Broadband SPICE Model
The Broadband SPICE Model is only available if you have purchased a Broadband SPICE Extractor license from Sonnet.
The Broadband SPICE Extractor uses S-parameter data to generate a SPICE model which is accurate across a broad band. In order to do this, it finds a rational polynomial which fits the S-parameter data, then uses this polynomial to generate an equivalent lumped element circuit. Since the S-parameters are fit over a wide frequency band, the model may be used in circuit simulators for AC sweeps and transient simulations.
Class of Problems
There are certain conditions for which the Broadband Spice Model may have difficulty converging to an accurate result:
- S-parameters which contain a sharp discontinuity such as those caused by box resonances
- S-parameters below about -60 dB
- S-parameters which are not passive
- S-parameters produced by sources other than Sonnet; for example, measured data or other EM simulators
Creating the Model File
You need a minimum of 50 frequency points in order to generate a Broadband Spice Model file. Therefore, we recommend you use an Adaptive (ABS) sweep unless you have a specific reason for using another type of sweep.
If your Broadband Spice Model is to be used for a transient analysis, you should analyze your project up to at least a frequency equal to 1/T, where T is the minimum time step of the transient analysis.
The processing time to create a Broadband Spice Model is proportional to the number of analysis frequencies times the square of the number of ports in your circuit. The Error Threshold also affects your analysis time.
There are two methods you may use to generate a Broadband Spice Model file:
- Automatic: You may set up your project so the EM solver will automatically generate the file after the EM simulation is complete. From the Project Editor, select Circuit > Settings > [Output Files] and then select Add File > Broadband Spice Model.
- Interactive: After simulating your project, you may generate the file from a Sonnet graph. Select a curve representing the desired project, and then select Output > Broadband Model File. Select the desired options and click the Extract button.
Model Options
You may obtain a short description for each option by hovering your mouse over the option in any dialog box. See the descriptions below for those options which require additional information.
Error Threshold
The Error Threshold is the average percentage difference between the Sonnet S-parameters and the Broadband Spice Model data. The calculation of the Broadband Spice Model stops when this error threshold is reached or when it proves impossible to improve the error. We recommend using the default value of 1.0% initially and not setting the threshold below 0.1%.
The lower the error threshold you set, the more processing time is required to calculate the model. A lower error threshold also produces a more complex model, which requires more time to process in the SPICE simulator.
Stability Factor
Although the extracted model may be a good fit to the S-parameters, a transient analysis which uses the model may be unstable. To help with this problem, Sonnet provides a control which pushes the poles away from the unstable region. However, pushing the poles too far could result in a less accurate fit, often seen as a decrease in the Q of the circuit. Therefore, you should only use this control if you are having stability problems with the model.
The Stability Factor allows you to control the amount by which the model fitting forces the poles of your model away from the unstable region. The factor represents a magnitude ratio for which the real part of a pole cannot be less than the magnitude of the pole. The higher the stability factor the greater the effect on the model. Reasonable values for the stability factor are between 1.0e-5 to 0.5. The default value is 0.001.
Predicted S-Parameters
By default, the predicted S-parameter data obtained from the model is output to a file. This allows you to visually check the accuracy of your model when it is complete. The base name of the file ends with the text "_predicted" and is located in the same folder as your Broadband Spice model file. If you do not wish to create a predicted file, click the Advanced button and unselect the Write data file checkbox.
By default, the predicted S-parameters consists of the original analysis band, plus a band from the highest frequency to three times the highest frequency. This default was chosen to allow you to verify that the model is stable above the analysis frequencies. You may override this default by selecting the Override default additional frequencies checkbox and entering the desired band. In addition, you can include a DC point by selecting the DC point checkbox.
If you are generating your Broadband Spice model from a Sonnet graph and the Write data file checkbox is selected, you may click the Plot button after the creation of the model has completed. This plots the original and predicted S-parameter which had the highest error. In addition, the loss factor for each port of the predicted S-parameters are plotted. For a passive circuit, any loss factor above 0.0 dB or any unexpected sharp resonance indicates a potential stability problem in the model.
Limit Modeling Band
By default, the full range of analysis data in the project is used to create the Broadband Spice Model. If you wish to limit the data used to create the model, click Advanced and enter the Lower limit and Upper limit you wish to use. Any frequencies outside this range will not be used by the Broadband SPICE Extractor.
Order
The Broadband SPICE Extractor uses the lowest order polynomial required to meet the error threshold specified. However, by default, it will not create a model using a rational polynomial with an order higher than 40. If you wish to change this value, click Advanced and enter a new value in the Maximum order field.