In Transient Analysis, also called time-domain transient analysis, Multisim computes the circuit’s response as a function of time. This analysis divides the time into segments and calculates the voltage and current levels for each given interval. Finally, the results, voltage versus time, are presented in the Grapher View.
Multisim performs Transient Analysis using the following process:
Assumptions: DC sources have constant values; AC sources have time-dependent values. Capacitors and inductors are represented by energy storage models. Numerical integration is used to calculate the quantity of energy transfer over an interval of time.
Consider the series RLC circuit shown in Figure 1. According to the theory, the characteristic equation modeling this circuit can be represented as:
Where α is the damping factor and w0 the natural frequency (or resonant frequency). They are defined by:
The value of the damping factor (α) in relation to the natural frequency (ω0) determines the behavior of the circuit’s response. There are three possible responses:
Note that as the value of α increases, the RLC circuit is driven towards an overdamped response. In this example you will use Transient Analysis to plot the step responses of the RLC circuit. Since α depends on the value of the resistance, you will use three different values for R: 40 W, 200 W and 1 kW. 3
Figure 1. Series RLC circuit.
Complete the following steps to configure and run a Transient Analysis:
The default settings are appropriate for normal use, providing the transient response of the selected output variables starting at time 0 seconds and stopping after 1 ms. Table 1 describes the Analysis Parameters tab in detail.
Table 1. Parameters used in Transient Analysis.
There are four options:
Start time (TSTART)
End time (TSTOP)
Maximum time step settings (TMAX)
Enable to manually set time steps. There are three options:
Set initial time step (TSTEP)
Estimate maximum time step based on netlist (TMAX)
Note: In SPICE, the command that performs a Transient Analysis has the following form:
.TRAN <TSTEP> <TSTOP> < TSTART <TMAX> > <UIC>
Where .TRAN initializes a Transient Analysis; <TSTEP> is the time increment for reporting results; <TSTOP> is the final analysis time; <TSTART> is the start time for reporting results; <TMAX> is the maximum step size used in incrementing the time during the analysis; <UIC> is used for initial conditions. Note that these are the same parameters that were defined in Table 1, however, in Multisim you do not have to worry about the complex SPICE syntax.
Figure 2. Analysis parameters for the Transient Analysis.
Figure 3. Output variables for the Transient Analysis.
Figure 4. Transient Analysis results.
As you can see, this is the typical underdamped response of a series RLC circuit.
Note: If you connect the Oscilloscope to the circuit and run the simulation, a similar analysis is performed.
In order to compare the three results, merge the plots in one. You can use Overlay Traces from the Graph menu. Figure 5 shows a comparison graph of the results.
Figure 5. Step responses of the RLC circuit.
In this example you executed the simulation three times in order to get the step responses of the RLC circuit, however, you can also use Parameter Sweep Analysis to verify the behavior of a circuit when a parameter is varied across a range of values.
Collaborate with other users in our discussion forums
A valid service agreement may be required, and support options vary by country.