Integrated Radio Electronics. Laboratory 3: Mixer

Transcription

1 Integrated Radio Electronics Laboratory 3: Mixer Niklas Troedsson, Henrik Sjöland, Pietro Andreani, Lars Sundström, Johan Wernehag, Kittichai Phansathitwong 30th January Introduction The purpose of this laboratory is to verify your design of the mixer (Gilbert Cell from Barrie Gilbert) in the hand in exercise 3 and also to learn to investigate mixer linearity with SpectreRF. It is important that you have done the hand in 3 before attending the laboratory. Initialize for the third time! For RFIC year 2006: > cd rfic2006 > inittde rfic Create a schematic for your Gilbert Cell In Cadence do the following: Create a schematic cellview for your mixer in your library. Draw the mixer circuit according to figure 1. Use the component values you calculated in hand in exercise 3. Specify also necessary signal and dc sources. 1

2 (a) Schematic in Cadence V DD R D - + R D V IF M 3 M 4 M 5 M 6 V LO M 1 M 2 V RF I SS (b) Schematic illustration Figure 1: Schematic for the mixer. 2

3 3 Basic Setting for Analog Environment Create a directory in /tmp, use your login name for example e00xyz, with command mkdir. The path will be: /tmp/e00xyz! In Analog Environment under Setup>Simulator/Directory/Host change Project Directory to: /tmp/e00xyz. Under Simulation>Options>Analog, set the values in TOLERANCE OPTIONS fields to following, see figure 2. Fill in tolerance options here. The default values are slightly too loose for accurate analysis. For these simulations we therefore use more tight tolerances. Put: reltol to 1e-5 vabstol to 3e-8 iabstol to 1e-13 Leave the rest of the form unchanged. Figure 2: Simulation>Options>Analog, TOLERANCE OPTIONS determine resolution and accuracy for the simulation. Smaller tolerance values mean that the simulation needs more memory and takes more time. 4 DC Analysis Simulate the circuit to verify the operating point of the transistors. In particular, make sure that all transistors operate in the saturation region and that the transconductances are what you expect from your calculations. Explain the causes if there are any significant differences in comparison to your calculations. Adjust DC levels if necessary. 5 Transient Analysis Set RF port to source type sine, frequency for RF signal to 1.8GHz and LO signal to 2GHz. The amplitude of the RF signal should be low enough to avoid distortion. Verify the functionality of the mixer using transient analysis. Estimate the conversion gain by direct inspection of the output signal. If the conversion gain is not what you expected, try to identify the cause. Does the mixer function as a double balanced mixer? 3

4 Try various amplitudes for the LO signal and check when the conversion gain changes. 6 Simulation of conversion gain using SpectreRF Source type dc should be specified for the RF port. Set XMAG to 1 for RF port under Display small signal parameters. The LO sources must have a frequency name, fill in a name. Choose pss-analysis. Set Fundamental (Beat) Frequency to 2GHz. Set Number of harmonics to 0. Under Options form, set Integration Method Parameters to gear2only and Accuracy Parameters to allocal and also maxiters to 15. Choose pxf-analys. 4

5 Figure 3: PXF Form. Choose Start and Stop to 1MHz and 200MHz, respectively. Set Sweep Type to Linear with 100 points. Choose Maximum sideband to 1. This means that we only are interested in the mixing products at the sum and difference frequencies of the RF and LO signals. Mark the differential output nodes as Positive Output Node and Negative Output Node in the schematic. Start the simulation. Results: Plot results using Results/Direct Plot/PSS: Choose pxf, voltage gain, db20 and mark the RF source in the schematic. The resulting plot shows which frequencies from the RF generator contribute to the specified (IF) band. Not only the conversion gain that can be analyzed this way. We may actually choose to investigate the output with respect to any source in the schematic. 5

6 For example we can find the PSSR (power supply rejection ratio) by marking the supply instead of the RF source, in Results/Direct Plot/PSS: Choose pxf, voltage gain, db20 and mark the supply source in the schematic. 7 Simulation of 1dB compression point using SPSS The variable rfamp should be swept in power, since the built in plotting functions in the PSS analysis are optimized for that. We, on the other hand, want to sweep the voltage so that we are not dependent on power matching. That is why we use a port that sweeps in power with an inner resistance of 50Ω and an outer load of 50Ω, see RF port in figure 1. The load ensures that the port is matched and correct power is delivered. In our case the voltage at the load is then delivered to a balun with VCVS:s with a voltage gain of 1/2. Below you can see the equations to convert from power to voltage: ˆv is peak voltage amplitude, R is the inner and outer resistor, and P is power in dbm. The factor 2 comes from the rms voltage (ˆv/ 2) in square divided with the resistance, resulting in power. ˆv = 2R P/10 P = 10log 10 ( ˆv 2 2R ) Specify source type to sine in the RF port and Amplitude 1 (dbm) to rfamp, the variable to be swept, also specify name the Frequency name 1. Choose pss-analysis. Set Fundamental (Beat) Frequency to 200MHz, which is the IF frequency. Set Number of harmonics to 1. Choose sweep and set Design Variable Name to rfamp, which is given in dbm. Fill in sweep interval from -30 to 10 (dbm) which corresponds to 10mV to 1V and choose linear sweep with 10 points. Start the simulation. Plot the results with Results/Direct Plot/PSS: Choose pss and 1dB compression point as well as set extrapolation point to the first point of sweep interval, which -30dBm, and mark the output port of the mixer. What is the compression point? Calculate the corresponding input RF voltage for the mixer. Is this result reasonable? 6

7 8 Simulation of third order intercept points with SPSS In the RF port insert a second frequency with a different frequency name. Set both frequency amplitudes (dbm) to rfamp. Set the frequencies to 1.80GHz and 1.84GHz. We will now perform a two-tone test. Choose pss-analysis. Set Fundamental (Beat) Frequency to 40MHz. Set Number of harmonics to 6. We can then see frequencies up to 6*40=240MHz. The tones of interest are IM3 at 120MHz and 240MHz, and fundamental tones at 160MHz and 200MHz. Keep the same sweep interval for the amplitude as was specified earlier, or reduce the interval by increasing Start to -20 as well as reduce the number of points (for example 5 points). Note that the simulation will take a long time. Start the simulation. The simulation took: Year Minutes Seconds. Results/Direct Plot/PSS: Choose "pss", "IPN curves" and set "extrapolation point to the first point of the sweep and mark the output port. What is the intercept point? Calculate the corresponding RF input voltage. 9 Simulating intercept points for third order intermodulation distortion with PSS+PAC Erase the field Amplitude 2 (dbm) and Frequency 2 from the RF port. Set the field PAC Amplitude (dbm) to rfamp under Display small signal parameters. Choose pss-analysis. Set Fundamental (Beat) Frequency to 200MHz. Set Number of harmonics to 2. Keep the sweep setting from the previous simulation. Choose pac analysis. 7

8 Figure 4: PAC form. itemize Set Frequency (Hz) to 1.82GHz. Choose Select from range and set From (Hz) to 100M, To (Hz) to 300M, and Max. Order to 3. Mark -8 and -10 to obtain the desired products. IM3 which lies on 220MHz is sideband -8 because 1820MHz+(-8)*200MHz=220MHz. In the same way you may obtain the other desired tone at 180MHz with 1820+(- 10)*200MHz=-180MHz. Start the simulation. Compare the simulation time with previous analysis. The simulation took: Year Minutes Seconds. Results/Direct Plot/PSS: Choose pac, IPN curves, choose 1st Order Harmonic and 3rd Order Harmonic to 180MHz and 220MHz, respectively. Mark the output port of the mixer. What is the intercept point? Compare the result to the previous simulation. 8