct method. Thus, Krylov solvers offer substantial memory usage savings for large circuit problems. Since the Krylov method solves the matrix problem to a loose tolerance, it is also much faster than the direct solver (but less robust). The computation time of the Krylov solver grows slightly faster than linear with the matrix size. For example, doubling the circuit size or doubling the number of harmonics will increase the simulation run time by slightly more than a factor of 2.
Setting Status Level and Understanding Output in the Status Window
During an HB simulation, the simulator prints information describing the simulation progress in the status server window. The Status level parameter (found on the Freq tab) controls the amount of detail in this information. Reading and understanding this information is critical to solving convergence problems.
The default status level is set to 2; however, when solving a convergence problem, it is best to set the status level to 4. For each Newton iteration the L-1 norm of the KCL residuals throughout the circuit is printed.
The KCL residual indicates how well the circuit has converged up to that point. A steadily decreasing residual implies successful convergence. For example, for an HB simulation at default (strict) tolerances, this residual should reach levels of pico amps at the end. A snap shot of the ADS Status Server Window is shown in the following figure.
When using the Krylov solver, it is useful to print additional information by setting the status level to 5, as shown in the following illustration.
---------------------------------------------------------------------------
Newton solver: Linear solver:
Iter KCL residual Damp % Sol update Iters Residual
----------------------------------------------------------------------------
11 115.983 mA 100.0 12 1.189e-03
----------------------------------------------------------------------------
Krylov solver (target tol = 0.00119):
Iter Residual
- - - - - - - - - - - - - - - - - - - - - - - -
0 1.000e-00
1 3.276e-01
2 2.180e-01
3 1.208e-01
4 6.767e-02
5 3.017e-02
6 1.818e-02
7 1.220e-02
8 4.739e-03
9 3.219e-03
10 6.449e-04
---------------------------------------------------------------------------
Newton solver: Linear solver:
Iter KCL residual Damp% Sol update Iters Residual
----------------------------------------------------------------------------
12 51.3821 mA 100.0 10 6.449e-04
----------------------------------------------------------------------------
Krylov solver (target tol = 0.001):
Iter Residual
- - - - - - - - - - - - - - - - - - - - - - - -
0 1.000e+00
1 5.178e-01
2 3.442e-01
3 2.976e-01
4 2.138e-01
5 9.809e-02
6 7.323e-02
7 3.645e-02
8 8.977e-03
9 7.924e-03
10 1.130e-03
11 1.130e-03
11* 7.830e-04
- The target tol indicates the desired Krylov solver tolerance.
- The residual at each Krylov solver iteration indicates how well the Krylov solver has converged up to that point. When the Krylov solver is performing well, the residual decreases quickly, and the Krylov solver reaches the target tolerance in fewer iterations.
- The Newton solver lines include a summary of the linear solver performance: the total number of Krylov iterations and the achieved Krylov tolerance (this information is also printed for status level set to 4).
- The Sol update (solution update) is largest amount of voltage change between two successive outer solver (Newton) iterations for all solution waveforms. This will get printed toward the end of the simulation, or in the case of a swept simulation, it will get printed at the end of each sweep point.
- Because the Robust convergence mode (for the Newton solver) was used in this example, the damping percentage of the solution update is also printed.
When using the Auto solver, set the status level to 5 to see the relevant circuit statistics, memory computations, and the chosen parameter settings.
After increasing the status level, it is recommended to insert an Options controller and check the box (found on the Output tab) labeled Issue Warnings (GiveAllWarnings=yes on schematic). Be sure to watch for these warning messages in the status window and act upon them accordingly.
Parameter Access
The most frequently used parameters can be accessed from the various HB controller tabs. A second group of parameters which are used less frequently can be accessed through the Harmonic Balance Display tab. Choose to display the parameter on the schematic and edit its value on the schematic. The final group of parameters are the hidden parameters. To activate these parameters, use the entry on the Display tab called Other. The format is
Other=HiddenParameter1=value HiddenParameter2=value HiddenParameter3=value....
The figures below show the Display tab from the HB controller and an example of how to use the Other parameter. Note that once the Other parameter has been selected to be displayed, it may be edited on the schematic. For example,
Other=RedRatio=0.8 NormCheck=0
Circuit Operation and Verification with Transient Simulation
It is important to verify that the circuit is operating properly, as intended by the designer. Performing a transient simulation prior to a harmonic balance simulation will enable you to check for unstable circuits and circuits with multiple solutions. After running a transient analysis, check to see if the waveforms blow up or have several spikes and sharp edges. In the case that the waveforms have these conditions, Harmonic Balance may require hundreds or even thousands of harmonics which in turn will significantly increase simulation run time and memory usage.
Harmonic Balance Controller Setup
When a circuit does not converge, it is important to check that the controller is set up correctly and with appropriate controller parameter settings.
Order
The Harmonic Balance solution is approximated by a truncated Fourier series. When convergence problems begin to occur, the first parameter to examine is the Order, which is the number of harmonics. The lower the Order, the greater the error due to Fourier truncation in the solution representation. The Order needs to be sufficiently large to represent nonlinear signals such as those with sharp transitions or square waves. If increasing the order causes the simulation speed to dramatically slow down or there is an excessive usage of memory, then it is best to switch from the direct solver to using the Krylov solver.
By setting the status level to 4 or more, an HB truncation error warning may be given in the status window upon a successful completion of an HB simulation. The warning contains a sorted table of the five waveforms in violation of the HB truncation error check with largest HB truncation errors. Note that the HB truncation error check is not the same as the circuit convergence check for the KCL residual; in fact, the HB truncation error warning can be generated only once the circuit has converged. The HB truncation error may not be distributed evenly across all of the computed harmonics.
If fewer than five waveforms violate the HB truncation error check, only those will be printed. If there are no violating waveforms, then the HB truncation error warning is not printed at all. Increasing the order will reduce the number of violating waveforms. An example of the warning message for HB truncation error is shown below:
Warning detected by HPEESOFSIM during HB analysis `HB1'.
An HB truncation error may be present.
o The HB truncation error is due to using a finite order
(number of harmonics) in the representation of the
circuit signals.
Waveform Trunc error Tolerance
---------------------------------------------------------
v2 6.576e-03 > 5.941e-06
v3 1.780e-03 > 1.043e-06
o Number of waveforms violating the HB truncation error check:
2 out of 2 waveforms.
o Estimated max HB truncation error: 6.576e-03 @ waveform v2.
o The maximal HB truncation error estimate is greater than the
achieved tolerance of 5.941e-06 for this waveform.
o A time-domain plot of the v3 waveform may show the error as
Gibbs ripples.
o To reduce the error, increase the order (number of harmonics)
and re-simulate.
It is recommended to create a time domain plot of the solution waveforms with large HB truncation errors (or a plot of any other solution waveform which has sharp features, spikes, or square waves) to get an idea for how much to increase the Order to reduce the truncation error. The truncation error in the plot is seen as Gibbs ripples. An increase in the Order will reduce the truncation error, decrease these ripples, and decrease the number of waveforms violating the HB truncation error check. The plots shown in the following figure give an example of the HB truncation error and show how it is reduced when increasing the Order. When the Order=7, there are large Gibbs ripples in the output waveform. When the Order is increased to 15, the amplitude of the ripples diminishes significantly. In the last plot, the Order is 63 and the HB truncation error is negligible.
For maximum computational efficiency when simulating with the Krylov solver, set the Order=7, 15, 31, etc. This suggestion is based on the fact that the Krylov solver's computational complexity depends on the size of the FFT.
Fundamental Oversample
In Harmonic Balance, nonlinear devices are evaluated (sampled) in the time domain, then converted to the frequency domain with the FFT (Fast Fourier Transform). When the time domain sampling rate is greater than twice the largest harmonic frequency, this is known as oversampling. See the diagram below for a waveform that is sampled with oversample set to 1 (no oversampling), and one that has oversample set to 2.
For a single-tone HB simulation, increasing the Fundamental Oversample parameter (found on the Params tab) can help convergence by ensuring that rapid transitions and sharp features in the device waveforms are more precisely sampled. As a rule of thumb, try Fundamental Oversample=2, 4, 8.
In a multi-tone HB simulation, it is possible to set the oversample for each tone. To do this, click More next to the Fundamental Oversample parameter. A new dialog box will appear enabling you to enter the Oversample values for each fundamental in the multi-tone simulation. Similarly to the single-tone case, try Oversample=2, 4, 8.
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.
Newton Solver Issues
The default Convergence mode is the Auto mode. This mode is preferred since it is fast and robust. The Auto mode works well on a wide range of circuits, including those which are fairly linear to those which are highly nonlinear and contain sharp edge waveforms. It also works well for circuits containing a large number of transistors, and for circuits that seem to go into arc-length continuation or source stepping in only a few number of iterations.
The alternate convergence modes are Fast and Robust. The Fast mode simulates quickly and works well for most circuits. The Robust convergence mode usually simulates slightly slower, yet works well for very nonlinear circuits (i.e., those with very high power levels). The Robust mode solver should exhibit more robust convergence than the Fast mode solver. If the KCL residual in the status window output fails to continue decreasing or exhibits a bouncing pattern (alternates between decreasing and increasing), the Robust convergence mode may also help.
All three convergence modes need an initial guess. The default initial guess is based on a DC solution. Certain circuits may not converge from this starting point.
The initial guess can be changed using the hidden parameter InitGuess . By default, InitGuess=0 (DC initial guess). Set InitGuess=1 to use zero voltages and currents for the initial guess.
Linear Solver Issues
If convergence issues occur while using the Direct solver, some parameters (located on the Harmonic Balance controller's Solver tab) can be modified to assist with convergence. If the Direct solver fails to converge, then set Matrix Re-use to Robust. This parameter controls how frequently the Jacobian is constructed and factored rather than being reused. Selecting Robust means that the Jacobian will be computed at each iteration and will not get reused for future iterations. A "*" next to an iteration number in the status window output indicates a re-computation of the Jacobian for that iteration.
The Jacobian matrix from the Direct solver within the Newton solver is a block matrix. A block matrix is a matrix whose elements are matrices and vectors. The blocks of the Jacobian are truncated to a specified threshold by default. The default threshold (bandwidth) is set by the parameter Matrix Bandwidth , and its default value is Fast. This bandwidth truncation speeds up the Jacobian factorization and saves memory, but can lead to convergence problems due to an innacurate Newton direction. In order to get the full bandwidth of the Jacobian blocks and improve the convergence, set Matrix Bandwidth to Robust. Typical values for the Custom entry range from 10 -4 to 0.
If convergence issues occur while using the Krylov solver, increase the status level to 5 and monitor the KCL residual and the Krylov solver residual in the status window. If the Krylov solver converges very slowly, its iterations may be terminated before the linear problem can be solved to an acceptable degree of accuracy. In such a case, the following message will appear in the status window output:
<name_of_Krylov_solver> terminating due to insufficient rate of convergence.
It is recommended to set the Krylov Restart Length (GMRES_Restart on schematic) parameter to Custom and enter a value between 10 and 100. The default setting is Robust. However, if there is a limited amount of memory available, then select Low Memory. This parameter determines the number of iterations after which the Krylov solver is restarted. Also, to prevent the Krylov solver from stopping too soon due to "insufficient rate of convergence", increase the Krylov Convergence Ratio (KrylovConvRatio on schematic). This is the amount by which the norm of the Krylov solution must decrease from one iteration to the next. The default is 0.9 and it should not be larger than 1.0.
As a last resort, it is recommended to change the Krylov preconditioner. A preconditioner is used to increase the rate of convergence of the Krylov linear solver by reducing the number of iterations performed. Thus, preconditioning is essential to making the Krylov solver effective. Click Advanced Krylov Parameters to choose the preconditioner.
The default preconditioner is DCP. Some of the Krylov solver's convergence problems arise due to the limitations of the DCP. There can be multiple reasons for these problems, such as strong nonlinearities in the circuit generating an ill-conditioned linear problem at each Newton iteration. As a result the Newton direction becomes inaccurate so that the nonlinear solver fails to converge. When the Krylov solver has trouble converging, it is recommended to change the preconditioner to BSP or SCP. The BSP typically is more efficient for medium to large size problems, while SCP works better for very large problems. Changing the preconditioner should be done only when an error message appears in the status window giving specific instructions to change the preconditioner.
The three types of preconditioners used by the simulator are summarized below. You must select one when using the Krylov solver:
- DC Preconditioner (DCP) This is the default preconditioner, which is effective in most cases, but fails for some highly non-linear circuits. It uses a DC approximation on the entire circuit.
- Block Select Preconditioner (BSP) This is recommended for instances when a Krylov HB simulation fails to converge using the DCP option. The BSP preconditioner is more robust than the DCP for highly nonlinear circuits. For the circuits that converge with DCP, the overhead introduced by the BSP preconditioner is small. For circuits that fail with the DCP, using the BSP option often achieves convergence at the cost of additional memory usage.
- Schur-Complement Preconditioner (SCP) This is also intended for use with circuits that fail to converge with the DCP preconditioner. This is a robust choice for highly nonlinear circuits. It uses the DC approximation for most of the circuit similar to DCP. The most nonlinear parts of the circuit are excluded and are instead factored with a specialized Krylov solver known as DMRES. The complex technology of the SCP preconditioner results in a memory usage overhead. This overhead is due to construction of a knowledge base enabling the SCP to be much more efficient in the later use of the harmonic balance solution process.
Sweeps as Convergence Tools
Parameter sweeps can be used to formulate a customized continuation method geared toward the particular circuit problem. Continuation methods provide a sequence of initial guesses that generate a sequence of solutions that approach the final desired solution.
There are two main ways to perform a parameter sweep in ADS. The first way is to use the Sweep tab within the HB controller. This is the most efficient way to perform sweeps, and thus is the preferred way. The second way is to include a Parameter Sweep controller, which is a separate controller from the HB controller. For single parameter sweeps (in which the swept parameter is not frequency), use the Sweep tab on the HB controller. For multi-dimensional sweeps, use the Sweep tab for the inner-most sweep parameter, and use the Parameter Sweep controller(s) for the outer-most sweep parameter(s). Frequency should always be selected as an outer-most sweep parameter even for multi-tone simulations.
When a single point HB simulation does not converge, a parameter sweep can be used as a convergence tool. Performing a sweep around a single point that does not converge helps to determine if there is a range of values for which the circuit can converge. Selecting which parameter to sweep is the first step. It is best to choose a parameter that can be set to a value for which the circuit will easily converge. Some examples are the source amplitude or power, a bias voltage or current, or any component parameter that controls the amount of nonlinearity in the circuit. Find the parameter value for which the circuit converges and make this the start point of the sweep. The actual parameter value for which the circuit does not converge should be the end point of the sweep. Perform a swept simulation up to the point for which the circuit converges, and save the solution to be used as an initial guess for single point simulation that does not converge. Simulate the single point with this initial guess. This may give the Newton solver a better initial guess than the DC solution.
In most cases, a linear sweep will work best. When performing a sweep, be sure that the Regenerate Initial Guess for Param Sweep (Restart) is not checked (i.e., Restart=no). This ensures that the sweep will be used as a continuation, or in other words, the solution from the previous sweep step is used as an initial guess for the next step. Having more sweep points will give a greater chance for success, but will result in a longer computation time.
Two diagrams are shown, one for each sweep method. The following figure shows the Harmonic Balance controller sweeping the variable Power_LO from -20 dbm to 10 dBm in steps of 1 dBm. A VAR equation needs to be included to initialize the parameter that is to be swept. The value of this parameter in the VAR equation can be set to an arbitrary number, since the value of the sweep start will override this value.
The following figure shows a parameter sweep setup using a Parameter Sweep controller. The parameter being swept is RFfreq, from 1700 MHz to 1900 MHz in steps of 20 MHz. For sweeping frequency, it is recommended to use a Parameter Sweep controller, and not the Sweep tab on the HB controller. When using a Parameter Sweep controller, the SimInstanceName must be set to the instance name of the Harmonic Balance controller, as shown for the parameter SimInstanceName[1]= "HB1".
When a swept Harmonic Balance simulation does not converge, you can
- adjust convergence parameters and keep restarting the swept simulation from the very beginning, or
- split the sweep into two parts, or
- perform a single point simulation at the value for which the swept parameter does not converge to determine if the simulation will converge for just that one particular point in the sweep.
The first option is feasible for small circuits that simulate quickly. The second option is preferred for larger circuits with longer simulation run times.
For example, consider sweeping the input power from -20 dBm to 10 dBm. If the circuit does not converge, reduce the range of the sweep so that the last point is the one for which the circuit will still converge (this is the first sweep). Suppose the circuit converged only up to 5 dBm. The 5 dBm solution can be saved in an output file: select the parameters Write Final Solution and enter the name of the file for the output to be saved. Adjust parameters such as Order, Oversample, and number of iterations; then try a second sweep from 5 to 10 dBm and see if the circuit will go beyond 5 dBm. The 5 dBm output file should be used as an initial guess for this second sweep: select Use Initial Guess and enter the name of the file.
As a more detailed example, consider sweeping the RF frequency in a mixer circuit (with the Fast convergence mode and Krylov solver) from 0.5 GHz to 1.5 GHz, using 11 sweep points (0.1 GHz step size). Suppose this circuit can only converge up to the RF frequency point of 1.0 GHz and fails at 1.1 GHz. At this point, it is recommended to follow these steps:
- Break the sweep into two parts (the first part will be a sweep over the range of frequencies for which the circuit converges, and the second part will be the remaining sweep points).
- Simulate the first part to generate an initial guess which can be used for the second sweep.
- Adjust parameters to achieve convergence for the second part of the sweep.
For this mixer example, it is desired to have 11 sweep points between 0.5 GHz and 1.5 GHz. This means that spacing between sweep points is (1.0 GHz)/10 = 0.1 GHz. The frequency sweep points are then placed at: 500 MHz, 600 MHz, 700 MHz, 800 MHz, 900 MHz, 1000 MHz, 1100 MHz, 1200 MHz, 1300 MHz, 1400 MHz, and 1500 MHz. Setup the simulation for the first sweep with a VAR block to define fstart1=0.5G, fstep1=1.0G/10, fstop1=fstart+5*fstep, and np1=6. Since the simulation does not converge beyond 1 GHz, the first sweep is done up to that point, which is 5 frequency points after the start i.e., fstop1=fstart+5*fstep. The total number of points for the first sweep is 6 (np1=6). The remaining 5 points will be used for the second half of the sweep.
Instantiate a Parameter Sweep controller, and set Start=fstart1, Stop=fstop1, and Num. of Points=np1. The sweep step size will be determined by the Num. of Points, and will be equivalent to the value for fstep. It is not necessary to specify the step size parameter when specifying the Num. of Points parameter. Next, on the Harmonic Balance controller's Params tab, select Write Final Solution and enter the name of the file that will be used as an initial guess for the second sweep. Run the HB simulation. After it completes, add the following equations to the VAR block - fstart2=fstop1+fstep1, fstop2=1.5G, np2=5. We want the second sweep to start from the point at which the original sweep failed, thus, fstart2=fstop1+fstep1. There are five remaining points, so np2=5. Go back to the HB controller, and on the Initial Guess tab, unselect Write Final Solution. Now select Use Initial Guess and enter the name of the file that was written during the first sweep. Next, return to the Parameter Sweep controller, set Start=fstart2, Stop=fstop2, and Num. Of Points=np2. (Or deactivate the Parameter Sweep controller and instantiate a new one with the sweep var as RFfreq but with the start and stop with the values for the second sweep). It is not necessary to enter the step size since that is determined by using the Num. Of Points, and the Start and Stop. The next step is to adjust certain parameters to achieve convergence. Recall that the nonconverging simulation was using the Fast convergence mode. For the second half of the sweep, it is then recommended to use the Robust convergence mode (found on the Solver tab) with the Krylov solver. For this mixer circuit, convergence was achieved using the Robust mode. Alternatively, the entire sweep could have been performed using the Robust convergence mode from the beginning rather than performing two sweeps. However, this approach is less efficient than the two part sweep due to the overhead computation required by the Robust mode in the first part of the sweep.
 | Note After doing a HB analysis, you may want to do an HB noise analysis. A saved final solution may be used as the initial guess for other simulations such as noise analysis (of the same circuit) so that the node voltages and branch currents do not have to be recalculated. |
Transient Assisted Harmonic Balance - TAHB
The DC solution is the default initial guess; however, a transient solution can be a better initial guess for the Newton solver. The size of the initial KCL residual (seen from the status window output) is a measure of the quality of the initial guess (the smaller the KCL residual, the better the initial guess). A better initial guess such as TAHB can yield several orders of magnitude improvement in the initial KCL residual. For circuits that are highly nonlinear and contain sharp-edged waveforms (such as dividers), a transient simulation often provides a good initial guess for the starting point of harmonic balance.
Automated TAHB
By default, the HB simulator will determine if there is a divider in the circuit. If so, a transient simulation will be performed to create an initial guess for the HB simulation. TAHB can also be turned on or off from the Initial Guess tab by selecting On or Off, respectively. When a divider is detected or if TAHB is set to On, the transient simulator will use intelligent defaults and determine a steady state solution as the initial guess for harmonic balance. It is not required to set any of the other parameters on the Initial Guess tab. The transient parameters can be set only when TAHB is set to On.
Setting Advanced Transient Parameters
Advanced transient parameters can be set when TAHB is set to On . Some are included on the Initial Guess tab in the Transient Assisted Harmonic Balance section under Advanced Transient Parameters. The first parameter is the StopTime, e.g., the ending time for the transient simulation. The default is 100 cycles of the commensurate frequency. (For a one tone analysis, this would be Freq[1]). If the transient simulator detects steady state, then the simulation will end one period after that time point, and thus earlier than the StopTime. The one period after the time point gets transformed to the frequency domain for harmonic balance. If transient does not reach steady state, then the last period before the StopTime will get transformed to the frequency domain, and harmonic balance will use that for the initial guess. If convergence is not achieved in this case, then it is recommended to increase the StopTime so that transient runs longer than 100 cycles.
The second parameter is MaxTimeStep. The default is 1/(2*4*Maximum frequency). In a single tone analysis, the maximum frequency would be Freq[1]*Order[1]. Be sure to set MaxTimeStep small enough to accommodate the largest frequency. The simulator will display the values that it determined for StopTime and MaxTimeStep in the status window.
The third parameter is Min Time for detecting steady state (SteadyStateMinTime on schematic). This is the earliest point in time that the transient simulator starts checking for steady state conditions. The default is two periods of the fundamental frequency for autonomous circuits, and 10 periods of the fundamental frequency for non-autonomous circuits such as an oscillator. The units for this parameter are in seconds. If your circuit exhibits a large amount of over/undershoot, then this to be larger than the default so that the detector will begin to check for steady state after some of the initial transients have settled.
The fourth parameter is IV_RelTol. This is the transient current and voltage relative tolerance, and the default is 1e-3. It is specific to the transient analysis and will override the relative tolerances on the Options controller if one is found in the schematic. If an Options controller is included in the schematic, be sure to set the IV_RelTol to a reasonable value, such as 1e-3. Otherwise the transient simulation would run for a very long time since it would use the relative tolerances on the Options controller which are set for harmonic balance.
Any transient parameter that is not found on the tab can be set using the Transient Other parameter. For example, one could set the following transient convolution parameter ImpMaxFreq=10 GHz.
When TAHB is set to On, a user-supplied initial guess is not able to be specified, and thus it is not interpreted at all. If one is given and TAHB is set to Auto (the default), the user-supplied initial guess takes the highest precedence.
Using a One-Tone Transient for a Multi-Tone Harmonic Balance
An initial guess generated by a single tone transient simulation may be used for a multi-tone harmonic balance simulation. This approach is strongly recommended, and will often result in much better convergence than with a multi-tone transient simulation. The parameter Use only Freq[1] for transient instructs transient simulator to perform a one tone simulation, and to only use the value of Freq[1] on the harmonic balance controller for determining the StopTime and MaxTimeStep. The default is yes. If there are multiple frequencies on the HB controller and this parameter is yes, then sources in the circuit at the other frequencies will be turned off for the transient portion only. Also, Freq[1] should be set to the frequency of the most nonlinear tone.
Swept and Optimizations Simulations with TAHB
Any optimization or statistical analyses such as optimization, yield, Monte Carlo, DOE, and yield-optimization are not supported with automated TAHB. The simulation will use the standard harmonic balance in those cases.
When sweeping a parameter on the sweep tab, a transient simulation is done for the harmonic balance simulation of the first sweep point only. When sweeping a parameter on the ParamSweep controller, a transient simulation will be done for the first sweep point only, unless the Regenerate Initial Guess for ParamSweep (Restart) parameter is set to yes, e.g., the check box is selected. In the case that the Restart is set to yes, a transient simulation will be done at each sweep point and thus generate a new transient initial guess for each sweep point of the harmonic balance simulation.
Divide-by-8 Example
Consider a divider with a divide ratio of 8, that may eventually follow an oscillator. It is recommended to use TAHB to simulate this circuit. One reason for using TAHB is because a divider, mathematically, has more than one solution, however, only one is physical. TAHB will provide the real solution. Another reason for using TAHB is that a phase noise analysis on the future oscillator can be determined. The simulator will determine that this is a divider, and generate a transient initial guess for harmonic balance. Set the Freq[1] to final divided frequency, and set the order large enough to get a good representation of the square-like waveforms. For divider type circuits, this can be very large - Order[1]=255 in this example. See the circuit diagram with the harmonic balance simulation setup in the following figure.
The results are shown in the next figure. The first waveform is the source input at 500 MHz. The waveforms which follow are the output after division by 2 (250 MHz), division by 4 (125 MHz), and ultimately division by 8 (62.5 MHz). The cross() function in data display was used to verify the correct frequencies of the output waveforms. The cross function computes the zero crossing going in positive slope direction, as indicated by the value of the second argument. The 1.5 V DC offset is also accounted for. To ensure accuracy of the computed mean value frequency, the first few periods are not included, as seen with the vector range notation [::] applied to the cross function.
Manual TAHB
If it is desired to perform a manual TAHB, there are two ways of doing so. The first way is to use the steady state detector in transient and allow the simulator to automatically capture the steady state portion for the initial guess. The second way is to manually adjust the transient StartTime and the StopTime to capture the steady state portion of the waveform.
Running Transient and Generating the Initial Guess
For TAHB, a transient simulation is done first. Lets take the first method and use the steady state detector. On the Freq tab of the transient controller, select Detect Steady State. It is required to give at least one frequency and order (Freq[1] and Order[1]) parameter, and set the Frequency on the Freq tab to the same Freq that will be used in the Harmonic balance simulation. The Order on the Freq tab of the Transient simulation controller can be set to be the same or larger than the Order used in the HB controller. In the box labeled Compute HB Solution, it is optional to check the box Apply Window. In the same box, check off Write initial guess for HB, and specify the name of the file. The transient simulator will report whether or not steady state was reached, and if so, the time at which it was reached and frequency of oscillation (when simulating an oscillator). The simulator will stop once steady state has been reached and transform just the last period of the solution. Thus, the transient simulation can end earlier than the StopTime, if steady state has been reached.
Next, lets consider the second approach of adjusting the transient start and stop time to capture the steady state portion of the waveform. The transient analysis needs to get as near steady state as possible. The conversion of transient (time domain) initial guess to the frequency domain is done from the start time to the stop time. Observe the transient waveform output in the data display. Set the start time appropriately so that the non-steady state portion is not transformed. For example, if the circuit is very near steady state after 50 nsec, then re-run the transient simulation with start time 50 nsec and end it with enough cycles (suppose 70 nsec is the end point). This way, the transient initial guess will only correspond to the part that is very near steady state (the waveform from 50-70 nsec) and not the part which is far from steady state (0-49 nsec). The quantity (stop time - start time) should be an integral number of commensurate periods. If the circuit topology is changed, then another transient simulation needs to be performed to generate a new initial guess file.
Set Max Time Step small enough to accommodate the largest signal frequency. For example, in a mixer circuit, the largest frequency is the LO+RF, and for a power amplifier it would be the third order frequency (2f 1 +f 2 ). A general rule of thumb is to take 16 time points per signal period, so this means (for the mixer example) Max Time Step = 1/[16*(RF+LO)]. In the case that the circuit has square wave like waveforms or rapid transitions, more points should be taken.
The initial TAHB guess does not need to contain all the HB frequencies, i.e., a multi-tone HB simulation can use a single tone TAHB initial guess. This is often a much more efficient approach because the transient simulation will have a faster run time. For example, you could do a one-tone transient simulation with just the very nonlinear LO, save that solution and then use it as the initial guess in the two-tone HB simulation. This approach works well in the above transceiver example. The exact frequencies do not have to match between the present analysis and the initial guess solution. (A single tone HB solution done with a 1 GHz fundamental can be used as an initial guess for a single tone HB solution at 1.1 GHz fundamental.) When using an initial guess file, the simulator reads the index information and not the absolute frequency. A single-tone HB simulation done at 2 GHz with an initial guess from a 1 GHz simulation, will use the 1 GHz fundamental value as the initial guess for the 2 GHz fundamental value, and not the 2 GHz second harmonic value.
The following figures illustrate the Freq and Integration tabs on the Transient simulation controller.
Reading the Initial Guess into HB
After running the transient simulation, you now have the initial guess for the HB simulation. To use the guess, select Use Initial Guess (on the Initial Guess tab) and enter the name of the file from the transient simulation. Now, run the HB simulation.
Note that if the circuit topology is changed, then another transient simulation should be run to generate a new initial guess. Be sure that the transient initial guess is a good one and that it is very near the steady state before doing the HB simulation; otherwise HB will still have trouble converging. Verify the transient initial guess by plotting the results in the data display. TAHB works well for highly nonlinear circuits and mixed signal circuits such as those with dividers, as long as there is a good initial guess.
TAHB for 1-Tone HB Simulation of an Oscillator and Divider Circuit
Consider a 1-Tone HB Simulation of an oscillator and divider circuit that does not converge. This type of circuit will have square-like waveforms with sharp edges or spikes and will require a large number of harmonics to represent the waveforms. Having a good initial guess from a transient simulation will help this type of circuit converge. It is important that the transient initial guess contains the waveforms when they are very near steady state, and not during circuit startup. Adjust the start and stop times to capture the steady state behavior of the waveform. Run the transient long enough to determine when it approaches steady state.
In this example, the frequency of the oscillator is 738 MHz and the divide ratio on the divider is 2. The transient simulation was run for 90 nsec to determine when the circuit was near steady state. Then it was re-simulated from 60 to 70 nsec since the circuit was very near steady state in that time range. In some cases it may take the circuit longer to reach steady state. It is strongly recommended to plot and verify the transient results before starting the HB simulation. See the waveform plots of the divider in the following diagram.
After generating the initial guess from transient, the single-tone HB simulation was performed. The frequency and order were the same as specified in the transient setup, namely Freq[1]=738 MHz and Order=31. Since the circuit had square wave forms, the transient solution was a very good initial guess for harmonic balance.
TAHB for 2-Tone HB Simulation of a Large Transceiver Circuit
Consider a 2-Tone HB Simulation of a large transceiver circuit that fails to converge due to a very large initial residual. The reason for this is that the DC initial guess is too far away from the actual solution. The circuit uses two tones: LO=2140 MHz and IF=260 MHz. The commensurate frequency (greatest common divisor) is 20 MHz. That is a 50 nsec period (13 cycles of the LO and 107 cycles of the IF). The number of periods required for the transient simulation will depend on how quickly the circuit approaches steady state. The best way to determine how fast the circuit approaches steady state is to plot the transient simulation waveforms. Since the transceiver in this example approaches steady state relatively quickly, 5 periods of the commensurate period is sufficient: thus the transient Stop time should be set to 5*50 nsec = 250 nsec. If the commensurate frequency is small and that circuit does not approach steady state quickly, the transient simulation to compute the TAHB initial guess would take a long time. In those cases, it is recommended to do a one-tone transient simulation using the more nonlinear tone, which is typically the LO.
The number of periods required to reach near steady state depends on the type of circuit. Divider circuits and DC coupled mixers will only need about 2 periods, while circuits with large time constants, and AC coupled mixers may require 20 periods or more.
For the transceiver example, both the IF and LO frequencies should be included on the Freq tab of the transient controller. Since the largest significant tone in this example is LO+RF = 2400 MHz (208 ps period), set the Max Timestep to (1/16) th of this period, i.e. to 13-15 ps.
When this two-tone TAHB guess is used in the HB simulation, the initial KCL residual shows 12 orders of magnitude of improvement and the circuit converges.
Changing the DC Convergence Algorithm
It is important to have a good initial guess for the Newton solver. When doing a Harmonic Balance simulation, the simulator will first do a DC simulation to generate an initial guess. In the case that the DC simulation does not converge, the simulator will halt and send an error message to the status window. If this occurs, deactivate the HB controller, and perform a DC analysis using an alternate convergence mode. The convergence modes for the DC simulation are located on the DC controller's Parameters tab; click Advanced . Some typical DC convergence problems and their remedies are described in the DC Simulation documentation. Please refer to them for further instruction. Repeat the DC simulation using one of the remedies mentioned in DC Simulation. Once convergence has been achieved, deactivate the DC controller and activate the HB controller. Insert an Options controller with the DC Convergence Mode parameters settings that produced DC convergence, and re-run the Harmonic Balance simulation.
It is possible for some circuits to have multiple solutions. Depending on the DC convergence mode, the simulator may find a solution but that solution may be non-physical. For example, it may determine node voltages which are greater than the supply voltage. In cases like these, follow the above instructions to select a different convergence mode in order to obtain the desired physical DC solution.
In the case that the DC simulation is slow, save that solution and use it as an initial guess for HB so that it does not have to be computed when doing multiple HB simulations for that circuit. If the circuit topology has changed, then DC solution will need to be recalculated by performing a DC simulation.
Device Models
Some device models may include equations, first and second derivatives with discontinuities. Model problems can cause the KCL residual to hit a threshold and remain stagnant or to exhibit random jumps (sudden increase in value). It is not recommended to use very old models, such as the Berkeley MOSFET Level 1, 2, 3. Also, it is best to use the latest version of the model, especially true for the BSIM3 model.
If the convergence problem is suspected to be due to a model, try replacing the model and resimulating. Another thing to try is to disable the devices that use the suspected model and resimulating. Yet another thing to try is to create a small circuit using the model, simulating and ensuring that the model is working properly. When using a particular device model, be sure that they give the expected DC I-V curves - ADS contains schematic design templates for this purpose. In the actual circuit, make sure that the transistors are biased properly, and that the model parameters are set to reasonable values.
SDD based device models need to be checked for equation discontinuities between regions, as well as for using unprotected functions that can blow up (such as exp, sqrt, log). It is not enough to insure continuity and limit the functions only in the operating range of the devices. This is because the Newton solver often takes a path that goes through points which are well outside the device operating range.
As an example, consider an HB simulation with input power sweep for a circuit which goes into arc-length continuation and fails at an input power of -4 dBm. The circuit contains TOM GaAs models. The reason that this circuit fails is that the TOM GaAs model parameters Gscap and Gdcap are set to 5 which corresponds to a non charge conserving model (physically inaccurate). The convergence remedy is to set Gscap and Gdcap to 6 which selects a charge conserving model. For efficiency, select the Robust convergence mode instead of Fast. The circuit converges up to a 50 dBm input.
Fourier Truncation Error
There are some circuits with square or pulse type transient waveforms. To represent these waveforms with Fourier series, many harmonics are needed. This is controlled and limited in the HB simulator by the parameter Order as discussed earlier. Circuits with square waveforms can have a difficult time converging in Harmonic Balance unless the Order is sufficiently high. In some cases Harmonic Balance may not converge, and in other cases the Harmonic Balance solution may converge, yet the solution waveforms contain Gibbs ripples. The plots below show the output waveform (charge pump current) of a phase frequency detector and charge pump simulated in transient and Harmonic Balance. To get a meaningful time domain plot, click Advanced in the Data Display Plot dialog box, and enter the expression: ts(v,,,NumOfPts), where v is the waveform name and NumOfPts is the size of the frequency-to-time conversion. When high orders are used, be sure to set NumOfPts to a sufficiently large number (a few thousand).
Transient Simulation
Harmonic Balance Simulation, Order=127
Circuits with such waveforms push the HB algorithm to its limits. In order to achieve convergence for this circuit in HB, the Oversample was set to 2, and the tolerances were very loose (V_AbsTol=10mV and I_AbsTol=100µA). The circuit converged with Order=127; but even when simulating with Order=511, the accuracy of the solution is not quite acceptable, as seen in the charge pump current plot below. The transient waveform, tran_pump, exhibits a real overshoot. While the HB waveform, hb_pump, tries to match this overshoot, due to the limited Order and large HB truncation error it exhibits significant Gibbs ripples:
Harmonic Balance Assisted Harmonic Balance
When performing a multi-tone harmonic balance simulation, the simulator will decide automatically which tones to use in generating the final HB solution. This is method is known as harmonic balance assisted harmonic balance (HBAHB). For example, instead of simulating a 3-tone circuit directly, it is possible to simulate a 1-tone, then use the result as an initial guess for a 2-tone, and finally use that result as an initial guess for the final 3-tone simulation. HBAHB is both fast and robust in particular for large multi-tone simulations of mixer circuits to determine gain and IP3.
HBAHB applies only to multi-tone simulations. By default, this feature is turned on within the simulator. The simulator will determine the optimal sequence of tones to simulate. Depending upon various conditions, the simulator may decide to first simulate using a 1-tone then use that result for a 3-tone, and skip the 2-tone simulation.
HBAHB can be found on the Initial Guess tab, in the section called Harmonic Balance Assisted Harmonic Balance. There are three choices - Off, On, and Auto. The default selection is Auto which means that the simulator automatically decides whether or not to perform HBAHB, and the optimal sequence of tones to simulate. The On selection means that HBAHB will always simulate each tone up to the last fundamental frequency. In other words, a simulation will be performed for each tone. The Off selection means that HBAHB will not be performed at all. When HBAHB is off, a standard multi-tone HB simulation will take place.
When using HBAHB, select the Auto convergence mode and the Auto solver type. Both of these parameters are found on the Solver tab of the HB controller. This ensures that simulating the intermediate tones will be both fast and robust, and not require user-intervention to tweak simulation parameters.
If a user-supplied initial guess file is provided, then HBAHB will not be performed to generate the initial guess. However, if the supplied file does not exist, then the simulator will decide whether or not to perform HBAHB. You may also save the final result to a file for later use.
When simulating an HB variant such as noise, the HBAHB will take place prior to simulating noise, and the noise analysis will not be performed when simulating the intermediate tones. When performing a swept HB simulation, HBAHB will take place only for the first, inner-most sweep point.
At any point during the HBAHB simulation, if non-convergence occurs, then the simulator will switch back to performing a standard HB simulation using a DC initial guess as the starting point. In the case that TAHB was enabled, then the transient initial guess will be restored as the starting point.
Changing the Tolerances
Sometimes a circuit may not converge because the tolerances are too tight. Adjusting the tolerances will help the Newton solver to achieve convergence. When using the Auto convergence mode, it is not necessary to change the tolerance levels. This is because the tolerances can be adjusted automatically by the HB simulator when a circuit is close to achieving convergence but cannot quite satisfy the default (or specified) tolerance levels. Alternatively, if the KCL residual for a circuit stagnates and cannot be further reduced, then the tolerance levels will be automatically adjusted for convergence. A descriptive warning message will be given in the status window when this occurs, and it will indicate the best tolerance level that was achieved for the given simulation setup. The message depends on which tolerance (relative or absolute) had more of an effect on the convergence criteria. Here is an example of the warning message when the current absolute tolerance is automatically adjusted to larger values by the HB simulator:
Warning detected by HPEESOFSIM during HB analysis `HB1'.
This is the best solution that can be achieved
for the given simulation setup.
The simulation has converged up to a current absolute
tolerance of 3.49787 pA.
The circuit was NOT able to achieve the target current
absolute tolerance of 1 pA.
Here is an example of the warning message when the current relative tolerance is automatically adjusted to larger values by the HB simulator:
Warning detected by HPEESOFSIM during HB analysis `HB1'.
This is the best solution that can be achieved
for the given simulation setup.
The simulation has converged up to a current relative
tolerance of 2.41e-06.
The circuit was NOT able to achieve the target
current relative tolerance of 1.00e-06.
When using the Fast or Robust convergence mode as the Newton solver, monitor the KCL residual in the status server window, and adjust the tolerances accordingly. With these convergence modes, the HB simulator will not adjust the tolerance levels automatically. Consider the following example of a circuit that nearly converges to with a few picoamps, but not quite to the default current absolute tolerance of 1 picoamp:
HB HB1[1] <5335.ckt> RFpower=(250e-03->4.5)
Number of frequencies: 11.
Number of time samples: 32.
Number of HB equations (problem size): 19866.
Convergence mode: Basic.
Linear solver: Krylov (GS_GMRES).
Preconditioner: DCP.
RFpower=250e-03 0.00% 1/18
------------------------------------------------------------------------
Newton solver: Linear solver:
Iter KCL residualSol update Iters Residual
------------------------------------------------------------------------
0 125 uA
1 27.3103 uA 1 4.165e-10
2 394.436 nA 2 1.431e-02
3 553.875 pA 3 1.025e-03
4 2.3978 pA 4 7.406e-05
5 2.49853 pA 4 1.354e-04
6 2.49881 pA 3 3.217e-04
7 2.49852 pA 3 4.317e-04
8 2.49853 pA 3 4.109e-04
9 2.49853 pA 3 3.398e-04
10 2.4988 pA 3 3.910e-04
11 2.49853 pA 3 3.243e-04
12 2.52273 pA 3 3.616e-04
13 2.49853 pA 3 2.825e-04
14 2.52301 pA 3 2.630e-04
15 2.49853 pA 3 3.826e-04
16 2.49853 pA 3 2.669e-04
17 2.49853 pA 3 4.079e-04
18 2.49881 pA 3 4.320e-04
19 2.52302 pA 3 2.911e-04
Switching to source-stepping...
Attempting solution at `sourceLevel' value of 0.5:
0 62.5 uA
1 6.57904 uA 1 4.545e-10
2 24.3022 nA 2 3.600e-03
3 77.6941 pA 2 3.110e-03
4 3.41004 pA 3 1.138e-04
5 3.50342 pA 3 1.096e-04
6 3.50328 pA 2 9.598e-04
As a side note, when the maximum number of Newton iterations is reached, the simulator switches to a continuation method known as source stepping. In this method, the simulator decreases the input source levels and attempts to converge. If this is successful then the source levels are gradually increased to the final level.
By increasing the current absolute tolerance to 5 picoamps, convergence is achieved in only a few iterations:
HB HB1[1] <5335.ckt> RFpower=(250e-03->4.5)
Number of frequencies: 11.
Number of time samples: 32.
Number of HB equations (problem size): 19866.
Convergence mode: Basic.
Linear solver: Krylov (GS_GMRES).
Preconditioner: DCP.
RFpower=250e-03 0.00% 1/18
------------------------------------------------------------------------
Newton solver: Linear solver:
Iter KCL residual Sol update Iters Residual
------------------------------------------------------------------------
0 125 uA
1 27.3103 uA 1 4.165e-10
2 394.436 nA 2 1.431e-02
3 553.883 pA 3 1.025e-03
4 2.39792 pA 4 7.406e-05
5 2.4988 pA 4.05239 pV 4 1.354e-04
RFpower=500e-03 5.88% 2/18
0 125 uA
1 29.5154 uA 2 1.232e-02
2 1.47481 uA 2 4.910e-02
3 3.05574 nA 4 2.831e-03
4 3.95315 pA 5 2.187e-04
5 2.00489 pA 85.8831 pV 5 3.522e-04
RFpower=750e-03 11.76% 3/18
0 125 uA
1 43.8438 uA 2 4.030e-02
2 1.08621 uA 4 2.400e-02
3 3.16865 nA 5 2.622e-03
4 4.6383 pA 6 7.839e-04
5 3.69573 pA 260.821 pV 6 6.887e-04
To adjust the tolerances, insert an Options controller on the schematic and go to the Convergence tab. Without an Options controller, the default tolerances for Harmonic Balance are set by the simulator. The following table shows the tolerances found on the Options controller, their description, and their default values.
| Name | Description | Default Value |
|---|---|---|
| I_RelTol | Relative current tolerance | 10-6 |
| V_RelTol | Relative voltage tolerance | 10-6 |
| I_AbsTol | Absolute current tolerance | 10-12A |
| V_AbsTol | Absolute voltage tolerance | 10-6V |
The controller allows for a choice of three tolerance presets: Strict, Intermediate, and Relaxed. The default tolerances shown above correspond to the strict preset. Looser tolerances will speed up the simulation run time, but may decrease the accuracy of the solution. (In a Transient simulation, the default RelTols are 10 -3 . Placing an Options controller with RelTols set to 10 -6 will slow down the simulation run time by about a factor of 10).
Some additional rules of thumb for adjusting tolerance parameters are:
- If the currents in the circuit are on the order of miliamps or amps, try increasing the relative current tolerance.
- If the currents in the circuit are on the order if microamps or smaller, try increasing the absolute current tolerance.
- If the status window output shows consecutive values in the Solution update (Sol update) column, then try increasing the voltage tolerances.
Privacy
Statement 
|
Terms of Use |
Legal |
Contact Us |
© Agilent 2000-2008
