Comparing Results

This section provides information on how to compare your translated design output results with your original netlist. Once you have translated, verified and simulated your netlist, compare your ADS results with your original version.

Comparing the Schematic

For wired or unwired import options, compare your translated ADS Schematic with your original netlist. For a small design, you can visually verify connections by matching node numbers. For information on nodes flagged with red diamonds, refer to Checking for Unconnected Nodes.

To compare a larger schematic with the original netlist, first generate an ADS netlist. To generate an ADS netlist from a schematic without starting a simulation:

1. Open the ADS command line from the Main window.
   Choose Options > Command Line.
2. Enter the following command in the Command field:

   de_netlist();

   After applying this command, the netlist is stored in a file called netlist.log in the current project directory.

3. Proceed to the next section for instructions on how to compare the translated ADS netlist to the original netlist.

Comparing the Netlist

You can compare your translated ADS netlist to your original netlist to verify that nodes were connected correctly and parameters were translated correctly. If you performed your translation from the command line and selected the -g option to create an ADS netlist, you can easily view and compare your translated netlist with your original netlist.

Since Spectre, SPICE, and ADS netlists are ASCII based text files, they can be viewed using any ASCII text editor. To view the original netlist, open a text editor and load the file defined as input_filename in the nettrans command. To view the translated ADS netlist, open a text editor and load the file netlist.log or the file defined as output_filename in the nettrans command.

You can now compare your original netlist to the translated ADS netlist noting the differences between Spectre and ADS.

Comparing Original and ADS Netlists

You can now compare your original netlist to the translated ADS netlist noting the differences between the original and ADS. SPICE Netlist vs. Translated ADS Netlist shows an example comparison of a simple SPICE netlist translation. The comparison is the same for Spectre.

SPICE Netlist vs. Translated ADS Netlist

Note The numbers in the left hand column of SPICE Netlist vs. Translated ADS Netlist coincide with the numbers in the descriptions below. Each number references a line or group of lines in the adjacent netlist.

Here are some details you might notice in the translated netlist in SPICE Netlist vs. Translated ADS Netlist:

1. There is a semi-colon preceding the first line in the translated netlist. The translator inserted the comment character even though there was no comment character in the SPICE file. This is because the SPICE simulator always considers the first line of a SPICE file to be a comment. To override this behavior in the translator, deactivate the First line is a comment check box in the Import dialog or use the -l command line option.
2. The .param keyword in the SPICE netlist indicates the beginning of a parameter list. Each of the parameters defined are written separately in the ADS netlist.
3. Components are indicated by a component designator (i.e. V_Source) followed by a colon and then a unique item name (i.e. v1).
4. If a component references a model (bjtm1), the unique model name will be listed first, instead of a component designator (V_Source).
5. The .model keyword in SPICE indicates the beginning of a model. The translator converts the SPICE model to an equivalent ADS model.
6. The .end (end of circuit) command has no equivalent in the ADS netlist file. The translator stops reading after encountering the .end command.

Now that you have compared your translated netlist to the original SPICE netlist and made some observations, you can view the translation log (nettrans.log) to help understand some other reasons the translated netlist appears as it does. For information on reviewing the nettrans.log file, refer to Viewing the Translation Log

Comparing Models and Devices

Compare each of your translated models and devices with those in your original netlist.
Model parameters are not always defined consistently for every simulator. There are differences between ADS, Spectre and SPICE. Additionally, each simulator may use different equations in their model calculations. These inconsistencies may lead to differences in simulation results for translated models.

If you have verified that the model parameters have translated as you expected by using the information in Translating a Device and Translating a Model, and your simulation results are not what you expect, please contact Agilent EEsof-EDA Customer Support for the latest information on model compatibilities. You may be asked to submit your archived project to help resolve the issue.

For information on troubleshooting your translation, refer to Troubleshooting.

Comparing ADS Results to Hspice

Hspice uses different values for the physical constants k and q. This can subtly affect some of the temperature scaling code. It can make small differences in kT/q, which is part of the equation for a forward biased diode.

Care must be exercised when comparing the currents flowing through reverse-biased PN junctions. A diode with Is=1x10^-14 should have a current of -1x 10^-14 at -5V; instead it will show -5 x10^-12. This is because ADS/Hspice adds a small conductance of size gmin (nominally 1x 10^-12 S) in parallel with every reverse biased PN junction to aid convergence. Thus if these currents are compared, all that is being compared is gmin and not the reverse-biased diode results.