|Multisim 14.0 and 14.0.1 Help|
|Multisim 14.1 Help|
|Multisim 14.2 Help|
Multisims 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:
Tip Use Auto Scale each time you change the parameters to get a better reading.
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, 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.
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.