RF Characterizer Analysis

Multisim Help

Edition Date: February 2017
Part Number: 375482B-01
View Product Info Multisim 14.0 and 14.0.1 Help Multisim 14.1 Help Multisim 14.2 Help

Multisim’s RF characterizer, found in the Network Analyzer, analysis tool helps designers study RF circuits in terms of their power gains, voltage gain, and input/output impedances. A typical application is an RF amplifier. The source signal at the input of an amplifier is usually provided by a receiver and its power is relatively small. The RF designer often intends to magnify the input signal and provide an output signal in terms of both voltage and current: that is, the output power delivered to the load is considerably higher than that of the input signal. That is why the power transferability of the designed circuit is of interest. The power gains in Multisim are calculated by assuming that source and load impedances are 50 Ohm. You can change these values by clicking the RF Param. Set button to specify that the RF simulator assumes:

Zl = Zo and Zs = Zo or Gs = Gl = 0.

Another aspect of a circuit is the input and output impedances of the amplifier. An RF amplifier usually has more than one stage of amplification. Each stage of the amplifier is loaded by the input port of the next stage.

The loading effect is best understood by studying the input/output impedances. Most engineers would like to design an amplifier which has maximum input impedance in low RF frequencies, to reduce its loading effect on the previous stage. On the other hand, the smaller the output impedance is, the better the output signal would be delivered. In higher RF frequencies, it is desirable to have an output impedance matching that of the load to minimize the reflection of signals. The Multisim RF characterizer analysis helps you to study these impedances and choose the most appropriate frequency of operation.

Complete the following steps to use the simulator in order to read the desired variable:

1. Connect the Network Analyzer to the amplifier.
2. Run the simulator. Ignore any DC warnings and wait until the AC analyses are complete.
3. Double-click on the Network Analyzer.
4. Click RF Characterizer in the Mode box.
5. Under the Trace options, set the desired variable, from among PG, APG, and TPG. While the curves are plotted versus frequency, the numerical values are displayed at the top of curves for each frequency point. Refer to the Power Gains section for more information.
6. From the Param. drop-down list, select Gains. The voltage gain (VG) is plotted versus frequency and its value is given at the top of the curve.
7. Tip Use Auto Scale each time you change the parameters to get a better reading.

8. From the Param. drop-down list, select Impedance. The input/output impedances are provided in the form of a curve as well as printed out at the top of the curves.
9. Use the frequency scroll bar at the bottom of the curves to select the desired frequency for a specific variable.
Power Gains

The Multisim RF Simulator calculates the General Power Gain (PG), Available Power Gain (APG) and Transducer Power Gain (TPG) for Zo = 50 ohms at a given frequency. The dBMag is derived as 10log10 |PG|.

PG is defined as the ratio of the power delivered to the load and the average power delivered to the network from the input, and is given as PG = |S21|2/(1-|S11| 2).

TPG is the ratio of the power delivered to the load to the power available from the source.

For Gs = GL= 0, TPG = |S21| 2 .

APG is the ratio of the power available from the output port of the network to the power available from the source and it is expressed as

APG = |S21|2 / (1- |S22| 2 )

Voltage Gain

Voltage Gain, VG, is obtained for Gs = Gl = 0 and is expressed as VG = S21/(1 + S11).

Voltage Gain expressed in dBMag is calculated as 20log 10 |VG|.

If you observe the time domain signals of the input and output while the transistors are operating in the linear region, you find that the amplitude of the output voltage signal (when 50 Ohm load and source impedances are used) to the amplitude of the input voltage signal is the same as VG given by Multisim. Note, however, that VG is calculated using S-parameters.

Input/Output Impedances

These values are calculated assuming Gs = Gl = 0. For this condition, we have:

Zin= ( 1 + Gin) / (1 - Gin) where Gin = S11 and

Zout= ( 1 + Gout) / (1 - Gout) where Gout = S22.

One must note that these values are normalized. The simulator prints denormalized values of Zin and Zout.