[ENGN2211 Home]

DC Sweep

PSPICE has a feature which allows you to automatically change a part value within a specified range and to simulate and graph the results. This is called DC sweep. For instance, resistor values, currents, or voltages can be swept.

As an example of this, suppose we want to experimentally determine the Thevenin equivalent of the circuit of Figure 9 to the left of the terminals a-b. This can be done by injecting a current and recording the voltage for each current value. PSPICE can do this automatically by using its DC sweep feature applied to the current source I2 of Figure 11.

  

Figure 11: PSPICE Thevenin experiment with current source set up for DC sweep.

Load the PSPICE file dcth1.sch corresponding to Figure 11. The DC sweep should be set up to vary I2 over the range -2-10 A with increments of 0.1 A (if not, see below). Simulate the circuit and obtain the graph shown in Figure 12.

  

Figure 12: Graph for PSPICE Thevenin experiment with current source set up for DC sweep.

Using Probe. The graph is displayed in the PROBE window. PROBE has its own menus for a wide range uses in examining the output from a PSPICE simulation. In the example, the current source I2 ranges over the horizontal axis, and the voltage V_ab (i.e. V(a)) is on the vertical axis. Figure 12 shows the use of the cursor, which is activated by:

Tools $\to$ Cursor $\to$ Display

There are two cursors controlled by the left and right mouse buttons, respectively. The small Probe Cursor window shows the measurements for the current cursor positions, including the difference.

Exercise. From your PSPICE graph, determine:

1.

The open circuit voltage $V_{ab; \ oc}$.

2.

The short circuit current $I_{ab; \ sc}$.

3.

The Thevenin equivalent circuit.

4.

Create a new schematic and enter your Thevenin equivalent. Apply a current source and use DC sweep to obtain the V-I graph for the Thevenin circuit and compare with the original.

Setting up DC sweep. In order to carry out the simulation you want, you have to tell PSPICE your requirements. The DC operating point analysis is done by default. For DC sweep, you need to set up as follows.

Analysis $\to$ SetUp...

The Analysis Setup dialog box, Figure 13 will appear.

  

Figure 13: Analysis Setup dialog box.

The Bias Point Detail should always be enabled. Enable DC Sweep and click on the DC Sweep button. The DC Sweep dialog box will appear, Figure 14.

  

Figure 14: DC Sweep dialog box.

In this case the sweep variable is a current source, and the sweep type is linear. The name we used in this schematic is I2, and the sweep range and increment is specified.

[ENGN2211 Home]