2 Simulating Low Noise Amplifiers

The SpectreRF simulator can simulate very linear circuits, such as Low Noise Amplifiers (LNA). This section uses the lna Simple circuit to illustrate how the SpectreRF simulator can determine the characteristics of an LNA design.

The first stage of a receiver is typically an LNA, whose main function is to set the boundary as well as to provide enough gain to overcome the noise of subsequent stages (for example, in the mixer and IF Amplifier). Apart from providing enough gain in addition to introducing as little noise as possible, an LNA should accommodate large signals without distortions, offer a large dynamic range, and provide good matching to its input and output. Good matching is extremely important if a passive band-select and image-reject filter precedes and succeeds the LNA because the transfer characteristics of many filters are sensitive to the quality of the termination.

In the LNA example that follows, you will plot the following characteristics of the low noise amplifier.

LNA Measurements (lnaSimple	Analyses
S-Parameter Analysis, Small Signal Gain	sp
Stability, Stability Circles	sp
Linear two-port Noise Frequency Measurements, Noise Circles	sp+noise
Third-Order Intercept Measurement	hb
Rapid IP3 Using Specialized AC Analysis	ac

To use this section, you must be familiar with the SpectreRF simulator analyses as well as know about LNA designs. For more information about the SpectreRF simulator analyses, refer to the various chapters in this user guide and also the SpectreRF Simulation Option Theory.

The lnaSimple Low Noise Amplifier Circuit

The lnaSimple circuit can be found in the ExampleLibRF library. Refer to the Introduction chapter for the instructions on accessing the ExampleLibRF library. The schematic for the lnaSimple circuit is shown below. It is a differential low noise amplifier.

Figure 2-1 Schematic for the lnaSimple Low Noise Amplifier

The following tables list some measured values for different aspects of the lnaSimple low noise amplifier.

Measurement	Measured
RF frequencies (Hz)	900M
Output frequency (Hz)	900M
RF voltage	200mV peak
RF power	-10 dBm
Gain	measurement needed
Stability Factor	measurement needed
Noise figure	measurement needed
1dB compression point	measurement needed
Input IP3 (from swept power)	measurement needed
Input IP3 (from AC analysis)	measurement needed

Design Variable	Default Value
prf (RF power)	-10 dBm
frf1 (RF frequency)	900M

Setting Up to Simulate the lnaSimple Low Noise Amplifier

Opening the lnaSimple Circuit in the Schematic Window

In CIW, choose File – Open.
The Open File form is displayed.
Choose ExampleLibRF from the Library drop-down list.
Choose lnaSimple from the Cells list box.
Choose schematic from the View drop-down list.
The completed Open File form will look like the one below.
Figure 2-2 Open File Form
Click OK.
The Schematic window for the lnaSimple circuit is displayed.
Figure 2-3 lnaSimple Schematic
In the Schematic window, choose Launch– ADE Explorer.
In the Launch ADE Explorer dialog, select Create New View.
The Create new ADE Explorer view form is displayed.
Figure 2-4 Create new ADE Explorer view
Leave each option to the default selections and click OK.
The Virtuoso ADE Explorer window is displayed, as shown below.
Figure 2-5 ADE Explorer Window

Choosing Simulator Options

Choose Setup – Simulator in the ADE Explorer
The Choosing Simulator form is displayed.
Figure 2-6 Choosing Simulator Form
Choose spectre from the Simulator drop-down list.
Click OK.
Now, set up the High-Performance Simulation Options, as follows:
In ADE Explorer, select Setup-High Performance Simulation. The High Performance Simulation Options window is displayed.
Figure 2-7 High Performance Simulation Options

In the High Performance Simulation Options window, select APS for Simulation Performance Mode. Note that Auto is selected for Multithreading options. The effect of this is to detect the number of cores on the system (up to 64) and then multi-thread on all the available cores.
The bigger the circuit, the more threads you should use. For a small circuit such as this, you may want to set the number of threads to 2. Using 16 threads on a small circuit might actually slow things down because of the overhead associated with multithreading. For more information, refer to the Spectre Classic Simulator, Spectre APS, Spectre X, and Spectre XPS.
Click OK.
In ADE Explorer, select Outputs – Save All.
The Save Options form is displayed.
Figure 2-8 Save Options Form
In the Select signals to output(save) section, ensure that allpub is selected.
This is the default selection. This saves all of the node voltages at all levels of the hierarchy, but it does not include the node voltages inside the device models.
To save the currents, select nonlinear in the Select device currents (currents) section if you just want to save the device currents, or select all if you want to save all the currents in the circuit.
Click OK to close the Save Options form.

Setting Up Model Libraries

In ADE Explorer, choose Setup - Simulation Files. The Simulation Files Setup form is displayed.
Figure 2-9 Simulation Files Setup Form
Verify that the Include Path is set, as shown above, and click OK to close the form.
In ADE Explorer, choose Setup – Model Libraries.
The Model Library Setup form is displayed.
Type in the name of the model file, as follows:
```
models/modelsRF.scs
```
Click Add.
The Model Library Setup form will look like the following:
Figure 2-10 Model Library Setup
Click OK.

SP Analysis and Small Signal Gain

The S-Parameter (sp) analysis is the most useful linear small signal analysis for low noise amplifiers. In this section, you will set up an sp analysis by specifying the input and output ports and the range of sweep frequencies.

The S-parameter analysis linearizes the circuit about the DC operating point and computes the S-parameters of the circuit taken as an N-port. In the netlist, the port statements define the ports of the circuit. Each active port is turned on sequentially, and a linear small-signal analysis is performed. Spectre converts the response of the circuit at each active port into S-parameters and outputs these parameters. There must be at least one active port statement in the circuit.

Three power gain definitions appear in the literature and are commonly used in LNA design.

The following gain quantities are valid only for two-port circuits:

GA (available gain) is the power gain obtained by optimally matching the output of the network.
GP (power gain) is the power gain obtained by optimally matching the input of the network.
GT (transducer gain) shows the insertion effect of a two-port circuit. This quantity is used in amplifier design.

Besides these three gain definitions, there are three additional gain definitions you can use to evaluate the LNA design.

Gumx (maximum unilateral transducer power gain)
Gmax (maximum available gain) shows the transducer power gain when a simultaneous conjugate match exists at both ports.
Gmsg (maximum stable gain) shows the gain that can be achieved by resistively loading the two-port such that k = 1 and then simultaneously conjugately matching the input and output ports. For conditionally stable two-ports, you can approach the maximum stable gain as you reduce the input and output mismatch. If you attempt a simultaneous conjugate match and k < 1, the two-port oscillates.

There are also two gain circles that are helpful to the design of input and output matching networks.

GPC: power gain circle
GAC: available gain circle

The next steps will walk you through these simulations and measurements.

Editing the Schematic

In the Schematic window, click the RF voltage source. This is the input port to lnaSimple.
Figure 2-11 RF Voltage Source in lnaSimple

Note that when you select the port, the Property Editor populates with the instance properties on the port. Note that the RF port has a Port Number of 1 and input Resistance of 50 Ohms. Leave the Source type parameter set to sine and disable the frequency source in the Design Variables section of ADE Explorer
Next, click the port on the right side of the schematic. This is the output port of lnaSimple. The Property Editor shows the instance properties on the output port.
Figure 2-12 lnaSimple Output Port

Note that the output Port Number is 2 and the reference Resistance (real part of the reference impedance) is 50 Ohms. The Source type is set to dc, as there is no large signal generated on this port.

Setting Design Variables

Perform the following steps to set the design variables to the values required for each simulation. The Design Variables section is located in the Setup pane of the ADE Explorer simulation window:

Figure 2-13 Design Variables Section of ADE Explorer Window

Change the design variables frf1 and frf2 to 0. To edit the value, simply click the value to the right of the variable name, and type in a value. Then press Enter. Setting the input frequency to 0 disables the production of waveforms for the large-signal analyses like tran, pss, and hb (harmonic balance.)
Figure 2-14 Edited Design Variables Section of ADE Explorer Window

The small-signal analysis begins by linearizing the circuit about an operating point. By default, this analysis computes the operating point, if it is not known, or recomputes it if any significant component or circuit parameter has changed.
In the ADE Explorer window, select Analysis - Choose or click the Choosing Analyses icon ( )on the right side of the ADE Explorer window.
The Choosing Analyses form is displayed.
Figure 2-15 Choosing Analyses Form
In the Analysis section, select the sp radio button. The form expands.
Figure 2-16 sp Choosing Analyses Form
In the Ports section, click Select. Next, click the input (RF) port, followed by the output port (PORT0). When finished with the two selections, press the Esc key. The form and schematic will look like the following:
Figure 2-17 Choosing Analyses Form with Ports Selected

If the list of active ports is specified with in the Ports field, the ports are numbered sequentially from one in the order given. Otherwise, all ports present in the circuit are active, and the port numbers used are those that were assigned on the port statements in the netlist (or in the Edit Properties form).
Spectre can perform AC/SP analysis while sweeping a parameter. The parameter can be frequency, temperature, component instance parameter, component model parameter, or netlist parameter. If changing a parameter affects the DC operating point, the operating point is recomputed at each step. After the analysis is complete, the modified parameter returns to its original value.
You can define sweep limits by specifying the end points or the center value and span of the sweep. Steps can be linear or logarithmic, and you can specify the number of steps or the size of each step. If you do not specify a step size parameter, the sweep is linear when the ratio of stop to start values is less than 10 and logarithmic when this ratio is 10 or greater. All frequencies are in Hertz.
You will be sweeping frequency in this simulation. In the Sweep Variable section of the Choosing Analyses form, select Frequency (this is the default value).
In the Sweep Range section, select Start-Stop. Enter 500M in the Start field and 4.0G in the Stop field.
Set Sweep Type to Linear. Select Number of Steps and set that to 50.
In the Do Noise field, select yes. This sets up the small signal (linear 2 port) noise analysis. The small signal assumption is valid when the input power level is low (at least 10dB below the 1dB compression point) and the circuit is operating in the linear range.
When donoise=yes is specified, the noise correlation matrix is computed. If in addition, the output is specified using Output probe (oprobe), the amount that each noise source contributes to the output is computed. Finally, if an input is also specified (iprobe), the two-port noise parameters are computed (F, Fmin, NF, NFmin, Gopt, Bopt, and Rn). When an input port is specified, the two-port noise parameters are computed (F, Fmin, NF, NFmin, Gopt, Bopt, and Rn).
Click Select to the right of Output port and click the output port (PORT0) in the schematic.
Click Select to the right of Input port and click the input port in the schematic (RF). Alternately, you can type /PORT0 in the Output port field and /RF in the Input port field.
In the Mode section, select Single-Ended. If you are simulating mixed-mode parameters, select the Mixed In/Out option. For more information, see the Spectre Circuit Simulator and Accelerated Parallel Simulator User Guide or type spectre -h sp at the command prompt.
Click OK at the bottom of the form. The Choosing Analyses form will look like the one below.
Figure 2-18 sp Choosing Analyses Form
Click OK.
Your ADE Explorer Setup Assistant will look like the following:
Figure 2-19 ADE Explorer

Running the Simulation and Plotting the Results

Start the analyses by clicking the green arrow icon in ADE Explorer or in the Schematic Editor.

This netlists the design and runs the simulation. A SpectreRF status window is displayed (spectre.out log file). When the analysis has completed, you may iconify the status window.

In ADE Explorer, select Results - Direct Plot - Main Form.
Figure 2-20 Invoking the Direct Plot Form

The Direct Plot Form is displayed. Alternately, you can click the Direct Plot icon in the Schematic window.
Figure 2-21 sp Direct Plot Form
In the Direct Plot Form, leave the Plotting Mode set to Append (this is the default).
In the Function section, select GT (for Transducer Gain). Transducer power gain, GT, is defined as the ratio between the power delivered to the load and the power available from the source.
When using the S-parameter Direct Plot Form, the Analog Design Environment assumes that the source (Γ_S) and load (Γ_L) reflection coefficients are zero. GT, therefore, plots the insertion gain assuming source and load impedances are matched.

(2-1) Transducer Gain with Source and Load Impedances Matched

In the Modifier section, select dB10 because you are plotting power.
The sp Direct Plot Form will look like the following:
Figure 2-22 sp Direct Plot Form
Click Plot.
In the Function section, select GA (for Available Power Gain). Available power gain, GA, is defined as the ratio between the power available from the network and the power available from the source.
When you use the S-parameter Direct Plot Form, Γ_S is set to zero, and therefore available gain (GA) is plotted as:

(2-2) Available Gain with Ts=0

Click Plot again.
In the Function section, select GP (for Power Gain). Power Gain is defined as the ratio between the power delivered to the load and the power input to the network.
The ADE Explorer environment assumes that Γ_in=0 (the input is matched) so the equation for power gain (GP) reduces to the equation below:

(2-3) Power Gain with TL=0.

Click Plot once more. All three gains (GT, GA, GP) plots are displayed on one window, as shown below.
Figure 2-23 Transducer, Available, and Power Gain

Note that GT is the smallest gain. Because the power available from the source is greater than the power input to the LNA network, the Power Gain is greater than the Transducer gain (GP > GT). The closer the two gains are, the better the input matching is. Similarly, because the power available from the LNA network is greater than the power delivered to the load , GA > GP. The closer these two gains are, the better the output matching is. The power gain GP is closer to the transducer gain GT than the available gain GA which means the input matching network is properly designed. That is, S11 is close to zero.
In the Direct Plot Form, change the Plot Mode to New SubWin (new subwindow).
Figure 2-24 Changing Plot Mode to New SubWindow
In the Function section, select Gmax (for maximum Transducer Power Gain) and click Plot.
Change the Plotting Mode to Append.
In the Function section, select Gmsg (for Maximum Stability Gain), and Click Plot.
In the Function section, select Gumx (for maximum Unilateral Transducer Power Gain), and click Plot again.
The three waveforms are appended to the previous graph, as shown below.
Figure 2-25 Adding Maximum Available, Maximum Stable, and Maximum Unilateral Gain Plots
- Maximum unilateral transducer power gain (Gumx) is the transducer power gain when you assume that the reverse coupling of the LNA S₁₂, is zero, and the source and load impedances are conjugately matched to the LNA. That is S11=Γ_s and S22= Γ _L

In the plots above, the maximum unilateral transducer power gain (Gumx) is very close to the maximum transducer power gain (Gmax) which means the reverse coupling S12 is small. The maximum stable gain (Gmsg) is the largest of the six gains plotted.

In the ViVA waveform window, choose File -Close All Windows to close the waveform window.
Next, you plot the gain circles. There are two types of gain circles: Power Gain Circles and Available Gain Circles. In the Function section of the Direct Plot Form, select GAC (Available Gain Circles). The form expands.
Figure 2-26 Direct Plot Form for Available Gain Circles

Available Gain Circle (GAC)
Available Gain (GA) is solely a function of the source reflection coefficient Γ_S . Thus, you can draw available gain contours on the Smith chart of Γ_S . The location for the peak of the contour corresponds to Γ_S producing the maximum available gain (GA). You can move the peak location by changing the design of the input matching network. The best location for the contour peak is at the center of the Smith chart, where Γ_S=0.
In the Plot Type section, choose Z-Smith. You will be plotting Gain Circles on the Impedance Smith Chart. (Y-Smith plots on the Admittance Smith Chart).
In the Sweep section, you can either choose Gain Level (dB) or Frequency (Hz). In this case, you will be sweeping Gain Level. The Frequency you specify depends on the operating frequency of your design. Since the lnaSimple circuit operates at 900MHz, enter that value in the Frequency (Hz) field.
In the Level Range (dB) section, set Start to 4, Stop to 14, and Step to 2.
The Direct Plot Form should look like the following:
Figure 2-27 Direct Plot Form for Plotting Available Gain Circles at a Constant Frequency
Click Plot. The available gain circles are plotted in the waveform window, as shown below.
Figure 2-28 Available Gain Circles on Z-Smith Chart

As you move your cursor around one of the Available Gain Circles, notice that the Tracking Cursor will read out both the Real and Imaginary part or the reflection coefficient directly from the Smith Chart in the Tracking Info section on the left side of the Smith Chart. The impedance or admittance at that point is also shown in the Reference point values section of the Legend.
In the Direct Plot Form, change the Plot Mode to New Window. Next, plot the Power gain circle (GPC).
Power Gain (GP) is solely a function of the load reflection coefficient Γ_L. Thus, you can draw the power gain contours on the Smith chart of Γ_L. The location for the peak of the contour corresponds to Γ_L producing the maximum power gain (GP). You can move the peak location by changing the design of the output matching network. The best location for the contour peak is at the center of the Smith chart, where Γ_L = 0.
In the sp Direct Plot Form, selectGPC in the Function section.
In the Plot Type section, select Z-Smith (it should be the default). You will be plotting Gain Circles on the Impedance Smith Chart.
In the Sweep section, your choices are frequency and Gain Level (dB). Choose Gain Level (dB). Since the lnaSimple operates at 900MHz, enter 900M in the Frequency (Hz) field.
In the Gain Level (dB) section, set Start to 4, set Stop to 14, and Step to 2. The Direct Plot Form should look like the following:
Figure 2-29 Direct Plot Form for Power Gain Circles
Click Plot. The power gain circles are plotted on the Smith Chart, as shown below.
Figure 2-30 Power Gain Circles

Next, you will look at circuit stability and plot Stability Circles.

Stability

After running an sp analysis, you can plot stability factor and stability circles.

Kf, the stability factor, is valid for two-port circuits only. Kf is defined as:

Figure 2-31 Equation for Kf, stability factor

The above equation is valid for small-signal stability only. Under large signal conditions, the circuit is less likely to be stable. In the presence of feedback paths from the output to the input, the circuit might become unstable for certain combinations of source and load impedances. An LNA design that is normally stable might oscillate at the extremes of the manufacturing or voltage variations, and perhaps at unexpectedly high or low frequencies. When K > 1 and D < 1, the circuit is unconditionally stable. That is, the circuit does not oscillate with any combination of source and load impedances. You should perform the stability evaluation for the S parameters over a wide frequency range to ensure that K remains greater than one at all frequencies.

In the Function section of the sp Direct Plot form, select Kf.
Set the Plotting Mode to New Window.
The sp Direct Plot Form should look like the following:
Figure 2-32 Plotting Kf from the sp Direct Plot Form
Click Plot.
The waveform window is displayed, as shown below.
Figure 2-33 Plotting Stability Factor Kf vs Input Frequency

The stability factor Kf is greater than 1 for all frequencies viewed, indicating that the circuit is stable at these frequencies. As the coupling (S12) decreases (reverse isolation increases), stability improves. You might use techniques, such as resistive loading and neutralization to improve stability for an LNA.
Next, plot the Stability Circles.
Close the waveform window by choosing File - Close All Windows and go back to the Direct Plot Form.
In the Function section, select LSB (Load Stability Circles). The form changes.
In the Plot Type section, choose Z-Smith (this is the default). You will be plotting Load Stability Circles (LSB) on the Impedance Smith Chart. (Y-Smith plots on the Admittance Smith Chart).
In the Frequency Range (Hz) section, enter Start 500M, Stop 4G, and Step 200M. The Direct Plot form should look like the following:
Figure 2-34 Direct Plot Form for Plotting Load Stability Circles
Click Plot. The Load Stability Circles are plotted, as shown below.
Figure 2-35 Load Stability Circles

By default, the graph is zoomed out to show all traces. Zoom into the Smith Chart by holding down the right mouse button and dragging a square around the section of the Smith Chart you would like to view. When you release the button, the graph redraws. You can also determine which trace belongs to which frequency by clicking on the + button to the left of LSB in the upper left section of the graph legend. This is shown in the next figure.
Figure 2-36 Zoomed in Load Stability Circles

Next, you will be plotting the Source Stability Circles.
In the Function section, select SSB (Source Stability Circles). The form changes.
In the Plot Type section, choose Z-Smith. You will be plotting Source Stability Circles on the Impedance Smith Chart.
In the Frequency Range (Hz) section, enter Start 500M, Stop 4G, and Step 200M. The Direct Plot Form should look like the following:
Figure 2-37 Direct Plot Form for Source Stability Circles
Click Plot. The Source Stability Circles are plotted, as shown below.
Figure 2-38 Source Stability Circles for lnaSimple

By default, the graph is zoomed out to show all traces. Zoom into the Smith Chart by holding down the right mouse button and dragging a square around the section of the Smith Chart you would like to view. When you release the button, the graph redraws. You can also determine which trace belongs to which frequency by clicking on the + button to the left of SSB in the upper left section of the graph legend. This is shown in the next figure.
Figure 2-39 Zoom in Source Stability Circles

When you release the mouse button, the plot redraws, as shown in the next figure.
Figure 2-40 Zoomed in View of Source Stability Circles

The source and load stability circles are also useful for checking for LNA stability. The input stability circle draws the circle Γ_out = 1 out on the Smith chart of Γ_S . The output stability circle draws the circle Γ_in = 1 on the Smith chart of Γ_L.
The non-stable regions of the two circles should be far away from the center of the Smith chart. In fact, it is better if the non-stable regions are located outside the Smith chart circles. This is the case for both Load and Source Stability circles.
In the ViVA waveform window, select File - Close All Windows. The waveform window closes.

The next measurement you will make is Noise Figure.

Linear 2-port noise analysis (NF, NFmin) and Noise circles

For cascaded stages, the overall noise figure is mainly determined by the first amplification stage, provided that it has sufficient gain. You achieve low noise performance by carefully selecting the low noise transistor, DC biasing point, and noise-matching at the input. The noise performance is characterized by noise factor, F, which is defined as the ratio between the input signal-to-noise ratio and the output signal-to-noise ratio. For equations to Noise Figure and minimum Noise Figure, see the Noise Calculations in the Simulator section in the Spectre® Circuit Simulator and Accelerated Parallel Simulator RF Analysis User Guide.

You have already run the simulation for linear two-port noise as part of the sp analysis. Now, you will plot the results.

In the sp Direct Plot Form, select NF in the Function section. The form changes.
In the Modifier section, select dB10 to plot Noise Figure. (If you want to plot Noise Factor instead, select Magnitude). The sp Direct Plot Form should look like the figure below.
Figure 2-41 sp Direct Plot Form for Plotting Noise Figure
Click Plot. The noise figure is plotted, as shown below.
Figure 2-42 lnaSimple Noise Figure Plot
In the Direct Plot Form, change the Plotting Mode to Append.
In the Function section, select NFmin. You will be plotting minimum noise figure.
Set the Modifier to dB10 to plot minimum noise figure. (Leave the modifier at the default value of magnitude to plot minimum noise factor).
The Direct Plot Form should look like the following figure:
Figure 2-43 sp Direct Plot Form for Minimum Noise Figure
Click Plot to plot minimum noise figure. The noise figure is plotted, as shown below.
Figure 2-44 lnaSimple Minimum Noise Figure

The y-axis label for Noise Figure and Minimum Noise Figure both show “Noise Factor (dB)”. View the legend at the upper left side of the plot. You will see NF dB10 and NFmin dB10. This shows that noise figure (rather than noise factor) is being plotted.
The Noise Figure plots are at a minimum at the frequency of operation.
Next you will plot Noise Circles.
In the Direct Plot Form, change the Plotting Mode to New SubWin.
In the Function section, select NC. The form changes.
In the Plot Type section, select Z-Smith. This plots the noise circles on the Impedance Smith Chart (Choosing Y-Smith plots the noise circles on the Admittance Smith Chart.)
In the Sweep section, select Noise Level (dB). You will be plotting circles of constant noise level at a single frequency.
In the Frequency(Hz) field, type 900M. This is the operating frequency of the lnaSimple circuit.
In the Level Range (dB) section, set Start to 4, Stop to 8, and Step to 0.5. The Direct Plot Form should look like the figure below.
Figure 2-45 Direct Plot Form for Noise Circles
Click Plot. The Noise Circle plot is displayed, as shown below.
Figure 2-46 Noise Circle Plot

The optimum location for the center of the noise circle is at the center of the Smith chart. However, it is hard to center both the available gain circle, GAC, and the noise circle, NC, in the Smith chart. When you design an LNA, plot NC, GAC, and the source stability circle, SSB, together in the same plot. Use this plot to trade-off the gain, noise, and stability for the input matching network design.
Clean up the screen for the next set of measurements.
1. Close the Results Display window by choosing Window - Close.
2. Close the ADE Explorer window by choosing Session - Quit.
3. In the Schematic window, choose File - Close.

Summary

In this section, you have looked at common measurements made on Low Noise Amplifier circuits, specifically Gain, Stability, and Noise. For other examples of Measurements, see Chapter 3: Frequency Domain Analyses: Harmonic Balance in the Virtuoso® Spectre® Circuit Simulator and Accelerated Parallel Simulator RF Analysis User Guide and the LNA Workshop located in the MMSIM hierarchy.

In the next section, you will measure the 1dB Compression Point and IP3 using two different methods.

Third-Order Intercept measurement with HB (2 tone HB)

In narrowband circuits, distortion is commonly measured by applying two pure sinusoids with frequencies well within the bandwidth of the circuit (call these frequencies f1 and f2). The harmonics of these two frequencies would be outside the bandwidth of the circuit, however, there are distortion products that fall at the frequencies 2f₁-f_2, 2f₂-f₁, and so on. These frequencies are within the bandwidth of the circuit and can be used to measure the intermodulation distortion, or IMD, produced by the circuit.

IP3 is an important RF specification. The IP3 measurement is defined as the cross point of the power for the 1st order tones, f₁ and f₂, and the power for the 3rd order tones, 2f₁−f₂ and 2f₂−f₁, on the load.

Assuming the input amplitudes are equal, the output first order terms will have the same amplitude and the output third order terms will also have the same amplitude.

As the first order components grow linearly and the third order components grow cubically, they eventually intersect as the input power level increases.

The third order intercept point is where the two output power curves intersect, as shown in the figure below.

Figure 2-47 1dB Compression Point and IP3 Curves

SpectreRF provides several different ways of simulating IP3 for a low noise amplifier. You will measure IIP3 (input IP3) using two different ways.

The first way is to use hb analysis with two RF tones applied. Generally, the RF power is swept over a range in the small-signal region. Hb is a large-signal simulation that calculates all the harmonics. Because the third-order product is quite small at low-input power, the accuracy of the simulation result must be kept quite high. This usually requires lengthy simulations.

The fastest approach is to select Rapid IP3 from the AC analysis. This is the fastest approach but it is limited to small-signal (at least 10dB below the 1dB compression point) IP3 measurements. In a small-signal application, both techniques produce answers typically within 0.1dB of each other.

Opening the lnaSimple LNACircuit in the Schematic Window

In the CIW, choose File – Open.
The Open File form is displayed.
Choose ExampleLibRF from the Library drop-down list.
Choose lnaSimple from the Cells list box. Leave the rest of the fields at their default values.
The completed Open File form appears like the one below.
Figure 2-48 Open File Form
Click OK.
The Schematic window for lnaSimple is displayed.
Figure 2-49 lnaSimple Schematic
In the Schematic, click on the RF port on the left side of the schematic.
Figure 2-50 RF Port Selected

Note that when you do this, the RF port properties are populated in the Property Editor pane. Examine the input port settings.
1. Source type sine means generate large signals for the time domain (transient, pss-shooting, qpss-shooting, envlp-shooting, and so on) or frequency domain (HB or envlp-HB) analyses.
  The port can generate one or two large signals. In this example, it is generating two signals. You need to specify a name for all of the large signals. This is done in the Frequency name 1 and Frequency name 2 property fields. The frequencies are set to a variable name. The value of the variables is set in ADE Explorer. This allows sweeps to be done in the Analog Design Environment. The amplitudes can be set in volts peak or in dBm. In this case, the amplitudes are set to a variable named prf. When the amplitude is set in dBm, the amplitude in volts cannot selected.
  The Display second sinusoid option is a display function only. If there is an entry there and the display option is off, the second waveform will still be generated. To switch to a single input, remove all the entries, or set the amplitude or frequency to zero in the Amplitude field or the Design Variables section of ADE Explorer.
  The amplitude for the small-signal analyses AC and PAC are set in the source. To view the small signal values, scroll down the form to the Display small signal parameter drop-down list and select true. The amplitude for AC and PAC can be either in Volts peak or dBm, but not both at the same time.
  Figure 2-51 RF Port Display small signal parameters.
  
  The form expands, as shown below.
  Figure 2-52 Expanded RF Port Display Small Signal Parameters
  
  The frequency of these signals will be set in the small-signal setup form in ADE Explorer. The amplitude for PAC can be either in volts peak or in dBm, again with the form not allowing both to be set at the same time.
In the Schematic window, choose Launch – ADE Explorer.
In the Launch ADE Explorer dialog, select Create New View.
The Create new ADE Explorer view form is displayed.
Figure 2-53 Create new ADE Explorer view
Leave each option to the default selections and click OK.
The Virtuoso ADE Explorer window opens.
Figure 2-54 Analog Design Environment Window