AC Analysis of an RC Network

RC Network Circuit shows a simple RC network with a DC and AC source applied. The circuit consists of two resistors, R1 and R2, capacitor C1, and the source V1. Node 1 is the connection between the source positive terminal and R1. Node 2 is where R1, R2, and C1 are connected. Star-Hspice ground is always node 0.

Figure 2-1: RC Network Circuit

The Star-Hspice netlist for the RC network circuit is:




.AC DEC 10 1K 1MEG

.PRINT AC V(1) V(2) I(R2) I(C1)

V1 1 0 10 AC 1

R1 1 2 1K

R2 2 0 1K

C1 2 0 .001U


Follow the procedure below to perform an AC analysis for the RC network circuit.

1. Type the above netlist into a file named quickAC.sp.

2. Run a Star-Hspice analysis by typing

hspice quickAC.sp > quickAC.lis

When the run finishes Star-Hspice displays

>info: ***** hspice job concluded

followed by a line that shows the amount of real time, user time, and system time needed for the analysis.

The following new files are present in your run directory:





3. Use an editor to view the . lis and . st0 files to examine the simulation results
and status.

4. Run AvanWaves and open the . sp file. Select the quickAC.ac0 file from the
Results Browser window to view the waveform. Display the voltage at node 2, using a log scale on the x-axis.

RC Network Node 2 Frequency Response shows the waveform that was produced by sweeping the response of node 2 as the frequency of the input was varied from 1 kHz to 1 MHz.

Figure 2-2: RC Network Node 2 Frequency Response

The file quickAC.lis displays the input netlist, details about the elements and topology, operating point information, and the table of requested data as the input is swept from 1 kHz to 1 MHz. The files quickAC.ic and quickAC.st0 contain information about the DC operating point conditions and the Star-Hspice run status, respectively. The operating point conditions can be used for subsequent simulation runs using the .LOAD statement.

Star-Hspice Manual - Release 2001.2 - June 2001