DC Sweep Analysis

Old Content - visit altium.com/documentation

Modified by Phil Loughhead on Mar 4, 2014

Description

The DC Sweep analysis generates output like that of a curve tracer. It performs a series of Operating Point analyses, modifying the voltage of a selected source in pre-defined steps, to give a DC transfer curve. You can also specify an optional secondary source.

Setup

DC Sweep analysis is set up on the DC Sweep Analysis Setup page of the Analyses Setup dialog (after the dialog appears, click the DC Sweep Analysis entry in the Analyses/Options list). An example setup for this analysis type is shown in the image below:

Parameters

Primary Source - the name of the independent power source in the circuit that is to be stepped.
Primary Start - the starting value for the primary power source.
Primary Stop - the final value for the primary power source.
Primary Step - specifies the incremental value to use over the defined sweep range.
Enable Secondary - allows you to sweep the primary power source over its full range of values, for each value of a specified secondary source.
Secondary Name - the name of a second independent power source in the circuit.
Secondary Start - the starting value for the secondary power source.
Secondary Stop - the final value for the secondary power source.
Secondary Step - specifies the incremental value to use over the defined sweep range.

Notes

The primary source is required and the secondary source is optional.

The Primary Source and Secondary Name parameters are chosen from drop-down lists containing all power and excitation sources in the circuit.

Data is saved for all signals in the Available Signals list, on the General Setup page of the Analyses Setup dialog.

The simulation results are displayed on the DC Sweep tab of the Waveform Analysis window.

Examples

Consider the circuit in the image above, where a DC Sweep analysis is defined with the following parameter values:

Primary Source = Vin
Primary Start = -700.0m
Primary Stop = -1.500
Primary Step = -20.00m
Secondary Name = V1
Secondary Start = 10.00
Secondary Stop = 15.00
Secondary Step = 1.000

The entry in the SPICE netlist will be:

*Selected Circuit Analyses: .DC VIN -0.7 -1.5 -0.02 V1 10 15 1

Running the simulation will yield the output waveform shown in the image below: