Using Circuit Envelope Simulation

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

License Requirements

The Circuit Envelope simulation uses the Circuit Envelope Simulator license (sim_envelope). You must have this license to run Circuit Envelope 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.

For RFDE, you must have the Circuit Envelope simulator license (included with the RFIC Pro and Premier suites, the RF Board Premier suite, or the Microwave Circuits Premier suite) to use the simulator.

When to Use Circuit Envelope Simulation

Circuit Envelope is highly efficient in analyzing circuits with digitally modulated signals, because the transient simulation takes place only around the carrier and its harmonics. In addition, its calculations are not made where the spectrum is empty.

• It is faster than Harmonic Balance, assuming most of the frequency spectrum is empty.
• It compromises neither in signal complexity, unlike Harmonic Balance or Shooting Method, nor in component accuracy, unlike Spice, Shooting Method, or DSP.
• It adds physical analog/RF performance to DSP/system simulation with real-time co-simulation with ADS Ptolemy.
• It is integrated in same design environment as RF, Spice, DSP, electromagnetic, instrument links, and physical design tools.

Circuit Envelope provides these advantages over Harmonic Balance:

• In Harmonic Balance, if you add nodes or more spectral frequencies, the RAM and CPU requirements increase geometrically. The Krylov solver improves this, but it is still a limitation of Harmonic Balance because the signals are inherently periodic.
• Conversely the penalty for more spectral density in Circuit Envelope is linear: just add more time points by increasing tstop. The longer you simulate, the finer your resolution bandwidth.
• Doing a large number of simple one-tone HB simulations is effectively faster and less RAM intensive than one huge HB simulation.
• With a circuit envelope simulation the amplitude and phase at each spectral frequency can vary with time, so the signal representing the harmonic is no longer limited to a constant, as it is with harmonic balance.

How to Use Circuit Envelope Simulation

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

For a successful analysis, be sure to:

• Use either time domain or frequency domain sources in your circuit. In a circuit employing a mixer, provide a source for the LO.
• Add the Circuit Envelope controller to the schematic. (From the Component palette, choose Simulation-Envelope. Add the ENV component to the schematic.) Double-click to edit it. Fill in the fields under the Env Setup tab:
  • A Circuit Envelope simulation runs in the both the time and frequency domain. Set the stop time and time step (start time is 0). Time step defines the maximum allowed bandwidth (± 0.5/Time step) of the modulation envelope. The analysis bandwidth (1/Time step) should be at least twice as large as the modulation bandwidth to ensure accurate results at the maximum modulation frequencies.
  • Enter fundamental frequencies and order.
• If your design includes an OscPort component, select the Env Oscillator tab and fill in the Oscillator options.
• You can use previous simulation solutions to speed the simulation process. For more information, see Reusing Simulation Solutions.

  Note Unless there are convergence problems, Agilent EEsof recommends that you leave the other parameters under the Env Params and HB Params set to their default values.

• After the simulation is complete, results appear in the data display window. Envelope data variables are identified by the prefix ENV.

What Happens During Envelope Simulation

The Envelope simulator combines features of time- and frequency-domain representation, offering a fast and complete analysis of complex signals such as digitally modulated RF signals. This simulator permits input waveforms to be represented in the frequency domain as RF carriers, with modulation "envelopes" that are represented in the time domain (Modulated signal in the time domain).

Modulated signal in the time domain

For details about the Envelope simulation process, see Theory of Operation for Circuit Envelope Simulation.