LNA_ design (设计实例)

ECSE6967-RFIC Design Fall2005Assignment_3 (Due Friday 23th)Make sure to state your assumptions if they are not given in the questions.1. The LNA Design is the same as in the last problem in the class tutorial on LNAs (You can compare the hand calculated and simulated results!!). The component values are relatively close to hand calculation. Only small changes have been done to enhance the gain and Noise Figure of single ended source degenerated LNA.To characterize the LNA following figure of merits are usually measured.1. Power Consumption and Supply Voltage2. Gain3. Noise4. Input and Output Impedance Matching5. Reverse Isolation6. Stability7. LinearityWe will use S-Parameters (SP), Periodic Steady State Analysis (PSS), Periodic AC (PAC) and Pnoise analysis available in SpectreRF simulator to simulate above parameter of LNA.Usually there is more than one method available to simulate the desired parameter; we will use the procedure recommended by cadence.1. S-Parameter Analysis• Small Signal Gain (S21, GA, GT, GP)• Small Signal Stability (Kf and ∆ or Bif )• Small Signal Noise (SP and Pnoise)• Input and Output Matching (S11, S22, Z11, Z22)2. Large Signal Noise Simulation (PSS and Pnoise)3. Gain Compression, 1dB Compression Point (Swept PSS)4. Large Signal Voltage Gain and Harmonic Distortion (PSS)5. IP3 Simulation (Swept PSS)6. Conversion Gain and Power Supply Rejection Ratio (PSS and PXF)LNA SimulationCircuit Simulation Setup:• We will be using the MOSFETS in IBM bicmos6hp process for this HW.• Load the Cadence and technology file using• Make a new library RF_HW3 in Cadence Library Manager• Create and draw the Schematics, LNA_testbench a as shown in Fig-1.1 and LNA as shown in Fig-1.2. The components values are listed below for your convenience.• Input Port in Schematic LNA_testbench•50 Ohms in Resistance• 1 in Port Number•Sine in Source Type•frf1 in Frequency name 1 field•frf in Frequency 1 field•prf in Amplitude1(dBm) field• Output Port in Schematic LNA_testbench•500 Ohms in Resistance• 2 in Port Number• Component Values in Schematic LNA_testbenchVdd = 3.3V, C1, C2= 10nF, CL= 500fF• Component Values in LNA SchematicM1, M2 = 200µm/0.35µm , Mbias = 60µm/0.35µmLs = 700 pH, Lg = 12 nH, Ld = 6 nH, Rd = 700 ΩC1, C2= 10nF, CL= 500fFFig. 1.1Fig. 1.2A. Small Signal Gain, NF, Impedance Matching and Stability ( S-Parameter )•• In the affirma window, select analysis-choose, the analysis choose window shows up Select sp for Analysis•In port field click on select and then activate the schematic (if not activated automatically), choose the input port first and then the output port. The names of two selected ports will appear in Ports field.•Sweep Variable Æ frequency•Sweep Range (start--stop) Æ 1G to 5G•Sweep Type Æ Automatic•Do Noise Æ Yes•Select Input and output ports accordingly by clicking Select and then clicking at the appropriate Port in Schematic•Make sure that Enabled Box is checked then click OK.• In the affirma window click on Simulation ÆNetlist and Run to start the simulation, make sure that simulation completes without errors.• Now in the affirma window click on the Results ÆDirect plot ÆS-parameters• The S-parameters results window appears.• Impedance MatchingIn the S-parameters Results window…•Select Function ÆSP•Plot Type ÆRectangular•ModifierÆdB20•Click S11 {S12, S22 and S21} press the PLOT button.•Plot (S11 and S22) in one plot and (S21 and S12) in another plot• NF (Noise Figure)In the S-parameters Results window…•Select Function ÆNF (and NFmin)•Plot Type ÆRectangular•Modifier ÆdB10•Press PLOT.• Stability Factor Kf and Bif (∆)•In the S-parameters Results window…•Select Function ÆKf and Bif (one at a time)•Plot Type ÆRectangular•Press the PLOT button.The Stern stability factor K and ∆can be plotted in two ways. The stability curves for K and ∆as plotted with respect to frequency sweep or they can be plotted as load stability circle (LSB) and source stability circle (SSB).B. NF by Large Signal Noise Simulation (PSS and Pnoise Analysis)Use the PSS and Pnoise analyses for large-signal and nonlinear noise analyses, where the circuits are linearized around the periodic steady-state operating point. (Use the Noise and SP analyses for small-signal and linear noise analyses, where the circuits are linearized around the DC operating point.) As the input power level increases, the circuit becomes nonlinear, the harmonics are generated and the noise spectrum is folded. Therefore, you should use the PSS and Pnoise analyses. When the input power level remains low, the NF calculated from the Pnoise, PSP, Noise, and SP analyses should all match.•Change the Input Port Parameters in the Schematico50 Ohms in Resistance, 1 in Port Number , DC in Source Type • Verify the variable values in the affirma windowfrf = 2.4 Ghzprf = -20 (Its meaning less in this simulation)•In the affirma window, select Analysis Choose•The Choose Analysis window shows up•Select pss for Analysis•Uncheck the Auto Calculate Box•Beat Frequency Æ 2.4G•Output Harmonics Æ 20•Accuracy Default Æ Moderate•Make sure that Enabled Box is checked then click OK.• Now at the top of choosing Analysis window•Select pnoise for Analysis•PSS Beat Frequency(Hz) = 2.4GHz appears automatically•Sweep Type ÆAbsolute•Frequency Sweep RangeÆ Start: 1G Stop: 5G•Sweep Type Æ Automatic•Maximum Sidebands Æ 20•In output Section• Select Voltage• Positive Output Node Æ Select net RF_OUT from Schematic• Negative Output Node Æ Leave Empty , it means GND• Input Sources Æ Select PORT• Input PORT Source Æ Select PORT1 from Schematic• Reference Side Band Æ 0•Noise Type ÆSources•Enable Box in the bottom should be checked.•Click OK• In the affirma window click on Simulation ÆNetlist and Run to start the simulation, make sure that simulation completes without errors.• Now in the affirma window click on the Results ÆDirect plot ÆPSS• The PSS results window appears.•Plot mode ÆAppend•Analysis Type Æpnoise•Function ÆNoise Figure•Add to Output ÆBox Unchecked•Also plot the input and output noise• The Pnoise analysis summery shows you the contributions of different noise sources in the total noise. This is very powerful feature to focus the effort to improve the noise performance of the device which contributes the maximum noise.• Now to see noise contribution in the affirma window click on the Results ÆPrint ÆPSS Noise Summary•Type ÆSpot Noise•Frequency Spot Æ2.4G•Weighting Æflat•Click on ALL TYPES button so that all entries are highlighted•Truncate ÆNone•Leave all other field as it is and press APPLY•The Noise Contribution of Different Sources appears in new window• Fill up the Table below indicating the noise contribution of different components.C. Large Signal Voltage Gain and Harmonic Distortion (PSS)• Change the Input Port Parameters in Schematic Window•50 Ohms in Resistance• 1 in Port Number•Sine in Source Type•frf1 in Frequency name 1 field•frf in Frequency 1 field•prf in Amplitude1(dBm) field• Verify the variable values in the affirma window•frf = 2.4 Ghz•prf = -20dBm• In the affirma window, select Analysis ÆChoose• The Choose Analysis window shows up• Select pss for Analysis•In Fundamental Tones following line should be visible• 1 frf1 frf 2.4G Large PORT1• Check the Auto Calculate Box•Beat Frequency Æ 2.4G (Automatically appears)•No of Harmonics Æ 10•Accuracy Default Æ Moderate•Enable Box in the bottom should be checked.•Click OK• In the affirma window click on Simulation ÆNetlist and Run to start the simulation, make sure that simulation completes without errors.• In the affirma window, select Results ÆDirect plot ÆPSS the analysis choose window shows up•Select Function as Voltage Gain•Modifier ÆdB20•Input Harmonics Æ2.4G•SelectÆOutput and Input nets and then activate the schematic window and select RF_OUT and RF_IN nets respectively.•At the top of PSS result window change the plot mode to append.•Now Select Function as Voltage•SweepÆSpectrum•Signal Level Æpeak•Modifier ÆdB20•SelectÆnet and the point to RF_OUT net in schematicAfter the PSS analysis, we can observe the harmonic distortion of the LNA by plotting the spectrum of any node voltage. Harmonic distortion is characterized as the ratio of the power of the fundamental signal divided by the sum of the power at the harmonics.D. 1dB Compression Point(Swept PSS)• Change/Check the Input Port Parameters in Schematic Window•50 Ohms in Resistance• 1 in Port Number•Sine in Source Type•frf1 in Frequency name 1 field•frf in Frequency 1 field•prf in Amplitude1(dBm) field• Verify the variable values in the affirma window•frf = 2.4 Ghz•prf = -20dBm• In the affirma window, select Analysis ÆChoose• The Choose Analysis window shows up•Select pss for Analysis•In Fundamental Tones following line should be visible1 frf1 frf 2.4G Large PORT1•Uncheck the Auto Calculate Box•Beat Frequency Æ 200K•No of Harmonics Æ 12•Accuracy Default Æ Moderate•High light the Sweep Button•Click Design Variable Button, small window appears, chooseprf in it•Sweep Range Æ Choose the start : -40dBm and Stop: 0dBm•Sweep Type ÆLiner and No of Steps =12•Enable Box in the bottom should be checked.•Click OK• In the affirma window click on Simulation ÆNetlist and Run to start the simulation, make sure that simulation completes without errors.• In the affirma window, select Results ÆDirect plot ÆPSS the analysis choose window shows up•Select Function ÆCompression Point•Select Port (Fixed R (Port))•Gain CompressionÆ1dB•Extrapolation Point Æ-40dB•Ist Order Harmonic Æ 2.4G•Activate the Schematic Window and click on Output PORT to plot the resultsA PSS analysis calculates the operating power gain. That is, the ratio of power delivered to the load divided by the power available from the source. This gain definition is the same as that for G P. Therefore, the gain from PSS should match G P when the input power level is low and nonlinearity is weak. In case of differential LNA the even mode disturbances will be suppressed.E. IIP3 (Swept PSS)Two-tone test is used to measure an IP3 curve where the two tones, ω1 and ω2. Since the first-order components grow linearly and third-order components grow cubically, they eventually intercept as the input power level increases. The IP3 is defined as the cross point of the power for the 1st order tones, ω1 and ω2, and the power for the 3rd order tones, 2ω1 – ω2 and 2ω2 - ω1, on the load side.• There are three ways to Simulate IIP3, Using Swept PSS, PSS and PAC and QPSS. We will use Swept PSS Analysis.• Change the Input Port Parameters in Schematic Window•50 Ohms in Resistance• 1 in Port Number•Sine in Source Type•frf1 in Frequency name 1 field•frf in Frequency 1 field•prf in Amplitude1(dBm) field•Click on the Box Display Second Sinusoid•frf2 in Frequency name2 field•frf+40M in Frequency2 field•prf in Amplitude2(dBm) field• Verify the variable values in the affirma window•frf = 2.4 Ghz•prf = -20dBm• In the affirma window, select Analysis Choose• The Choose Analysis window shows up•Select pss for Analysis•In Fundamental Tones, the following lines should be visible1 frf1 frf 2.4G Large PORT12 frf1 frf+40M 2.44G Large PORT1•Check the Auto Calculate Box•Beat Frequency Æ 40M (Automatically appears)•No of Harmonics Æ 65•Accuracy Default Æ Moderate•High light the Sweep Button•Select Design Variable, small window appears, choose prf in it•Sweep Range Æ Choose the start : -30dBm and Stop: 0dBm•Sweep Type ÆLiner and No of Steps =12•Enable Box in the bottom should be checked.• Click OK In the affirma window click on Simulation ÆNetlist and Run to start the simulation, make sure that simulation completes without errors.• In the affirma window, select Results ÆDirect plot ÆPSS the analysis choose window shows up•High light the Replace in Plot Mode•Select Function as Compression Point•Analysis ÆPSS•Function ÆIPN Curves•Select Port (Fixed R (Port))•Highlight variable Sweep Prf•Extrapolation Point Æ-30dB•Highlight Input Referred IP3•Order Æ3rd•1st Order Harmonic Æ2.4G•3rd Order Harmonic Æ2.48G•Activate the Schematic Window and click on Output port to view the results.F. Conversion Gain and Power Supply Rejection Ratio (PSS and PXF)The PXF analysis provides frequency dependent transfer function from any specific source to the designated output (RF_OUT in this case). If the specific source is power supply node then we can measure the PSRR.• Change the Input Port Parameters in Schematic•50 Ohms in Resistance• 1 in Port Number•DC in Source Type• Variable values in affirma window•frf = 2.4 Ghz•prf = -20• In the affirma window, select Analysis Choose• The Choose Analysis window shows up•Select pss for Analysis•Uncheck the Auto Calculate Box•Beat Frequency Æ 2.4G•Output Harmonics Æ 4•Accuracy Default Æ Conservative• Now at the top of choosing Analysis window•Select pxf for Analysis•PSS Beat Frequency(Hz) = 2.4GHz (appears automatically)•Frequency Sweep RangeÆ Start: 1G Stop: 5G•Sweep Type ÆLinear and Step Size Æ40M•Maximum Sidebands Æ 0•In output Sectiono Select Voltageo Positive Output Node Æ Select net RF_OUT from Schematico Negative Output Node Æ Leave Empty , it means GNDo Click OK• In the affirma window click on Simulation ÆNetlist and Run to start the simulation, make sure that simulation completes without errors.• Now in the affirma window click on the Results ÆDirect plot ÆPSS• The PSS results window appears.• Select Analysis Type Æpxf•Sweep ÆSpectrum•FunctionÆVoltage Gain•ModifierÆdB20•Activate the Schematic window, click on INPUT port, OUTPUT port and VDD symbols. The Plots window will pop up•Please note that PSRR is extremely poor. Why?Problem 2. Use the circuit shown in Fig. 2 to design an LNA with the following specifications.Frequency range: 925 MHz ~ 960 MHzInput impedance Zin @ 940 MHz: |Zin| = 50 ohm ± 5%.M I: finger number / channel width / channel length = 40 / 5 µm / 0.35 µmM B: finger number / channel width / channel length = 2 / 5 µm / 0.35 µmAll parasitic effects for resistors, inductors, and the package are ignored.(a) Find the values for L F and L S.(b) Use SpectreRF to simulate Zin v.s. f, Av v.s. f, NF v.s. f, P1dB (@ 940 MHz), andIIP3 (@ 940 MHz, 950 MHz). Attach the simulated waveforms.Fig. 2。