ADS设计压控振荡器VCO.doc

应用ADS设计VCO1.振荡器的基本知识和相关指标1.1振荡器的分类：微波振荡器按器件来分可以分为：双极晶体管振荡器；场效应管振荡器；微波二极管(踢效应管、雪崩管等)振荡器。按照调谐方式分可以分为：机械调谐振荡器；偏置调谐振荡器；变容管调谐振荡器；YIG调谐振荡器；数字调谐振荡器；光调谐振荡器。1.2 振荡器的主要指标： 振荡器的稳定度：这里面包括：频率准确度、频率稳定度、长期稳定度、短期稳定度和初始漂移。频率准确度是指振荡器实际工作频率与标称频率之间的偏差。有绝对频率准确度和相对频率准确度两种方法表示。绝对频率准确度：其中实际工作频率；标称频率。相对频率准确度式绝对频率准确度与标称频率准确度的比值，计算公式为： 频率稳定度：频率稳定度是指在规定的时间间隔内，频率准确度变化的最大值，也有两种表示方法：绝对频率稳定度和相对频率稳定度。频率稳定度还可以分为长期频率稳定度、短期频率稳定度和瞬间频率稳定度。 调频噪音和相位噪音：在振荡器电路中，由于存在各种不确定因素的影响，使振荡频率和振荡幅度随机起伏。振荡频率的随机起伏称为瞬间频率稳定度，频率的瞬间变化将产生调频噪音、相位噪音和相位抖动。振荡幅度的随机欺负将引起调幅噪音。一次，振荡器在没有外加调制时，输出的频率不仅含振荡频率f0，在f0附近还包含有许多旁频，连续分布在f0两边。如下图所示，纵坐标是功率，f0处是载波，两边是噪音功率，包括调频噪音功率和调幅噪音功率。图1正弦信号的噪声边带频谱图2 相位噪声的定义如图2所示，（单边带）相位噪声通常用在相对于载波某一频偏处，相对于载波电平的归一化1Hz带宽的功率谱密度表示（dBc/Hz）。1. 3振荡器的物理模型下图所示的是振荡器的物理模型，主要由谐振网络、晶体管和输入网络这三部分组成。图3本节论述的振荡器采用共基极反馈振荡器，这种类型的振荡器的物理模型如下图所示。图4图5电路组态在微波频率范围内的低频端，常应用集中元件构成振荡器，基本的振荡器电路组态有三种：考毕兹型、哈特莱型及克拉泼型振荡器。如图5所示。考毕兹型(a)应用一电容器作为调谐电路中的分压器，以提供适当的回授能量。哈特莱型(b)应用一抽头式电感调谐电路，而克拉泼型振荡器(c)则相似于考毕兹型，不同的式另外用了一只电容与电感相串连，以改善频率稳定性。在较高的微波频段内，晶体管的极间电容、包括封装寄生电容可提供部分或者全部的回授作用。另外加入反馈网络的目的，则在于增加负阻电阻值，以获得最佳功率输出。 振荡器的直流偏置：微波双极晶体管、场效应晶体管偏置电路的设计如同振荡器的射频电路设计一样重要。因为它关系到微波振荡的稳定性、相位噪音、功率、效率的高低，故应当正确设计偏置电路，并选择最佳直流工作点，以达到最高的射频性能。设计的原则取决于应用。例如用作低噪声振荡器：采用硅双极晶体管时Vce可以在510V、Ice可在38mA内选择；采用砷化镓场效应管时VDS大概为3.5V，IDS大概为810mA，一般选择相当低的漏源电压VDS和电源IDS。1. 4微固态振荡源的设计方法微固态振荡源的传统设计方法，是设计者从给定的技术指标出发，选择振荡器件及电路形式，按简化的等效电路或图解方法，按照现有的设计资料或者以往的经验，初步设计制成电路，调测其特性，然后根据所测性能与技术要求进行比较。如果不满足给定指标，再修改电路直到满足要求为止。而引入了微波电路设计CAD后，这个过程可以作出适当的调整，调整为：定模、分析、最优化。2 设计目标设计一个VCO，要求工作在2.3GHz左右，带宽为400MHz左右。3硅双极性管等效模型分析模型本节的振荡器采用HP公司生产的AT41411硅双极管。主要的指标有：低噪音特性：1GHz时噪音系数是1.4dB；2GHz时噪音系数是1.8dB；高增益：1GHz是增益为18dB；2GHz时增益为13dB；截至频率是：7GHz，有足够宽的频带；直流偏置：Vce8V；Ic10 mA封装形式：STO143 因为该振荡器工作的频率有2GHz这么高，这个时候晶体管之间的结电容和封装管子引入的引线电感和分布电容就必须要考虑了。图6是双极性硅管的高频信号模型，具体的典型参数值在后表。图7是考虑了封装后的双极性硅管的高频信号模型，具体的典型参数值也见后表。由于这些参数HP公司是没有提供的，只提供了S参数，所以我们不能用这种小信号模型来做仿真，只能利用这些小信号模型来估算振荡器其他部件的参数值。HP_AT41411在ADS的器件库里面带有，可以直接使用。图6图7符号元件名典型值Re2发射极扩展电阻8.6 ohmRe1发射极空间电荷电阻0.7 ohmRs集电极扩展电阻7.0 ohmCe发射极基极结电容1.0 pFCc集电极发射极电容0.005 pFCce集电极发射极电容0.05 pFRb基极扩展电阻14.7 ohmo零频率是共基极电流放大倍数0.99表1 硅双极管管芯等效电路元件典型值符号元件名典型值C1、C2各封装点之间的电容C1:0.06-0.1 pFC2:0.01-0.012 pFC3:0.001-0.003 pFC4:0.01-0.013 pFC3、C4C5输出、输入端之间的电容0.005 pFL1、L4参考面与封装边缘之间的引线电感L1:0.2-0.3nH；L4:0.4-0.6nHL2、L3封装边缘与金属丝接点之间的引线电感0.2-0.5nHL5芯片至发射极端子的金丝电感0.3-0.6nH表2 封装参数典型值4 确定实际电路图8是本节振荡器采用的具体电路，其电路结构如图9所示图8图9把结电容和封装电感、电容考虑进去后，振荡器的谐振回路等效为图10所示，这样需要设计的只有：偏置电路、变容管的VC特性和振荡器的调试以及相位噪音分析。图10 谐振回路等效电路5 具体设计过程5.1创建一个新项目 启动ADS 选择Main windows 菜单FileNew Project，然后按照提示选择项目保存的路径和输入文件名 点击“ok”这样就创建了一个新项目。 点击，新建一个电路原理图窗口，开始设计振荡器。5.2偏置电路设计 在电路原理图窗口中点击，打开Component library 按“ctrl+F1”打开搜索对话窗口 搜索器件“ph_hp_AT41411”这就是我们在该项目中用到的Agilent公司的晶体管 把搜索出来的器件拉到电路原理图中，按“Esc”键可以取消当前的动作。 选中晶体管，按可以旋转晶体管，把晶体管安放到一个合适的位置。 在中选择probe components 类，然后在这个类里面选择并安放在适当的位置，同理可以在“SourcesTime Domain”里面选择，在lumped components里面选择，并按照图11放好。 在optim/stat/Yield/DOE类里面选择，这里需要两个，还有一个 在SimulationDC里面选择一个 上面的器件和仿真器都按照下图11放好，并单击连好线 按这时会出现一个这样的对话框，输入你需要的名字并在你需要的电路图上面点一下，就会自动给电路接点定义名字，如图11所示定义“Vcb”，“Veb”节点名称图11直流偏置计算 双极，把该I_Probe的名称改为ICC 同样，另外一个接晶体管S极的I_Probe改为“IEE” 双击其中一个并修改里面的内容，如图12所示图12 双击另外一个，并修改里面的内容如图13所示图13 双击并把里面的Optimization Type修改为“Gradient”类型 把接在“C极”上的电阻改为，把电源改为“12V” 把接在“S极”上的电阻改为，把电源改为“5V” 按“F7”快捷键进行仿真 在Data Display窗口，就是新出来的窗口中，按键，会选择“R.R1；R.R2”这样就会显示出优化的直流电阻的数值，如图14所示。图145.3变容管测量 新建一个电路原理图窗口 如上面的做法一个，建立如图15所示的电路图，其中“Term”、“S-PARAMETE”、“PARAMETER SWEEP”都可以在“SimulationS_Param”里面找到。变容管的型号是“MV1404”可以在器件库里面找到，方法可以参考上面查找晶体管的方法。图15 可变电容VC曲线测量 按并双击它，修改里面的项目，定义一个名为：“Vbias”的变量 修改电源的属性，把Vdc改为“Vbias” 双击，并修改属性，要求单点扫描频率点2.3GHz，并计算“Z参数” 双击，并修改属性，要求扫描变量“Vbias” ，选择Simulatuion1“SP1” 按“F7”进行电路仿真。 在“Date Display”按，并在对话框里编辑公式为： 按，并单击“advance”选项，把“C_Varactor”输入对话框里面，点击“确定”就可以显示如图16所示的曲线。图16 VC曲线 按，同样单击单击“advance”选项，把“C_Varactor”输入对话框里面，点击“确定”就可以显示如图17所示的表格。图17利用该VC曲线，结合硅双极管的管芯模型和封装模型，按照典型值，利用等效谐振图可以计算出该振荡器的谐振频率在反馈电感为0.2nH级这个数量级的时候，振荡频率为4.0GHz左右，考虑到该模型只有定性参考价值，所以确定该振荡器结构，并可以在仿真过程中，不断的修改和优化电路参数，使得振荡器达到设计要求。5.4振荡器瞬时仿真利用Transient Simulation仿真器可以做振荡器的瞬时仿真，看到实时波形。 新建一个电路原理图文件 在这张电路原理图中，按照上面的方法，建立如图18所示的电路图图18振荡器电路原理图注意：记得要添加“Vout”这个节点名称，还有假如器件找不到的，在器件库里面查找，具体情况可以参考查找“晶体管”一节。 在“SimulationTransient”类里面找到瞬时仿真器，并双击修改里面的参数，如下图19所示。其中“star time”表示开始仿真的时间；“stop time”表示结束仿真的时间，“MaxTimeStep”表示最大的抽样时间，这里按照抽样定理对最大的抽样时间是有要求的，具体的算法和介绍可以参考ADS的帮助文档，在文档里面查找“Transient“就可以了。图19 瞬时仿真器配置 按“F7”开始仿真 在出来的“Data Display”窗口里面，按，选择“Vout”按确定，这样就可以看到“Vout”点的瞬时波形，按，并“new”一个新的“Marker”，在“Vout”的瞬时波形图中，点击一下，然后移动鼠标，把“marker”移动到需要的地方，就可以看到该点的具体数值。结果如下图20所示。图20 按，编辑公式：这表示要对“Vout”在“Marker”m1，m2之间进行一个频率变换，这样出来的“Spectrum”就是m1和m2之间的频谱。 按，在“advanced”里面加入“Spectrum”点击“OK”就可以看到m1和m2之间的频谱分量，加入“marker”m3就可以知道振荡器大概振荡的频率。如图21所示。图20 m1，m2之间的频谱5.5振荡器的谐波平衡仿真 新建一个电路原理图或者就在“Transient仿真电路图”里面，把电路原理图改为如下图21所示的电路图图21 谐波平衡仿真的电路图这和瞬时仿真唯一不同的就是多加入了一个“OscPort”器件在反馈网络和谐振网络之间，这是谐波平衡法仿真相位噪音的需要，具体的情况可以参考ADS的帮助文档，查找“OscPort”就可以看到很具体的帮助信息。其中“OscPort”是在类“Simulation-HB”里面。 在类“Simulation-HB”里面把仿真器拉出来，并双击配置这个谐波平衡仿真器第一步：设置频率和“Order”如下图22所示图22第二步设置参数，主要是把“OverSample”改为4，如下图23所示图23第三步：设置噪音计算，把最后一行的“Nonlinear noise”和“Oscillator”都选上，然后在“Noise frequency”里面选择的扫描方式是“log”相位噪音的计算从1Hz到10MHz，并把“FM noise”调频噪音也计算出来，具体如下图24所示。图24第四步：“noise2设置”主要就是把“Vout”加进去，并选择“sort by value”具体见下图图25第四步：在“Osc”选项里面把Osc1加进去，这就是我们加入的那个OscPort类器件。图26其他地方也不用修改了，最后就得到配置好的谐波平衡仿真器，见图27图27谐波平衡仿真器 按“F7”进行仿真。 在“Data Display”窗口里面按照上面的方法，把需要的数据都显示出来见下图图28 时域波形图28是时域波形，注意是要加入“Eqn”的图29谐波频率和幅度 图30相位噪音仿真结果这里的pnmx是相位噪音，单位为dBc/Hz；anmx是调幅噪音，单位为dBc/Hz；pnfm是附加相位噪音，单位为dBc/Hz。其中pnfm和anmx都是通过频率灵敏度分析来获得的，pnmx是通过混频分析获得的。具体分析，可以参考ADS帮助文档，查找“pnmx”就可以。图31相位噪音的具体数值5.6振荡器振荡频率线性度分析 把控制变容管电压的电源属性修改一下，“Vdc”设置为变量“Vtune”，增加一个VAR变量“Vtune” 修改谐波平衡仿真器，这时不计算噪音，只是扫描变量“Vtune”，所以可以把最后一行的“Nonlinear noise”不给予选上。 建议把原来做过谐波平衡，分析相位噪音的谐波平衡仿真器去掉，在重新拉一个回来，这样修改的项目就不多，下面以新来的谐波平衡仿真器为例，说明一下，现在这个谐波平衡仿真器应该修改的地方。第一步：修改频率图32第二步：修改“Sweep”，这是说明扫描Vtune变量的具体情况的，参见图33图33第三步：加入“Osc1”这和前面的一样的，不再重复。 按“F7”进行仿真 显示仿真结果如下图所示：图33电压频率曲线图34功率频率曲线图36频率、谐波功率曲线6总结从最后的仿真结果可以看出，设计的任务还是完成了，因为ADS涉及的内容太多了，所以建议大家都看看帮助，帮助里面的查找功能非常强大的，基本上在ADS上遇到的问题都可以从帮助里面找到答案，另外ADS器件库的搜索功能除了慢点外，其他的也是挺好的，假如有什么器件一时找不到了，也建议使用器件库来搜索。7 附录Manuals Intro and Simulation Components Chapter 5: Simulation Control Items Print version of this Book (PDF file) Simulation Parameters: HB The tabs in the Harmonic Balance dialog box allow you to set the following parameters: Freq sets parameters related to the frequencies of fundamentals. Sweep sets parameters related to sweeps, and references sweep plans. Params sets status and device operating point levels, as well as parameters related to FFT oversampling and convergence. Small-Sig sets parameters related to small-signal/large-signal simulation. Noise (1) sets parameters related to noise simulation, including sweeps. Input and output ports can be defined here. FM noise can be selected for oscillator simulations. Noise (2) selects nodes at which to calculate noise data, and sorts the noise contributors. Port noise options are provided here also. NoiseCons is used to specify which NoiseCon nonlinear noise controllers should be simulated, allowing more flexible noise simulations to be performed than Noise(1) and Noise(2) allow. Osc sets parameters related to oscillator simulation. Solver allows you to choose between a Direct or Krylov solver or to enable an automatic selection. Output allows you to selectively save your simulation data to a dataset. Display shows or hides parameters in the Schematic window. The available parameters and options are described in the following sections. Nodes for Calculation of Noise Parameters Use this area to select nodes at which you want linear noise data to be reported. Noise voltages and currents are reported in rms units. Freq Fundamental Frequencies Maximum order is the maximum order of the intermodulation terms in the simulation. For example, assume there are two fundamentals and Order (see below) is 3. If Maximum order is 0 or 1, no mixing products are simulated. The frequency list consists of the fundamental and the first, second, and third harmonics of each source. If Maximum order is 2, the sum and difference frequencies are added to the list. If Maximum order is 3, the second harmonic of one source can mix with the fundamental of the others, and so on. The combined order is the sum of the individual frequency orders that are added or subtracted to make up the frequency list. Frequency is the frequency of the fundamental(s). Order is the maximum order (harmonic number) of the fundamental(s) that will be considered. Select edits the fundamental frequencies and their orders (by double-clicking). Add adds a frequency and its associated fundamental and order. Cut deletes a frequency and its associated fundamental and order. Paste takes a frequency item that has been cut and places it in a different order in the Select window. Sweep Refer to Sweep. Params Budget Perform Budget simulation reports current and voltage data into and out of devices following a simulation. Current into a device is identified as .device_name.t1.i, and out of that device as .device_name.t2.i. Voltage at the input to a device is identified as .device_name.t1.v, and at the output of that device as .device_name.t2.v. Levels Refer to Levels. FFT Oversample sets the FFT oversampling ratio. Higher levels increase the accuracy of the solution by reducing the FFT aliasing error and improving convergence. Memory and speed are affected less when the direct harmonic balance method is used than when the Krylov option is used. More brings up a small dialog box. To increase simulation accuracy, enter in the field an integer representing a ratio by which the simulator will oversample each fundamental. Convergence Auto mode automatically adjusts key convergence parameters and resimulates to achieve convergence. As it trades efficiency for ease of use, it is suited to beginning ADS users who are unfamiliar with the ADS parameters to control the convergence. Manual mode enables an advanced damped Newton solver. This solver guarantees a robust and steady march toward the solution with each harmonic balance iteration. The convergence rate is enhanced by its selection of a near-optimal damping constant, choice of several individual norms in the convergence checks, and control over the residual reduction threshold at each iteration. Max. iterations is the maximum number of iterations to be performed. The simulation will iterate until it converges, an error occurs, or this limit is reached. Restart instructs the simulator not to use the last solution as the initial guess for the next solution. Use Initial Guess (Harmonic Balance) Check this box to save your initial guess to a dataset that can be referred to for a subsequent harmonic balance simulation, including circuit envelope.For example, if you have saved the HB solution, you can later do a nonlinear noise simulation and use this saved solution as the initial guess, removing the time required to recompute the nonlinear HB solution. Or you could quickly get to the initial HB solution, and then sweep a parameter to see the changes. In this later case, you will probably either want to disable the Write Final Solution (see following topic), or use a different file for the final solution, to avoid over-writing the initial guess solution. If no file name is supplied, a default name is generated internally, using the design name and appending the suffix .hbs. A suffix is neither required nor added to any user supplied file name. The Annotate value specified in the DC Solutions tab in the Options block is also used to control the amount of annotation generated when there are topology changes detected during the reading of the initial guess file. Refer to the section DC Solutions. Since HB simulations also utilize the DC solution, to get optimum speed-up, both the DC solution and the HB solution should be saved and re-used as initial guesses. The initial guess file does not need to contain all the HB frequencies. For example, one could do a one-tone simulation with just a very nonlinear LO, save that solution away and then use it as an initial guess in a two tone simulation. The exact frequencies do not have to match between the present analysis and the initial guess solution. However, the fundamental indexes should match. For example, a solution saved from a two tone analysis with Freq1 = 1GHz and Freq2 = 1kHz would not be a good match for a simulation with Freq1 = 1kHz and Freq2 = 1 GHz. If the simulator cannot converge with the supplied initial guess, it then attempts to a global node-setting by connecting every node through a small resistor to an equivalent source. It then attempts to sweep this resistor value to a very large value and eventually tries to remove it. Final Solution (Harmonic Balance) Check this box to save your final HB solution to the output file. If a filename is not supplied, a file name is internally generate using the design name, followed by an .hbs suffix. If a file name is supplied, the suffix is neither appended nor required. If this box is checked, then the last HB solution is put out to the specified file. If this is the same file as that used for the Initial Guess, this file is updated with the latest solution. Transient simulations can also be programmed to generate a harmonic balance solution that can then be used as an initial guess for an HB simulation. Refer to the section, Compute HB Solution. Small-Sig This feature employs a large-signal/small-signal method to achieve much faster simulations when some signal sources (a) are much smaller than others, and (b) can be assumed not to exercise circuit nonlinearities. For example, in a mixer the LO tone could be considered the large-signal source and the RF the small-signal source. To edit these parameters and request a small-signal analysis, click Small-signal at the bottom of the dialog box. Small-signal frequency Refer to Sweep. Use all small-signal frequencies solves for all small-signal mixer frequencies in both sidebands. This default option requires more memory and simulation time, but is required for the most accurate simulations. Merge small- and large-signal frequencies By default, the simulator reports only the small-signal upper and lower sideband frequencies in a mixer or oscillator simulation. Selecting this option causes the fundamental frequencies to be restored to the dataset, and merges them sequentially. Noise (1) To edit these parameters and request a noise analysis, click Nonlinear noise at the bottom of the dialog box. Noise frequency Use this area to select the frequency(s) at which nonlinear noise is computed. Sweep Type Refer to Sweep Type. Input Frequency Because the simulator uses a single-sideband definition of noise figure, the correct input sideband frequency must be specified here. This parameter identifies which input frequency will mix to the noise frequency of interest. In the case of mixers, Input frequency is typically determined by an equation that involves the local oscillator (LO) frequency and the noise frequency. Either the sum of or difference between these two values is used, depending on whether upconversion or downconversion is taking place. The above parameters do not need to be specified if only the output noise voltage is desired (that is, if no noise figure is computed). Noise input port is the number of the source port at which noise is injected. This is commonly the RF port. Although any valid port number can be used, the output port number is frequently defined as Num=1. Noise output port is the number of the Term component at which noise is retrieved. This is commonly the IF port. Although any valid port number can be used, the input port number is frequently defined as Num=2. Include FM noise (osc. only) causes an FM noise analysis to be performed in addition to a mixing noise analysis for oscillator phase noise. This simulates a second model for phase noise, which may be more accurate at small offset frequencies. Noise (2) To edit these parameters and request a noise analysis, click Nonlinear noise at the bottom of the dialog box. Nodes for noise parameter calculation Use this area to select named nodes at which the simulator will compute noise. NoteThe fewer the number of nodes requested, the quicker the simulation and the less memory required. Edit selects the named node(s) for the simulator to consider. Select holds the names of the nodes the simulator will consider. Add adds a named node. Cut deletes a named node. Paste takes a named node that has been cut and places it in a different order in the Select window. Noise Contributors Use this area to sort contributions to noise, as well as a threshold below which noise will not be reported. Mode provides the following options: Off causes no individual noise contributors (nodes) to be selected. The result is simply a value for total noise at the node. Sort by value sorts individual noise contributors, from largest to smallest, that exceed a user-defined threshold (see below). The subcomponents of the nonlinear devices that generate noise (such as Rb, Rc, Re, Ib, and Ic in a BJT) are listed separately, as well as the total noise from the device. Sort by name causes individual noise contributors to be identified and sorts them alphabetically. The subcomponents of the nonlinear devices that generate noise (such as Rb, Rc, Re, Ib, and Ic in a BJT) are listed separately, as well as the total noise from