Transient and Convolution Simulation Description

The transient and convolution simulators are SPICE-like in their operation. They solve a set of integro-differential equations that express the time dependence of the currents and voltages of the circuit under analysis. The result is a nonlinear analysis with respect to time and, possibly, a swept variable.

The main difference between the transient and convolution options lies in how each analysis characterizes the distributed and frequency-dependent elements of a circuit, as discussed below.

Transient Analysis

A transient analysis is performed entirely in the time-domain, and so is unable to account for the frequency-dependent behavior of distributed elements such as microstrip elements, S-parameter elements, and so on. Therefore, in a transient analysis, such elements must be represented by simplified, frequency-independent models such as lumped equivalents, transmission lines with constant loss and no dispersion, short circuits, open circuits, and the like. These assumptions and simplifications are usually very reasonable at low frequencies.

Convolution Analysis

A convolution analysis represents all the distributed elements in the frequency domain and hence accounts for their frequency-dependent behavior. The characterization of many RF and microwave distributed elements is best accomplished in the frequency domain, because the exact time-domain equivalents for these elements cannot always be obtained.

Convolution converts the frequency-domain information from all the distributed elements to the time domain, effectively resulting in the impulse response of those elements. The time-domain input signals at an element's terminals are convolved with the impulse-response of the element to yield the output signals. Elements that have exact lumped equivalent models-including nonlinear elements-are characterized entirely in the time domain without using impulse responses.

Note
In a convolution analysis, all elements are characterized by means of the full frequency-domain model, through the use of either an exact time-domain model or convolution. However, there may be minor differences between the results of a convolution simulation and the results of a transient simulation of the same circuit.

A convolution analysis requires both a convolution license and a transient license, and is performed whenever a convolution license is available. If the simplified approximate models are preferred, in this situation (for speed), set the Use Approximate Models When Available option to yes.

Transient/Convolution Simulation Process

The following steps describe how both the transient and convolution simulators operate:

The user specifies a time-sweep range, tolerances, and iteration limits.
A DC analysis is conducted to determine the system solution at zero time.
Inside the simulator, a breakpoint table is constructed to deal with frequency-domain-devices and data. Independent source waveforms frequently have sharp transitions that may not normally coincide with the time step calculated by the program. Such is the case with the piecewise linear sources. The breakpoint table contains a sorted list of all the transition points of the independent sources. During the simulation, whenever the next time point is sufficiently close to one of the breakpoints, the time step is adjusted to land exactly on the breakpoint. This prevents unnecessary time-step reductions in the vicinity of the transitions.
An internal control variable updates the current time, and the values of the independent sources are calculated at that time.
An attempt is made to solve the system of equations through numerical integration and a finite number of Newton-Raphson iterations. If the number of iterations exceeds Max iterations per time point, then the time step is reduced by a factor of Integration coefficient mu divided by 8. If this new time step is acceptable, the analysis is repeated from step 4. If Integration coefficient mu = 0, backward-Euler numerical integration is used. Otherwise, trapezoidal numerical integration is used.
Following convergence, the local truncation error is calculated. The default Trapezoidal integration method is used to estimate the error, unless Gear's method is selected.
The time step interval is calculated. By default, the time step is computed for transient analysis by means of the truncation error estimate method.
The error tolerance is compared with the value in the Local truncation error over-est factor field (under the Integration tab). If the error is within acceptable limits, the results are stored and analysis continues at the next time point. Otherwise, the analysis is repeated at a smaller time step.
Steps 3 through 9 are repeated until the user-specified time-sweep range has been analyzed.

Time Step Control Characteristics

These are the specific characteristics for time step control.
Local Truncation Error:

Estimates the LTE made on every capacitor and inductor.
Determines the time step size to ensure the largest LTE remains within the accepted tolerance.
The estimated LTE is inversely proportional to TruncTol.
The accepted tolerance is proportional to I_RelTol x TruncTol and V_RelTol x TruncTol.

Iteration-Count:

Determines the time step size based on the number of Newton iterations required for previous time point.
No direct relationship between iterations and LTE.
Effectively controlled by Max time step (for linear circuits).

Fixed:

The time step is fixed and equal to Max time step.

Break Points:

Generated by built-in independent sources whenever an abrupt change in slope occurs.
Ensure that corners in waveforms are not missed.
ADS always places time points on a break point (except fixed time step).
Backward Euler is used on time points that are the first time step after break points.
The step size is reduced when time point is close to a break point.

Integration Methods Used in Transient-Convolution Simulation

Like SPICE, this simulator uses the trapezoidal integration method described by the following equation as the default method for calculating derivatives at each time step t in the simulation.

For most circuits, this method will succeed. For those that do not, the simulator also supports Gear's backward difference method:

In this equation, the index k is called the order of the integration.

For most circuits, Gear's method is no more accurate than the default trapezoidal integration technique. However, if a circuit analysis fails to converge, Gear's method may succeed where trapezoidal integration fails. In particular, oscillator circuits and any circuit that is characterized by stiff state equations may benefit from Gear's method.

Note
For a discussion of Gear's method and stiff state equations, refer to Chua and Lin, Computer-Aided Analysis of Electronic Circuits: Algorithms and Computation Techniques, Prentice-Hall, 1975.

If Time Step Control is set to TruncError and Max Gear order (under the Integration tab) is set to a number between two and six, the simulator will use Gear's method along with an adaptive stepsize algorithm that picks the largest possible step size at each point in the simulation. For each time step, the order of Gear's method will be chosen (up to the value of Max Gear order ) to maintain accuracy with the largest possible time step. This potentially speeds up simulations with no loss in accuracy. If Gear Integration is selected with fixed timestep, then the integration will always be done at the fixed order given by Max Gear order.

The integration order at each time step is output to the dataset as the variable tranorder. This data is used by the fs() function, in data display, to do accurate interpolation of the data when an FFT is required. For the default trapezoidal integration, this will normally have a value of two, except at source-induced breakpoints where it will be one.

Using the Steady State Detector and Transient Assisted Harmonic Balance

You can perform a transient simulation with the steady state detector to find out the steady state conditions of a circuit. This includes whether or not steady state was reached, the time at which steady state was reached, and the frequency of oscillation in the event of having an oscillator circuit. To get this information, enable the Detect Steady State parameter and enter the frequency of the source that is driving the circuit for Freq[1] (or the potential oscillation frequency for an autonomous circuit). The resulting steady state values will appear in the ADS status window.

The Transient simulator may also be used to generate an initial guess for a harmonic balance simulation. 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.

Transient assisted harmonic balance is automated and can be set to Auto, On, or Off mode from the TAHB tab on the Harmonic Balance simulation controller. However, if you prefer to perform a manual TAHB simulation, there are two ways to do it.

On the Freq tab, fill in the frequency fields as you would for a harmonic balance simulation. The Frequency values can still be used, independent of this solution mode, to define the fundamental frequencies and _freqN variables used in sources. The Order and Maximum order information is used to determine the number of frequencies for which to compute a harmonic balance solution.

The first way is to enable the steady state detector and allow the transient simulator to capture the steady state portion of the solution waveforms. When taking this approach, be sure to give at least one the frequency and order parameter (Freq[1], Order[1]), and select the box labeled Write initial guess for HB. 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.

The second way is to manually adjust the StartTime and StopTime to capture the steady state portion of the solution. As with the first method, at least one frequency and order parameter (Freq[1], Order[1]) must be given and Write initial guess for HB should be selected. The time to frequency domain transform does not start until after StartTime has been reached, so set StartTime appropriately so that the non-steady state portion is not transformed. StopTime should be set so at least one full period of the steady state solution occurs after StartTime. Set MaxTimeStep small enough to accommodate the largest signal frequency. With this approach, it is recommended to plot the transient results in the data display and verify that the waveforms are very near steady state. For best results, especially in multi-tone applications, enable Apply Window. This applies a window to the time domain data. This window helps to minimize the spectral leakage when multiple frequency tones are present.

In both cases, the name for the initial guess file should also be entered for the File parameter.

For circuits with multiple sources, it is strongly recommended to do a single tone transient simulation when generating the initial guess for harmonic balance. In other words, use only Freq[1] and Order[1] when setting up the fundamental frequency for a Transient simulation. This should be the most nonlinear tone. This is typically the tone with the largest power that would drive the circuit into compression.