Low Noise Amplifier Simulation

LNA : Low Noise Amplifier Simulation

Requires: Gateway, SmartSpiceRF and SmartView

Minimum required Versions: Gateway 2.12.10.R, SmartSpiceRF 1.6.5.R

Gateway Schematic Capture

Start Gateway and load the workspace file LNA.workspace by selecting File->Open->Workspace. When the browser window appears, navigate to the directory where RF Demo PDK Examples were installed, descend into the ./LNA directory, and select LNA.workspace file.

Loading LNA Schematic

To load the LNA example circuit schematic, select File->Open->Schematic. When the file browser appears, navigate to the ./LNA directory and select the file LNA.schlr. The LNA example circuit schematic will appear in the window.

Generating Netlists

Netlists are ASCII files used to describe device connectivity and element properties of the circuit. Gateway can create two different netlist formats: SmartSpice for circuit simulation, or Guardian for layout design. See the Gateway user manual for more information on these formats.

To generate a netlist in SmartSpice format, either select Simulation->Create Netlist , or click on the SmartSpice Netlist icon in the tool bar. LNA netlistWill then appear in a new window.

Simulator Setup

In Gateway, check that your preferred simulator is set to SmartSpiceRF. Click on Edit->Preferences to open the preferences setup window. Choose Tools->Simulator and set Simulator to SmartSpiceRF. Version number is set to Default (the latest installed version) in the Version window. You can also define any specific version.

Control File

SmartSpiceRF needs more than just a circuit netlist to perform meaningful simulations. It needs Circuit Netlist, Voltage or Current stimulus, set of Options, Analysis Statements, and active devices Model parameters or Libraries. All of this information comes together in the form of an Input Deck file (*.in, *.inp, *.cir, *.sp, *.sm, *.scs, etc.) which provides SmartSpiceRF with all the necessary information to run simulations and generate output data.

Click on the simulation tool bar icon "Edit Control File".

The control filewill be opened in the text editor Sedit window. The control file consists of the path to the SILVACO RF Demo PDK model library file as well as SmartSpiceRF .OP, HNET, and .HARM Analyses statements. The control file combined with the circuit netlist and list of vectors to be saved creates an Input Deck for SmartSpiceRF. There are two RF simulation runs for this example to provide S-parameters, Noise Figure, and 1dB compression point calculations.

SmartSpiceRF Simulation

.HNET Analysis

Periodic Steady-State HNET Analysis is a two-port network small-signal analysis which is used to compute scattering parameters (S-parameters) of the circuit.

Uncomment the .HNET analysis statement section in the LNA circuit control file.

.HNET will first perform a PSS analysis with the 10GHz fundamental. Although there are no signals at 10GHz in this circuit, using .HNET will allow us to make use of the extended s-parameter measurements for Noise, Load Stability, Source Stability, Gain and Power circles that HNET provides.

Click on Gateway->Simulation->Run to begin the SmartSpiceRF simulation.

.HNET Analysis Simulation Results

SmartSpiceRF outputs simulation results of the Large-Signal PSS and Small-Signal HNET analyses and statistic information into the output window and creates number of plots with Waveforms, Spectra, Hnet Data, Measurement results, etc. .HNET analysis outputs Large-signal steady-state waveforms and spectra of circuit variables.

SmartSpiceRF Plots and Vectors

.HNET analysis produces the number of plots: hnet plot consists of the two-port network analysis results.

hop_sp plot consists of the frequency-domain spectra. The results are calculated at the frequency points k*fund, where fund is the circuit fundamental frequency, and k=0, 1, ..., nharm.

hop_wf plot consist of the waveforms at unified time grid with the number of time points defined by a specified number of harmonics nharm. This plot is output if the keyword WAVES was specified in analysis statement. If not, only the spectra plot hop_sp will be output.

.PRINT, .PROBE, .SAVE and .MEASURE statements must use the analysis and/or specific plot names HNET, HOP_WF, HOP_SP and so on, to make any measurement and output separate results. The output statements without the analysis type name will output all types of results for all types of analysis.

SmartView Graphic Postprocessor

Simulation results in the form of plots will be loaded into SmartView, and the SmartView Data Browser window will be opened.

Open hnet1 plot, then select vectors s11_h0h0, s12_h0h0, s21_h0h0, s22_h0h0, and click Plot.

Then select View->Layout->Tile. Right-click on the picture and select Properties and select dB(MAG) as the Data Map Type.

Select Chart->Split->Split-all/Selected and View->Layout->Tile to get the result plot. You can also change the grid details, colors, and line width by selecting Edit->Preferences.

The result shows that at 2.4 GHz, LNA has S11= -13.1 dB, S22= -18.4 dB, S21= 16.9 dB, S21= -28.8 dB.

Press on the left-side of SmartView window, choose S11_h0h0 and S22_h0h0, and click Plot to draw it on the E-Smith chart.

To display the Noise Figure plot, select the vector NFssb and click Plot . The LNA noise figure at 2.4 GHz is 5.3 dB.

To plot the stability factor , select the vector K_h0h0 and click Plot.

To display the Gain, Power Gain, and Stability Circles over a single frequency, use the Data Filter to filter out the desired single frequency and click Plot. The LNA circles for the frequency 2.4GHz are shown.

1dB Compression Point Calculation (P1dB)

The Input Referred 1dB Compression Point is the input signal level at which the actual gain departs from the theoretical gain by -1dB. SmartSpiceRF allows you to compute Input Referred 1dB Compression Point using the measurement statement COMPR1DB.

P1dB Simulation Setup

To calculate P1db, comment the .HNET analysis and uncomment the .HARM analysis in LNA.ctr.

Click on Gateway->Simulation->Run to begin the SmartSpiceRF simulation.

P1dB Simulation Results

Simulation results in the form of plots will be loaded into SmartView, and SmartView Data Browser window will be opened.

To display the P1dB simulation results, from the SmartView Data Browser window open meas1 plot, choose vector dbout and press Plot.

P1dB Simulation Plot will be appear.

To view the value of P1dB result, select vector r_1dbcompression for meas1 from SmartView and press View Data. The measured input referred 1dB compression point is -27.2 dBm.

Third-Order Intercept Point Calculation

It is the nature of third-order products in the output signal to emerge from the noise at certain input levels and increase as the cube of the input levels. Thus, the slope of the third-order line increases 3dBm for every 1-dBm increase in the response to fundamental signal. The gain line can be continued to a point where it intersects with the gain line of the fundamental signal. This point is the third-order intercept point. The input signal level corresponding to this point is Input Referred IP3 Point.

Loading LNA Schematic

To load LNA circuit schematic for IP3 calculation, select File->Open->Schematic. When the file browser appears, navigate to the ./LNA directory and select the file LNA_iip3.schlr. The LNA circuit will appear in the window.

In this simulation, a two-tone signal is applied to the RF input in a form of multitone Port instance (PRF) as follows:

Name Value

MTS1_MAG prf

J1 48

MTS2_MAG prf

J2 49

IP3 Simulation Setup

Click on to generate netlist, then open the control file, to view .HARMONIC analysis and measurement statements to calculate IP3.

Click on Gateway->Simulation->Run to begin the SmartSpiceRF simulation. Simulation results in form of plots will be loaded into SmartView, and the SmartView Data Browser window will be opened.

IP3 Simulation Results

Simulation results in the form of plots will be loaded into SmartView, and the SmartView Data Browser window will be opened.

To display the IP3 simulation results, from SmartView Data Browser window open meas1 plot, choose both vectors pout_1 and pout_3 , and press Plot.

IP3 Simulation Plot will appear.

To view the calculated IP3 value, select vector resip3 for ip3_meas1 from SmartView and press View Data.