Overview Process Simulation
3D 2D 1DDevice Simulation
3DStress Simulation Interactive Tools Virtual Wafer Fab TCAD Videos
Victory Device Device 3D Giga 3D MixedMode 3D Quantum 3D Luminous 3D TFT 3D LED 3D Magnetic 3D Thermal 3D2D
Mixed Signal, RF
Overview Gateway SmartSpice Verilog-A Language SmartSpice RF Harmony Utmost III Utmost IV Spayn InVar EM/Ri-Thermal
Custom IC CAD
Downloads & Support
PDK Design Flows
Overview Available PDKs Foundry Partners Quality and Testing Maintainability PDK Development Services Documentation & Training Migration to Silvaco PDKs
Overview TCAD Services SPICE Modeling Parasitic Extraction PDK Development Cell Libraries and Blocks
VCO : Voltage Controlled Oscillator Simulation
Requires: Gateway, SmartSpiceRF & SmartView
Minimum required Versions: Gateway 2.12.10.R, SmartSpiceRF 1.6.5.R
In this example of an RF Voltage Controlled Oscillator we will setup and run the Oscillator analysis and noise analysis to enable us to measure the oscillator operating frequency and phase noise.
Start Gateway and load the workspace file VCO.workspace by selecting File->Open->Workspace.
To load the VCO example circuit schematic, select File->Open->Schematic and open VCO.schlr. The VCO schematic will appear in Gateway.
Editing Circuit Schematic
To make some changes to the VCO schematic, double click on the symbol of Voltage source V2 to open the Attributes Instance window. Set the DC voltage DCVAL = 0.5.
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 Create in the tool bar.
The VCO netlist will then appear in a new window.
Check in Gateway that your preferred simulator is set to SmartSpiceRF. In Gateway click on Edit->Preferences to open the preferences setup. Choose Tools->Simulator and set Simulator to SmartSpiceRF. Version number is set to Default (the latest installed version) in the Version field. You can define any specific version available here.
SmartSpiceRF needs more than just a circuit netlist perform a meaningful simulations. It needs Circuit Netlist, Voltage or Current stimulus, set of Options, Analysis Statements, and active devices Model parameters or Libraries. All this information comes together in the form of Input Deck file (*.in, *.inp, *.cir, *.sp, *.sm, *.scs, etc.), which provides SmartSpiceRF with all needed information to run simulation and generate output data.
Click on the simulation Tool Bar icon Edit Control File
The control file will be opened in the text editor Sedit window. The control file contains the path to the model library file as well as SmartSpiceRF .OP and .HNOISE Analyses statements. The control file combined with the circuit netlist and a list of vectors to be saved creates an Input Deck for SmartSpiceRF.
VCO Noise Analysis Setup
Oscillator Noise Analysis is a two-stage process:
1) Periodic Steady-State analysis is provided to find out Frequency of Oscillation, Amplitude of the Carrier, and Shape of the Output signal.
2) The following Small-Signal analysis is provided to compute Noise PSD and Phase Noise at the Given Output over desired Frequency range, offset from the Frequency of Oscillation.
The completed VCO.in input deck was created from the vco.net netlist and the vco.ctr control file.
The .HNOISE analysis performs a frequency sweep of (+1KHz -> +100MHz) relative to the defined Frequency of Oscillation. PSS is calculated by the Shooting method.
Click on Gateway->Simulation->Run to begin the SmartSpiceRF simulation.
After the simulation is finished, the oscillation frequency of 2.08 e+09 Hz is shown in the Simulation Output window.
SmartSpiceRF Noise Simulation Results
SmartSpiceRF outputs simulation results of Large-Signal PSS and Small-Signal Noise analyses and statistic information into the Output window and creates number of plots with Waveforms, Spectra, Noise, Measurement results, etc. .HNOISE analysis outputs Large-signal steady-state waveforms and spectra any of circuit variables.
As an example, the Output window may show the following information:
Frequency of Oscillation Fosc = 2.499878e+007 Hz
Carrier: Total Power Psig = 1.719005e+000 Wt
1st Harmonic's Power Psig1 = 7.844351e-001 Wt
Effective amplitude Ac = 1.854187e+000 V
SmartSpiceRF Plots and Vectors
Simulation results in the form of plots will be loaded into SmartView, and a SmartView Data Browser window will be open.
.HNOISE analysis produces the number of plots:
hopsh_wf plot consists of the periodic steady-state waveforms at the final Shooting iteration.
hop_sp plot consists of the frequency-domain spectra. The results are calculated from hopsh_wf waveforms by Inverse Fourier Transform at the frequency points k*fund, where fund is the calculated fundamental frequency of oscillation, 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 the analysis statement. If not, only the spectra plot hop_sp will be output.
hinit_wf plot consists of the initial transient analysis waveforms,, if the keyword SAVEITER was specified in the analysis statement.
hiter_wf plots consist of the shooting iteration time-domain waveforms if the keyword SAVEITER was specified in the analysis statement.
.PRINT, .PROBE, .SAVE and .MEASURE statements must use the analysis and/or specific plot names HOPSH_WF, HOP_WF, HOP_SP and so forth, 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
The number of plots and associated vectors depends on type of analyses provided and used methods. Open plot hnoise2, select vector PhaseNoise2, and click Plot. The Phase Noise plot is shown in the SmartView window. The oscillation frequency of 2.08 GHz is shown in the header. The phase noise at close to 100kHz offset frequency is -100.73dBc/Hz.
Return to Gateway schematic window and edit the schematic. Set the DC voltage of V2 to DCVAL = 1.5 V. Run the second simulation.
After the simulation finishes, select vector PhaseNoise2 from hnoise4 plot and click Plot. The oscillation frequency of 2.04 GHz is shown in the header. The phase noise with 1,5V tuning voltage at 100kHz offset frequency is -100.45 dBc/Hz.
So the tuning range is 2.04 GHz to 2.08 GHz for the tuning voltage of 0.5 V to 1.5 V.
Remember that we've added the saveinit flag into .HNOISE statement to save results of the Initial Transient analysis of the Shooting method. Next we see what the start-up behavior of the oscillator looks like. In the Data Browser Panel, select hinit_wf2 plot, then select vector V(vcop) and click Plot to display the oscillator node vcop for tuning voltage of 1.5V.