Designing a L Band Oscillator with QUCS Studio. Volume (I) Issue 02

Transcription

1 Designing a L Band Oscillator with QUCS Studio Volume (I) Issue 02 Jose M. Campelo Ortiz. Page 1

2 SOMETHING LIKE A DISCLAIMER In the following hundreds of pages, or so, of this tutorial, the design of an L Band oscillator using QUCS Studio is presented. Once the document is considered as a whole, it is clear that there are many other ways of facing this problem, and it is sure that in case of having to do so, some of the assumptions made in this document are, at least, discussable. Some of the options taken, steps analyzed and solutions presented are not the most suitable ones to complete the task of designing and L Band Oscillator. Even it is possible that some of them are useless. But these decisions were taken in order to cover all the possible options that can come up during the design process, and to show how they can be handled using QUCS Studio. Of course, I am also sure that there are analysis that are not included in this document and they are very useful to solve issues presented during the discussions. On the other hand, it is not my intention to teach Microwave Design to anybody. It is exactly the opposite. After thirteen years working in the business I have learnt to be always ready for learning, from everybody in every time. I have done the things my way, but I am aware it is not the only way. The whole point of the following document is to encourage the use of QUCS Studio and to show that it is possible to use it in Microwave Designs, not only for low frequency applications. Finally, I would like to thank very much Michael Margraf for his corrections to the first issue of this document, and for finding a rather ugly mistake that has been quickly and dilligently erased from the face of the Earth. I hope this time, in this issue the number of these ugly mistakes have been reduced to a tolerable number. If you have read this document and you have any comment, suggestion, correction... and you want to share them with me, you can reach me at josemanuelcampelo@hotmail.com Jose M. Campelo Ortiz. Page 2

3 The following document presents the basic steps that can be easily followed by a beginner in the usage of QUCS Studio in order to design an oscillator capable of working in the L Band frequencies. The activities that involve the design of an oscillator will be commented in the following points, here after: 1) Choosing the transistor. It is the most important element of the oscillator. It will be essential to the design to chose the best option available. 2) Choosing the resonant circuit. If the transistor is considered the most important element in the oscillator, (that can be the object of an argument for sure) in the second place it must be considered the resonator. There are several structures that can be studied to perform as the resonator circuit of the oscillator and they will be reviewed during the design process. 3) Choosing the topology for the oscillator. There are quite a few schematics that can eventually produce oscillator circuits. All of them with their advantages and disadvantages. One of them will be considered and analyzed for the present design. 4) Linear analysis of the Ideal Lumped Elements Oscillator. The oscillators at microwave frequencies can be divided into two different parts: the tank circuit and the resonator circuit. Both of them will be analyzed from the linear point of view, which will suppose the basic stage of the design. In this first approximation, the circuit will be considered to be composed by ideal lumped elements. 5) Non Linear analysis of the Ideal Lumped Elements Oscillator. Once the linear design is completed, it is necessary to verify the oscillation. It means that the design will need to be verified in terms of non linear analysis, testing the waveforms and the spectrum obtained from the circuit. As in the previous stage, the circuit analyzed will be composed by ideal lumped elemets. 6) Linear analysis of the Microstrip Lines Real Elements Oscillator. If the previous ideal design works at the desired frequencies, it will be necessary to consider the microstrip lines that connect the components of the circuit, and the real models of them. 7) Non Linear analysis of the Microstrip Lines Real Elements Oscillator. To conclude the design, as in the previous stage numbered as 5, it will be mandatory to verify the oscillation in terms of non linear analysis. Transient analysis will be used to get the most representative waveforms, and Harmonic Balance will be used to obtain the spectrum of them. This script presented before will be followed as the backbone of the present document. Jose M. Campelo Ortiz. Page 3

4 STAGE 1. CHOOSING THE TRANSISTOR. Several basic rules, that could be applied to many of the design issues in microwave circuits, will be analyzed to choose the transistor. They are the following: 1) Microwave Performances. They are the most relevant constraint to be considered. It is obvious that if the transistor does not meet the minimum requirements it will be useless. 2) The design information available. It is necessary to have all the design information that is possible to gather in order to assure the most accurate results from the simulations. The ideal situation is to have scattering parameters for numerous biasing conditions, and a SPICE model for the non linear analysis, verified against the mentioned scattering parameters 3) Availability of the component. Everything mentioned in the two previous points will be useless if the chosen transistor is not available in the commercial vendors. 4) Price. Finally, if the price is not sensible... Many different models of RF transistors can be considered. One of them is the BFR93A. It is a model manufactured by several semiconductor manufacturers and its performances meet the requirements to design a L Band Oscillator. The following figure, shows a summary of the main features of this transistor. It is a transistor in a plastic SOT-23 package. That ensures low occupation in the eventual layout. The RF typical performances are summarized in the following figure: Jose M. Campelo Ortiz. Page 4

5 The figures in the tables offer the clear conclusion that the transistor was manufactured to work at frequencies near to 1 GHz. Since the aim of this design is to get an oscillator able to work at 1200 MHz the transistor can be suitable for the task. Jose M. Campelo Ortiz. Page 5

6 Regarding the technical information necessary for the design, in the case of the BFR93A, there is plenty of it in the NXP website or in the Infineon one. There is a SPICE file, which is mandatory for the non linear analysis of the design, and several scattering parameter files, that can be used for testing the previous SPICE model and for the linear analysis of the circuit. The best of everything is that the SPICE models offered by the two vendors are different. At first sight that could be a problem, but in practice it is not. One of the tests that must be done regarding the SPICE models, is to check if they match the scattering parameters that are also available from both vendors. Usually, non linear models, like the SPICE model, are obtained from the scattering parameters measurements. So, they should reproduce the scattering parameters biased in the same conditions. That analysis will be performed later in this document. Finally, in terms of availability, the transistor can be found in the stock of most of the commercial vendors websites, and at a reasonable price. So, the transistor selected will be the BFR93A. Jose M. Campelo Ortiz. Page 6

7 STAGE 2. CHOOSING THE RESONATOR. It is well known that the oscillators are composed by two main parts: The tank circuit, which is the part of the circuit that amplifies the oscillation once is generated during the start up of the circuit. The resonator, which is the block that filters and feeds back the signal from the initial oscillation that is primarily originated due to the white noise that are always present in the electronic circuits. There are several basic structures that can act as a resonator. The key in this issue is the frequency. There are elements that actually perform as resonators at high frequencies that are useless at lower frequencies. The same idea applies to those structures that are used in low frequency bands, that are another thing at high frequencies. Taking into account that the oscillator, that we want to deal with for the design, will be design to work in the L Band of frequencies, (more precisely around 1200 Mhz) there are structures that can not be even considered. The Dielectric resonator, for example, is the first one to be eliminated from the list. Dielectric resonators are the best option for oscillators working at really high frequencies. If we want to design an oscillator working at 4 GHz of further, this would be the best solution. Dielectric resonators offer the best performances in terms of phase noise, and stability. The main problem for considering dielectric resonator for the present design is the availability. They are not easy to purchase in the commercial websites. The size of the piece could be another problem, but here the thing is that they are not easy to get. The coaxial resonators are other option for oscillator design. The pros and cons that goes with the coaxial resonator are very similar to the ones commented before for the dielectric resonator. So, for the present design, it is not an option Jose M. Campelo Ortiz. Page 7

8 It is clear that we need a cheaper and available solution for the resonator. The cheapest one, maybe, is the one that consist on making the resonator from lumped components. The idea is to get a commercial and high Q capacitor and the same with an inductor, and making with both the resonator circuit. This solution will be analyzed later in the present document. There is another option that should be considered and it will, during the design process. One interesting type of resonator can be made using microstrip transmission line. One opened or shorted transmission line will resonate and the idea is to design it for resonating at the frequency needed in our case. The most interesting of the pros of the microstrip resonator is the cost. It is included in the cost of the PCB. Another interesting advantage is that it is possible to tune with a very simple method that will be analyze in following chapters of this document. Jose M. Campelo Ortiz. Page 8

9 STAGE 3. CHOOSING THE TOPOLOGY FOR THE OSCILLATOR. There are many different oscillator topologies that have been analyzed in the technical literature. Colpitts, Hartley, Clapp, Meissner, Pierce Even, each topology can work in different ways depending on what terminal of the transistor is used as the common one. There is a common base Colpitts topology, a common colector Colpitts topology, and a common emitter one. In this way, many of the other topologies mentioned before will work the same way. It is not the aim of this document to discuss all of them. The objective is to focus just in the design process. However, two different topologies will be used for the design. The first topology that will be considered will be the Colpitts. This is one of the most known and documented of all the available. Next figure depicts the basic structure of the Colpitts topology: As it was said before, this Colpitts topology can be presented in three different ways depending on what terminal is used as the common one. In the previous figure, the common colector Colpitts topology is presented. But it is possible to design the oscillator using the base terminal of the transistor as the common one in the network. This situation will be analyzed later on this document. Jose M. Campelo Ortiz. Page 9

10 The other topology that will be used will be the Vackar one. It is not the most famous one, but the performances that can be achieved using this topology are really interesting. The topology is as follows, in the following figure: As it was said before, there are a lot of other different topologies. But the point of choosing these two topologies commented before in this document is to present two of the most used methods for analyzing oscillator networks, and to show how these two simulations can be performed using QUCS Studio. Jose M. Campelo Ortiz. Page 10

11 STAGE 4. LINEAR ANALYSIS OF THE IDEAL LUMPED ELEMENTS OSCILLATOR. The first step to be taken in the process of analyzing an oscillator circuit from the linear point of view is to get the linear model of the transistor, which is, in fact, the core of the design. The linear method of analyzing non - linear behaviors, is always a good starting point. At least a good forward step. Non - linear equations and models for the transistor are quite difficult to handle. So, linearizing the transistor analysis makes the solution simpler. If the case was the analysis of a capacitor or a resistor, the idea should be similar to the situation of analyzing a transistor. In the case of those passive components, the steps will be the following: 1. Search for the scattering parameters of the element in the website of the manufacturer or some analogue place. 2. Replace the ideal model of the element in the schematic with its equivalent scattering parameters file. 3. Perform the analysis. In the case of the transistor, the first step arises a problem. According to the schemas of the topologies shown in the previous figures, the oscillators (and amplifiers and many of the circuits that use transistors) work with one of the pines connected to ground, but not all of them use the pin that normally is connected to ground when the manufacturers measure the scattering parameters of transistors. Nearly all the times, the transistor is measured in a common emitter configuration. That is a problem because many of the most used topologies in oscillators need the transistor working in other configuration different from this common emitter configuration. Technically speaking, the problem of using the common emitter configuration for the analysis of a Colpitts oscillator, for example, is that the emitter in the circuit is not grounded in terms of signal. Jose M. Campelo Ortiz. Page 11

12 Neither in terms of DC. In the Colpitts topology, the emitter is connected to an impedance different from 0, both in AC and DC. So it would be a mistake (a big one) to use the common emitter configuration scattering parameters for a Colpitss design. And, what about the other two transistor configurations? If the scattering parameters were measured in the proper configuration, they would be valid for the design process. But normally (90% of the times even more), as it was said before, the scattering parameters available for the transistor are measured in common emitter configuration. One solution for this situation is to dig into the technical documentation and papers, and find something very elegant and theoretic. There is a way of getting a three port scattering parameter file from the two ports one. I have not tried this solution yet. It would be a fantastic theoretic work to do. No doubt it is useful. But in this case, there is, at least, one better and easier solution. And this is to refer the common port in the scattering file box, to the needed point. This option is implemented in QUCS Studio. There is no need to make this calculations because they are implicit when the reference port is connected to the node in the schematic. Another real solution to this situation is to use the non - linear model. Obtained from this non linear model, it is possible to get information for many different bias point in the transistor, and with Jose M. Campelo Ortiz. Page 12

13 the configuration needed each time. For doing so, there is something very important to do and very easy to understand. It is mandatory to test the non-linear model versus the scattering parameter files available and mentioned several times before. It is easy to understand that, if the non-linear model is not representative of the actual model, it will not be very useful actually. Being representative means to be able to reproduce the scattering parameters curves obtained from the non linear model under test. If both curves are reasonable similar the model is good. Otherwise, there is another problem. So, how can it be tested a non - linear model?. The process is the following: 1. To import the non linear model in QUCS Studio. Normally, the non linear model available is delivered in a file where all the parameters for the transistor model are included with the SPICE format. In QUCS Studio it is possible to import this kind of file. In this way, only in one step, it is possible to use the model of the transistor. The steps are the following: 1) In the main menu click on Project Import Data Jose M. Campelo Ortiz. Page 13

14 Another windows will pop up. In this windows there are two text fields. In the one labeled as Input File it will appear the name of the.cir file that it is going to be imported to the QUCS Studio browser. In the Output File text field it will appear the name of the new QUCS Studio schematic where we get the translation of the.cir file that we want to import. Going to the Browse button of the window, we can navigate to the folder where the.cir file is located. Once selected, the text filed Input File shows the path to the.cir file: Jose M. Campelo Ortiz. Page 14

15 After doing that, it is only a question of converting the file. Clicking in Convert button of the main window Convert Data File and the task will start. At this stage, it is not strange getting an error and failing in the process. Depending on how you get the.cir file, it is possible to find errors in the conversion. SPICE models of the devices are well known and they are spread all over the internet, but there are parameters in those descriptions that are not understood by QUCS Studio. Jose M. Campelo Ortiz. Page 15

16 The first time I tried a conversion of a BJT SPICE Model I got this error message: In this case it was the conversion of the BFR93A BJT SPICE model. There is a parameter included in the description that provokes the problem. It is the IRB parameter. If you look for the definition of this parameter in the official SPICE user's guide and reference manual, (Michael B. Steer, ed 1.3 July 2, 2007) is the following: This parameter is not one of the most important among all the parameters that defines the BJT model in SPICE, so the best option to proceed in this case is to remove the definition of the IRB in the SPICE file that we are trying to convert. Note. This parameter will be included in future versions of QUCS in the BJT model. In this other case, I tried to import the NPN BJT SPICE model of the ZXTN19100CZ. Jose M. Campelo Ortiz. Page 16

17 The result obtained for the importing process of this.cir file, was the following: In this case, there are six different parameters that provokes a problem in the importing process. Consulting them in the SPICE User guide mentioned before, there are three of them that do not even exist for the BJT SPICE model description: GAMMA, RCO and QUASIMOD. GAMMA parameter exists for the definition of the MOSFET, but RCO and QUASIMOD are not referenced in the manual at all. The other three parameters, TRB1, TRC1 and TRE1 are defined as follows: These parameters are relevant if you have to consider the effect of the temperature in the design, which is something that happens quite often. In this case, the omission of these parameters will lead to a lack of accuracy of the model. But the procedure if this transistor is needed for the design is the same as before. They have to be removed from the list of parameters before importing the.cir file. Jose M. Campelo Ortiz. Page 17

18 Coming back to the BFR93A.cir file, once the IRB is removed from the model contained in the.cir file, and the process is finished, a new schematic will appear in the project browser of QUCS Studio. In order to use this circuit in the proper way, it is necessary to remember the structure of the.cir file, and what kind of things were contained in the file. In this case, it is not only the NPN BJT model of the transistor. In the SPICE description, the effect of the package was included in the model. Something that is really important and useful for RF simulations regarding the accuracy of the results. In the structure of the.cir file the SOT-23 parasitic model is taken into account by means inductors and capacitors. That is why we find the nets connected to the transistor itself and other nets connected to the ports. Working only a little with the elements resulting from the import process the non linear model of the BFR93A is ready to be used. Just for clarification, the name of the ports have been changed according to the SPICE model. (Click on the right button over each port, we choose Edit Properties and the name can be edited) Jose M. Campelo Ortiz. Page 18

19 This group of elements, now included in QUCS Studio in one schematic, can be used as a new element. QUCS Studio allows you to create new symbol for a schematic and after then, it will be available for a new design. How can we get a symbol for the schematic? Click the right button over the schematic containing the model and select Edit Circuit Symbol Jose M. Campelo Ortiz. Page 19

20 Just after clicking on Edit Circuit Symbol a basic rectangular symbol appears in the window. This basic shape can be easily altered. Got to the tabs on the left side of the project navigator window and click on Components. The only set of components available in the combo button in the symbol editor mode is the Paintings Basic geometric figures are available for painting almost any symbol that you can imagine. All the shapes can be edited (right button of the mouse over the shape and choose Edit Jose M. Campelo Ortiz. Page 20

21 Properties ) in terms of color, width, length so it is very easy to get the symbol of a transistor, like the one shown in the previous figure. Once the symbol is finished, each time you drag and drop the schematic, where the symbol has been edited, to a new schematic, all the elements defined in the original.cir file can be handled like a unique component, with the symbol previously designed. 2. To import the linear data for the transistor. Once the non linear model is available in QUCS Studio, the next step is to include the scattering parameter files. The process is described hereafter: For the scattering parameter file, it can be used the element dedicated to this task. (See the figure in the next page) 1.- In the tabs in the left side of the screen select Components. 2.- In the combo just above the window of the elements select devices. 3.- Among the elements displayed, it is the S-Parameter file. Dragging and dropping the element it will be available in the working space of the schematic. Jose M. Campelo Ortiz. Page 21

22 For including the desired S-param. File it is necessary to edit the element: 1.- Click on the right button of the mouse and select Edit Properties Jose M. Campelo Ortiz. Page 22

23 2.- In the menu that appears, select Browse and in the windows that pops up just immediately, look for the S parameters file that you are interested on: 3.- After select Open in the last window, the Edit Component Properties window will look like the following: Jose M. Campelo Ortiz. Page 23

24 After selecting the button Apply the file will be included in the element and it will be available for the simulations. Just to clarify, the symbol of the S parameter element can be edited. It can be selected one more suitable by doing the following: 1.- Right button of the mouse over the element S param. in the schematic 2.- Click on Edit Properties and the Edit Component Properties will appear in the screen 3.- In the options window placed in the left, go to Symbol and a combo will be available in the right side of the window. In that combo it is possible to choose among several pre-defined symbols, like FET, coil, capacitor or BJT, which is (obviously) the best this time. (See the next figure in the following page) Jose M. Campelo Ortiz. Page 24

25 After clicking in the Apply button, the proper symbol will appear in the schematic 3. To build the schematic for the comparison. The scattering parameters files contain information regarding the small signal behavior of the transistor. The idea is to reproduce the scattering parameters obtained from the non linear model of the transistor and compare them to the ones archived in the scattering parameters files used as reference for the test. That is what is needed to be built in the schematic where the comparison is made. The transistor must be biased in a specific point, defined by a collector emitter voltage and a collector current. For doing so, it is necessary to include voltage and current sources, which are necessary to meet the DC requirements (the bias point), and decoupling elements to only consider the transistor itself when the small signal analysis is performed. The schematic must be as follows: Jose M. Campelo Ortiz. Page 25

26 The idea beneath this schematic is the following: the transistor is biased by means ideal DCBlocks, C1 and C2 in the schematic, and an ideal DC Feed, L1. These elements provide the biasing for the transistor without interfering in the AC response. They are needed to reproduce the situation which the real transistor where measured in, the situation which the S parameter file was obtained in. The elements included in the previous schematics can be found in the following locations: 1) The non linear model for the transistor is something that was obtained before. It is included in the Content label of the project as a file, with the name that was chosen when the.cir file was imported. Dragging and dropping the file from the project tree viewer in the left side of the window, to the schematic window, the element will appear. Jose M. Campelo Ortiz. Page 26

27 2) The rest of the elements included in the schematic are components included in QUCS Studio. So in this label of the project tree viewer is where they can be found. a) The ideal elements for biasing the transistor can be found in the Components label, choosing in the combo box, located above the project tree viewer, the lumped components Jose M. Campelo Ortiz. Page 27

28 b) The sources that can be seen are available in the sources option included in the combo box: c) The current probes can be found in another option of the mentioned combo box, the devices one. d) Finally, the element that allows to include the scattering parameters in the schematic, can be included as it was in the previous paragraphs. Jose M. Campelo Ortiz. Page 28

29 4. To analyze and to compare the results. After building the schematic, it is time to get results. QUCS Studio allows many different types of analysis. The one needed now is the scattering parameters analysis. This type and many other can be found in the same Component label of the project tree viewer, choosing simulations in the same combo box as before: All the elements needed are already included in the schematic, and now, it is time to get the results. The scattering parameter file contains information valid for a determined frequency bandwidth. This should be the bandwidth specified in the S parameter simulation box included in the schematic. The format of the scattering file can be consulted from QUCS Studio. Clicking on the right button of the mouse over the scattering parameter file element, the following window will pop up: Jose M. Campelo Ortiz. Page 29

30 In the emerging window, click on Edit and the scattering parameter file will be opened as another window available in the working area of QUCS Studio This file informs that the frequency bandwidth used for the measurements is from 10 MHz to 3000 MHz. This will be the bandwidth specified for the S Param box in the schematic. Jose M. Campelo Ortiz. Page 30

31 Once everything is set up, the schematic can be analyzed. The first of all is to analyze the biasing point. This can be done in two different ways. 1. One, is to include a dc simulation box from the simulations as it was explained before, and name the nodes in the schematic where the voltage is going to be consulted. Naming the nodes means to put a name that, after the simulations, can be recognized and invoked in the results window. This step can be done using the element remarked in the following figure with a red square. After that, current probes can be included in the schematic in the relevant branches of the circuit. Finally, the DC analysis will be performed by pressing the wheel in the toolbar. This wheel will perform any kind of analysis included in the schematic. It must be taken into account that only one type of analysis can be active each time in a schematic. Jose M. Campelo Ortiz. Page 31

32 Note that there is only one simulation box activated in the schematic. Also take note that the collector node of the transistor is named as COLECTOR. After analyzing the circuit, the results window will appear, and it can be included a Tabular graph where all the voltages of the named nodes and all the current probes can be included. This is what the following figure tries to depict: Jose M. Campelo Ortiz. Page 32

33 2. The best of both is this one. Next to the wheel in the tool bar is located another wheel. This one has the letters DC over itself. This is a special wheel that will work for getting the DC values in the schematic. That means that pressing this wheel will make appear over the nodes and the current probes included in the schematics the corresponding values. That can be seen in the following figure: In this case, this wheel only works analyzing the DC values. All the nodes of the circuit will be shown in this DC analysis. There no need to name all of them. This is Jose M. Campelo Ortiz. Page 33

34 one of the advantages. Another can be the possibility of having a simulation box different from the DC one, and, at the same time, the DC figures for the schematic can be consulted. It is time to test the non linear model. Once the bias point is set for the transistor, the scattering parameters can be analyzed. The results are the following: In the previous figure the four S parameters of both, the non linear model, and the S parameters file, are shown. The first thing that seems relevant to be remarked is the great resemblance between the results obtained for the non linear model and the scattering parameters. It is true that this resemblance is poor in the case of the S22, but for the rest of the parameters it is really remarkable. If we had to decide the quality of this non linear model under test only taking into account this bias point it would be sensible to conclude that the model is valid, because of the great resemblance mentioned before. But in this case, there are other scattering files that can be used for testing the non linear model. This was the next step. Other two different bias points was tested and the results where almost the same to the first bias point analyzed. This means that the non linear model is able to reproduce the scattering parameters of several bias point fo the transistor. So, it is clear Jose M. Campelo Ortiz. Page 34

35 that the non linear model is fully valid for designing. It will be used as the base of the design process. NOTE. There is another analysis that is very useful to test a non linear model. There are a set of DC curves that are well known for bipolar transistors which are the collector current curves versus collector emitter voltage, maintaining the base current as a constant: This curves can be reproduced in QUCS Studio obtained from the non linear model. The schematic for doing so is very simple. It is shown in the following figure in the next page. The only thing that is necessary and it has not been presented yet is the Parameter Sweep box. This element is designed in QUCS Studio for sweeping variables. It is located in the label Components of the project tree viewer, choosing in the combo box the option simulations. Among the other type of analysis already presented in this document, it can be found the Parameter Sweep. For getting the type of curves that we are searching, two instances of this box must be included in the schematic. It is because the current collector is obtained sweeping the collector emitter voltage and taking into account one particular value of the base current. So, for each value of the VCE voltage, the base current IB must be swept. It is a double swept and that is why two boxes are needed. Jose M. Campelo Ortiz. Page 35

36 The results are very useful for biasing the transistor. These are the following: Now it is time to focus on the design, once it is clear that the tools available are suitable for the task. Jose M. Campelo Ortiz. Page 36

37 The first topology that is going to be analyzed is the Colppits. This topology will be used to present the main steps that needs to be carried out in order to design an oscillator using the Negative Resistance method. This method is well known and described in the technical literature. Therefore, regarding this document, it is only a question of reminding the main points: For the analysis, the oscillator circuit is divided into two different parts. The tank circuit, which is the part where the transistor is included and it is responsible for supplying the energy for the oscillation, and the resonator which is the part that defines the oscillation frequency. 1. The theory establishes what are the conditions for a network to oscillate. The following expression lead to obtain the quite famous equations of the negative impedance criteria for designing oscillators. If we consider the two separate building parts, the tank circuit and the resonator, and if we set that the input impedance of the tank circuit is ZTANK and the input impedance of the resonator is ZRES, the oscillator composed by the union of this parts will oscillate if the following equations are met. 2. Let's consider the Kirchoff law, regarding the voltages of a closed network. The sum of all voltages must be equal to zero (V TANK +V RES )=0 (Z TANK + Z RES ) I =0 Jose M. Campelo Ortiz. Page 37

38 Connecting both parts, and considering the steady state, the oscillation will persist after the start up if the current I in the equation is not equal to 0. (Z TANK + Z RES )=0 Let's consider R as the real parts, and X as the imaginary part, the previous equation can be written: { RTANK + R RES =0 X TANK + X RES=0 } For passive loads, RRES is always bigger than 0; so: RRES> 0 RTANK< 0 Regarding the imaginary parts of the impedances, one must the complex conjugate of the other one. In terms of admittances, this equations can be re-written and the criteria will be the same. It is important to remark that this conditions summarized in the previous equations are valid in the steady state of the oscillation. But the critical moment for the circuit is the start up. When the oscillation is just beginning. It is well described in the technical literature. In order to enhace the first response of the oscillation, the value of the negative resistance of the tank circuit must comply with a determined amount. Jose M. Campelo Ortiz. Page 38

39 RRES = RTANK 3 The compliance of the previous equations is necessary but not sufficient. The analysis must go one step forward. For the oscillation to be stable, it is necessary to meet the Nyquist criterion. 3. The Nyquist criterion is a stability test for time invariant linear systems. It is based on the complex analysis result known as Cauchy s principle of argument. By applying Cauchy s principle of argument to the open-loop system transfer function, we will get information about stability of the closed-loop system transfer function and arrive at the Nyquist stability criterion. For a clasic feedback system the closed-loop transfer function is given by the expression: M (s)= XO= G( s) 1+G( s) H (s) G( s) X 1+G( s) H (s) I The transfer function of a generic feedback system can be written in the form shown in the previous equation where the X values are generic input or output amplitudes, G(s) is the gain function, and H(s) is the feedback function. The Nyquist stability criterion for such a system is as follows: For a stable open-loop transfer function, G(s) H(s), the closed-loop system will be unstable if the point (- 1,0) of the s-plane is encircled at least once by the polar plot of G(jw) H(jw) for - < w <. Next figure shows a microwave system which can be described in a manner analogous to the last equation. Jose M. Campelo Ortiz. Page 39

40 Where ZIN is ZTANK and ZL is ZRES. Solving the flow graph of the previous figure, the expression obtained is as follows: a L= a N Γ I 1 Γ I Γ L Using the notation referring the tank circuit and the resonator, the expression will be as follows: a L= an Γ TANK 1 ΓTANK Γ RES There is another and more intuitive way of getting this expression. The network to be analyzed is as follows: (the subindex TANK y RES replace by 1 and S to simplify the equations) Once the steady state is achieved there is a standing state wave in between the two blocks that compose the oscillator. Let's assume that we can monitorize the reflections of the waves among this two blocks. When the oscillator starts-up, the first reflection between the blocks sets this equation valid: a1=bs A portion of a1 is reflected because of G1 b1=γ1 a1 Γ1 b S a S=b 1 as=γ1 b S Jose M. Campelo Ortiz. Page 40

41 Since: b S=Γ S as Γ S Γ1 b S Therefore: a1 '=ΓS Γ1 b S This is a new term to be added to the first one. a1=bs + ΓS Γ1 b S But this second rebound of the first signal, also is affected by the reflection coefficient G1. The expression is calculated similarly to the previous one, and the result is the following: a1 ' '=(Γ S Γ1) ΓS Γ1 b S ( ΓS Γ1 )2 bs Then: a1=bs + ΓS Γ1 b S +(ΓS Γ1 )2 bs So, considering the n rebounds in between the two blocks can be expressed as the sum of a geometric progression, as it can be seen in the following equation: a1=bs + ΓS Γ1 b S +(ΓS Γ1 )2 bs +(Γ S Γ1)3 b S +...+(Γ S Γ1 )n b S Each term of this geometric progression (or geometric sequence) is the result of multiplying the previous one by a constant value non equal to cero, called common ratio. The general expression is the following one: a, a r, a r 2,a r 3,... a r n There is an expression that allows to calculate the sum of all this terms. It is the one hereafter; n a+ a r +a r 2 +a r a r n a r n 0 a (1 r n) 1 r So the previous expression for a1 can be re-written as: b S (1 (Γ1 Γ S )n) a1= b S (Γ1 ΓS ) 1 Γ1 Γ S 0 n n As all the reflection coefficients, G1 and GS are values which absolute value is less than the unity. So, the product of both, will also be less than the unity. Jose M. Campelo Ortiz. Page 41

42 It is clear that a value less than one raised to a large number tends to be zero. Mathematically, we have: lim (Γ1 ΓS )n=0 n So, eventually, the expression that is obtained for a1 is the following: a1= bs 1 Γ 1 Γ S Once the expression for a1 is obtained, it is very easy to deduce the expressions for b1 and bs: b1=γ1 a1 bs Γ1 1 Γ1 ΓS b S=Γ S b 1 b S Γ 1 Γ S 1 Γ 1 Γ S Now, the system can be described in terms of its closed loop response. Both blocks working together can be analyzed as a closed loop system, depicted in the following manner: The transfer function of the closed loop system can be obtained by the following equation: b S Γ 1 b1 1 Γ1 Γ S Γ1 = bs bs 1 Γ1 ΓS Jose M. Campelo Ortiz. Page 42

43 As it was set at the beginning of this short explanation regarding the Cauchy principle, both reflection coefficients depend of the frequency. The system described with this closed loop equation will be unstable if b S grows from some initial value when b1 is zero. Assuming G1 represents a potentially unstable device (unstable only after connecting the resonator), the overall system will be unstable if the point (+ 1, 0) of the complex s plane is encircled at least once by the polar plot of G1 (jw) GS (jw) with - < w <. This indicates that the overall system has right half plane poles. The existence of these right half plane poles ensures the oscillation to grow up and to reach the steady state. How can it be tested this situation in a simulation?. Using the following set up depicted in the next figure: Jose M. Campelo Ortiz. Page 43

44 Now, the following step in the design is to analyze each block separately. The first one will be the Tank circuit. It is time to choose the proper bias point to get the best performances for the oscillator. Let's review some of the most important aspects that must be considered for the active part of the oscillator: 4. The transistor used must have the lowest noise figure possible. In this case, the transistor was already chosen. But the specified value in the datasheet regarding this parameter is good enough to meet a good performance. Low phase noise is one of the most relevant parameter in the operation of the oscillator. High current bias in the transistor will lead to a degradation of the phase noise because it will increase the 1/f noise in the system. However, a low value of this current will decrease the transition frequency of the transistor in a high amount. So, therefore, the use a medium power transistor biased in the medium range of collector current will offer the best performances in terms of phase noise. The power is another important performance for an oscillator. The higher the collector current, the higher the power will be delivered to the fundamental harmonic. But it is necessary to consider a trade off, regarding the parameters mentioned before. Even more when the rest of the harmonics produced besides the fundamental, will grow up too. Enough theory. Let s take all these concepts and make a circuit tank for the oscillator. The process of designing whatever circuit that it can be imagined consists of, basically, translating into real elements what it works in the theoretical plane. The aspect of a theoretical tank circuit is the following: Jose M. Campelo Ortiz. Page 44

45 The circuit represented in the previous figure is the ideal tank circuit built using the Colppits topology. As it can be seen, there are two different circuits that can be analyzed, depending on what type of configuration is chosen for the tank circuit: the common emitter configuration or the common collector configuration. Building up one schematic like the depicted in the previous figure is quite easy. All the elements that compose the circuit have been introduced previously in this document, so it is no necessary to describe the process again. In the schematic there are several components marked with red X s. This means that those components are not considered for the analysis. Those components marked with these red X s are virtually erased from the schematic. This is achieved by clicking in the tool bar the button that represents a bipolar transistor marked by a red X. At this stage of the design, the circuit is analyzed from the linear point of view. The expressions that will allow to progress in the design and that they will be analyzed come from the scattering parameters analysis. As it has said many times in the document, the tank circuit should provide the negative resistance that will allow the oscillator to start. So the first, and the most important analysis to be performed in the tank circuit is the input impedance. The real part of this input impedance is the one that must be negative in a wide range of frequencies. The bigger range of frequencies the better tank circuit we will have. The input impedance of a network can be evaluated using the following expression: Z TANK = Z0 (1+S 11 ) (1 S 11 ) where Z0 is the characteristic impedance of the circuit. S 11 is the scattering parameter measured at the input port of the circuit. Essentially, the S 11 is a reflection coefficient, and that is why it can be taken for the previous expression. It is clear that it is necessary to include a S Parameters simulation box as it was seen before in this document Jose M. Campelo Ortiz. Page 45

46 After that, we need the equations to get the input impedance of the tank circuit. For doing so, an equation instance must be included in the schematic. This element is located in the tool bars Dragging and dropping the equation element into the schematic, and double clicking on it, the Edit Component Properties window will pop up. In this window the equations can be edited. The equation is described by a field labeled Name, in the case of the input impedance it will be ZTANK, and another field labeled as Value where the relations among the variables that compose the equation must be written. There is another field labeled as Description. This one is optional and it can be used for describing the essence of the equation in a few words. This is very useful when the number of equations included in an instance of the element equation is really big. Jose M. Campelo Ortiz. Page 46

47 The basic elements for starting the simulation are already present in the schematic. The last point that must be covered is the bias point of the transistor. As we discussed before, the bias point should be with a medium level of collector current and a voltage that can be tuned for getting the best performances in terms of negative resistance. The schematic of the circuit should look like the following one: For getting the same results, QUCS Studio has several built-in mathematical functions that allow Jose M. Campelo Ortiz. Page 47

48 the designer to do the same in terms of calculating the input impedance of the circuit. It is very convenient to review all these functions and expressions to save time and headaches. Pressing F1 in the keyboard while QUCS Studio is on, shows the Help window like in many other software. Among all the different topics that are available to consult, the most relevant this time is the one called Mathematical Functions. Clicking on it, all the variables, constants, prefixes, functions and expressions available in QUCS Studio to analyze the circuits (depending on the type of analysis included each time) will be listed. The deepest knowing of this list will allow you to get better and faster results from the tool. In the case of the input impedance of the tank circuit, the function that saves time is rtoz(x,z) This function provides the impedance from a reflection coefficient taking into account the characteristic impedance that is considered in the circuit. In this case the Z0 is 50 ohms and the reflection coefficient is the S11 parameter, as it was said before. The final aspect of the equations using this function rtoz(x,z) is the following: If these expressions are equivalent to the other ones shown before, the results should be the same. And they are, of course, as it can be seen in the following figures: Jose M. Campelo Ortiz. Page 48

49 How can we get these graphics? In the schematic window, once everything is ready to start the analysis, (all the variables have the proper value, all the necessary equations are built, etc ) the button for running the analysis is located in the tool bars, next to the DC wheel that was used for the DC analysis before. After a blink of an eye (hopefully, if your computer is from this decade) a new tab just beside the schematic tab will appear, but this one with the same name of the schematic and ending in.dpl. This is the results tab. At the beginning, the first time the simulation is done, absolutely empty like the following one: As it can be seen in the figure, in the left side of the screen, what we are calling the project tree in, all the available types of diagrams are located to be dragged and dropped in the results tab. Jose M. Campelo Ortiz. Page 49

50 The most suitable for most of the curves obtained from the typical simulations is the Cartesian diagram. Dragging and dropping this Cartesian diagram in the results tab, the Edit Diagram Properties window will pop up. All the measurements that can be represented in the diagram are listed in the left side of the window, in the area marked as Dataset. Clicking over one of the expressions contained in the Dataset, and it will appear in the right side of the window, in the Graph listbox. At the same time, the expression selected will appear in the text field labeled as Graph Properties. This field can be edited. The expression contained can be manipulated using the equations and formulas cataloged as Functions for Diagrams only, explained in the list that appears when the key F1 is pressed as we seen before. (See page 49). This allows the designer to get more complex expressions, using as base the scattering parameters for example. Jose M. Campelo Ortiz. Page 50

51 Looking for the equations that were included in the schematic, it is possible to represent them in the graphs, and, eventually, test the performances of the tank circuit in terms of negative resistance. The scales of the diagram are set by default, but they can be changed. It is something very useful so, it deserves an explanation. The scaling can be done in two different ways. The first one is as follows: Double click over one of the diagram in the results tab, and the Edit Diagram Properties will appear again. In this window there are several tabs: Data, Properties, Limits Choose the tab Limits and the values of the scales for both axis of the Cartesian diagram will be available to be edited. Ticking the option manual as is depicted in the following figure, the text fields become ready to be edited. Jose M. Campelo Ortiz. Page 51

52 The second way of scaling the axis in the diagram is using the magnifying glass located in the tool bars. This one: Once is selected, the shape of the cursor will change. It will look like a magnifying glass (of course) and you will be able to zoom in any portion of the grid inside a diagram. The previous figure shows how can the limits of the diagrams be edited using any of the options Jose M. Campelo Ortiz. Page 52

53 explained. There is another item included in the diagram that is has not been introduced yet. It is the marker. Essential to all this diagrams stuff. To include one marker in a diagram, it is only a question of pressing the right button, as always. It is located in the tool bars. The following one: Each time one marked is needed, this element must be chosen. There is another feature that would be interesting to use in some cases. If the expression that is included in a diagram is complex and long, all the markers included in the diagram will reflect this length and can mess all the representation of the curve. The expression of the previous figure is the input impedance of the tank circuit. It is quite long, so each marker included in the diagram, will be rather big. Jose M. Campelo Ortiz. Page 53

54 There is a way of reducing the size of these markers. In the Edit Diagram Properties (remember that this window will show up when you double clicks over a diagram) there are several tabs. One of the is the one labeled as Legend When you click on this tab, the expression contained in the diagram (it is the same idea if there are more than one) will appear on the left side of a text field. In this text field the long and messy expression can get an alias. It is only necessary to fill this text field with the alias that best represents the expression. Once there is an alias, the diagram will appear a little bit more clear. Going back to the design of the tank circuit, it is time to focus on the specifications set for the oscillator. In this case, the negative resistance is quite large at low frequencies but it is not at high frequencies. This can be a problem, if the oscillator is to be designed at high frequency, as it is in this case. Jose M. Campelo Ortiz. Page 54

55 The next step is to study how to improve the negative resistance at high frequencies. The topology sets the most part of the bandwidth where the oscillator can be designed. This topology is limited not only by the performances of the transistor itself, but also for the elements that compose the tank circuit. In this case, the capacitors are quite relevant on the bandwidth achieved by the circuit. The feature that includes QUCS Studio that can be useful to study this bandwidth related with the values of the capacitors is the Parameter Swep. Let s analyze the effect of the capacitor CE1 in the negative resistance. CE1 is connected as follows: Sweeping the value of CE1 from the minimum commercial value, that can be easily obtained in commercial sites, to a maximum value of 5 pf leads to the following diagram: Jose M. Campelo Ortiz. Page 55

56 It is clear, as it could be expected, that the lower value of CE1 offers the best peformances in terms of bandwidth. This results are quite evident. But once the first relevant variable is analyzed and the results are clear, the features of the Parameter Sweep become more interesting. Taking into account the best value for one parameter under analysis, in this case the capacitor CE1, it is possible to sweep other parameters to get the best value for them, once the first one is fixed to the best possible. The objective of these analysis is to get the maximum negative resistance up to a frequency that ensure the oscillation in the frequency specified; 1200 MHz. Next analysis will be the dependency of the negative resistance with respect to the current base. The idea is to get the optimum value for the I B. It only a question of including more Parameter Sweep to the schematic, if the idea is to conserve the previous analysis, just in case. The schematic will be as the following one: Jose M. Campelo Ortiz. Page 56

57 Using this boxes of Parameter Sweep it is possible to determine which are the best values for the variables that really have an impact on the negative resistance. In this case, the current base I B, the inductor LE, and the feedback resistance RE. Jose M. Campelo Ortiz. Page 57

58 In this case, the effect at high frequencies of the current IB and LE is limited. But this is not the case for the RE. Next figure shows how the negative resistance varies versus the value of RE: There are some values of RE better for lower frequency bands and others for higher ones. It is quite useful the magnifying glass and more markers, to determine which values are in those bandwidths mentioned before. Jose M. Campelo Ortiz. Page 58

59 There are two different options that deserve further analysis. Both R E=30 and RE=150, offer approximately the same values in terms of negative resistance in the frequency of 1200 MHz so it will be interesting to test the rest of their performances. Finally, in this analysis focused on the improving of the negative resistance, is also interesting to examine what is the dependency on this feature with respect the inductor connected to the emitter of the transistor. The limits of the inductance must be chosen taking into account that inductance values lower than 1 nh are not usual, and higher than 20 nh can be near to the resonace frequency, making the inductor useless. The procedure must be the same as before. To use the Parameter Sweep box to sweep the LE value, as it can be seen in the next figure: The results are the following: Jose M. Campelo Ortiz. Page 59

60 It is important to notice that the rest of the parameters remain constant. Therefore, the R E has to be set to any of the two values analyzed previously. The curves presented in the last figure was set to 30 ohms. For the other value of RE, 150 ohms, the results are shown in the next figure: The effect of the inductance is less in this case than the R E equal to 30 ohm, as it can be expected. Therefore, this analysis determines the values of both parameters: RE and LE. Jose M. Campelo Ortiz. Page 60

61 Regarding the negative resistance, the best performances for the circuit are achieved using the R E of 30 Ohm and the LE of 20 nh. That will be the chosen parameters for the design. It is convenient to remark that if other performances were being analyzed may be the decision would be different. The power consumption of the circuit that includes the chosen elements is bigger than the other one. That is a very critical feature in many occasions, so that is why the decision could be different depending on the features privileged in each case. After the analysis of the circuit tank, the next step must be the simulation of the resonant circuit. Resonant circuits are based in a combination of a capacitor and an inductor and this will be the first approximation to the solution. 5. To analyze the basics of the resonant circuit another schematic will be necessary. To do that, in the main menu, we chose File New and another schematic will appear in the design window. In this new schematic, a basic parallel resonant circuit will be included. The following figures show the basic results that can be expected from a basic parallel resonant frequency. There is no much science in a parallel resonant circuit, so let s move on to the next stage. Jose M. Campelo Ortiz. Page 61

62 Jose M. Campelo Ortiz. Page 62

63 As it is well known, the resonant circuit sets the frequency for the overall oscillator. While the tankk circuit provides the negative resistance (eventually, the energy) necessary to initiate and sustain the oscillation, the resonant element selects the frequency of this oscillation. But, in order to get a voltage controlled oscillator, it is obvious that is mandatory to include an element that is able to change the frequency with a voltage applied. That is, a varicap diode. The first step, then, is to choose one varicap diode among those that are available in the market. The main constraint is, of course, its availability, but the second, and not less important is the information that is available regarding the electrical performances. More precisely, the availability of a non linear model, package model, etc One model that seems to be suitable for the task, is the following: The Infineon BB833 has a non linear model available in the website of Infineon. More precisely, a SPICE file modeling the die of the semiconductor, and also it is available the model for the package. It is included a file where it is contained the information regarding the frequency of usage for the model. It is valid up ot a frequency of 6 GHz. After downloading the file, the next step is to include the element among all the others available for Jose M. Campelo Ortiz. Page 63

64 the simulation in Qucs. The procedure is the same that was made for the transistor, but it will be described one more time. In the case of this diode, since the information is divided into two separate sources, the best way to proceed is to combine both files, the die model and the package model, into one unique SPICE file. The result is presented here after: * >>> SOD323 <<< (RF-DIODE-PACKAGE) * FILENAME: SOD323.TXT * (C) 2001 INFINEON TECHNOLOGIES AG * Version 1.2 June 2001 A.Boehme **************************************************************** * * CAC * (10) (2) * * * LAO * * A---LLL--+ (100) LCO +--LLL---C * LAI * +--LLL---A' CHIP * (200) (1) C' (2) * LAI nH CAC fF LAO 10 LCO nH nH **************************************************************** * PACK = NAME OF PACKAGE BLOCK, DEFINED AS 4-PORT * 1 = ANODE OF CHIP * 2 = CATHODE OF CHIP * 100 = ANODE OF COMPLETE DIODE IN PACKAGE * 200 = CATHODE OF COMPLETE DIODE IN PACKAGE * * Add Spice model or discrete equivalent circuit for chip * between terminals (1) and (2) Jose M. Campelo Ortiz. Page 64

65 **************************************************************** ********************************************************************* * Infineon Technologies Discrete & RF Semiconductors * * SPICE2G6 Model: Varactor Diode BB833 series (Chip model) * * Filename: D339_v3.txt * * Version: 3.0 * * Date: March 2003 * * Author: A. Boehme * ********************************************************************* * -Parallel-resistor R1 for a better reverse behaviour. * * -The temperature-dependence of the reverse breakdown voltage and * * the ohmic series resistance (parameter RS) are in SPICE2G6 not * * adaptable. * * -Parallel-capacitor C1 and very high value for VJ applied for a * * * better C-V curve approximation between VR=0.5 to 28V. ********************************************************************* D1 1 2 D1 R e9 C p.MODEL D1 D(IS=2.82p N=1.407 RS=0.096m XTI=3.0 EG= CJO=12.19p M=12.6 VJ=38.53 FC=0.5 TT=120.0n BV=32.0 IBV=5.0u).END To convert the SPICE file into something useful for QUCS, in the man menu, click on: Project Import Data In the window that pops up inmediately after it can be browsed the location of the SPICE file, and once is selected in the text fields, convert it into a schematic usable in QUCS. (See next figures here after) Jose M. Campelo Ortiz. Page 65

66 Jose M. Campelo Ortiz. Page 66

67 Once the circuit is imported, the equivalent circuit will be the following: After that, ports must be included in the design to build an element that can be handled by QUCS. Clicking on the right button of the mouse over the schematic where the model is contained (of pressing the F9 key on the keyboard) will allow to open the window for editing the symbol that will be linked to the model of the diode. The procedure for editing the symbol of the diode has been presented previously in this document. It will be not repeated because it is not essential (after all, the equivalent circuit can be used without editing the symbol) and it can be consulted in the previous explanation. Please refer to it, in case of being necessary. After the edition of the symbol, the equivalent circuit of the packaged diode will look like the following: Jose M. Campelo Ortiz. Page 67

68 The varicap diode is ready to be used. But, as it was done for the transistor, if it is possible to test the model of this element, it is a very good practise to do it. If the model does not fit the parameters depicted in the datasheet of the component it will not be useful for designing. In this case, the first feature to be tested in a varicap diode, should be the variation of the capacitance that presents the element versus the voltage applied to its terminals. Checking the mentioned datasheet of the BB833 the following curve can be found: Jose M. Campelo Ortiz. Page 68

69 It is the variation of the capacitance versus the reverse voltage applied, measured at 1 MHz. If the model of the diode is accurate enough, it should be able to reproduce this curve. The next schematic, is the circuit that can be used to test this issue: It consists of the diode biased to work in reverse mode. The way of biasing the element is very important because it is necessary that the elements of the biasing network do not interfere with the measurement. In this case, the voltage is applied to the diode by means a 10 KΩ resistor and a huge inductor of 10 H. This inductor is something unreal. It is not possible to get this kind of values for an inductor. But it assures that the biasing network will be totally transparent to the measurement. Since the frequency of the test is rather low, only 1 MHz, the value of the biasing inductor must be really high. The combination of the resistor and the inductor produces a really high impedance that, in terms of the test frequency, ensures that the biasing network is an open circuit. It doesn t exist in terms of the AC signal but it actually does in terms of DC biasing. The block capacitor or the schematic must be a very low impedance in terms of AC at the test frequency. This is why the value of this capacitor is also unreal, 10 Farads, as the biasing inductor. The analysis that has to be done for the schematic is based in the following steps: Jose M. Campelo Ortiz. Page 69

70 1. The varicap diode is essentially one capacitor. Ideally speaking the diode can be replaced by a capacitor. But in the real world, the model of a varicap is the following: 2. If the frequency is low enough, (and the diode with quality enough) the contribution of the parasitics of the diode will be negligible. And this is case for the on going test. The test frequency of 1 MHz is low enough to consider that the parasitics can be ignored. 3. One way of testing this approximation is calculating the input impedance of the schematic shown in the previous page. This input impedance working at 1 MHz is basically composed by the variable capacitance forming the imaginary part, and some parasitic resistance forming the real part. 4. So, the capacitance can be calculated following the next expressions: Z INP =Z 0 1+ S 11 1 S11 Z INP =ℜ(Z INP )+ ℑ( Z INP ) 5. Assumed that the imaginary part of the input impedance of the circuit is basically due to the value of the capacitance, this figure can be calculated from the next equation: ℑ( Z INP )= CVARICAP = ( 1 j w CVARICAP 1 ) j w Im(Z INP ) The simulation of the circuit presented previously offers the results for the capacitance of the varicap diode. Since the equations that calculates the real part and the imaginary part of the input impedance are included in the Equation box of the schematic, these expressions will be available to be included in Jose M. Campelo Ortiz. Page 70

71 the graphs of the results window: The real part, and the imaginary part of the input impedance is presented in the next figure: As it can be seen in the curve, the real part of the impedance is very close to zero, (so the assumption explained before is correct) and the imaginary part describes a curve that must be analyzed to extract the capacitance of the varicap. How can we obtain the curve of the capacitance versus the DC reverse voltage? Just follow the next procedure: Drag and drop in the results window a cartesian diagram. In the window that pops up once the cartesian diagram is dropped, go to the text field where the expressions are included and type the equation of the capacitance that was describe in the last discussion Jose M. Campelo Ortiz. Page 71

72 The curve obtained is the following: Jose M. Campelo Ortiz. Page 72

73 Comparing both curves, the one obtained in QUCS and the one depicted in the datasheet of the BB833, it can be affirmed that both are reasonably alike. Furthermore, they seem to be practically alike. That means that, in terms of capacitance, the diode model is accurate and it can be used in the design process. The next step is to verify the behavior of the varactor diode at high frequencies. The analysis performed before validates the usage of the diode at low frequencies. But for RF applications it should be demonstrated that the model is also valid. The manufacturer of the BB833, in this case Infineon, offers in its website scattering parameters for many biasing conditions of this element. Since the scattering parameters are available for this varicap diode, it is possible to test the model we are being dealing with at high frequencies. For this task, it is possible to base the schematic in the previous one. It is only a question of adding to the schematic the necessary element to use the scattering information: For the scattering parameter file, it can be used the element dedicated to this task. (See the figure in the next page) 1.- In the tabs in the left side of the screen select Components. 2.- In the combo just above the window of the elements select devices. 3.- Among the elements displayed, it is the S-Parameter file. Dragging and dropping the element it will be available in the working space of the schematic. Jose M. Campelo Ortiz. Page 73

74 For including the desired S-param. File it is necessary to edit the element: Click on the right button of the mouse and select Edit Properties. That will pop up the Edit Component Properties window. Jose M. Campelo Ortiz. Page 74

75 The scattering files that were obtained previously from the Infineon website are one-port scattering parameters files. It is normal because this is the usual configuration of the varicap diodes when they are used this way. The S parameters file element is, by default, set to be for two-ports scattering parameters files, while the varicap diode files are only one-port files. So, this must be changed. It is necessary to edit the suitable property: After editing the number of ports, and set this option to one port, the shape of the element in the schematic changes. One of the ports, of course, disapears. Jose M. Campelo Ortiz. Page 75

76 Once the number of ports are correct, it is time to choose the parameter file. Click on the Browse button and look for the folder where the scattering parameters files are. Once the file is chosen, the path to the file appears in the schematic It is time to test the model and compare it with the measurements contained in the scattering parameters file. Depending on the reverse voltage applied to the diode, it will be necessary to change the scattering file. Each file corresponds to one reverse voltage applied to the diode. Since the idea is to vary the capacitance of the diode from 0 volts to 6 volts (that is the available range of voltage obtained from the supply of the tank circuit) it will a good idea to test all the reverse voltages applied to the diode (in one volt steps, for example) if there are scattering files available. And there are actually scattering files from 1 volt to 30 volts. The test will be as following: In the equation component where the variable VD is defined, set the first reverse voltage for the test; 1 volt, to begin with. In the Browse property of the S parameters file element,,choose the file for the 0 voltage of reverse voltage: BU1V00U0.S1P Jose M. Campelo Ortiz. Page 76

77 Simulate the schematic. Remember: In the results tab that appear once the simulation is completed, add a three Cartesian diagrams: one for the S(1,1), the results of the diode circuit in the schematic, another for the S(2,2), the actual measurement obtained from the scattering file, and a third one, which will contain a mathematical expression for analyzing the accuracy of the model. It is just the mathematical expression of the relative error, taking into account that the real measure should be the value reproduced by the model: Error= (S (1,1) S (2,2)) 100 (S (2,2)) Jose M. Campelo Ortiz. Page 77

78 It is obvious that the minimum relative error goes with the best approximation. In terms of values, a relative error near to the 10% validates the model and can be considered valid for designing. If this process is repeated changing the VD from 1 volt to 6 volts it can be registered the relative error of the model for each step decided before. Focusing the attention to the band where the model must be used, the results for the relative error are summarized in the following table: VD Freq. (Mhz) Error (%) 9,85 11,6 14,1 19,8 29,4 33,3 Freq. Max Error (Mhz) Max Error (%) 10 12,6 15,1 20,3 29,5 35,4 BB833 It is clear that relative errors far beyond than 25% and, even worse, in most of the cases near the frequency of usage, are not affordable. This model, at least, offers many doubts of its suitability. If there was not other option, it would be a serious drawback for the design. The results could not be accurate because the model is not either. The best option, is to find another varicap diode with a more accurate model. Jose M. Campelo Ortiz. Page 78

79 Fortunately there are other options. From the same manufacturer there is another varicap diode that can be used for this type of applications. It is the BB857. For this varactor diode, the manufacturer also offers all the information that can be obtained for the BB833. Therefore the same validation process can be carried out the same way as it was done before. Once the model is included in the project, and all the scattering parameters and Spice model are available, the BB857 can be tested the same way. And, fortunately, in this case, the results of the testing are better than the previous BB833. The next table summarizes the comparisons between the model and the real measurements for the BB857: VD Freq. (Mhz) Error (%) 12,5 11,6 Freq. Max Error (Mhz) Max Error (%) 14,4 14,5 9, ,4 6, ,8 BB857 Among all the information regarding the specifications of the BB857 it is also available the curve of the varactor capacitance versus the reverse voltage applied to the diode. This was the first parameter to be tested for the BB833. For the BB857 it is necessary to do the same. Jose M. Campelo Ortiz. Page 79

80 Checking the values of both curves it can be seen that the approximation is quite good. Enough the expect good results in the simulations. The model obtained for the BB857 can be considered validated for the design task. Now it is time to get a valid resonator for building the voltage controlled oscillator. The schematic used at the beginning of this discussion, formed by a parallel of an inductor and a capacitor is useless. This network is fixed regarding the frequency. But it is useful to base a new design. It is a question of reproducing the performances of this very easy circuit, with another which the frequency can be varied in. The resonance frequency of the resonator element must be higher than the frequency where the tank circuit presents the maximum negative resistance if the aim is to have the oscillator working at this frequency. This is due to the equation that sets the condition for the oscillation: Z TANK + Z RES =0 The frequency range where the combination (the addition) of the ZTANK curve and the ZRES one that complies with the previous equation is always located at frequencies below the resonance frequency of the resonant network. It is not direct but, it can be understood if both curves are compared together: The only frequency range where the imaginary part of the previous equation can be zero combining both terms (tank and resonator) is located on the left side of the resonance frequency. The real part of the equation will be lower than 0 in order to comply with the start up condition of the oscillator. Jose M. Campelo Ortiz. Page 80

81 That means that the resonator must resonate always at a higher frequencies than the one specified for the design. And it was said before, the resonator circuit must be capable of changing the frequency by means a varicap diode. So a possible structure for this resonator could be the following depicted in the next figure: The idea beneath the schematic is composing the capacitor of the resonator with two varicap diodes connected in series and in parallel to both, the inductor. Why two diodes? The capacitance of only one is too big for the frequency range that is necessary to achieve. Two DC blocking capacitors are needed to bias properly the diodes and to block this DC component to avoid it getting out of the circuit. What frequency range can be covered with this design? That can be analyzed using S parameter simulation and the Parameter sweep, as it is shown in the next figure: Jose M. Campelo Ortiz. Page 81

82 The equation introduced allows to calculate the impedance of the resonator and, since the voltage of the DC source in the schematic is swept, the capacitance of the diodes change, and this impedance is varied in frequency. In the results window, this Z_RES, which is the name of the variable that calculates the input impedance of the resonator can be represented in a cartesian diagram looking as follows: It is clear that this schematic covers a wide range of frequencies, so it is perfectly usable for the application of the VCO that is being designed. Sweeping from 1 volt to 5 volts the voltage applied to the diodes, the margin of frequencies covered is huge indeed. It is time to put both blocks altogether. The circuit tank, and the resonator that have been analyzed in the previous pages. It is necessary to analyze the performance of the combination of both and to ensure the they will work together. Jose M. Campelo Ortiz. Page 82

83 Copying and pasting each blocks of the circuits simulated previously, it is easy to get a new schematic where all the next simulations will be carried out. The first analysis to be performed in the new schematic is to ensure that booth networks working together can comply with the fundamental condition for the oscillation. The one that was introduced in the previous pages: Z TANK + Z RES =0 In terms of admittances, the expression is almost equal to the impedances one: Y TANK +Y RES =0 If the entire circuit is to oscillate, both equations should be satisfied. This is a basic condition that needs to be complemented by further analysis. But this will be explained later. To perform these basic analysis it is necessary to introduce an equation item in the schematic, and then introduce the equations that define the impedance expression and the admittance one. The item will be as follows: Jose M. Campelo Ortiz. Page 83

84 Once this set of equations is available in the circuit, the expressions of the sum of impedances, or sum of admittances, can be displayed in the results window. They are the following: These curves are obtained setting a reverse voltage in the diodes of 1V. It is clear that nor the impedances equation, nor the admittances one, are strictily satisfied by the circuit simulated. The sum of the real terms of both expressions are not equal to zero. But this is indeed necessary to initiate the oscillation, as it was explained before in this document. It is something that is well described in the technical papers and technical literature. The initial condition for the oscillators to start up is the one analyzed in the circuit before. Although the equation sets that the sum of the real part of the equations must be equal to zero, and the same for the imaginary part, this situation is valid for the steady state situation of the oscillator. Once the Jose M. Campelo Ortiz. Page 84

85 steady state is reached this equations are satisfied. We can try another approximation for a better understanding. We can view an oscillator as an amplifier that produces an output when there is no input. Thus it is an unstable amplifier that becomes an oscillator. If we consider the oscillator as a conditionally stable amplifier, and instead of choosing load or source impedance in the stable regions of the Smith Chart, we purposely choose the load or source impedance in the unstable impedance regions, this will result in either G1 > 1 (reflection coefficient at port 1) or G2 > 1 (reflection coefficient at port 2). Having a reflection coefficient magnitude for sigma1 or G2 greater than one implies the corresponding port resistance R1 or R2 is negative. That is why the name for this type of oscillator was chosen in the first place. Choosing the load impedance ZL at the unstable region, we could ensure that G1 > 1. Then it is a question of choosing the source impedance properly so that G1 GS > 1 and oscillation will start up. Once the oscillation starts, an oscillating voltage will appear at both the input and output ports of a 2-port network. So it does not matter whether we enforce G1 GS > 1 or G2 GL > 1, enforcing either one will cause oscillation to occur (It can be shown later that when G1 GS > 1 at the input port, G2 GL > 1 at the output port and vice versa). R1 can be made negative by modifying the amplifier circuit (e.g. adding local positive feedback), producing the sum R1 + RS < 0. Usually a transient voltage that occur in the circuit, (normally the switching on of the circuit) or noise signal from the environment will form the seed in which the oscillation builts up. When the signal amplitude builds up, nonlinear effects such as transistor saturation and cut-off will occur, this limits the beta (b ) of the transistor and finally limits the amplitude of the oscillating signal. The effect of decreasing the beta of the transistor ( b ) is a reduction in the magnitude of R 1 (remember R1 is negative). This reduction takes place until the steady state is reached. The current through the transistor in the circuit increases during the start up period. Jose M. Campelo Ortiz. Page 85

86 The previous figure is the shape of the bias current of curve registered by simulation So, a more general way of expressing the requirements for oscillation to start-up and achieve steady state are the following: ℜ(Z TANK )+ ℜ( Z RES )< 0 ℜ(Z TANK )+ ℜ(Z RES )=0 ℑ( Z TANK )+ ℑ( Z RES )=0 ℑ( Z TANK )+ ℑ( Z RES )=0 Start up equations Steady State equations As it was mentioned in the previous theoretical point explained before, this question about the start up of the oscillation is really an issue. Experience shows that many times, the equations shown before are satisfied, everything seems to be ok and the circuit designed does not oscillate ever. It is time to use the Nyquist Criterion introduced in the page 43 of the present document, to analyze the oscillator. It is necessary to reproduce the set up depicted in the last figure in this page 44. The final aspect of the circuit to perform this analysis is shown in the next figure: Jose M. Campelo Ortiz. Page 86

87 The previous figure shows the complete structure of the oscillator, where several ports are included. The idea is to use the same circuit to perform more than one analysis. This is one of the most simple and, maybe, useful capabilities of QUCS Studio. Just choosing the option in the tool bar, it is possible to eliminate one component from the current analysis of the circuit but not from the circuit itself. That prevents the user from removing and placing components one and again each time that they are (or not) useful in the results. With the arrange of ports and straps of the circuit presented before, it is possible to simulate the performances of the resonator circuit, the performances of the tank circuit, and the behavior of both sub circuits working together. This is the case. Now, it is question of applying the Nyquist criteria. This is possible working with the circuit shown in the previous figure. The most relevant information that can be obtained is the plot of the expression G1 (jw) GS (jw) with - < w <. Jose M. Campelo Ortiz. Page 87

88 It is the following one: The type of graphic that must be used to represent the reflection coefficient as the way it is shown in the last figure is Locus curve included in the set of diagrams available: Jose M. Campelo Ortiz. Page 88

89 The conclusion of the simulation are clear. The idea is to test if the response of the reflection coefficient encircles clockwise the point (+1, 0) of the locus curve. If that is the case, the oscillations that will be initiated in the circuit will be sustained in the steady state. In other words; the circuit will perform actually as an oscillator. (See page 44 of this document for a little bit more technical explanation) Using the markers for the curves, it is very easy to prove that, with the increasing frequency, the curve encircles the (+1, 0) point of the diagram. And the best of all, the point is encircled clockwise. Jose M. Campelo Ortiz. Page 89

90 STAGE 5. Non Linear analysis of the Ideal Lumped Elements Oscillator Once all the linear analysis show that the circuit seems to be an oscillator, the next and final point is to get the waveform in the time domain. This will be the ultimate evidence of the design. If the circuit working all together oscillates, all the design process is a sucsses. To obtain the waveform, the Transient Simulation box must be included in the circuit. It is also necessary that some of the elements of the initial circuit are excluded (crossed from the schematic) and others included. The final aspect of the circuit will be the following: The elements enclosed by the green shapes are the ones that must be included in the simulation. Those enclosed by the red shapes, must be excluded. It is also necessary to label the node where the oscillation is expected. In the schematic, this node is labeled as OUT. That will be the way of referring the point in the result diagrams. The way of doing that is very simple. In the tool bars that are placed above the schematic, look for this symbol: It is something like the mathematical symbol for the addition with the letter N over something Jose M. Campelo Ortiz. Page 90

91 that seems to be a wire in the schematic. Pretty clear. Add a Name to a wire. OK. Let s do it. Click over that symbol and a hand will take the place of the cursor. Take this hand to the electrical node and click over it. A text box will appear over the schematic and it will be a question of filling it with the name of the node. OUT, for example. NOTE. The power source located at the output node labeled previously as OUT, must be edited to ensure that the contribution to the output signal of the oscillator is none. The amount of power that must deliver this power source must be set to -90 dbm and the frequency, far away from the one used for the design. In any case, the best option is to replace this power source for a 50 ohm resistor. Jose M. Campelo Ortiz. Page 91

92 After many failures in the transient analysis due to convergence problems, that can be analyzed later, the result after running the transient analysis simulation is the following: This result is very interesting for several reasons: 1. The shape of the waveform indicates that its harmonic content is very high. The squarer the signal, the higher content of harmonics. That is something that can provoke the analysis to fail. The convergence of the algorithm used for the calculations of the signals in the time domain can easily fail under these circumstances. In fact, the normal outcome of this simulation in this situation is a failure in the convergence calculations. 2. This failure in the convergence of the analysis is something quite normal. It is not a bug or a lack of QUCS Studio. Many other simulation tools will also fail in this situation. So, don t blame to the software it is really cool indeed!!! 3. This shape of the output signals informs that it is necessary to rethink some of the Jose M. Campelo Ortiz. Page 92

93 approximations made during the first stages of the design. Due to the high number of significant (in terms of power) harmonics that can be foreseen in the output signal, the results can not be trusted. Even more when it is necessary to control many of the parameters of the transient analysis to finally get the convergence in the simulation. Just think about the previous simulation. There are a lot of peaks in the signal very shortly spaced. The waveform is very peaky. So, to eventually achieve the convergence of the analysis, is necessary to set very short time steps to ensure that the ratio of change in the waveform under analysis is low enough to obtain the convergence. From one iteration to the following, the difference between the values obtained must decrease. But, sometimes, depending on the spectral content of the signal evaluated, this conditions can not be satisfied. From the perspective of the analysis, the options that are available to go through this issue are the following: Decrease the time step in the transient analysis. Whether increasing the number of points or reducing the time to stop the analysis, the overall effect will be the same. It can be done by double clicking over the Transient simulation box in the schematic and changing the options in the fields: Jose M. Campelo Ortiz. Page 93

94 Of course, the increment of the number of points, will affect directly to the time of the simulation. Change the method of integration of the transient analysis. There are six different methods of integration to solve the circuit. Depending on the type of signal that is evaluated, some of these methods are better than the others in order to get the convergence of the calculation. To choose the integration method, select the Properties tab in the Edit Component Properties window, and select one of the options in the combo box where the method is located. There are other options that configure the transient analysis. The convergence criteria can be changed to help to achieve a of the analysis. In any case, the information that provides the figure of the page 93 of this document, the signal obtained from the transient analysis, is very interesting. Even more than the signal itself, the difficulty in achieving the convergence of the transient analysis is the most relevant piece of information that can be collected from this simulation. This kind of signal is normally not acceptable as the output of an oscillator. Many harmonics and other Jose M. Campelo Ortiz. Page 94

95 intermodulation products can not be delivered to any other circuit. It is necessary to fix the problem. Instead of filtering the signal, which is equivalent to add at least one filter, and even an amplifier buffer, the solution must come from the circuit design. In the topology there is a way of controlling the modulus of the negative resistance. The ouput capacitor labeled in the schematic as COUT controls the negative resistance of the tank circuit. To analyze the relation between the value of COUT and the negative resistance of the oscillator, the Parameter sweep box will be of utility. Let s include the Parameter sweep box in the schematic and let s program a sweep for the COUT value. The box will appear as follows: The purpose of this analysis is to determine what are the changes in the equations that were presented in this document in the page 84 and 85. The results from this swept are the following shown in the next diagram: Jose M. Campelo Ortiz. Page 95

96 The increasing of the COUT means a significant reduction in the modulus of the negative resistance. From an absolute value of more than 100 ohms, to a range of 30 to 40 ohms. In terms of the impedance analysis, the results are the following: In both dimensions, in the impedance domain, and in the admittance domain, the reduction in the Jose M. Campelo Ortiz. Page 96

97 modulus of both expressions, the negative resistance, and the negative impedance, will ensure a reduction of the overall power delivered to the load when the whole oscillator is analyzed. For obtaining both previous figures, the schematic that was simulated was the following: As it can be noticed, this schematic is the same that was used for the simulation of the transient analysis. It is just a combination of the signal ports, and enabling or not the proper elements in the circuit, what allows to obtain results from different types of analysis. The previous diagrams of the impedance and the admittance show the compliance to the condition that is necessary for the oscillation to occur. But, as it has been explained before in this document, this condition is not sufficient. So, next step must be to sweep the COUT and obtain the results of applying the Nyquist criteria. In other words, the plot of the expression G1 (jw) GS (jw) with - < w <. Hereafter, the schematic to simulate: Jose M. Campelo Ortiz. Page 97

98 And the results: The good news are that for all the evaluated values of COUT, every one of them encircles the key point (+1, 0). It is also interesting that the changes in the curves are relevant for the first values of the programmed swept. So the effect of the variations in COUT is not lineal. Checking the results it easy to note that varying COUT far from 10 pf seems useless. Combining the results of this last analysis, and the previous one, choosing 10 pf for COUT would work out our problem of the spiky signal. The next step is the transient analysis; as the following: Jose M. Campelo Ortiz. Page 98

99 The result int the OUT node, labeled in the first transient analysis performed, is the following: Definitely, we have an oscillation. And it is a stable one. It is not rare to get an initial oscillation that fades away with time. This is not the case. The oscillation is stable in the steady state. At least, it seems that 2 us is enough to consider this time as the steady state. The problem of searching the actual steady state, is that it is really demanding in computational resources. Just to see how demanding is a further transient analysis in terms of simulating time, it is a question of double the simulating time, doubling the number of points of the analysis too, just to preserve the convergence conditions of the analysis. Jose M. Campelo Ortiz. Page 99

100 This time, the signal obtained in the node OUT is the following: Clearly, this time, the steady state is reached without any doubt. Examining the envelope of the signal obtained during the simulation, the difference between the transient period of the signal, and the steady state, can be easily determined. (See the next figure; the green shadowed area is the transient period of the signal, while the red shadowed area is the steady state period) So, eventually, the design has proved to be an actual oscillator. But this is just the beginning. The schematic simulated is an ideal one. Very far from a real circuit. This gap must be removed. The last useful information that can be obtained from this ideal circuit is the spectrum of the output signal. Jose M. Campelo Ortiz. Page 100

101 The way of getting the spectrum of a signal in QUCS Studio is by using one of the functions that are available for diagrams. NOTE: Remember that all the mathematical functions that are supported by QUCS Studio can be consulted by pressing the F1 key on the keyboard. The mathematical function needed is time2freq(x). This function provides the fast Fourier transform of the signal x that is used as argument. As the argument x, a node signal of the circuit under analysis must be included. In the case of the schematic of the oscillator, the signal will be OUT. There are several points that must be considered to get the most accurate results from the FFT (fast Fourier transform): 1. The larger the time slot analyzed, the more accurate the results obtained will be. The frequency step of the analysis (the frequency resolution, which is the minimum frequency bandwidth in between two data points of the frequency vector) is related with the inverse of the whole time of the simulation, following the expression: Minimum Frequency Step= 1 Simulation Time 2. The grater number of time samples simulated, the better results under the mandatory Jose M. Campelo Ortiz. Page 101

102 condition of being a multiple of 2. Otherwise, the accuracy of the result will be compromised. 3. The sample frequency, which is defined as the inverse of the time step set for the transient analysis, must be, at least, double of the maximum spectral component foreseen in the signal that is submitted to the FFT algorithm. This will allow the calculation to comply with the Nyquist criteria for the frequency sampling, avoiding aliasing and other mathematical artifacts in the frequency vector calculated by the FFT. NOTE: There is a very detailed and didactic tutorial written by Gunthard Kraus, regarding the basics of QUCS Studio, where the author dedicates a chapter to the FFT calculations. It can be found in the site of the author, or in the QUCS Studio site, in the download section. The procedure to obtain the spectrum of the output signal of the oscillator designed once the transient analysis is performed is the following: 1. Go to the tab result window that comes up next to the schematic one, and grab a new Cartesian Diagram from the project tree window in left side of the screen. In the combo box just above the project tree window the option diagrams must be present. 2. Once the Cartesian Diagram is placed in the result window, the Edit Properties dialog box will appear as normally. In the combo box which is located after the label Dataset all the results windows of the current project are available. This means that it is possible to Jose M. Campelo Ortiz. Page 102

103 represent signals and information in general from any design included in the same project. By default, the dataset selected in the combo box is the one from the schematic that invoked the results window. Just beneath the mentioned combo, all the signals from the labeled nodes in the schematic that have been simulated in the active analysis are available. In this case, OUT.Vt is the interesting one. The sufix.vt is the way of QUCS Studio to note that the information contained in the variable OUT is related to a transient analysis. Jose M. Campelo Ortiz. Page 103

104 3. In the text field right beneath the label Graph Properties is where the time2freq(x) function is going to be used. Click over the OUT.Vt in the Dataset list of variables and it will appear in the text field. Then, it is a question of write down the equation using the proper functions. In this case, they are going to be two of them: the already commented time2freq(x), and the dbm(x). This last one converts in dbm the voltage obtained in one node x of the circuit. These functions can be edited directly in the text field. Once the expression is written, press Apply and Ok in the dialog box and the spectrum will appear as follows: In the previous figure, all the frequency components of the output signal are displayed. It is clear that further than 2e10 Hz, which means 20 GHz, there is no relevant frequency components. Those are the good news. The number of points and the frequency sample chosen are correct. The bad news are several frequency components that are contained in the spectrum analyzed. Normally, as the output of any oscillator it can be foreseen a reduced number of frequency components, corresponding to the frequency of oscillation, normally referred as the fundamental frequency, and a limited number of harmonics. It seems pretty clear that this output signal contains some more Jose M. Campelo Ortiz. Page 104

105 components than those mentioned before. The next step is to analyze if there is some sort of mathematical miscalculation or the problem is other rather different. There is only one possible improvement in the mathematical procedure regarding the FFT. As it was seen in the figure depicted in the page 100, there is an initial lapse of time where the output signal is still going through the transient period. This period of time is included in the calculation of the FFT and this can cause errors in the spectrum obtained. The transient period of the signal lasts until 2.5 or 3 ms. This part of the signal can be removed from the transient analysis and, therefore, from the FFT calculation. This can be done by double clicking over the Transient Simulation box and, in the Edit Component Properties window, setting a new Start of the analysis. By defining a non zero value in this text field, it can be changed the initial time point of the signal register. This means that the first time point registered in the OUT.Vt variable will be, in the example, 4 ms, while the transient simulation will last for 0 ms to 8 ms. Jose M. Campelo Ortiz. Page 105

106 Taking into account that the transient period can be considered to last up to 3 ms, from 4 ms to 8 ms the signal will get the steady state. The previous figure shows that the OUT.Vt reaches the steady state in the lapse of time defined. The shape of this signal in the steady state is the following: Comparing this result of the spectrum with the previous one, the first thing that is really relevant in the output power of the fundamental frequency. In the spectrum where the transient period of the signal is included in the calculation, the power estimated is hardly above 0 dbm. In the second calculation this power Jose M. Campelo Ortiz. Page 106

107 is clearly above 0 dbm. This is a first difference. If the time signal is not properly selected, the data obtained from the spectrum can not be trusted. Another useful comparison can be done. In a frequency band up to 10 GHz the spectrum before (considering the transient period in the analysis) and after are the following: Before: After: Jose M. Campelo Ortiz. Page 107

108 The difference between both spectra is tiny but sufficient to be considered. The first spectrum is less defined than the second one. It seems that the high frequency components have a certain bandwidth which is not something that can be foreseen in the spectrum of an oscillator. The oscillator will produce the fundamental frequency what it was designed for and a series of harmonics. Each of these frequency components should be much more like Dirac deltas in frequency than to some sort of modulated signal. Therefore, the inacuracies shown in the first spectrum analyzed, denotes that the data supplied to the FFT algorithm was not the best to get the more accurate results. The improvement consisting of removing the transient period from the OUT.Vt signal is mainly noticeable looking at the definition of the high frequency components. One important remark in the processing of the spectrum obtained by the FFT is the use of windows for the time2freq(x) function. All the spectrum obtained so far, has been processed before depicting it in all the cases. In the red box of the next figure, it is shown how to apply a window function to the spectrum obtained: Windows are mathematical functions that are used with the FFT to prevent an effect that is kwon as "leakage". This phenomenom occurs when the data that are supplied to the FFT funcition are not exactly periodic. For better understanding how the windows works, please consult "Understanding FFT and Windowing" by National Instruments, or the Application Note AN014 "Understanding FFT Jose M. Campelo Ortiz. Page 108

109 Windows" in the LDS Group website. I also recommend to consult the article FFT Windows Types. Hanning, Flattop, Uniform, Turkey and Exponential by Siemens, where the basics of FFT handling are explained in detail. The available windows for the time2freq function are the following: (extracted from the help file) transforms from time into frequency domain with windowing w (0=none, time2freq(x) 1=Parzen, 2=Welch, 3=Hanning, 4=Hamming, 5=Blackman, 6=30dB/octave roll-off) There is wide consensus that the Hanning window is 95% of the times the best for processing the spectrum of any periodic signal. However, Hanning window is know to have average performance in terms of the accuracy for the amplitude. The window must be used if the time register contains the transient part of the response. If it does not, and the time signal is pure periodic, no window function would be necessary. In fact, it is very easy to verify that the result of the windowing processing using different methods is similar when the time signal submitted to the FFT is periodic and the register contains enough information The windowing has quite an effect in the shape and the absolute values of the components. Next figure depicts the spectrum obtained by removing the windowing calculation included in the previous processed spectra: Spectrum obtained with no window applied. Jose M. Campelo Ortiz. Page 109

110 The spectrum of the oscillation achieved in the present design is processed using different windows. To compare the properties of the different windowing methods, the results of applying each window type available for the time2freq function are shown in the following figures. The input signal to the FFT algorithm has the following parameters: samples of the steady state OUT.Vt signal from 8 us to 20 us. Spectrum obtained using Parzen windowing. Jose M. Campelo Ortiz. Page 110

111 Spectrum obtained using Welch windowing. Spectrum obtained using Hanning windowing. Jose M. Campelo Ortiz. Page 111

112 Spectrum obtained using Hamming windowing. Spectrum obtained using Blackman windowing. Jose M. Campelo Ortiz. Page 112

113 Spectrum obtained using 30dB/octave roll-off windowing. Since the time signal provided to the FFT algorithm was obtained from two absolute time points, from 8 us to 20 us, and there was not special care to determine how the signal started and how it finished, it is almost sure that the time register processed by the FFT will not be pure periodic. That means the use of windowing, is mandatory in order to get the most accurate shape of the spectrum. Another important point to be considered is the frequency up to where the transistor non linear model. Frequencies further than 6 GHz, as it is explained in the spice file where the model is provided by the manufacturer, are not usable. The non linear model is only valid up to 6 GHz. The spectrum of the signal beyond 6 GHz must not be considered. It is time to move forward. Next step in the design must be the transformation into real elements the ideal topology analyzed up to now Jose M. Campelo Ortiz. Page 113