DC Sweep Analysis is used to calculate a circuits’ bias point over a range of values. This procedure allows you to simulate a circuit many times, sweeping the DC values within a predetermined range. You can control the source values by choosing the start and stop values and the increment for the DC range. The bias point of the circuit is calculated for each value of the sweep.
Multisim performs DC Sweep Analysis using the following process:
Assumptions: Capacitors are treated as open circuits, inductors as shorts. Only DC values for voltage and current sources are used.
In this section you will use two example circuits to learn how to configure DC Sweep Analysis.
In this case, the 1N4462 component has a Zener voltage (VZ) of 7.5 V and a 5% tolerance. The minimum and maximum input voltages that can be regulated by the Zener diode are 7.41 V and 26.41 V respectively. You will use DC Sweep Analysis to study the behavior of the regulator circuit when the input voltage is varied from 0 V to 40 V.
Figure 1. Zener regulator.
Table 1. Parameters used in DC Sweep Analysis.
Note: In SPICE, the command that performs an DC Sweep Analysis has the following form:
.DC <SOURCE_NAME> <START_VALUE> <STOP_VALUE> <INCREMENT>
Basically these are the same parameters that were defined in Table 1 but in Multisim you do not have to worry about the SPICE syntax.
Figure 2. Analysis parameters for the DC Sweep Analysis.
As you can see, V1 will be vary from 0 to 40 V with increments of 1 V. Note that you can add a second source to the analysis by enabling the Use source 2 option. This is useful to perform a nested sweep (see Example 2).
Figure 3. Output variable for the DC Sweep Analysis.
Figure 4. DC Sweep Analysis results.
From the Grapher View you can observe that the output voltage steadies at around 7.5 V, which is the nominal Zener voltage for the 1N4462. Use the cursors to calculate the minimum and maximum voltages that this component can regulate.
V1 and V2 (from Figure 5) need to be swept to obtain the characteristic curves. Note that in order to convert the current flow through the drain to a voltage (for display on the Grapher View), a current controlled voltage source (V3) has been added to the circuit.
Figure 5. MOSFET circuit.
Figure 6. Analysis parameters for the nested DC sweep.
Note that a second sweep variable (V2) has been added so that the analysis can perform a nested sweep. The first sweep (V1) will be done for each value of the second sweep. The number of output curves will be equal to the number of points for the second source.
In this example V2 will be set to 0 V (the Start value) and then V1 will be sweep from 0 V to 10 V; this will generate the first curve. In the next loop V2 will be set to 1 V and V1 will be sweep again from 0 V to 10 V generating the second curve. This process will continue until the Stop value for V2 is reached.
Figure 7. DC Sweep Analysis results.
In Multisim, you can also generate current-voltage curves using the IV Analyzer instrument.
Collaborate with other users in our discussion forums
A valid service agreement may be required, and support options vary by country.